Tech-World Manufacturing. Design. Level two. CELL Guide. Edition E0

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1 Tech-World Manufacturing Design Level two Edition E0

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3 FIFTH EDITION First Printing, February 2011 Copyright 2005, 2006, 2007, 2008, 2009, 2010, 2011 Lab-Volt Systems, Inc. All rights reserved. No part of this publication may be reproduced, stored in a retrieval system, or transmitted in any form by any means, electronic, mechanical, photocopied, recorded, or otherwise, without prior written permission from Lab-Volt Systems, Inc. Information in this document is subject to change without notice and does not represent a commitment on the part of Lab-Volt Systems, Inc. The multimedia Tech-World software and other materials described in this document are furnished under a license agreement or a nondisclosure agreement. The software may be used or copied only in accordance with the terms of the agreement. ISBN Lab-Volt and Tech-World are registered trademarks of Lab-Volt Systems, Inc. Windows is trademarks of Microsoft Corp. SolidWorks is a registered trademark of SolidWorks Corp. Lab-Volt recognizes product names as trademarks or registered trademarks of their respective holders.

4 Lab-Volt License Agreement By using the software in this package, you are agreeing to become bound by the terms of this License Agreement, Limited Warranty, and Disclaimer. This License Agreement constitutes the complete agreement between you and Lab-Volt. If you do not agree to the terms of this agreement, do not use the software. Promptly return the software and all other materials that are part of Lab-Volt's multimedia Tech-World product within ten days to Lab-Volt for a full refund or credit. 1. License Grant. In consideration of payment of the license fee, which is part of the price you paid for this Lab-Volt product, Lab-Volt, as Licensor, grants to you, the Licensee, a nonexclusive, nontransferable license to use this copy of the software with the corresponding curriculum resources. Lab- Volt reserves all rights not expressly granted to the Licensee. 2. Ownership. 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You may make copies of the software solely for backup purposes provided the copyright notice is reproduced in its entirety on the backup copy. 4. Permitted Uses. This software and all accompanying documentation is licensed to you, the Licensee, and may not be transferred to any third party for any length of time without the prior written consent of Lab-Volt. You may not modify, adapt, translate, reverse engineer, decompile, disassemble, or create derivative works based on the Lab-Volt product without the prior written permission of Lab-Volt. Written materials provided to you may not be modified, adapted, translated, or used to create derivative works without the prior written consent of Lab-Volt. 5. Termination. This agreement is effective until terminated. It will terminate automatically without notice from Lab-Volt if you fail to comply with any provisions contained herein. Upon termination you shall destroy the written materials, Lab-Volt's software, and all copies of them, in part or in whole, including modified copies, if any. 6. Registration. Lab-Volt may from time to time update the software. Updates can be made available to you only if a properly signed registration card is filed with Lab-Volt or an authorized registration card recipient. 7. Miscellaneous. This agreement is governed by the laws of the State of New Jersey. Limited Warranty and Disclaimer This software has been designed to assure correct operation when used in the manner and within the limits described in the Tech-Lab Multimedia Installation & User s Guide. As a highly advanced software product, it is quite complex; thus, it is possible that if it is used in hardware configurations with characteristics other than those specified in Tech-Lab Multimedia Installation & User s Guide or in environments with non-specified, unusual, or extensive other software products, problems may be encountered by a user. In such cases, Lab-Volt will make reasonable efforts to assist the user to properly operate the software but without guaranteeing its proper performance in any hardware or software environment other than as described in the Tech-Lab Multimedia Installation & User s Guide. This software is warranted to conform to the descriptions of its functions and performance as outlined in the courseware documentation. Upon proper notification and within a period of one year from the date of installation and/or customer acceptance, Lab-Volt, at its sole and exclusive option, will remedy any nonconformity or replace any defective compact disc free of charge. Any substantial revisions of this product, made for purposes of correcting software deficiencies within the warranty period, will be made available, also on a licensed basis, to registered owners free of charge. Warranty support for this product is limited, in all cases, to software errors. Errors caused by hardware malfunctions or the use of nonspecified hardware or other software are not covered. LICENSOR MAKES NO OTHER WARRANTIES OF ANY KIND CONCERNING THIS PRODUCT, INCLUDING WARRANTIES OR MERCHANTABILITY OR OF FITNESS FOR A PARTICULAR PURPOSE. LICENSOR DISCLAIMS ALL OBLIGATIONS AND LIABILITIES ON THE PART OF LICENSOR FOR DAMAGES, INCLUDING BUT NOT LIMITED TO SPECIAL OR CONSEQUENTIAL DAMAGES ARISING OUT OF OR IN CONNECTION WITH THE USE OF THE SOFTWARE PRODUCT LICENSED UNDER THIS AGREEMENT. Questions concerning this agreement and warranty and all requests for product repairs should be directed to Lab-Volt field representative in your area. LAB-VOLT SYSTEMS, INC. P.O. Box 686 Farmingdale, NJ Attention: Program Development Phone: (732) or (800) LAB-VOLT Fax: (732) Technical Support: (800) Technical Support

5 Table of Contents Table of Contents Introduction... 1 Topic 1 Product Design... 3 Activity 1 Learning New Features in SolidWorks... 4 Activity Directions: Creating a Candlestick... 4 Activity 2 Designing to Specification Activity Directions: Design and Model Topic 2 Universal Design Activity 1 Applying the Principles of Design Activity Directions: Modifying the Design Activity 2 Universal Design for Play Activity Directions: Creating your Toy Activity Directions: Visualization Topic 3 Final Project - Basic Parts of the Mountain Board Activity 1 Creating the Basic Parts Activity Directions: Creating the Binding Anchor Activity Directions: Creating the Binding Base Plate Activity Directions: Creating the Binding Assembly Activity 2 Creating the Revolved Features Activity Directions: Creating the Hub Activity Directions: Importing Data Activity Directions: Importing Data Activity 3 Creating the Deck Activity Directions: Creating the Deck Topic 4 Final Project - Multibody Parts of the Mountain Board Activity 1 Creating the Axle and Truck Activity Directions: Creating the Axle Activity Directions: Creating the Truck Activity 2 Springs and Binding Activity Directions: Creating the Springs and Binding Topic 5 Final Project Final Assembly Activity 1 Final Assembly Activity Directions: Final Assembly Activity 2 Presenting the Results i

6 Table of Contents Activity Directions: Final Rendering Appendix A Internet Resources...A-1 ii

7 Introduction INTRODUCTION This is to be used with the multimedia presentation and Student Guide/Portfolio. The remains at the workstation and contains information and procedures that are specific to the CELL. This includes topic information, hands-on instructions, and appendices specific to the CELL. The information in the follows the arrangement below: topic objective topic overview new terms and words activity objectives procedures for completing activity tasks Appendices include Safety, Internet Resources, or other CELL specific tables or charts. Tips for navigating the multimedia presentation are detailed in the Tech-Lab Multimedia User Guide. There should be a copy of this at the student workstation. If this is not available, please ask your instructor. 1

8 Introduction 2

9 Topic 1 Product Design TOPIC 1 PRODUCT DESIGN Objective When you have completed this topic, you will have experience implementing the design process and have an opportunity to express your creativity and ingenuity. You will explore new features in SolidWorks and use these features to create your designs. Overview Welcome to the Tech-World Level 2 Design CELL. In Level 1 you learned the steps of the design process and explored design criteria. You were introduced to SolidWorks and learned how to create 3D objects made up of features. You also demonstrated how to create 2D drawings of the 3D parts and assemblies you designed. In Level 1 you explored traditional design cycles and demonstrated the benefits of design analysis. In Level 2 you will continue to use SolidWorks, learning new features and applying these features to your designs. You will apply the skills you learn to a series of design projects. You will read design briefs and brainstorm possible solutions. 3

10 Topic 1 Product Design Activity 1 Learning New Features in SolidWorks Objective When you have completed this activity, you will have the knowledge and skills to explore new features in SolidWorks and use these features to create your designs. You will be able to: demonstrate the revolved boss, swept boss, extruded cut, and fillet features in SolidWorks. create a candlestick using SolidWorks. create the candlestick handle by using a sweep in SolidWorks. Activity Directions: Creating a Candlestick SolidWorks should be on your screen. If it isn't, click on the Application Launch button and choose SolidWorks from the menu. 1. To create a new part, click on the Standard toolbar. The New SolidWorks Document dialog box appears. 2. Click the Tutorial tab. (Note: If the Tutorial tab is not visible, click on the Advanced button first.) Select the Part icon. Click OK. 3. A new part document window appears. (If the Quick Tips window is open, click on Help and select Quick Tips to remove the window.) 4. Remember, if you place your mouse over a command or tool, the description of that item appears. Take a moment to mouse-over the commands to get reacquainted with the SolidWorks tools. 5. Click on the Features tab to display the Features toolbar and then click on Revolved Boss/Base. 6. The Front, Top, and Right planes appear. Select the Front plane. A sketch opens on the Front plane. 4

11 Topic 1 Product Design 7. Click on View and make sure Sketch Relations is selected. If not, select it. 8. Click Line on the Sketch toolbar. Sketch a vertical line from the origin, and then sketch the two horizontal lines as shown. Do not worry about the length of the lines; you ll dimension the lines next. *Remember, to first move the pointer to the sketch origin. *The pointer is on the origin when the pointer changes to. Click, hold, and drag to draw the line. Release the mouse to complete the line. Repeat for all the lines. (Press the Esc key to exit the Line tool.) 9. Click the Smart Dimension tool on the Sketch toolbar. Dimension the lines as shown. *Remember, when the pointer shape changes to click on the vertical line. Move the mouse to the left of the line and click to display the dimension text. Enter the dimension shown, 220, and press Enter. Do the same for the horizontal lines, entering the dimensions shown. Press the Esc key to exit Smart Dimension. All the lines are black and the bottom of the screen reads Fully Defined. If the sketch is not fully defined, select Edit/Undo and dimension the lines again. 5

12 Topic 1 Product Design NOTE: Press Z on the keyboard and/or Shift + Z to zoom in and out. 10. Save your work by selecting File and then Save. Save your part in the C:\DesignL2 folder. Name your part Cstick your last name.sldprt. Click Save. You will now create the small arc at the top of the sketch. 11. Click the 3 Point Arc tool on the Sketch toolbar. 12. Click the endpoint of the top horizontal line, and then move the pointer downward. (As you sketch, inferencing pointers and lines help you align the pointer with existing sketch entities and model geometry.) 13. When the length is approximately 20mm (L=20), click again. Move the pointer to the right to adjust the angle of the arc. When the angle of the arc is 180 (A=180 ) and the radius is approximately 10mm (R=10), click again. Click Smart Dimension on the Sketch toolbar and dimension the arc radius to 10. Press the Esc key to exit Smart Dimension. The arc is black. NOTE: Press Z on the keyboard and/or Shift + Z to zoom in and out. 6

13 Topic 1 Product Design Next, you will create another vertical line and the second arc. 14. Click Line on the Sketch toolbar. 15. Click, hold, and drag to sketch a vertical line downward approximately 150mm long, starting at the lower endpoint of the arc, release the mouse. Do not dimension the line at this time. 16. Click 3 Point Arc on the Sketch toolbar. 17. Sketch an arc so that the arc endpoints are coincident with the line. (Watch for the pointer.) Use the following measurements: length approximately 40mm (L=40) angle 180 (A=180) radius approximately 20mm (R=20) 7

14 Topic 1 Product Design 18. Click Smart Dimension on the Sketch toolbar. Dimension the arc radius to Click Trim Entities on the Sketch toolbar. In the PropertyManager, under Options, click Trim to closest button. Click OK. 20. Select the line between the endpoints of the arc you just drew to delete it. 21. Select Smart Dimension and dimension the upper vertical line to 40, as shown. NOTE: Press Z on the keyboard and/or Shift + Z to zoom in and out. 22. Save your work. 8

15 Topic 1 Product Design 23. Click Select on the Standard toolbar, then hold down Ctrl and select the vertical lines on each side of the lower arc. 24. In the PropertyManager, under Add Relations, click the Equal button. Click OK. The Equal relation ensures that both vertical lines will maintain equal length. 25. Click Tangent Arc on the Sketch toolbar, and then click the endpoint of the lower vertical line. 9

16 Topic 1 Product Design 26. Move the pointer downward to create an arc that has an angle of 90 and a radius of approximately 60mm. Click to place the arc. 27. Now move the pointer until the endpoint of the arc is coincident with the endpoint of the bottom horizontal line as shown. 28. Your drawing should look like this: 10

17 Topic 1 Product Design 29. Click View, Sketch Relations to hide the sketch relations in the graphics area. 30. Dimension the rest of the sketch as shown. HINT: 31. When you are done dimensioning, the sketch is fully defined (all lines and endpoints are black). 11

18 Topic 1 Product Design 32. Save your work and then click Exit Sketch on the Sketch toolbar. The Revolve PropertyManager appears. 33. Click on the center line. 34. Under Revolve Parameters: Select One-Direction in Revolve Type. Set Angle to 360. Click OK. 35. Save your work. 12

19 Topic 1 Product Design Sketching the Sweep Path A sweep is a base, boss, or cut created by moving a section along a path. You will create the candlestick handle by using a sweep. 1. First, you will sketch the sweep path. Select the Front plane in the FeatureManager design tree. 2. Click Sketch on the Sketch toolbar to open a new sketch (or click on the down arrow on the Sketch button and select Sketch). 3. Click Front on the Standard Views toolbar. 4. Click Hidden Lines Removed on the View toolbar. 13

20 Topic 1 Product Design 5. Click View, Temporary Axes. Notice that the temporary axis of the revolved base appears. 6. Select Line from the Sketch toolbar, and move the pointer over the temporary axis. The pointer changes to temporary axis. indicating that the pointer is exactly on the 7. Click, hold, and drag to sketch a horizontal line as shown. Dimension the line to Select Tangent Arc from the Sketch toolbar. 9. Sketch an arc starting at the endpoint of the line. Dimension the arc to a radius of 150. Click again to end the arc. *Remember to click Zoom to Fit to see your part. 10. Using Smart Dimension set the vertical dimension to 65 by first clicking on the starting endpoint of the arc and then clicking on the final endpoint. 11. Save your work. 14

21 Topic 1 Product Design 12. Select Tangent Arc and then sketch another arc as shown. Dimension it to a radius of Click Select on the Standard toolbar. Hold down the Ctrl key and select the endpoints of the tangent arc you just sketched. The Properties PropertyManager appears. The two endpoints are listed under Selected Entities. 14. Under Add Relations, click Horizontal. 15. Click OK. The dimensions and relations prevent the sweep path from changing size and shape when moved. 16. Click on the down arrow on the Sketch button and select Display/Delete Relations. 17. In the PropertyManager, under Relations, select All in this sketch in the drop down box. 18. Click OK. 19. Save your work. 15

22 Topic 1 Product Design 20. Now you will dimension the sweep path with respect to the revolved base. Using Smart Dimension, dimension the distance between the horizontal line of the sweep path and the bottom edge of the revolved feature to

23 Topic 1 Product Design 21. The sweep path is fully defined. Save your work. Click Exit Sketch on the Sketch toolbar. Sketching the Sweep Section After you sketch the sweep path, you need to sketch the sweep section. 1. Select the Right plane in the FeatureManager design tree and then click Sketch on the Sketch toolbar to open a new sketch. 2. Click Normal To on the Standard Views toolbar. 17

24 Topic 1 Product Design 3. Click Ellipse on the Sketch toolbar, or select Tools, Sketch Entities, Ellipse. Move your cursor anywhere in the graphics area. Position the pointer at the center of the ellipse. Click the left mouse button, and then move the pointer horizontally to define the width of the ellipse. Click the left mouse button a second time. Move the pointer vertically to define the height. Click the left mouse button a third time. This completes sketching the ellipse. 4. Click Select on the Standard toolbar. Hold down the Ctrl key and click the endpoints of the ellipse. 5. In the PropertyManager, under Add Relations, click Horizontal, and then click OK. This relation ensures that the ellipse is not slanted. 6. Using Smart Dimension, dimension the ellipse as shown. Press the Esc key to exit Smart Dimension. *Remember, click the left and right endpoints for the 35 dimension; and the top and bottom endpoints for the 10 dimension. 7. Click Isometric on the Standard Views toolbar. 18

25 Topic 1 Product Design 8. Hold down the Ctrl key and click the center point of the ellipse and the endpoint of the horizontal line of the (handle) sweep path. (Do not select the origin point). *Remember, press Shift + Z to zoom in. 9. In the PropertyManager, under Add Relations, click Coincident, and then click OK. This coincident relation ensures that the center point of the sweep section lies on the plane of the sweep path. 10. Click View, Temporary Axes to hide the temporary axis. 11. Click Exit Sketch on the Sketch toolbar. 12. Save your part. Now you will combine the sweep path and sweep section sketches to create the sweep. 13. Click Swept Boss/Base on the Features toolbar. 19

26 Topic 1 Product Design 14. Select Sketch3 (the ellipse) in the graphics area for Profile by clicking on the ellipse. Sketch3 appears in the PropertyManager. 15. Select Sketch2 (the path) in the graphics area for Path by clicking on the handle. Sketch 2 appears in the PropertyManger. A profile of the sweep appears in the graphics area. Note how the colors in Profile and Path match those in the graphics area. 16. Under Options, select Follow Path in Orientation/twist type. 17. Click OK to create the sweep. Creating a cut for the candle 1. The final step is to create a cut to hold a candle. Select the top face of the revolved base feature, and then click Extruded Cut on the Features toolbar. 20

27 Topic 1 Product Design 2. Click Normal To on the Standard Views toolbar. 3. Click Circle on the Sketch toolbar, and select the sketch origin. Sketch and dimension a circle as shown. 4. Click Exit Sketch on the Sketch toolbar. 5. In the PropertyManager, under Direction 1: Select Blind in End Condition. Set Depth to 25. Click the Draft On/Off button, and set Draft Angle to 15. Click OK. 6. To see the angled cut, click Hidden Lines Visible on the View toolbar, and rotate the part using the arrow keys on the keyboard. 7. Select Shaded with Edges on the View toolbar. Use the arrow keys to see all views of your part. 8. Save the part. Print your part by selecting File and then Print. Close all Windows. Click on the Forward arrow to resume the activity. 21

28 Topic 1 Product Design Activity 2 Designing to Specification Objective When you have completed this activity, you will have the knowledge and skills to determine a design solution that satisfies the requirements of a design brief. You will be able to: design a product to meet the design specifications. demonstrate how to use the revolve and sweep features in SolidWorks. Activity Directions: Design and Model SolidWorks should be on your screen. If it isn't, click on the Application Launch button and choose SolidWorks from the menu. The following instructions are to guide you with your own design. You can make your mug simple or complex. SAMPLE MUG 1. Click on new part, click on the Standard toolbar. 2. Click on the Features tab to display the Features toolbar and then click on Revolved Boss/Base. 3. Select the Front plane. 4. Click Line on the Sketch toolbar. Sketch a vertical line from the origin, and then sketch the two horizontal lines as shown. Dimension the lines as shown also. 22

29 Topic 1 Product Design *Remember - press the Esc key to exit the current tool or command. NOTE: Press Z on the keyboard and/or Shift + Z to zoom in and out. 5. Save your work by selecting File and then Save. Save your part in the C:\DesignL2 folder. Name your part Mug your last name.sldprt. Click Save. 6. Click the 3 Point Arc tool on the Sketch toolbar. 7. Click the endpoint of the top horizontal line, and then move the pointer downward. 8. When the length is approximately 20mm (L=20), click again. Move the pointer to the right to adjust the angle of the arc. When the angle of the arc is 180 (A=180 ) and the radius is approximately 10mm (R=10), click again. 9. Dimension the arc radius to Click Line on the Sketch toolbar and sketch a vertical line from the endpoint of the arc to the bottom horizontal line, as shown. 23

30 Topic 1 Product Design 11. Save your work and then click Exit Sketch on the Sketch toolbar. The Revolve PropertyManager appears. 12. Click on the center line. 13. Under Revolve Parameters: Select One-Direction in Revolve Type. Set Angle to 360. Click OK. 14. Save your work. 24

31 Topic 1 Product Design Sketching the Sweep Path 1. First, you need to sketch the sweep path. Select the Front plane in the FeatureManager design tree. 2. Click Sketch on the Sketch toolbar to open a new. 3. Click Front on the Standard Views toolbar. 4. Click Hidden Lines Removed on the View toolbar. 5. Click View, Temporary Axes. Notice that the temporary axis of the revolved base appears. 6. Select Line from the Sketch toolbar, and move the pointer over the temporary axis. 7. The pointer changes to indicating that the pointer is exactly on the temporary axis. 8. Click, hold, and drag to sketch a horizontal line as shown. Dimension the line to Select Tangent Arc from the Sketch toolbar. 10. Sketch an arc starting at the endpoint of the line. Dimension the arc to an angle of 180 and a radius of *Remember to click Zoom to Fit to see your part. 12. Save your work. 13. Click Exit Sketch on the Sketch toolbar. 25

32 Topic 1 Product Design Sketching the Sweep Section 14. After you sketch the sweep path, you need to sketch the sweep section. 15. Select the Right plane in the FeatureManager design tree and then click Sketch on the Sketch toolbar to open a new sketch. 16. Click Normal To on the Standard Views toolbar. 17. Click Ellipse on the Sketch toolbar, or select Tools, Sketch Entities, Ellipse. Move your cursor anywhere in the graphics area. Position the pointer at the center of the ellipse. Click the left mouse button, and then move the pointer horizontally to define the width of the ellipse. Click the left mouse button a second time. Move the pointer vertically to define the height. Click the left mouse button a third time. This completes sketching the ellipse. 18. Click Select on the Standard toolbar. Hold down the Ctrl key and click the endpoints of the ellipse. 19. In the PropertyManager, under Add Relations, click Horizontal, and then click OK. This relation ensures that the ellipse is not slanted. 20. Using Smart Dimension, dimension the ellipse as shown. Press the Esc key to exit Smart Dimension. 21. Click Isometric on the Standard Views toolbar. 26

33 Topic 1 Product Design 22. Hold down the Ctrl key and click the center point of the ellipse and the endpoint of the horizontal line of the (handle) sweep path. *Remember, press Shift + Z to zoom in. 23. In the PropertyManager, under Add Relations, click Coincident, and then click OK. 24. This coincident relation ensures that the center point of the sweep section lies on the plane of the sweep path. 25. Click View, Temporary Axes to hide the temporary axis. 26. Click Exit Sketch on the Sketch toolbar. Save your part. Now you will combine the sweep path and sweep section sketches to create the sweep. 27. Click Swept Boss/Base on the Features toolbar. 28. Select Sketch3 (the ellipse) in the graphics area for Profile by clicking on the ellipse. Sketch3 appears in the PropertyManager. 29. Select Sketch2 (the path) in the graphics area for Path by clicking on the handle. Sketch 2 appears in the PropertyManger. 30. A profile of the sweep appears in the graphics area. Note how the colors in Profile and Path match those in the graphics area. 27

34 Topic 1 Product Design 31. Under Options, select Follow Path in Orientation/twist type. Click OK to create the sweep. Hollowing out the mug 1. Select the top face of the revolved base feature, and then click Extruded Cut on the Features toolbar. 2. Click Normal To on the Standard Views toolbar. 3. Click Circle on the Sketch toolbar, and select the sketch origin. Sketch and dimension a circle as shown. 4. Click Exit Sketch on the Sketch toolbar. 5. In the PropertyManager, under Direction 1: Select Blind. Depth 180 mm. Click OK. 6. To see the angled cut, click Hidden Lines Visible on the View toolbar, and rotate the part using the arrow keys on the keyboard. 7. Select Shaded with Edges on the View toolbar. Use the arrow keys to see all views of your part. 8. Save the part. Print your part by selecting File and then Print. 9. When you are finished, exit SolidWorks and click on the Forward arrow to resume the activity. 28

35 Topic 2 Universal Design TOPIC 2 UNIVERSAL DESIGN Objective When you have completed this topic, you will have experience applying the Principles of Design, developed by the center of the Universal Design, to your designs. You will have the knowledge to demonstrate and explain Universal Design. You will evaluate the designs that you created in SolidWorks and integrate features that meet the needs of as many users as possible toward the goal of Universal Design. Overview Universal design is an approach to the design of products, services, and environments to be usable by as many people as possible regardless of age, ability, or situation. The Principles of Universal Design are intended to focus attention on those characteristics of design that most impact all users younger and older, larger and smaller, left- and right-handed, with and without disabilities. In this topic, you will be introduced to Universal Design what it is, where is began, and how to implement it. 29

36 Topic 2 Universal Design Activity 1 Applying the Principles of Design Objective When you have completed this activity, you will have the knowledge and skills to explain Universal Design and demonstrate how to apply the Principles of Design to existing designs. You will be able to: explore the meaning of Universal Design. identify the Principles of Universal Design. evaluate existing designs for the Principles of Universal Design. apply the Principles of Design to your design. Activity Directions: Modifying the Design SolidWorks should be on your screen. If it isn't, click on the Application Launch button and choose SolidWorks from the menu. You will now have the opportunity to modify your mug design and apply as many principles of design elements as you can. Click File and then Open. Double-click on your mug (C:\DesignL2\Mug your last name.sldprt). Make changes to your existing design, or design a new mug. Save your new mug in the C:\DesignL2 folder using a different name. When you are finished, save your design and print out a copy. Select File and then Exit and click on the Forward arrow to resume the activity. 30

37 Topic 2 Universal Design Activity 2 Universal Design for Play Objective When you have completed this activity, you will have the knowledge and skills to apply Universal Design concepts to toy design. You will also use PhotoWorks to add realistic surface materials, lighting, and visual effects to display your model in a more realistic view. You will be able to: apply the Principles of Design to toy design. demonstrate the features of SolidWorks. add visual effects to display your model using PhotoWorks. view your design realistically. Activity Directions: Creating your Toy SolidWorks should be on your screen. If it isn't, click on the Application Launch button and choose SolidWorks from the menu. You will now create your toy using the tools you have learned in SolidWorks. Refer back to the previous activities in this guide for instructions on features that you would like to include in your design. Click New to start a new part. Be sure to save your part in the C:\DesignL2\ directory. Name your part, Toy your last name.sldprt. When you are finished, save your design and print out a copy. Complete the Activity Directions: Visualization in this. *If you need help or an idea, the following are general directions for creating a toy top using the Revolve Feature. You can use this design as a guide try to add something unique to make it your own. 1. Click on the Features tab to display the Features toolbar and then click on Revolved Boss/Base. 2. Select the Front plane. 31

38 Topic 2 Universal Design 3. Click Line on the Sketch toolbar. Sketch a vertical line from the origin, and then sketch the other lines as shown. *Remember - press the Esc key to exit the current tool or command. NOTE: Press Z on the keyboard and/or Shift + Z to zoom in and out. 4. Save your work by selecting File and then Save. Save your part in the C:\DesignL2 folder. Name your part Toy your last name.sldprt. Click Save. 5. Click the 3 Point Arc tool on the Sketch toolbar and sketch an arc similar to the one shown. Remember, use these directions as a guide. 32

39 Topic 2 Universal Design 6. Click on the Tangent Arc tool and sketch an arc similar to the one shown. 7. Click Exit Sketch on the Sketch toolbar. The Revolve PropertyManager appears. 8. Click on the center line. Under Revolve Parameters: Select One-Direction in Revolve Type. Set Angle to 360. Click OK. Use the arrow keys to see your toy in different views. 9. Save your part. Select File and then Print to print a copy of your toy. 33

40 Topic 2 Universal Design Activity Directions: Visualization You will now use PhotoWorks to create a more realistic model of your toy. 1. Your toy should be on the screen. Activate PhotoWork by clicking Tools, Add-Ins from the Main menu. Check PhotoWorks. Click OK from the Add- Ins box. 2. Select the Office Products tab, and click Options on the PhotoWorks toolbar. 3. On the Document Properties tab, under Anti-aliasing quality, select Medium. 4. Click Close. 5. Switch to the Render Manager Tab and select your toy. 6. Click Appearances. 7. In the Appearances PropertyManager, click Advanced, and select the Color/Image tab. 8. Under Appearances, click Browse. View the materials listed. Select the material folder for the material you want for your toy. More choices appear specific to your material. Choose a folder, and then select a material. Click OK. 9. Click Render from the PhotoWorks tools. Your toy is rendered with the selected appearance. 10. On the RenderManager Tab, expand Appearances and doubleclick on the material. 11. Click the Illumination tab and select Mirror for Material type. 12. Click OK. This created a highly reflective material. 13. Click Render from the PhotoWorks tools. 34

41 Topic 2 Universal Design You will now apply a scene to display your toy. 14. Click Scene from the PhotoWorks tools. The Scene Editor opens. Select the Room tab. 15. Under Size/Alignment: Select Preserve length/width ratio. Enter 530 for the length and press Enter. The width value changes too. Enter 360 for the height. Select Model X-Z Plane. Under Visibility and appearances, click the in the Floor row. 16. In the Appearances/PhotoWorks Task Pane, under Appearances, browse to Stone, Architectural, Marble, and select pink marble polished. 17. Click OK 18. In the North row, click. 19. In the PropertyManager, select the Color/Image tab. 20. Under Appearance, browse to the Materials\Organic\wood\maple folder and select a finish from the list. 21. Click OK. 22. In the Scene Editor window, select Link all walls. 23. Select Visible and Reflective for North, South, East, West, and Floor. 24. Click Apply and then Close. 25. Click Render. 26. Save your work then print out a copy. Select File and then Exit and click on the Forward arrow to resume the activity. 35

42 Topic 3 Final Project Basic Parts of the Mountain Board TOPIC 3 FINAL PROJECT - BASIC PARTS OF THE MOUNTAIN BOARD Objective When you have completed this topic, you will have the knowledge and experience to design basic parts of a mountain board. Using SolidWorks you will create the binding anchor, binding, wheel hub, and the deck. You will determine the design intent for each part being created. You will also complete an initial analysis of your design using SimulationXpress. Overview Designers create, plan, and develop the products and environments we use and experience in our everyday lives. Design is everywhere. Whatever we wear, sit on, live in, drive, and work with - including our tools, vehicles, toys, furniture, home or commercial environments - a designer has had a hand in its creation and development. There is an ongoing demand for new design. In the next three topics you will be designing and analyzing a mountain board, which is comprised of the deck, truck, axle assembly, wheels, and the bindings. Individual parts will be created and then assembled into several subassemblies until the finished mountain board is complete. In this topic, you will begin the design process by completing the basic parts, the revolved features, and the thin features of the mountain board. 36

43 Topic 3 Final Project Basic Parts of the Mountain Board Activity 1 Creating the Basic Parts Objective When you have completed this activity, you will have the knowledge and skills to create the basic parts for your final project, the mountain board. You will be able to: evaluate the design intent for the parts you are to create. create the binding anchor using SolidWorks. create the binding base plate using SolidWorks. create the binding assembly. Activity Directions: Creating the Binding Anchor Click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. 1. Click File and then Open on the Standard toolbar. 2. The Open dialog box appears. Navigate to the C:\Mountain Board Training Templates folder in the Look in: box. In the Files of type: box, click on the down arrow and select All Files. Double-click on the Part_MM.prtdot file. 3. Save the Template. Click File and then Save As. Navigate to the C:\Mountain Board folder. Enter Part_MM your last name for the filename. 4. In the FeatureManager design tree, select the Top plane. 5. Click Sketch on the Sketch toolbar. The sketch opens on the Top plane. 6. The first feature will be a short cylinder, 75 mm in diameter and 3.5 mm thick. Click the Circle tool. Move the cursor over the origin until an orange circle appears. Click, hold and drag to create a circle about 32 mm. 7. Dimension the circle at Next extrude the part to create the first feature. Click Extrude Boss/Base on the Features toolbar. 37

44 Topic 3 Final Project Basic Parts of the Mountain Board 9. In the PropertyManager, change the settings to: End Condition = Blind (Depth) = 3.5 mm 10. Click OK. 11. Change the display mode. Click Hidden Lines Visible on the View toolbar. 12. Click File and then Save As. Save the part in the C:\Mountain Board folder as Binding Anchor your last name. Select Part from the Save as type: drop-down list. Click Save. The.sldprt extension is automatically added to the filename. 13. Change the view of the model to the Bottom view. Click on the Standard Views toolbar. 14. The second feature will be another cylinder, slightly smaller than the first. Select the bottom face of the cylinder. It will turn green to show that it is selected. 15. Start a new sketch by clicking Sketch on the Sketch toolbar. 16. Select Circle on the Sketch toolbar. Draw a circle, slightly smaller than the size of the cylinder. It does not have to be centered on the cylinder. The circle is blue, indicating that the sketch is Under Defined. 17. Click Add Relation on the Sketch toolbar. Add Relation will appear in the PropertyManager. 38

45 Topic 3 Final Project Basic Parts of the Mountain Board 18. Select the circle and the edge of the cylinder. 19. Click Concentric in the Add Relations box. Then click OK. The circle will move to a position where it is centered on the cylinder. 20. Dimension the circle as Change the viewpoint to Dimetric by clicking on the Standard Views toolbar. 22. Extrude the second feature. Click Extrude Boss/Base on the Features toolbar. Select Blind for the type of extrusion. Type 3 mm for the depth. Click OK. Material needs to be removed from the top of this part. 23. Orient the part to the Top view by clicking on the Standard Views toolbar. 24. Select the top face of the model, and click Sketch to start a new sketch. 25. Click Circle on the Sketch toolbar. 26. Draw a circle from the center of the top face. Make its radius about 30 mm. 39

46 Topic 3 Final Project Basic Parts of the Mountain Board 27. Dimension the circle to be 63 mm in diameter. 28. Reorient the model to the Isometric view. 29. Click Extruded Cut to use the circle to cut away some material. 30. Type 3 mm for the depth. Click OK. The Cut Extrude command removed a cylinder shaped volume from the part. To make the position of the binding adjustable, the binding anchor will have four slots. These will allow the position of the bindings to be moved along the centerline of the deck. The slots are symmetrical, so you will use a function called mirroring to make sure the slots always remain symmetrical if you need to change their size later. 30. Select the face of the part created by the cut. 31. Open a sketch by clicking on the Sketch toolbar. Change to the Top view by clicking on the Standard Views toolbar. 40

47 Topic 3 Final Project Basic Parts of the Mountain Board 32. You will now create a centerline. Click Centerline on the Sketch toolbar. Sketch a vertical centerline. The length is not important. Make sure the cursor displays a, indicating a Vertical relationship will be added. 33. Click Dynamic Mirror Entities on the Sketch toolbar. A pair of parallel marks will appear at each end of the centerline to show that you are in the mirror mode. 34. Sketch a vertical line to one side of the centerline. As soon as you finish drawing the line, a mirror image will be drawn automatically on the other side of the centerline. 41

48 Topic 3 Final Project Basic Parts of the Mountain Board 35. The sketch of the slot is composed of two straight lines and two arcs. The arcs must be tangent to both lines. Click Tangent Arc on the Sketch toolbar. 36. Place the cursor over the end of the right vertical line, click and drag an arc up and around to the right until you get cursor feedback showing you have gone 180 degrees. Click the mouse again. 37. When you release the mouse button, a second symmetric arc will be drawn automatically. 38. Draw another vertical line, from the end of the arc, vertically downward until you get a blue inference line from the bottom end of the first line. 42

49 Topic 3 Final Project Basic Parts of the Mountain Board 39. Finish the sketch with another Tangent Arc. Turn off the sketch Dynamic Mirror Entities tool by clicking on the Sketch toolbar. To complete the pattern of slots, you will now mirror the two slots across a horizontal centerline. 40. Sketch a horizontal centerline from the origin to the right. Turn off the Centerline tool by clicking on the tool again. 43

50 Topic 3 Final Project Basic Parts of the Mountain Board 41. Click Mirror Entities on the Sketch toolbar. 42. Hold down the Ctrl key on the keyboard and select the four lines and the four arcs and the horizontal centerline for the entity to Mirror about. Make sure you do not have the vertical centerline selected. 43. Click OK. 44. To fully define the sketch, you must add dimensions to position the slots and define their size. Even though you only drew one of the slots, the dimensions can be on any of the slots. 45. Add dimensions to the upper right slot as shown. To add the 16 mm dimension, select the two arcs, not the vertical line. 44

51 Topic 3 Final Project Basic Parts of the Mountain Board 46. Add dimensions as shown to the upper left slot to position it. Both of these dimensions go from the lower arc to one of the centerlines. 47. The four slots must cut completely through the binding anchor. When you create the cut, it must be done so that if you need to change the thickness of the material later in the design process, the slots do not have to be redone. 48. Click Insert, Cut, Extrude from the menu. 49. Change the view Isometric. 50. From the list in the PropertyManager select Through All. Click OK. 45

52 Topic 3 Final Project Basic Parts of the Mountain Board All the features shown in the FeatureManager design tree can be renamed. Renaming features can make them easier to locate as the parts become more complex. 51. In the FeatureManager design tree, click once on CutExtrude2. Press F2 on the keyboard. The feature name now has a box around it and a flashing cursor. 52. Type Rounded Slots for the new name. Press Enter on the keyboard. All the existing edges in this model are sharp. To meet your design intent, all the exposed edges need to be rounded. 53. Click Fillet on the Features toolbar and select the edge shown. 54. Type 1.5 mm for the fillet radius. The following should be set by default. If not, change them as follows: Fillet Type - Constant radius Tangent propagation - Selected Full preview - Selected 55. Click OK. 46

53 Topic 3 Final Project Basic Parts of the Mountain Board 56. You need to add a fillet to the inside edge. Click Fillet on the Features toolbar. Select the inside edge. Type 1 mm for the fillet radius. Click OK. The inside edge now has a fillet. 57. In the FeatureManager design tree, right-click the feature Fillet2 and select Edit Feature from the Context toolbar. The PropertyManager will now show the same information as when you first applied the fillet. 58. Select the edge shown. 59. Once selected, the preview will show that the edge will be rounded as part of the Fillet2 feature. Click OK. 60. Save and Print the part. Add Material 61. Click Edit, Appearance, Material from the Main menu. 62. The Materials Editor will open. Click the Plus sign next to Aluminum Alloys to expand the list. Select 2014 Alloy. Click Apply and then Close to apply the material. 63. Select Shaded with Edges. Save the part. Select File and then Close. Complete the Activity Directions: Creating the Binding Base Plate. 47

54 Topic 3 Final Project Basic Parts of the Mountain Board Activity Directions: Creating the Binding Base Plate Before you begin the steps to create the binding base plate you need to know the design intent for this part. Go to your Student Guide/Portfolio, Data Sheet- Design Intent: Binding Base Plate, in Topic 3, Activity 1. SolidWorks should be on your screen. If it is not, click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. The binding anchor you just created was created by adding material on top of material to get the basic geometry. For the binding base plate, the approach will be to create an oversized block of material and use a cookie cutter to cut away the material around the final part. 1. Click File and then Open on the Standard toolbar. The Open dialog box appears. Navigate to the C:\Mountain Board folder in the Look in: box. In the Files of type: box, click on the down arrow and select All Files. Doubleclick on the Part_MM your last name.prtdot file. 2. In the FeatureManager design tree, select the Top plane. Save the new part before going any further. Click File and then Save As. Save the part in the C:\Mountain Board folder as Binding Base Plate your last name. Select Part from the Save as type: drop-down list. Click Save. The.sldprt extension is automatically added to the filename. 3. Click Sketch on the Sketch toolbar. Click on the Top plane. 4. Click View, Sketch Relations, if it is not already selected. From the origin, create a vertical and horizontal line as shown. The vertical line should be about 200 mm and the horizontal line 75 mm. 48

55 Topic 3 Final Project Basic Parts of the Mountain Board 5. Create another horizontal line from the end of the vertical line. Make this line about 35 mm. 6. Create a line from the end of the first horizontal line. Make sure that this line is NOT vertical. 7. Click Tangent Arc on the Sketch toolbar. Draw an arc from the endpoint of the angled line to the end of the top horizontal line. 49

56 Topic 3 Final Project Basic Parts of the Mountain Board Check the relationships of the arc. There was a tangent relationship added between the arc and the line where the arc started. 8. Notice that there is no tangent relationship between the arc and the top horizontal line. The automatic tangent relationship is only added to the starting end of the arc. To test this, drag the left end of the upper horizontal line to the left. If a tangent relationship is required at the finish end, it must be added manually. 50

57 Topic 3 Final Project Basic Parts of the Mountain Board 9. Click on the Sketch toolbar. Select the arc and the upper horizontal line. 10. Click Tangent. Click OK. The arc and upper horizontal line are now tangent. 11. Fully define the sketch by adding the dimensions shown. All the sketch geometry should now be black. 51

58 Topic 3 Final Project Basic Parts of the Mountain Board 12. Extrude the feature by clicking Extruded Boss/Base on the Features toolbar. 13. Create a Blind extrusion to a depth of 25 mm. Click OK. To get the shape you are interested in, you need to use an Extruded Cut to remove the unwanted material from your base feature. 14. Select the face shown and open a new sketch. 15. Click on the Standard Views toolbar to change the view so that you are looking normal to the sketch plane Select the Line tool. 52

59 Topic 3 Final Project Basic Parts of the Mountain Board 17. Position the cursor over the lower edge of the part. 18. When you are over the edge, the cursor feedback will be. This is the feedback for coincident, meaning you are on the edge. Sketch a line to the right. 19. Add a Tangent Arc. Draw a tangent arc from the right endpoint of the line to the midpoint of the right vertical edge. The midpoint is displayed with a square with two diagonal lines. Once the arc is drawn there will be a midpoint relationship established with the right vertical line. 20. Add a Tangent Arc from the left end of the line to the midpoint of the left vertical edge. 21. Dimension the sketch as shown. Save your work. Offset Sketch Entities The Offset Entities tool is used to make a copy of sketch entities, or edges, offset from the original by some specified distance. 22. Click any of the three sketch entities (line, left tangent arc, or right tangent arc). 23. Click Offset Entities on the Sketch toolbar. Select Chain will be selected by default; this will select all sketch entities that are continuously connected to the one you selected. 24. Enter 3 mm for the offset. Select Reverse, if necessary, to make the preview appear above the other sketch entities. Click OK. Each arc and the line are duplicated at an offset distance of 3 mm. 53

60 Topic 3 Final Project Basic Parts of the Mountain Board 25. The sketch must be closed to extrude the cut. You will add two lines to connect the ends of the arcs. These lines need to be perpendicular to the arcs. This means that the lines must point through the centers of their respective arcs. 26. Draw a line to connect the ends of the two arcs on the left. The line should become fully defined (black). If the line does not become fully defined, you need to add a relationship to make the line perpendicular to the arc. Because you cannot add a perpendicular relationship between the arc itself and the line, you will add a coincident relationship between the line and the center point of the arc. By basic geometry this will make the line perpendicular to the arc. Click Add Relation on the Sketch toolbar. Whenever the PropertyManager or a dialog box has an entry box colored in the salmon color, anything selected in the graphics area will be entered in the box. Select the arc center point and the line. Click to add a Coincident relationship. The line will now be black as it is fully defined. 27. Repeat the procedure to close the sketch between the arcs on the right. Cut to the Outside The Extruded Cut command can either cut what is enclosed by the sketch or everything outside the sketch. 28. Click Extruded Cut on the Features toolbar. 54

61 Topic 3 Final Project Basic Parts of the Mountain Board 29. Select Through All for the end condition. By default, the cut will remove the material inside the sketch. 30. Select Flip side to cut. Now the cut will keep the material that is inside the sketch and remove the material that is outside the sketch. 31. Click OK. Change to view to Isometric. Save and Print the part. 55

62 Topic 3 Final Project Basic Parts of the Mountain Board Creating the Side Tabs The two side tabs provide the mounting locations for the binding straps that go over the rider s foot. They must be offset from the base plate to allow for the thickness of the strap. They must also be a uniform thickness as the final product will be cut from flat material and bent into the final shape. 1. Select the face shown and open a sketch. 2. Change the view orientation to Normal To by clicking on the Standard Views toolbar. 3. Select the Rectangle tool from the Sketch toolbar. 4. Start the rectangle with a coincident relationship to the bottom edge of the binding base plate. Drag the rectangle until you get a coincident relationship with the top edge. 56

63 Topic 3 Final Project Basic Parts of the Mountain Board The two coincident relationships control the height and vertical position of the rectangle. To make it fully defined, only a width dimension and a single positioning dimension are need. 5. Add the two dimensions shown. 6. Select Extruded Boss/Base and extrude the sketch to a Blind depth of 4mm. Create the tab 7. Create a new sketch on the new face created by the offset. 57

64 Topic 3 Final Project Basic Parts of the Mountain Board 8. Sketch a rectangle. Start the rectangle at the lower left corner of the offset. The cursor feedback will show the yellow coincident callout to indicate you are on the endpoint of the edge. 9. Add a relationship. Click Add Relation on the Sketch toolbar. Select the right vertical line of the sketch and the right vertical edge of the offset. 10. Click Collinear and click OK. The rectangle will now stay the same width as the offset. 11. Dimension the height of the rectangle to 32 mm. 12. Extrude the sketch, Blind to a depth of 3 mm. Binding Attachments The binding straps will attach to the base plate through two curved slots. The slots need to be curved to allow the binding straps to rotate as the foot is pushed into the binding. 58

65 Topic 3 Final Project Basic Parts of the Mountain Board 13. Select the outside face of the tab and open a sketch. With the outside face of the tab still selected, click. 14. Click Zoom to Selection on the View toolbar. This will make the selected entity fill the graphics area. The two slots are symmetrical. To create them, you will sketch one and mirror it get the second. 15. Create a centerline. Start the centerline at the midpoint of the top edge and make sure it is vertical. 16. To mirror as you sketch, click Tools, Sketch Tool, Dynamic Mirror, and then click on the centerline. 59

66 Topic 3 Final Project Basic Parts of the Mountain Board Drawing the Centerpoint Arc is a two step process. You first drag from the center of the arc to the start point of the arc. Release the mouse button, then press and drag the length of the arc. 17. Select the Centerpoint Arc from the Sketch toolbar. 18. Start the arc from the centerline and drag the radius/start point as shown. Release the mouse button. This will be the point where the arc begins. 19. Click the mouse button and drag until the arc is as shown, then release the mouse button. 60

67 Topic 3 Final Project Basic Parts of the Mountain Board 20. Draw another Centerpoint Arc using the same centerpoint. This makes the arcs concentric. 21. Draw Tangent Arcs to close up the sketch. Add Tangent relationships to make sure all the arcs are tangent to the arcs they are connected to. 22. Turn off Dynamic Mirror. 23. Add the Dimensions shown. 24. To create the 6 mm dimension between the arcs, pick the arcs on each end of the slot. As you drag the cursor, the dimension preview will show: 61

68 Topic 3 Final Project Basic Parts of the Mountain Board 25. To lock in the type of dimension you want, click the right mouse button to set it. That type of dimension will stay active no matter where you then move the cursor. 26. Next Extrude a cut. Select Up To Next. Click OK. 27. You will now create another tab on the other side of the Binding Base Plate. Create the offset feature on the face shown. 28. Position the offset 70 mm from the vertex shown. This part will be manufactured from a flat piece of metal. It will first be cut to shape, and then the tabs will be bent, followed by the front a back curves. Because the part will be manufactured from a single piece of metal, the model must have a uniform thickness. You will add the bends manually using fillets. 62

69 Topic 3 Final Project Basic Parts of the Mountain Board 29. You must add a fillet to the inside edge of the tab at the correct radius to keep the material uniform. To calculate the fillet radius: The radius of the inside fillet = radius outside fillet - material 30. Apply a 1 mm fillet to the inside edge. The finished bend now has a uniform thickness. Add bends 31. Select the top flat face of the Binding Base Plate. This will be the face that will be fixed. All the bends will move relative to this face. 32. Click Insert, Sheet Metal, Bends from the menu. 63

70 Topic 3 Final Project Basic Parts of the Mountain Board 33. Set the bend radius. Change the Bend Radius to 3 mm, which is the material thickness. Leave the remaining option as shown. Click OK. 34. Three new features are added to the FeatureManager design tree. Sheet-Metal1 contains the sheet metal definitions such as the bend radius we entered in the last step. Flatten-Bends1 creates a flat pattern or the part. Process-Bends1 contains the information to bend the flat pattern into the final part. Rollback The model can be rolled back to a previous state by moving the rollback bar at the end of the FeatureManager design tree. To rollback the FeatureManager design tree, move the cursor over the rollback bar (the line that is normally at the bottom of the FeatureManager design tree). The cursor will change to a hand, then drag the rollback bar to the desired position. 35. In the FeatureManager design tree, move the cursor over the rollback bar and drag the rollback bar to a position between Flatten-Bends1 and Process-Bends The part will flatten. 64

71 Topic 3 Final Project Basic Parts of the Mountain Board Add Fillets The sharp corners need to be rounded to make the part look better and for safety reasons. 37. Add 15 mm fillets to the corners shown. 38. Add 6 mm fillets to the corners of the tabs as shown. 39. Add 2 mm fillets to the corners shown. 40. Bend the part by moving the rollback bar to the end of the FeatureManager design tree. The part will bend to its final shape. 65

72 Topic 3 Final Project Basic Parts of the Mountain Board Center Hole To hold the Binding Base Plate to the deck, you will have to create a hole. This hole will also fit the Binding Anchor you previously created to the deck. 41. Rollback the part to before Process-Bends1. *Note: Rollback can also be done through the right mouse button menus. Right-click on Process-Bends1 and select Rollback. 42. Create a sketch on the top face of the part. Sketch a circle and dimension it as shown. *Note: You want to cut the hole just slightly larger than the size of the boss on the Binding Anchor part. You want the fit tight, but not so tight that it is hard to assemble. 66

73 Topic 3 Final Project Basic Parts of the Mountain Board 43. Extrude a cut. You ll notice a new end condition appears called Link To Thickness. This is because the part has been turned into sheet metal by the Insert Bends command. This makes the cut depth the same as the material, even if the material thickness changes. 44. Bend the part. Right-click the feature Process-Bends1 and select Roll To End. Because you are concerned with the overall weight of the product, material should be attached to each part as you build them, this will make it easier to check the weight of the entire product as you assemble it. 45. Attach the material Aluminum 2014 to the part. Either click Edit Material on the Standard toolbar or select Edit, Appearance, Material from the menu. 46. In the Materials Editor, expand the Aluminum Alloys category by clicking the plus sign. Select 2014 Alloy and click OK. 47. Save and Print the part. Complete the Activity Directions: Creating the Binding Assembly. 67

74 Topic 3 Final Project Basic Parts of the Mountain Board Activity Directions: Creating the Binding Assembly You will now create an assembly of the two parts of the binding that you made. 1. To create a new assembly, click Make Assembly from Part/Assembly on the Standard toolbar. 2. Select the template Assembly and click OK. Because you selected to make an assembly, only assembly templates are shown. Insert Component is automatically activated by SolidWorks when you open a new assembly. This is done just to save time. You only have one file open, so it is automatically selected and a preview of the part is attached to our cursor. The part will move with the cursor. If the part was not open, you could select the Browse button to locate it. *Note: If you do not see the preview graphic when your cursor is in the graphics area, select Graphics preview in the PropertyManager. 3. Place the part by moving the cursor to the assembly Origin. When the cursor is over the Origin, it will change to the part.. Click on the Origin to place You may remember from Level 1, that the initial component added to the assembly is fixed. Fixed components cannot be moved and are locked into place wherever they fall when you insert them into the assembly. By using the cursor during placement, the component s origin is at the assembly origin position. This also means that the reference planes of the component match the planes of the assembly, and the component is fully defined. There are six degrees of freedom for any component that is added to the assembly before it is mated or fixed: translation along the X, Y, and Z axes and rotation around those same axes. How a component is able to move in the assembly is determined by its degrees of freedom. The Fix and Insert Mate options are used to remove degrees of freedom. 68

75 Topic 3 Final Project Basic Parts of the Mountain Board 4. Open your part Binding Anchor part. You saved this part in the C:\Mountain Board folder as Binding Anchor your last name. 5. Tile the windows by clicking Window, Tile Vertically from the menu. Close the part window of the plate part - keep the assembly1 window and the binding anchor window open (see below). 6. Drag the top level icon from the FeatureManager design tree of the Binding Anchor into the graphics area of the assembly. 7. The Binding Anchor is now added to the assembly. 8. The Binding Base Plate is fixed, but the Binding Anchor still has all six degrees of freedom. Maximize the assembly window by clicking Maximize on the Assembly window title bar. Select Zoom to Fit. One or more selected components can be moved or rotated to reposition them for mating using the mouse or the Move Component and Rotate Component commands. Also, moving under defined components simulates movement of a mechanism through dynamic assembly motion. Mate the Binding Anchor The Binding Anchor holds the Binding Base Plate to the deck of the mountain board. It will require two mates to position it correctly. A Concentric mate will hold the Binding Anchor in the center of the hole in the Binding Base Plate. The second mate will position the top face of the Binding Base Plate coincident to the underside of the lip of the Binding Anchor. 69

76 Topic 3 Final Project Basic Parts of the Mountain Board 9. Move the Binding Anchor to a position near the Binding Base Plate by selecting the Binding Anchor, then holding down the left mouse button and dragging the Binding Anchor to the desired position. 10. Most mates are between faces of parts. To make the selection of faces easier, turn on the Face Filter. Click Toggle Selection Filter Toolbar on the Standard toolbar to show the Selection Filter toolbar. Select the Filter Face tool. 11. Click Mate on the Assembly toolbar to add a mate. 12. Select the two faces shown. When you pick the second face, the parts will move into alignment for a concentric mate and the Mates toolbar will appear. *Note: The Binding Anchor has been rotated in the graphic to make it easier to see the two faces. You will have to rotate the model to be able to select both faces. 13. Click to apply the Concentric mate. 14. Click Insert, Mate from the menu. 15. Select the top flat face of the Binding Base Plate. 70

77 Topic 3 Final Project Basic Parts of the Mountain Board 16. Rotate the model and pick the face shown on the Binding Anchor. 17. The Mate Pop-up will show that Coincident is selected. 18. Click to apply the mate. 19. Toggle off the Face Filter. 20. Click File, Save. Save the file in the C:\Mountain Board as Binding your last name. SolidWorks will add the extension.sldasm to indicate this is an assembly file. Save and Print the binding. 21. Close all the windows and Exit SolidWorks. Click on the Forward arrow to resume the activity. 71

78 Topic 3 Final Project Basic Parts of the Mountain Board Activity 2 Creating the Revolved Features Objective When you have completed this activity, you will have the knowledge and skills to create the parts required to complete the wheel assembly for the mountain board project. You will be able to: create the wheel hubs. import the tire and tube from another source. create parts using the SolidWorks toolbox. assemble the parts of the wheel. Activity Directions: Creating the Hub 1. Click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. 2. Click File and then Open on the Standard toolbar. The Open dialog box appears. Navigate to the C:\Mountain Board folder in the Look in: box. In the Files of type: box, click on the down arrow and select All Files. Doubleclick on the Part_MM your last name.prtdot file. 3. Click File and then Save As. Save the part in the C:\Mountain Board folder as Wheel Hub your last name. Select Part from the Save as type: drop-down list. Click Save. 4. The hub center will be created as a simple revolved feature. Create a sketch on the Right plane. 5. Sketch a rectangle, approximately 25 mm by 25 mm, with the Origin at the lower right. 6. Sketch a centerline from the Origin, horizontally to the right. The length is not important. You will revolve the rectangle around this centerline to form a cylinder. 72

79 Topic 3 Final Project Basic Parts of the Mountain Board 7. Change the dimension of the top line to 21 mm. This is the thickness of the hub center. 8. Add a dimension from the top horizontal line to the Centerline. When the cursor is on the side of the centerline closest to the selected line, you get a radius dimension. When the cursor is on the side of the centerline away from the selected line, you get a diameter. Dimension the diameter to 40 mm. 9. Revolve the hub. Click Revolved Boss/Base on the Features toolbar. The preview shows that the rectangular sketch will be revolved around the centerline. 10. Select One-Direction and 360 deg for the type and angle. Click OK. 11. Rename this Revolve feature on the FeatureManager design tree to Hub. 73

80 Topic 3 Final Project Basic Parts of the Mountain Board You will now cut the center holes. Cuts can also be created as revolved features. 12. Create a sketch on the Right plane. 13. Reorient the view to the Right view. Sketch the profile shown, including the centerline from the Origin to the right. 14. Dimension the sketch as shown. The larger diameter cut will be to house the wheel bearing and the smaller bore will be a clearance hole for the axle shaft. 74

81 Topic 3 Final Project Basic Parts of the Mountain Board 15. Revolve a cut. Select Revolved Cut on the Features toolbar. If a dialog box appears stating The Sketch is currently open. A non-thin revolution feature requires a closed sketch. Would you like the sketch to be automatically closed? Click Yes. Another box may appear stating The profile could not be closed without creating self-intersecting entities. Click OK. 16. Choose One-Direction and 360 deg. Click OK. A dialog box Bodies to Keep may appear. Select the radio button called Selected bodies. Click Body 1 and OK. 17. Rename this Revolve feature to Bearing Cut. 18. Save the part. Create a spoke To create the three spokes, only one will be modeled. The remaining spokes will be created as a circular pattern. 1. Create a sketch on the Front plane and change the view orientation to the Front View. Make sure Hidden Lines Visible is selected. 2. Sketch a vertical centerline from the Origin. 75

82 Topic 3 Final Project Basic Parts of the Mountain Board 3. Click Tools, Sketch Tools, Dynamic Mirror. Click on the center line. Sketch a line from the Hub outward. 4. A symmetric line will be drawn automatically. Turn off Dynamic Mirror. 5. Add a Coincident relationship. Click Add Relation on the Sketch toolbar to add a relationship. Select one of the lines and the Origin. Click Coincident relationship. Click OK. to add a 6. Add an angular dimension. Click Smart Dimension, then select the two lines. Because the two lines are not parallel, the dimension will be an angular dimension. Place the dimension then type 40 degrees in the spin box. 76

83 Topic 3 Final Project Basic Parts of the Mountain Board 7. You need to draw a centerpoint arc to close the top of the sketch. Select Centerpoint Arc on the Sketch toolbar. Start the arc at the origin and drag it to the top end of one of the lines. Release the mouse button, then press the left mouse button again and drag to the top of the other line. 8. Dimension the arc. Set the radius equal to 43 mm. 9. Select the outside edge of the hub. Click Convert Entities on the Sketch toolbar. 10. The entire circular edge has been converted into a circle in our sketch. To trim the circle, select Trim Entities from the Sketch toolbar. The cursor will change to the Trim Cursor. 11. Select Trim to Closest in the Property manager. Click the part of the circle to be trimmed away. Click OK. 77

84 Topic 3 Final Project Basic Parts of the Mountain Board Extrude the Spoke 1. You will now extrude the sketch. Select Extruded Boss/Base from the Features toolbar. Extrude to a Blind depth of 15 mm. Click OK. 2. Rename this feature Spoke. 3. Save your part. Construction Geometry Construction geometry is used to locate other sketch entities or features. Any piece of sketch geometry can be converted into construction geometry or viceversa. Construction geometry is considered to be reference geometry and does not have to be fully defined. To convert sketch geometry into construction geometry: Select the geometry, then click on the Sketch toolbar. Select the geometry, then in the PropertyManager select For construction. Create the Bolt Hole 1. Create a sketch on the face shown. 2. Reorient to the Front view. 3. Sketch a circle with its center at the Origin. 78

85 Topic 3 Final Project Basic Parts of the Mountain Board 4. Dimension the circle to diameter 63.5mm. 5. Select the circle, then in the PropertyManager select For construction. The circle will turn into a construction circle. Click OK. 6. Sketch a line from the Origin, vertically upward until it passes the circle. The intersection of the line and circle will be the location for the bolt hole. 7. Use the PropertyManager to change the line into a construction line. 8. Exit the sketch by clicking Exit Sketch for the Sketch toolbar. 79

86 Topic 3 Final Project Basic Parts of the Mountain Board Add the Bolt Hole The hole in the spoke needs to be multi-functional. Because two hubs will be positioned back to back, the hole must have a hexagonal cutout to capture the nut as well as be sized so that the bolt head can turn to be tightened. You will first create a clearance hole for the bolt shaft, then the hexagonal cut. The Hole Wizard is used to create specialized holes in a solid. It can create simple, tapered, counterbored, and countersunk holes using a step by step procedure. 1. Select the face of the spoke. 2. Click Insert, Features, Hole, Wizard from the menu. This starts the Hole Wizard. 3. Click the Hole button. Using the pull-down lists, select: Standard: Ansi Metric Screw type: Screw Clearances Size: M6 End Condition: Through All 4. Click on the Positions tab. You can now edit the sketch that determines the hole position(s). The message tells you to locate the hole center(s). 5. Turn off the Point tool by clicking it once on the Sketch toolbar. The sketch entity Point is automatically turned on so that you can place several holes. You are only placing one hole so you can turn off the tool. 6. Position the hole. Click to add a relationship. Select the Point, Construction Line, and Construction Circle. There will only be one relationship available, Intersection. Click then OK. 7. Complete the wizard. Click OK. The correct size clearance hole for an M6 metric bolt is created. You ll notice that a new construction circle was created inside the hex. 80

87 Topic 3 Final Project Basic Parts of the Mountain Board The hex cut will be made by creating a hex sketch and extruding a cut. 8. Create a sketch on the face shown. With the face still selected, click Normal To on the Standard Views toolbar to change the view so that you are looking normal to the face. 9. Click Zoom to Selection on the View toolbar. The selected face will now fill the screen. 10. Select the Polygon tool from the Sketch toolbar, or select Tools, Sketch Entities, Polygon from the Main menu. Sketch a Polygon by selecting the center point and dragging to some radius. The size and position are not important as we will set those in the following steps. 11. Add a Concentric relationship between the new construction circle located inside the hex and the circular edge of the hole. 81

88 Topic 3 Final Project Basic Parts of the Mountain Board 12. Dimension the new construction circle to 10.5 mm. Why dimension the construction circle? Part of the design intent is that this hex cut captures the nut, but also that the bolt head must be able to rotate inside the cut. The dimension represents the size of a clearance hole for the bolt head. You could have also dimensioned the hex hole from flat to flat, but it doesn t represent the design intent as clearly as dimensioning the circle diameter. 13. Add a Horizontal relationship to one of the lines of the hexagon. This is necessary to fully define the sketch. Without this relationship, the sketch is free to rotate about its center. Click OK. 14. Create an Extrude Cut to a depth of 6.5 mm. Select Surface/Face/Plane in the from drop down box. Click on the Hex surface. Click OK. 15. Right-click on the centerline and select Hole. Do the same for the construction circle. 16. Rename this feature Hex-Cut. 82

89 Topic 3 Final Project Basic Parts of the Mountain Board You will now add a Chamfer. Select the Chamfer tool from the Features toolbar. 17. Select Angle distance. 18. Select one of the edges of the hex cut. 19. Set the Chamfer dimension. You want a.793 mm chamfer. 20. Click OK. 21. You really need to chamfer all six edges, but only selected one. Edit Feature provides a simple method to change the information used to create a feature. To edit any feature, right-click the feature either in the FeatureManager design tree or the graphics area, and select Edit Feature. 22. Right-click the feature Chamfer1 in the FeatureManager design tree and select Edit Feature. The Chamfer PropertyManager will open. 23. Select the remaining five edges of the Hex-Hole. 24. Click OK. All six edges of the hex hole are now chamfered. 25. Rename this feature Hex-Cut Chamfer. 26. Save the Wheel Hub. 83

90 Topic 3 Final Project Basic Parts of the Mountain Board Revolve the Rim The wheel rim will be constructed as another revolved feature. 1. Reorient to the Right view. 2. Create a sketch on the Right plane. 3. Draw a centerline from the Origin horizontally to the left. This will become the axis of rotation for this sketch. 4. Create the geometry shown. 84

91 Topic 3 Final Project Basic Parts of the Mountain Board 5. Add the dimensions shown. Remember to dimension the four diameters, the centerline must be selected as one end of the dimension. 6. Add the following dimensions in this order: Top vertical 9 Bottom vertical

92 Topic 3 Final Project Basic Parts of the Mountain Board 7. To add the following sketch relationships to fully define the sketch, select Add Relation. Click on the three angled lines shown and select Parallel. Then click on the two angled lines shown and select Equal. Click OK. 8. Revolve the rim. Click Revolved Boss/Base on the Features toolbar. 86

93 Topic 3 Final Project Basic Parts of the Mountain Board 9. Revolve One-Direction, 360 degrees. Click OK. 10. Rename this feature Rim. Pattern the Spokes The Wheel Hub will have three spokes. You have created one and will create the other two as a pattern of the first. By creating the spokes as a pattern, you can quickly change the number of spokes as well as their design. Circular Patterns Circular Patterns create copies, or instances, in a circular pattern controlled by a center of rotation, an angle, and the number of copies. The instances are dependent on the originals. Changes in the originals are passed on to the instanced features. Axes SolidWorks has two types of axes: Temporary Axe: These are created by SolidWorks any time a cylindrical or conical solid is created. Axes: These are created manually by the user. 1. View the temporary axes. Click View, Temporary Axes. This will be the axis that will be used to pattern the spokes. 2. Create a circular pattern. Click Circular Pattern on the Features toolbar. 3. Select the Temporary Axis in the graphics area. 87

94 Topic 3 Final Project Basic Parts of the Mountain Board 4. Click the Features to Pattern box to make it active. 5. Click the Circular Pattern title at the top of the PropertyManager to fly-out the FeatureManager design tree. 6. Select Spoke, M6 Clearance Hole1, Hex-Cut and Hex- Cut Chamfer. These are all the features we want to pattern. 7. For the number of instances either type 3 or use the arrows to change the number to Make sure Equal spacing is selected and the angle is set to 360 degrees. 9. Click the Bodies to Pattern box to make it active. Click on the front surface of the hub. (Go to the Front View.) 10. Click OK. The spoke, along with the two holes and the chamfer have been patterned. Add Fillets Fillets need to be added to the spokes to round all the edges. Rather than add the fillets to all three spokes individually, you will just add the fillets to the first spoke, then include the fillets into the pattern. 1. In the FeatureManager design tree, select the feature named Spoke. By selecting a feature in the FeatureManager design tree, the feature will be highlighted in the graphics area. 88

95 Topic 3 Final Project Basic Parts of the Mountain Board 2. Add a 4 mm fillet to both sides of the spoke where it contacts the hub. 3. Rename this feature Fillet R4. 4. Add a 2 mm fillet to the three edges shown. 5. Rename this feature Fillet R2. 6. Right-click the feature CirPattern1 in the FeatureManager design tree and select Edit Feature. 89

96 Topic 3 Final Project Basic Parts of the Mountain Board You want to add the two fillets into the definition of the circular pattern; however they are grayed out and cannot be select. They cannot be selected because they were created later in time than the circular pattern, so when the circular pattern was created, the fillets did not exist. 7. Exit the circular pattern by clicking Cancel. Features can be reordered in the FeatureManager design tree by simply dragging and dropping the feature in a new location. When dragging a feature, the cursor will change to indicating that the new location will be under the feature highlighted. If you drag the feature too far up the FeatureManager design tree, the cursor will change to, indicating that you cannot drop the feature at this location. The parents and children of any feature determine its relationships. Parents are used to create the new feature; the new feature is then dependent on the parent. For the child feature to exist, the parent feature must exist. 8. In the FeatureManager design tree, right-click Fillet R4 and select Parent/Child from the menu. 9. The fillet has two parents, the Spoke and the Hub. This is logical as the fillet connects the two features. The fillet has no children, in other words, no features depend on the fillet. Select Close. 90

97 Topic 3 Final Project Basic Parts of the Mountain Board 10. Reorder the features. Drag the feature Fillet R4 to a position between the Rim and the CirPattern Drag the feature Fillet R2 to a position after Fillet R In the FeatureManager design tree, right-click CirPattern1 and select Edit Feature. 13. Select Fillet R4 and Fillet R2 and add them to the Features to Pattern. 14. Click OK. The fillets have now been added to the circular pattern and appear on all the spokes. Add Additional Fillets Because the spokes were patterned before the rim was created, fillets between the two cannot be added to the pattern. You can add all the fillets to the three spokes individually, but this is a lot of work. You might try to fillet one spoke and pattern the fillets, however this doesn t work. Fillets need to be patterned with the underlying geometry. To allow the fillets to be added to the pattern, you must roll back the model to before the circular pattern. 91

98 Topic 3 Final Project Basic Parts of the Mountain Board 1. In the FeatureManager design tree, right-click CirPattern1 and select Rollback from the menu. 2. Click Insert, Features, Fillet/Round from the menu. 3. Add additional fillets to round remaining sharp edges. Add a 3 mm fillet. Select the face and edges shown. When you select a face, all edges of that face will be filleted. 4. Rename the Fillet to Fillet R3. 5. Finish the front by adding a 0.5 mm by 45 degree chamfer to edge of the hole where the bearing will be inserted. Click OK. 92

99 Topic 3 Final Project Basic Parts of the Mountain Board 6. Roll the model forward to the end. Right-click in the FeatureManager design tree and select Roll to End. Add Index Pins and Index Holes Index pins and holes provide two functions; first they help to line up the parts as they are put together in the assembly process. Second, they prevent the two halves from rotating, relative to one another, when they are in use. 1. Change to the Back view by clicking Back on the Standard Views toolbar. Change to Shaded with Edges. 2. Create a sketch on the back face of the model by clicking on the face. 3. Sketch a circle with its center on the Origin. Dimension the circle to 77 mm. The pins and holes will be placed on this circle. You do not want this circle to create an extrusion or cut, you just want to use it to line up other sketch entities. 93

100 Topic 3 Final Project Basic Parts of the Mountain Board 4. In the PropertyManager for the circle, select For Construction. The circle now changes to a construction line. 5. Create two construction lines. The end points of each line must be coincident with the construction circle and each line must be horizontal. 6. Add angular dimensions. To fully define the construction geometry, add the angle dimensions show. Select the Smart Dimension tool, and then select the Origin and each end of a line. Drag the dimension to the position shown. Repeat for the other dimension. 94

101 Topic 3 Final Project Basic Parts of the Mountain Board The four endpoints will be the locations for the pins and holes. 7. Sketch a circle at the endpoint of each line. 8. Dimension the two top holes. Dimension the circle on the right 3.9 mm and the circle on the left 3.8 mm. The larger circle will be used to create the hole and the smaller circle the pin. The difference in dimensions allows for a slight clearance to make sure the pins don t stick. 9. Add an Equal relationship between the two circles on the right. Repeat with the two circles on the left. This will make the two holes the same size and the two pins the same size. The sketch is now fully defined. 10. Click Extruded Boss/Base to create an extrusion. 11. Set Direction 1 to Blind and the depth to 4.5 mm. Rotate the model to allow you to see the preview. Do not click OK yet. 95

102 Topic 3 Final Project Basic Parts of the Mountain Board 12. In the PropertyManager, click the down arrow next to Selected Contours to expand the selection box. Click the two left circles to select their contours. Only the two circles will now be extruded, nothing else. 13. Click OK. 14. Rename the feature Index Pins. 15. You will now cut the Index Holes. Click the plus sign next to Index Pins and select the sketch under the feature. 16. Click Extrude Cut. 17. Set Direction 1 to Blind and the depth to 5.5 mm. Rotate the model to allow you to see the preview. 96

103 Topic 3 Final Project Basic Parts of the Mountain Board 18. In the PropertyManager, click the down arrow next to Selected Contours to expand the selection box. Click the two right circles to select their contours. Only these two circles will now be cut, nothing else. 19. Click OK. 20. Rename the feature Index Holes. 21. Click the plus sign next to Index Pins and Index Holes to show the sketch underneath. Notice that both features use the same sketch and that the sketch icons show the hand which indicates sharing. You will now add a Chamfer to the top of the Index Pins because you do not want to leave sharp edges on a small feature. 22. Click Chamfer then select the edges of the two pins. Select Distance distance for the type of chamfer and set the two distances to 1.5 mm and 1.0 mm. 23. Click OK. 24. Save and Print the Wheel Hub. Hole for Tube Stem The tire that will be used has a tube. There must be a cutout in the hub for the tube stem so that the tube can be inflated. You will create a revolve cut opposite one of the spokes. 1. Change to the Back view by clicking Back on the Standard Views toolbar. 2. Create a sketch on the back face of the model, by clicking on the face. 97

104 Topic 3 Final Project Basic Parts of the Mountain Board 3. Sketch a vertical centerline from the Origin. 4. Sketch a rectangle roughly in the position shown. 5. Add two Coincident relationships as shown. This will insure that we cut all the material in the rim. 6. Add a Collinear relationship between the left side of the rectangle and the centerline. 7. Dimension the width of the rectangle to 5.8 mm. 8. Create a revolved cut by clicking Revolve Cut on the Features toolbar. The cut can revolve 360 degrees even if it is only cutting material for 180 degrees. 9. Add a 0.5 mm by 45 degree chamfer to the edges of the cut as shown. 10. Save, Print, and Close the wheel hub. 98

105 Topic 3 Final Project Basic Parts of the Mountain Board Activity Directions: Importing Data For the mountain board, you are not going to design and manufacture the tire and the tube; you are going to use a supplier that makes both of these items. To include the tire and tube in your assembly, you need a CAD model. The supplier uses a CAD system that saves files in a format not supported by SolidWorks direct translators. To get the CAD model, the supplier has provided them in two neutral formats. 1. Click File, Open from the menu. 2. Select IGES (*.igs, *iges) from the Files of type list. 3. Examine the list to see the other files types that can be opened in SolidWorks. 4. Select the file Tire.igs from C:\Mountain Board Parts Library folder. 5. Click the Options button. You can change the settings for the import process. Set the options to: Surface/solid entities o Try forming solid(s) Perform full entity check and repair errors Automatically run import diagnostics 6. Click OK then Open. Watch the progress as the new solid is created. Notice that this can be a long process depending on the complexity of the model and the speed of your computer. When asked, click Yes to run Import Diagnostics on the part. When Import Diagnostic complete, click OK. 99

106 Topic 3 Final Project Basic Parts of the Mountain Board 7. Examine the FeatureManager design tree. There is only one feature for the tire called Imported1. The translation process, through neutral translators, does not provide any of the individual feature information, only a single body. You can add additional features to this model, but you cannot change anything about Imported1. 8. Select File, Save As. Save the tire in the C:\Mountain Board folder as Tire your last name.sldprt. 9. Select File and then Close. Import the Tube The Tube was provided as a STEP file. STEP is also a neutral format like IGES but is newer and gaining more popularity. 1. Click File, Open from the menu. 2. Select STEP AP203/214 (*.step,*.stp) from the Files of type list. 3. Select the file Inner Tube.STEP in the C:\Mountain Board Parts Library folder. 4. Click Open. The Inner Tube will open much faster than the Tire because it is a much simpler part. Again there is only one feature, Imported1. 5. This takes seconds to run. Click Yes if the Import Diagnostics window appears. 6. Click File and then Save As. Save the inner tube in the C:\Mountain Board folder as Inner Tube your last name.sldprt. 7. Select File and then Close to close the Inner Tube. 100

107 Topic 3 Final Project Basic Parts of the Mountain Board Create the Wheel Assembly You now have the basic parts to create a wheel assembly. You will use two Wheel Hubs plus the Tire and Inner Tube. You saved the three parts you need for this assembly in the C:\Mountain Board folder Wheel Hub, Tire, and Inner Tube. 1. Create a new assembly. Click File, New and select the Assembly template. 2. Insert the first part. Click the Browse button in the PropertyManager. Locate the part Wheel Hub and click Open. The wheel hub will appear transparent; drag it to the assembly Origin. When the cursor changes to release the mouse button. If there is no origin in the window, select Origin in the View menu drop down. 3. The Wheel Hub is now fixed in space with its Origin mated to the assembly Origin and its three principal planes mated to the three planes of the assembly. You will add another instance of the Wheel Hub. The wheel assembly will use two wheel hubs mounted back to back. Because you already have one instance of the wheel hub in the assembly, you can insert another instance by dragging it from the FeatureManager design tree. 4. Hold down the Ctrl key on the keyboard and drag the Wheel Hub from the FeatureManager design tree and drop it in the graphics area. The FeatureManager design tree shows two instances of the Wheel Hub. Instance one is fixed in space and the second instance still has some degrees of freedom as noted by the minus sign. 101

108 Topic 3 Final Project Basic Parts of the Mountain Board 5. Most of the mating entities you will be choosing are faces. To make it easier to select faces, you will turn on a filter so that only faces can be selected. Click Toggle Selection Filters Toolbars on the Standard toolbar to open the Filter toolbar. Then click Filter Faces. With the filter on, the cursor will indicate that you are on a face by changing to. When not over a face, the cursor will show that a filter is applied by changing to. 6. Add a Concentric mate. Hold down the Alt key and drag Face 1 to Face 2. When the cursor changes to Alt button., indicating a concentric mate, release the 7. The two Wheel Hubs will align coincident and the Mate Popup toolbar will appear. 8. Reverse the alignment. Press the Flip Mate Alignment button. This will toggle the two possible alignments. When the two hubs are facing in opposite directions, release the mouse button. 102

109 Topic 3 Final Project Basic Parts of the Mountain Board 9. Click to accept the mate. To move the second Wheel Hub, you need three mates to properly position it. First is the Concentric mate, already added. Second is a Concentric mate between an Index Pin and the corresponding Index Hole. Finally a Coincident mate between the inside faces of the two Wheel Hubs to keep them together. 10. It is easier to select the Index Pin and Index Hole if the two parts are moved apart. Drag the second Wheel Hub to the right to separate it from the first Wheel Hub. The exact distance is not important, only that you can select the pin and hole. 103

110 Topic 3 Final Project Basic Parts of the Mountain Board 11. Mate an Index Pin to the corresponding Index Hole. Click on the Assembly toolbar then on Mate. Select the cylindrical edge of an Index Pin. Rotate the view so you can see the corresponding Index Hole, then click the inside face of the hole. Click OK. 12. Mate the inside faces of the two Wheel Hubs together with a Coincident mate. Click on the Assembly toolbar. Select the inside faces of the two Wheel Hubs, then click OK. 13. Save the assembly as Wheel Assembly your last name in the C:\Mountain Board folder. 14. Turn off the Face Filter. 15. Save and Print the wheel assembly. Add the Tube The Inner Tube must be mated to the Wheel Assembly. The difficulty is that it doesn t have any surfaces that lend themselves to mating to the wheel hub. The Tube will be mated to the assembly using reference geometry. 1. Open the part Inner Tube. Click Window, Tile Vertically to tile the windows. 2. Drag the top level icon from the Inner Tube FeatureManager design tree into the assembly window. 104

111 Topic 3 Final Project Basic Parts of the Mountain Board 3. In the FeatureManager design tree, click the plus sign next to the part Inner Tube to expand the listing. 4. Click on the Assembly toolbar. Select the Front plane of the assembly and the Front plane of the Inner Tube. Coincident should be selected for Standard Mates. 5. Click OK. The Inner Tube will move into the plane of the hub. 6. Repeat the above step to mate the Top planes of the assembly and Inner Tube Coincident, then the Right planes, also Coincident. 7. Check the assembly. The Inner Tube should be correctly positioned on the Wheel Hub with the Tube Stem coming through the hole in the Wheel Hub. 8. Close the inner tube window. 105

112 Topic 3 Final Project Basic Parts of the Mountain Board Add the Tire The procedure for adding and mating the Tire is essentially the same as for adding the Inner Tube. 1. Locate the Tire.sldprt you created earlier. 2. Drag the Tire.sldprt into the assembly window. 3. Add mates between the three principal planes of the Tire and the Hub assembly. 4. Save and Print the wheel assembly. You will now use the SolidWorks Toolbox to create a new part for each fastener. 5. Click Tools, Add-Ins from the menu. 6. Select both SolidWorks Toolbox and SolidWorks Toolbox Browser. Click OK. Toolbox will be added to the Design Library. 7. Click Toolbox, Configuration from the menu. 8. Select the Browser tab, then Document Properties. Select Always create copy. 9. Click Browse then navigate to the C:\Mountain Board Parts Library folder. Click OK. 106

113 Topic 3 Final Project Basic Parts of the Mountain Board Open Toolbox Browser 1. Expand Toolbox on the Design Library Task Pane (located on the right side of your screen). The Toolbox Browser appears. 2. Click the pushpin to keep the Design Library open as you select other things. 3. Select the folder Ball Bearings under SKF \Bearings. 4. Drag a Radial Ball Bearing and drop it on the bearing cutout in the Hub. 5. The Radial Ball Bearing property box will appear. 6. Select the size 6001 and a Display of Detailed. Click OK. A bearing part will be created and added to the assembly. 7. There will still be a bearing preview on your cursor, rotate the assembly so you can see the other side and drop a second bearing at the other bearing cutout. 8. Click Cancel in the PropertyManager to stop adding bearings. 9. Add a Concentric and Coincident mates to position the bearing so it is bottomed in the bore of the Wheel Hub. 10. Change the view orientation to the Front view. 11. Select the Ansi Metric, Bolts and Screws, Socket Head Screws folder under Toolbox. 107

114 Topic 3 Final Project Basic Parts of the Mountain Board 12. Press and hold the Ctrl key and select the three edges of the bolt holes. 13. Right-click the nut Socket Head Cap Screw Ansi B18.3.1M and select Insert into assembly. 14. Select the following properties: Size: M6 Length: 25 Drive Type: Hex Thread Length: 25 Thread Display: Simplified 15. Click OK. Add the Nuts The three nuts can be added with the same procedure. One difficulty will be aligning the flats of the nuts with the holes as the Toolbox nuts do not have mate references to create this alignment. 1. Change the view orientation to the Back view. 2. Select the Ansi Metric, Nuts, Hex Nuts folder under Toolbox. 108

115 Topic 3 Final Project Basic Parts of the Mountain Board 3. Press and hold the Ctrl key and select the three edges of the bolt holes. *Note: You must be careful to select the edge of the bolt holes and not one of the edges of the bolt. If you have the wrong edges selected, one or more of the bolts will not be able to be mated in the assembly and will cause an error. 4. Right-click the nut Hex Nut Style 1-ANSI B M and select Insert into assembly. 5. Select the sizes shown, and then click OK. Three nuts will be inserted into the assembly. 109

116 Topic 3 Final Project Basic Parts of the Mountain Board 6. Add a Parallel mate between a flat on the nut and the flat in the hole. Zoom in on one of the nuts. Turn on the Filter Face by clicking toolbar. on the Filter If the face you are trying to select is hidden behind another object, in this case, the nuts in your current assembly, Select Other is used to select hidden faces or the model without reorienting it. 7. Click Insert, Mate to open the Mate PropertyManager. 8. Place the cursor as shown and right-click. Choose Select Other. The top face of the nut will become transparent and you are looking at the faces on the inside of the nut. 9. The cursor will change to. Move your cursor over the list. Each face will highlight when the cursor moves over it in the list. Click the left mouse button over the face of the B M Hex nut to accept this face. This face will now be listed in the Mate PropertyManager. 10. Select one of the flat faces of the Hex-Cut. Depending on the orientation of the model and the nut, you can either pick the face directly or use Select Other. 11. Apply a Parallel mate. The nut will now rotate to the correct position. 110

117 Topic 3 Final Project Basic Parts of the Mountain Board 12. Repeat the above steps to align the other two nuts. 13. Save the assembly. 14. Orient the model to the Isometric view. 15. Click Display, Section View on the View toolbar. 16. In the PropertyManager, click to select the Right plane as the section plane. Click OK. 17. Reorient the model to the Right view. 18. Examine the model. Check the fit of the bolts and bearings. While in the section view, you can zoom and pan to get a better look at the individual features. 19. To return to the normal view, either click Section View on the View toolbar or clear View, Display, Section View on the menu. 20. Save, Print, and Close the assembly. 21. Exit SolidWorks. Click on the Forward arrow to resume the activity. 111

118 Topic 3 Final Project Basic Parts of the Mountain Board Activity 3 Creating the Deck Objective When you have completed this activity, you will have the knowledge and skills to import and modify the deck of the mountain board. You will be able to: import the mountain board deck using SolidWorks. apply a material to the deck. Activity Directions: Creating the Deck SolidWorks should be on your screen. If it isn't, click on the Application Launch button and choose SolidWorks from the menu. The model of the deck has been created for you. Select File and then Open. Navigate to the C:\Mountain Board Parts Library. Select Part for the Files of type drop down box. Double click on the part Deck. The model of the deck appears on the screen. Select Yes if a dialog box appears stating that the file will open as Read Only. Before you go any further, save the deck. Select File and then Save As. Save the part in the C:\Mountain Board folder as Deck your last name. Add a Material and Texture The next task is to add a material and texture to the model. The material will be used for weight calculations and the Bill of Materials that will be added to the drawings. 1. In the FeatureManager design tree, right-click Material and select Edit Material. 2. Click the plus sign next to Plastics to expand the list. 3. Select Acrylic (Medium-high impact). 4. Click OK to accept this material. 5. Select the top level icon in the FeatureManager design tree. By selecting the top level icon, you are selecting the entire part. 6. Click Edit Texture on the Standard toolbar. 112

119 Topic 3 Final Project Basic Parts of the Mountain Board 7. For Texture Selection, click the plus sign next to Plastics. Select Acrylic (Medium-high impact). 8. Click Apply. 9. Adjust the Texture properties. The two sliders adjust the Scale and Angle of the pattern. Adjust them to achieve the look you want. 10. Save and print the part. 11. Click on the Forward arrow to resume the activity 113

120 Topic 4 Final Project Multibody Parts of the Mountain Board TOPIC 4 FINAL PROJECT - MULTIBODY PARTS OF THE MOUNTAIN BOARD Objective When you have completed this topic, you will have the knowledge and experience to design multibody solids. You will explore the three Boolean operations that can be used to combine multibody solids within SolidWorks by evaluating the design of the mountain board s axle. You will create several of the features of the mountain board s truck by creating individual solid bodies, then combining them into the final shapes. You will also create the spring and the binding straps for the mountain board. Overview Multibody solids occur when there is more than one solid body in a part. Multibody solids are created in several ways. You will explore commands in SolidWorks that have the option of creating multiple solid bodies from a single feature. Using multibody techniques, you will create parts and features. You will first create extrusions based on the standard views of the final part, and then you will combine them into a single body. 114

121 Topic 4 Final Project Multibody Parts of the Mountain Board Activity 1 Creating the Axle and Truck Objective When you have completed this activity, you will have the knowledge and skills to explore how the axle was designed and create the truck for the mountain board. You will be able to: evaluate the design intent for the axle and the truck. explore the combined bodies technique in SolidWorks. use multibody techniques to create the truck. use extrusions and revolves to create features for parts. Activity Directions: Creating the Axle Click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. The Axle was created for you. You will evaluate the features of the Axle by exploring how the model was designed. You will see how two individual solid bodies were combined into the final shape. 1. Click File and then Open. The Open dialog box appears. Navigate to the C:\Mountain Board Parts Library folder in the Look in: box. In the Files of type: box, click on the down arrow and select Part. Double-click on the Axle file. 2. Click on File and then Save As. Save the part in the C:\Mountain Board folder as Axle your last name. Select Part in Save As type. This design started with the following sketch created on the Front plane and extruded to a depth of 11 mm. 115

122 Topic 4 Final Project Multibody Parts of the Mountain Board Then the following sketch was created on the Top plane with both arc being tangent to each other and to the lines they are attached to. The sketch was then extruded to a Blind depth of 46 mm. Examine the results of the two solid bodies. Because the results of the two extrusions were not merged, each remains separate. Look at the graphic. Notice that there is no edge where the two bodies intersect. 116

123 Topic 4 Final Project Multibody Parts of the Mountain Board The two solid bodies were combined using the Combine tool on the Features toolbar. The Common tool was used to create a single solid body from the volume that is common to the two bodies. There are four possible choices for combining the two solid bodies. 117

124 Topic 4 Final Project Multibody Parts of the Mountain Board The following sketch was then created on the Top plane and extruded to a depth of 11mm. The following sketch was created on the Front plane and extruded to a depth of 50mm. There are now three solid bodies. All the bodies were then combined to make a single solid. This was done in two steps. First, Extrude3 and Extrude4 were combined to get the common volume. Then the two combined volumes were added together. 118

125 Topic 4 Final Project Multibody Parts of the Mountain Board A rectangle was sketched, extruded, and a collinear relationship was added. A fillet was then created to the extruded rectangle and fillets were added to the edges. Full Round Fillets were added, edges were trimmed and filleted. 119

126 Topic 4 Final Project Multibody Parts of the Mountain Board In the final steps, the connections to the other components were made. Tapped holes were added, king pin holes were created, and a material was applied to finish the design. 1. Select File and Close to close the axle. 2. Go to the next section in this, Activity Directions: Creating the Truck. Activity Directions: Creating the Truck SolidWorks should be on your screen. If not, click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. The approach to create the Truck is similar to how the Axle was created by creating several features as separate bodies, and then combining them. 120

127 Topic 4 Final Project Multibody Parts of the Mountain Board Create the Basic Shape 1. Click File and then Open on the Standard toolbar. The Open dialog box appears. Navigate to the C:\Mountain Board Training Templates folder in the Look in: box. In the Files of type: box, click on the down arrow and select All Files. Double-click on the Part_MM.prtdot file. 2. Click File and then Save As. Save the template in the C:\Mountain Board folder as Truck your last name. Select Part from the Save as type: dropdown list. Click Save. 3. Create a sketch on the Front plane. 4. Use the centerline and sketch mirroring to create the sketch. 5. Add a dimension between the arc and the base line. By default, the dimension will be placed at the center of the arc. 6. With the dimension selected, drag the end of the extension line from the center of the arc to the arc itself. 121

128 Topic 4 Final Project Multibody Parts of the Mountain Board 7. Once the dimension goes to the top of the arc, it can be changed to the correct value of 72 mm. 8. Sketch a circle and add the two dimensions shown. The center of the circle should be coincident to the centerline. 9. To fully define the sketch, add a Concentric relationship between the circle and the arc. 122

129 Topic 4 Final Project Multibody Parts of the Mountain Board Mid Plane Extrusion The Mid Plane extrusion creates the feature so that it has an equal amount of material to each side of the sketch plane. The distance specified is the total depth of the extrusion. 10. Extrude the sketch. Select Mid Plane for the direction and type 100 mm for the depth. Click OK. 11. Create the following sketch on the Right plane. 12. The top of the sketch should be Collinear with the top of the model and the two top lines should have an Equal relationship. 123

130 Topic 4 Final Project Multibody Parts of the Mountain Board 13. Extrude the sketch Up To Vertex. Select the Vertex shown. Select Direction 2 and choose Up To Vertex. Select the Vertex shown. Clear Merge result and click OK. 14. Create a new Sketch on the Top plane. Sketch the following geometry. 15. The sketch is symmetrical. Use the centerline and Dynamic Mirror under Tools, Sketch Tools. 124

131 Topic 4 Final Project Multibody Parts of the Mountain Board 16. Add 45 mm, 25 mm and 12 mm sketch fillets. You will have to delete the centerline to add the 25mm fillets. 17. Add a Tangent relationship to the two R45mm fillets. The sketch should now be fully defined. 125

132 Topic 4 Final Project Multibody Parts of the Mountain Board 18. Clear Merge result and Extrude the sketch Up To Vertex. Click OK. 19. To combine the three extrusions, click Combine and select Common from the Insert, Features menu. Select the three solid bodies. Click OK. 20. Save the part and Print a copy. 126

133 Topic 4 Final Project Multibody Parts of the Mountain Board Create the Bearing Holes 1. Orient the model to the Front view. Click Sketch, and then click the surface that the hole is on. 2. Sketch a circle as shown, centered on the existing hole in the Truck. Dimension the hole to 28 mm. 3. Create a Blind, Extruded Cut to a depth of 8 mm. Reorient the model to the Back view and repeat the cut. 127

134 Topic 4 Final Project Multibody Parts of the Mountain Board Hex Nuts The Hex Nuts will be molded into the Truck during the manufacturing process. You will create holes in the Truck to account for them. 1. Orient the model to the Top view. Create a sketch on the top face of the model by clicking Sketch and then clicking on the face where the hex nuts are shown. 2. Sketch a centerline vertically from the Origin. 3. Click Dynamic Mirror from the Tools, Sketch Tools menu. 4. Click the Polygon tool and sketch two polygons. If the Polygon tool is not on the Sketch toolbar, select Tools, Sketch Entities, Polygon from the menu. 5. The number of sides to the polygon is adjusted in the PropertyManager. Select

135 Topic 4 Final Project Multibody Parts of the Mountain Board 6. Turn off Dynamic Mirror. 7. Add a Horizontal relationship between the Origin and the centers of the two polygons you created. You can select the two centerpoints and the Origin in the same command. 8. Notice that there are no centerpoints on the two polygons created by the Sketch Mirror. 9. Select one edge from each of the two polygons you drew and add a Vertical relationship. This keeps the polygons from rotating. 10. Select the to circles that are inscribed in the polygons and add an equal relationship. With the circles equal, you only need to add size dimensions to one of the polygons. *Note: You may have to zoom in on the polygons to be able to select the circles. 11. Dimension the sketch as shown. 12. Extrude a cut, Through All. 13. Rename this feature Hex Cuts. 129

136 Topic 4 Final Project Multibody Parts of the Mountain Board Create Standoffs When assembled, the axle flanges will be positioned between the two bearings. To reduce the contact area, you will add standoffs to the sides of the Truck. 1. Create a sketch on the face shown. 2. Click Normal To on the Standard View toolbar to orient the view to the selected face. 3. The face we are sketching is hidden. Change the display to Hidden Lines Visible by clicking on the Views toolbar. 4. Create a headstone sketch. Add a Concentric and Collinear relationship. Dimension the arc to 18 mm. 130

137 Topic 4 Final Project Multibody Parts of the Mountain Board 5. You need to make sure the standoff has a hole that matches the center hole in the Truck. 6. Select the edge of the hole and click Convert Entities on the Sketch menu. 7. Extrude the sketch to a Blind depth of 2 mm. 8. Create a matching standoff on the other inside face of the Truck. 9. Save the part. Add ribs to vertical bosses 1. Create a sketch on the Right plane. Change the model view to the Right view. 2. Sketch a single line making each end point coincident to the edges shown. 3. Click the Rib tool on the Features menu. 131

138 Topic 4 Final Project Multibody Parts of the Mountain Board 4. Select Both Sides. Select Parallel to Sketch. 5. Type 2.5 for the rib thickness. 6. Examine the sketch in the graphics area. Make sure the gray arrow is pointing towards the intersection of the vertical boss and base plate. If it is not, right click on the arrow or select Flip material side in the PropertyManager. 7. Click OK. 132

139 Topic 4 Final Project Multibody Parts of the Mountain Board 8. Now that you have one rib, the remaining ribs can be made using a pattern. Click Insert, Pattern/Mirror, Linear Pattern. 9. Select the two edges shown for direction 1 and Set the spacing to 12 mm for each direction and the number of instances to Select Pattern seed only. This will create the pattern in the second direction with only the original seed element (the rib). 12. Click in the box Features to Pattern to make it active, and then select the Rib either in the graphics area or the FeatureManager design tree. You should now have a preview of the ribs. Click OK. 133

140 Topic 4 Final Project Multibody Parts of the Mountain Board 13. Repeat the above procedure to create ribs for the other vertical boss. Remove Material from the Base You can reduce the weight of the Truck by removing material from the three thick areas and then adding ribs to maintain the stiffness of the truck and restore some of the strength. The first part of the task is to remove material from the base plate. 1. Create a sketch on the bottom face of the Truck by selecting Sketch and then clicking on the bottom face. 2. Click on the bottom face again to create an offset from the edges. 3. Click Offset Entities on the Sketch toolbar. 4. Select Reverse to get the sketch inside the edge of the truck and enter 2.5 mm for the offset distance. Click OK twice. 134

141 Topic 4 Final Project Multibody Parts of the Mountain Board 5. Show the sketch used to create the Hex Holes by expanding Hex Cuts in the Feature Tree, and then right click on Sketch and select Show. 6. Sketch two circles centered on the two hex holes on the right. 7. Add an equal relationship. Dimension one of the circles to 22 mm. 8. Trim the overlapping part of the circles to leave a sketch that looks like the figure shown above. Select Trim Entities from the Sketch menu. Select the overlapping arcs. 9. Sketch a vertical centerline from the origin. The length is not important. 10. Select the centerline and the two arcs that make up the figure shown above by holding down the Ctrl Key, then click Mirror Entities. 135

142 Topic 4 Final Project Multibody Parts of the Mountain Board 11. Click Extruded Cut. 12. Select Offset From Surface for the end condition, then select the top face of the truck. 13. Type 2.5 mm for the distance. 14. Check the preview. Click OK. 15. Hide the sketch under Hex Cut feature. 16. Create four bosses for the holes that will connect the truck to the deck of the mountainboard. 17. Create a sketch on the bottom face of the Truck. 18. Sketch a vertical centerline through the origin. With the centerline selected, click Dynamic Mirror from the Tools, Sketch Tools menu. 136

143 Topic 4 Final Project Multibody Parts of the Mountain Board 19. Sketch two circles to the right of the centerline, SolidWorks will create two mirror images of the circles. 20. Add an Equal relationship between the two circles you sketched. 21. Add a Vertical relationship between the centers of the two circles that SolidWorks drew. 22. Turn off Dynamic Mirror Entities. 23. Add a dimension of 9.5 mm to one of the circles. It doesn t matter which of the four circles you add the dimension to, the symmetric and equal relationships will take care of the remaining circles. 24. Add the dimensions shown to fully define the sketch. 137

144 Topic 4 Final Project Multibody Parts of the Mountain Board 25. These new bosses you are creating need to be the same height as the bosses for the hex nuts. To make sure they are always the same height, you can extrude your sketch Up To Surface. 26. Click Extrude Boss/Base. Select Up To Surface for the end condition, and then select the face shown. 27. Notice that the face changes to magenta, the same as the color in the PropertyManager. Click OK. Create Strengthening Ribs You can not leave the base plate hollowed out because it will not have enough stiffness to keep the vertical bosses upright. To strengthen it, you will add a web of ribs that look like this. 28. Examine the ribs. Notice that with the exception of the center vertical rib, all the remaining ribs radiate from a single point between the hex holes on each side. To construct this set of ribs, you will start with a layout sketch. 138

145 Topic 4 Final Project Multibody Parts of the Mountain Board Construction Geometry 29. Create a sketch on the 2.5 mm wide bottom face of the model. 30. Click to start a centerline. A centerline is a line used for construction. 31. Sketch a centerline between the two vertices as shown. 32. Click Point on the Sketch toolbar. 33. Move the cursor over the centerline until the midpoint symbol appears. Click on the midpoint symbol to create a point at the midpoint of the centerline. 139

146 Topic 4 Final Project Multibody Parts of the Mountain Board 34. Sketch a centerline from the midpoint of the top arc to the midpoint of the bottom inside edge. 35. This represents the center of the part. 36. Sketch the centerlines shown. Each centerline starts at the point. Except for the horizontal and vertical centerlines, the other end of each centerline is coincident to the endpoint of an arc on the inner edge of the base. 140

147 Topic 4 Final Project Multibody Parts of the Mountain Board 37. Create the centerline and point on the right side of the model and create the remaining centerlines. 38. Sketch lines on top of the centerlines. These lines do not have to extend all the way to the edges because the rib tool will automatically extend the rib up to the next geometry. Each line however must cross all the other lines in the sketch. If they do not, the rib will stop at the next line rather than extending all the way to the existing part geometry. See the darker lines in the graphic below. 141

148 Topic 4 Final Project Multibody Parts of the Mountain Board 39. Click Rib and set the rib width to 2 mm. 40. Select Both Sides and Normal to Sketch. This will center the ribs on the sketch lines and extrude the ribs in a direction normal to the sketch plane instead of in the sketch plane as was done in the previous rib. 41. Examine the ribs, they should look like this. 142

149 Topic 4 Final Project Multibody Parts of the Mountain Board 42. If part of a rib is missing, edit the sketch used to create the rib and extend the line into the area where the rib is missing. As an example: Add Ribs to Vertical Boss In this task, you will need to remove material from each of the vertical bosses, and then add ribs to stiffen the part. 43. Orient the model to the Front view. Create a sketch on the face shown. 143

150 Topic 4 Final Project Multibody Parts of the Mountain Board 44. Select the three edges shown by holding down the Ctrl key, and then click Convert Entities on the Sketch menu. This will give you three lines in your sketch that are tied to the underlying edges. 45. Right-click the top circular edge and click Select Tangency. Three edges are selected. 46. Click Offset Entities from the Sketch menu. Set the offset to 2.5 mm to the inside (see yellow line) and click OK. 47. You now have five lines and an arc that are all fully defined. While they are fully defined, their lengths can still be adjusted. Extend can be used to lengthen sketch geometry. (See ends of yellow line). 48. Click Extend on the Tools, Sketch Tools menu. When you move the cursor over a line, the extended line will be previewed. Extend Entities will extend the line until it intersects the next sketch entity. 144

151 Topic 4 Final Project Multibody Parts of the Mountain Board 49. Extend the two lines as shown. 50. Select Trim Entities on the Sketch toolbar to obtain a single closed profile. Click on the line segments shown by the arrows in the graphic below. Click OK. 51. Create an additional 2.5 mm offset. Click on the edge of the circular cutout and then select Offset Entities from the Sketch toolbar. This will be used to hold the bearing. Click OK. 145

152 Topic 4 Final Project Multibody Parts of the Mountain Board 52. Extrude a cut from the Features toolbar using Offset From Surface. Enter 2.5 mm for the offset distance. 53. Select the inside face around the vertical boss as the offset surface. 54. Add a 5.0 mm Fillet (Features toolbar) to the inside bottom edge. (See the shaded areas in the graphic below). 55. Repeat the above steps to the other vertical boss. Orient the model to the Back view. Add Ribs 1. Orient the model to the Front view. Create a sketch on face shown. 2. Click Point from the Sketch toolbar and add a point and Coincident to the center of the hole using Add Relation. 146

153 Topic 4 Final Project Multibody Parts of the Mountain Board 3. Create the following sketch. For this sketch, just add a Coincident relationship between each radial line and the point at the center of the circle. 4. Add the additional arcs and lines to complete the sketch. Create Ribs 5. Use the rib tool to create ribs that are 2mm thick and have 2 of draft. 147

154 Topic 4 Final Project Multibody Parts of the Mountain Board Add Fillets 6. Add an 8 mm fillet to the three edges as shown. 7. Repeat the process for the other vertical boss. *Note: Use Mirror Entities and Symmetric relationships to reduce the amount of sketching. Remove More Material The final task is to remove some material along the top of the vertical bosses. You can remove the material to reduce the weight of the part. 8. Click Chamfer on the Features toolbar. 9. Select the edge shown. 10. Select Distance distance for the type of chamfer. Enter 5.5 mm for the first distance and 10 mm for the second distance. 148

155 Topic 4 Final Project Multibody Parts of the Mountain Board 11. Examine the callout to make sure the 10 mm is applied to the top side of the vertical boss and the 5.5 mm is down the side. If the directions are reversed, enter 10 mm for direction 1 and 5 mm for direction 2. Click OK. 12. Apply another Chamfer to the other vertical boss. Create Cuts for Mounting 13. Orient the model to the Bottom view. Select the bottom rib face of the model. 14. Click the Hole Wizard on the Features toolbar. Click the Hole button. 15. Set the properties of the hole as follows: Standard: Ansi Metric Screw Type: Screw Clearances Size: M4 End Condition: Up To Surface 16. Once you select Up To Surface, you must select the surface. Rotate the model and select the top face of the base plate. 149

156 Topic 4 Final Project Multibody Parts of the Mountain Board 17. Click the Positions tab. Orient the model to the Bottom view. 18. You want each hole to be centered on its respective boss so they must each be concentric to the boss. Move the cursor over the circular edge of a boss and pause. The centerpoint will be calculated and displayed. 19. Move the cursor to the centerpoint and select it. This will add a concentric relationship between the point and the circular edge. 20. Repeat this procedure for the remaining three bosses. 21. Click Point to turn it off. 22. There is one additional point on the bottom face. This was created when you initially selected the bottom face. Select this point and delete it as it is not needed. 23. Complete the hole by clicking OK. 150

157 Topic 4 Final Project Multibody Parts of the Mountain Board Model refinement Examine the model. The holes you just added come very close to some of the ribs. When the Mountainboard is assembled, a bolt will go through each of these holes and screw into a hex nut. You must have enough room around each of the holes to fit the nut. 1. Locate the pattern feature that created this series of ribs, it should be LPattern1. 2. Right-click the pattern feature and select Edit Feature. *Note: If you added and removed patterns while creating the Truck, the feature name might be different. 3. Locate the section Instance to Skip in the PropertyManager and click the down arrow. This will expand the Instance to Skip section and place a magenta dot over each pattern instance in the graphics area. 4. Select the two magenta dots. The preview will show that the rib instances will be removed. Click OK. The two ribs have been removed and we now have enough room for the nuts. 5. Save the part. 151

158 Topic 4 Final Project Multibody Parts of the Mountain Board Adjust the part s appearance The manufactured part will be black in color. In this task you will change the appearance of the part to black and adjust its reflective properties. 1. Select the Appearance tab on the Task Pane. 2. Expand the Appearances and Plastic folders and select Textured. 3. Press and hold the Alt key and drag the appearance PW-MT11250 into the graphics area. This will apply the appearance to the entire part. The PropertyManager will now show the properties of this appearance. 4. Click OK. 5. Save, Print, and Close the part. 6. Exit SolidWorks. Click on the Forward arrow to resume the activity. 152

159 Topic 4 Final Project Multibody Parts of the Mountain Board Activity 2 Springs and Binding Objective When you have completed this activity, you will have the knowledge and skills to create the springs and the binding straps in SolidWorks for the mountain board project. You will be able to: create the springs as a sweep feature. demonstrate a composite curve. create the four pieces of the binding strap. apply material to a part. Activity Directions: Creating the Springs and Binding SolidWorks should be on your screen. If not, click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. Crate a Helix A spring is created by forming a rod into the shape of a helix. To create a spring, you will sweep a circle along a helix. 1. Click File and then Open on the Standard toolbar. The Open dialog box appears. Navigate to the C:\Mountain Board Training Templates folder in the Look in: box. In the Files of type: box, click on the down arrow and select All Files. Double-click on the Part_MM.prtdot file. 2. Click File and then Save As. Save the template in the C:\Mountain Board folder as Spring your last name. Select Part from the Save as type: dropdown list. Click Save. 3. Create a sketch on the Top plane. 4. Sketch a circle and dimension its diameter as 25 mm. 5. Click Insert, Curve, Helix/Spiral from the menu. Select Height and Revolutions from the Defined By list. Enter 45 mm for Height and 5.5 for Revolutions. Select Counterclockwise for the rotation direction and 0 for the Start angle. Uncheck the Reverse Direction box. 153

160 Topic 4 Final Project Multibody Parts of the Mountain Board 6. Click OK. The helix will be the sweep path for the spring. Create a Profile The sketch used as the sweep profile must be created on a plane that is on the end of the sweep path. 7. Create a sketch for the profile on an plane normal to the end of the helix. Select the helix near the end closest to the origin. Then click Sketch. 8. Sketch a circle. The position should be approximately as shown. You do not have to position it exactly; you will do that with a relationship. 154

161 Topic 4 Final Project Multibody Parts of the Mountain Board Pierce Relationships The Pierce relationship is used in sweeps. It can be thought of as a 3D Coincident relationship. In our spring, the circle will follow the helix. Think of the helix as a thin piece of wire and the profile sketch as being drawn on a piece of paper. If you stick the wire through the paper at the center of the circle, this would be a pierce relationship. 9. To add a Pierce relationship, select both the center of the circle and the helix by holding down the Ctrl key. There should only be one relationship shown, Pierce. Apply the Pierce relationship. 10. Dimension the circle to a diameter of 4 mm. The sketch should be fully defined. 11. Exit the sketch. When you create extruded or revolved features, only one sketch is involved, so you normally select Extrude or Revolve while you are still in the sketch. Because a sweep requires more than one sketch (profile and path) you must not be in Edit Sketch mode to start the sweep. 12. To create the sweep, click on the Features toolbar. Select the circle for the profile and the helix for the path. The callouts and color help to identify which sketch is which. 155

162 Topic 4 Final Project Multibody Parts of the Mountain Board 13. Set Options to Follow Path. This will keep the profile sketch normal to the path curve as it sweeps. Click OK. You now have the center section of the spring. You need to make some additions to create a realistic spring. Compression springs have the last turn at each end at a tighter pitch and the ends are ground flat to create more contact area. Create the Lower Helix 14. Select Sweep1 in the FeatureManager design tree and press Delete. You only want to delete the sweep feature, not the underlying sketches and helix. Make sure that Also delete absorbed features is cleared (not checked). Click Yes. 15. Delete the profile sketch (Sketch2). 16. Create another sketch on the Top plane. 17. Sketch a circle and dimension it to 25 mm. 18. Click Insert, Curve, Helix/Spiral. 19. Select Pitch and Revolution in Defined By:. Set the pitch to 4 mm and 1.0 revolutions. The Start angle must be 0.00 degrees to make the helix end where the original helix begins. 20. Select Reverse direction and Clockwise. Check the preview graphics to make sure the new helix is going in the correct direction. It should look like an extension to the original helix. Click OK. Create the Upper Helix 21. Click Insert, Reference Geometry, Plane. 22. Expand the Flyout FeatureManager design tree by clicking on the plus sign next to the part icon. Select the Top plane in the FeatureManager design tree and the top of the helix. 156

163 Topic 4 Final Project Multibody Parts of the Mountain Board 23. Because you selected a plane and a point, SolidWorks will default the type of plane to Parallel. Click OK. 24. You will now create a sketch on this new plane. Sketch a Circle, centered on the Origin and dimension the diameter to 25mm. 25. Create a helix by selecting Insert, Curve, Helix/Spiral. Set the Helix options as shown: 26. Click OK. Save the part. Create a Composite Curve A Composite Curve enables you to combine reference curves, sketch geometry, and model edges into a single curve. This curve can then be used as a guide or path when sweeping or lofting. 27. Click Insert, Curve, Composite from the menu. Either in the graphics area or the FeatureManager design tree, select the three Helixes. 28. Click OK. The three Helix/Spiral features and their sketches will now be absorbed by the CompCurve1 feature. If you select CompCurve1 in the FeatureManager design tree, the entire helix will highlight in the graphics area showing that the three curves have been combined. Create The Sweep 157

164 Topic 4 Final Project Multibody Parts of the Mountain Board 29. Create a sketch at the end of the composite curve. Sketch a circle, dimension it as 3.9 mm in diameter. 30. Add a Pierce relationship between the center of the circle and the composite curve. 31. Exit the sketch. 32. Create a Sweep using CompCurve1 as the path. Click OK. 33. Hide the sketch plane by right-clicking on the plane and select Hide. Create End Cuts 34. Create a sketch on the Front plane. Reorient the model to the Front view. 35. Draw a vertical centerline from the Origin downward. Draw a horizontal line. 36. Add a Midpoint relationship between the end of the centerline and horizontal line. 37. Dimension the sketch as shown above. 38. Click Insert, Cut, Extrude on the menu. Because this is an open sketch, the default end condition will be Through All. Notice that Direction 2 is also checked and Through All is the end condition. 158

165 Topic 4 Final Project Multibody Parts of the Mountain Board *Note: If your cut results in just a little piece of the spring being left, edit the feature and select Flip side to cut. 39. Click OK. 40. Repeat this procedure for the other end of the spring. The total length of the spring should be 53 mm. 41. Save your part. Create Reference Geometry Thinking ahead to the task of creating an assembly using this spring, you will need to create some reference geometry to make it easier to mate the spring in the assembly. 1. Click Insert, Reference Geometry, Axis from the menu. 2. Select the Front and Right planes. By selecting two planes, the axis will be created at the intersection of the planes. Click OK. 3. Rename the Axis as Centering. 159

166 Topic 4 Final Project Multibody Parts of the Mountain Board 4. Click Insert, Reference Geometry, Plane. 5. Select the bottom face of the spring. 6. With only one plane selected, the default plane type will be distance. You want this plane to be at the mid-point of the spring which is 53 mm tall. You could divide 53 by 2 to get the distance, then enter the value in the property manager. An easier way is to enter 53/2. When you press Enter, SolidWorks replaces the equation with the result 26.5 mm. 160

167 Topic 4 Final Project Multibody Parts of the Mountain Board 7. Check the preview to insure that the direction places the new plane in the middle of the spring. If not, select Reverse direction. Click OK. 8. Rename the plane Center Plane. 9. Save the part. Create an Assembly Creating the final assembly of the mountainboard will be easier if you create the subassemblies as you go along. 10. Click File and then Open on the Standard toolbar. The Open dialog box appears. Navigate to the C:\Mountain Board Training Templates folder in the Look in: box. In the Files of type: box, click on the down arrow and select All Files. Double-click on the Assembly_MM file. 161

168 Topic 4 Final Project Multibody Parts of the Mountain Board 11. Select File and then Save As. Save the assembly in the C:\Mountain Board folder as Spring Assembly your initials. Select Assembly in the Save As Type. Click Save. 12. Because the Spring is still open, it will be listed in the Open documents box in the PropertyManager. Select Insert Component and then select the Spring. A transparent copy of the Spring will be on the screen and move with the cursor. 13. Move the cursor over the Origin of the assembly. When the cursor changes to click on the Origin. 14. Add the Spring Dampener by clicking Insert Components on the Assembly toolbar. Click Browse. Navigate to the C:\Mountain Board Parts Library folder and select the Spring Dampener. 15. Click in the graphics area to insert the part. 16. Turn on the Axes and Temporary Axes by clicking View, Axes and View, Temporary Axes from the menu. 17. Click Mate on the Assembly toolbar. 18. Select the axis of the Spring and the temporary axis of the Spring Dampener. The default mate will be Coincident. Click OK. This positions the Spring Dampener inside the Spring. 19. Click Mate on the Assembly toolbar. Click on the plus sign to expand the Assembly Flyout. Then expand the Spring and Spring Damper. 20. Hold down the Ctrl key and select the Center Plane in the Spring and the Top plane of the Spring Dampener. The default mate will be Coincident. Click OK. 162

169 Topic 4 Final Project Multibody Parts of the Mountain Board 21. To add a Spring Retainer, click Insert, Component, Existing Part/Assembly. Click Browse and locate the Spring Retainer in the C:\Mountain Board Parts Library folder. Click in the graphics area to drop the part. 22. To mate the Temporary Axis of the Spring Retainer to the Centering axis of the Spring, select the two faces shown, and then click Mate. Add a Coincident mate. Click OK. 23. In the FeatureManager design tree, expand the Spring features by clicking the plus sign next to the Spring part. Right-click the Center Plane and select Hide from the menu. 24. To add another Spring Retainer to the assembly, hold the Control key and drag the Spring Retainer from the FeatureManager design tree into the graphics area. 163

170 Topic 4 Final Project Multibody Parts of the Mountain Board 25. You will now mate the second Spring Retainer to the Centering axis of the Spring and the top ground face, like you did for the first Spring Retainer. This time, after you have selected the faces and clicked Mate, click the Anti-Align button (bottom of the Standard Mates box) to reverse the retainer. 26. Add a Fender Washer (from the C:\Mountain Board Parts Library folder) to the assembly and mate it to the top Spring Retainer. Use the Insert Component tool. Position the fender washer on top of the spring retainer like you did before with the retainer into the spring. 27. Save the assembly. Print and then Close the assembly. You are ready to create the Binding Straps. Create the Binding Straps 1. Open the part Binding Start Sketch in the C:\Mountain Board Parts Library folder. Make sure All Files is selected for Files of Type. Select Yes if a dialog box appears. This part only contains sketches, and reference geometry. It is used to set the spacing and interrelationships between the different parts of binding. 164

171 Topic 4 Final Project Multibody Parts of the Mountain Board The rectangles and centerlines represent the positions of the posts of the Binding Base Plate. The straps will later attach to these posts. The four blue curves will become the paths and guide curves when we sweep the straps. 2. Select File, Save As. Save the part in the C:\Mountain Board folder as Binding_straps your last name. 3. Create a sketch on the Top plane. Sketch a rectangle as shown. The size and position are not critical. 4. Right-click on the line shown and choose Select Midpoint from the menu. 5. Click Add Relationship. Click OK. 6. Select the line shown. Make sure you select the line and not the curve. If you select the curve instead of the line, you will not be able to add a Pierce relationship. 7. Select Pierce in the PropertyManager. 165

172 Topic 4 Final Project Multibody Parts of the Mountain Board 8. Add another Pierce relationship between the corner point of the rectangle and the guide line. 9. Dimension the width of the rectangle to 4 mm. 10. Exit the sketch. 11. Rename the sketch to Profile Create a sweep. Click Features, Swept Boss/Base. 13. Select Profile1 as the profile sketch and CompCurve1 as the path. 166

173 Topic 4 Final Project Multibody Parts of the Mountain Board 14. Click OK. Examine the feature. Notice that there is a twist in the sweep. 15. To correct the twist, you will use the guide curve. Guide Curves Sweeps can contain multiple guide curves which are used to shape the solid. As the profile is swept, the guide curves control its shape. 16. Right-click the sweep and selecting Edit Feature from the menu. 17. Expand the sections Options and Guide Curves by clicking the downarrow. 18. Select CompCurve2 for the guide curve. 19. Select Follow path and 1st guide curve for Orientation/twist Type. This will cause the profile to keep the corner point on the guide curve and prevent the twist you saw in the previous step. 20. Click OK. The sweep now stays flat. 167

174 Topic 4 Final Project Multibody Parts of the Mountain Board Full Round Fillets 21. Select Fillet. 22. Select Manual, then Full round fillet for Fillet Type. The Items To Fillet box will expand to require three faces to be selected. 23. Select the three faces shown. Note: The third face is on the far side NOT the top. 24. Click OK. The strap now has a full round on the end. 168

175 Topic 4 Final Project Multibody Parts of the Mountain Board Create the Second Strap Creating the second strap will be essentially the same as creating the first strap except that you will not round off the end because you attach the clasp assembly to it later. 25. Create a sketch on the Top plane. 26. Click the Rectangle tool and then select the 3 Point Center Rectangle in the PropertyManager. 27. Create Pierce relationships between the midpoint of the left side of the rectangle shown by the small dot in the graphic below and ComCurve3, and between the corner point of the rectangle and CompCurve Dimension the width of the rectangle to 4 mm. 29. Exit the sketch. 169

176 Topic 4 Final Project Multibody Parts of the Mountain Board 30. Rename the sketch Profile Create a sweep using the sketch Profile2 as the profile and CompCurve3 as the path and CompCurve4 as the Guide Curve. 32. Clear Merge results. Click OK. 33. Examine the FeatureManager design tree. Near the top is a folder called Solid Bodies. Click the plus sign to expand the folder. Each solid body takes the name of the last feature used to create it. Fillet1 is the first strap that was created with Sweep1 and Fillet1. Sweep2 is the strap you just created. 34. Rename the Solid Bodies to Strap_right and Strap_left. 35. Save and Print the part. 170

177 Topic 4 Final Project Multibody Parts of the Mountain Board Create the Foam Pad The binding needs a pad to spread the load out on the top of the rider s foot. This part will be molded in the flat state. When installed in the binding, it will take a shape defined by the straps and the rider s foot. Lofting Lofting enables you to create features that are defined by multiple sketches. The system constructs the feature - either a boss or a cut - by building the feature between the sketches. 36. Open the part Foam Pad.sldprt in the C:\Mountain Board Parts Library. Select File, Save As. Save the part in the C:\Mountain Board folder as Foam Pad your last name. 37. The preview should look like this: 38. Save and Close the part. Multibody Parts You created the two binding straps in the same part file. You will now add the foam pad to this part. When complete, each of the three multibodies will be saved to a separate file. Create a Curved Foam Pad 1. Open the Binding straps part you created in the C:\Mountain Board folder. You saved it as Binding_straps your last name. 2. Select the sketches Loft Section 1 through Loft Section 7. Right-click any of the selected sketches and select Show. 171

178 Topic 4 Final Project Multibody Parts of the Mountain Board These are the same loft sections used in the flat Foam Pad. The only difference is that they are all on planes that are normal to the edges of the straps. Some of the sections are also rotated to keep the rectangular slot aligned with the straps. 3. Create a Loft between the seven sketches. Click Lofted Boss/Base on the Features toolbar. 4. Select the seven sketches in turn. Make sure you select each sketch near the same point. Zoom in as necessary to make sure you select the correct point. 5. Clear Merge results. Click OK. 6. Examine the Solid Bodies folder in the FeatureManager design tree. There should be three solid bodies. Rename the solid body Loft1 to Foam_Pad. 7. You will now hide the sketches. Expand the Loft1 Feature in the FeatureManager design tree by clicking the plus sign next to the Loft1. Select the seven sketches. Right-click any selected sketch and click Hide. Do the same for Sketch1 and Sketch2. 8. Leave the part open. Click File and then Open. Browse to the C:\ Mountain Board Training Templates and select All Files in Files of Type. Doubleclick on Part_MM.prtdot template. Minimize this widow. 9. Maximize the Straps window. In the Solid Bodies folder, right-click Strap_right and select Insert into New Part. The Save As dialog will open. 10. Name the new file Strap_right your last name.sldprt and save it to the C\Mountainboard folder. 172

179 Topic 4 Final Project Multibody Parts of the Mountain Board 11. Save the remaining two solid bodies to separate parts called Strap_left your last name.sldprt and Foam_Pad_curved your last name.sldprt. Create the Strap Assembly 1. Click File, Open and choose the Assembly_MM.asmdot template from the C:\Mountain Board Training Templates folder. Make sure to select All Files for Files of Type. 2. Select Insert, Component, Existing Part/Assembly from the Main menu. All the open parts will be listed in the Open documents section of the PropertyManager. Select Strap_right your last name. The part Strap_right will now be previewed on the cursor. 3. Click the plus sign next to the Assembly icon on the fly-out FeatureManager design tree to show the existing components. Click on the Origin. This will insert the part Strap_right on the assembly Origin with its three planes aligned to the corresponding planes in the assembly. 4. Click Insert, Component, Existing Part/Assembly from the menu and insert the Strap_left your last name and Foam_Pad_curved your last name part using the same method. Because the three parts all came from the same original file, their origins and default planes all line up. This allowed us to insert them into the assembly without having to add additional mates. Notice that each part has an (f) in from of it. This means that the parts are fixed in space and can not be moved. 173

180 Topic 4 Final Project Multibody Parts of the Mountain Board 5. Save the assembly in the C:\Mountain Board folder as StrapAssembly your last name. Select Assembly for Save As Type. Print the assembly. Select Window, Close All. Add the Clasp Assembly 1. Re-open the Strap Assembly and open the assembly Clasp Assembly.sldasm in the C:\Mountain Board Parts Library folder. Select All Files for Files of Type. 2. Tile the SolidWorks windows by clicking Windows, Tile Vertically. Drag the top level icon for the Clasp assembly into the Strap Assembly. Close the Clasp Assembly and Maximize the Strap Assembly. 174

181 Topic 4 Final Project Multibody Parts of the Mountain Board Hide Components Hiding a component temporarily removes the component s graphics but leaves the component active within the assembly. 3. To hide your parts Strap_Right and Foam_Pad_curved, select the two parts, either in the graphics area or the FeatureManager design tree, then click on the Hide/Show Components Assembly toolbar. Mate Considerations 4. Add a Tangent mate between the top of the strap and the top of the slot in the clasp. 5. Add a Coincident mate between the midpoint of the strap and the midpoint of the edge of the clasp. 175

182 Topic 4 Final Project Multibody Parts of the Mountain Board 6. Add a Coincident mate between the vertex of the strap and the edge of the clasp. 7. The clasp is now fully mated to the strap. Select the Strap_right and Foam_Pad_curved then click Hide/Show Components. 8. Select File/Save As. Save the assembly in the C:\Mountain Board folder as Strap Assembly your last name. Print the assembly. 9. Collapse the assembly. Insert a Sub-Assembly into an Assembly Assemblies can be added to other assemblies in the same way parts are added to assemblies. Assemblies inside other assemblies are call sub-assemblies, however, they are exactly the same file type within SolidWorks. 176

183 Topic 4 Final Project Multibody Parts of the Mountain Board 1. Open the Binding assembly, Binding your last name, you created in Topic 3, Activity 1 in the C:\Mountain Board. 2. Tile the windows vertically. Drag the top level icon of the Strap Assembly into the Binding. Maximize the Binding window by clicking Maximize on the Window Title Bar. 3. Click to add a Mate. 4. Expand the Strap Assembly in the FeatureManager design tree and select the Top plane of the Strap Assembly. 5. Select the top face of the Binding Base Plate. 6. Click to add a Distance mate. Enter 12 mm for the distance. Click OK. 7. Add a Tangent mate between the face shown and the top face of the Strap_right. 8. Add a Coincident mate between the vertex and face shown. The Strap Assembly should now be fully mated into the Binding assembly. 177

184 Topic 4 Final Project Multibody Parts of the Mountain Board 9. Save the assembly. Create Strap Buttons 10. Select your part, Strap_right, then right-click and select the Edit Part tool. *Note: The Edit Component tool is a toggle. It switches you between Edit Part mode and Edit Assembly mode. It also acts as a visual indicator of which mode you are in. It is depressed when you are in Edit Part mode. 11. The strap you are editing turns pink as well as its representation in the FeatureManager design tree. Select the face of the Binding Base Plate as shown and click Insert, Sketch. 12. Even though you are editing your part Strap_right, you can create a sketch from a plane in another part. 13. Click Normal To on the Standard Views toolbar. 14. Click Zoom To Selection on the View toolbar. 15. Sketch a vertical centerline from the midpoint of tab. 178

185 Topic 4 Final Project Multibody Parts of the Mountain Board 16. Turn on Dynamic Mirror by selecting Tools, Sketch Tools from the Main menu. 17. Sketch a circle in one of the slots. The second circle will be drawn by the mirror command. *Note: The colors of the components and their transparency are controlled in Tool, Options, System Options, Color. The colors and transparency on your system may be different from the colors shown in these graphics. 18. Add two Tangent relationships between one of the circles and the sides of the slot. 19. Dimension the distance between the circles. 179

186 Topic 4 Final Project Multibody Parts of the Mountain Board 20. Turn off Dynamic Mirror Entities. 21. Hide the Binding Base Plate. 22. Click Extrude. 23. Click to reverse the direction of the extrusion. 24. Select Up To Next for direction. Up To Next extends the feature from the sketch plane to the next surface that intercepts the entire profile. (The intercepting surface must be on the same part.) 25. Click OK. 26. Right-click your Strap_right part and select Open Part from the menu. 27. Select the top face of one of the pins and open a sketch. 180

187 Topic 4 Final Project Multibody Parts of the Mountain Board 28. Click the Offset Entities tool. Enter 1 mm for the distance. Click OK. 29. Select the top of the other pin, and repeat the previous step. Click OK. 30. Extrude the sketch to a depth of 1 mm. Add a.5 mm fillet to the top of each button. 31. Return to the Binding assembly by clicking Window from the menu and selecting Strap_right -in-binding.sldasm from the list. 32. You are still in the Edit Part mode. Click Edit Component to return to the Edit Assembly mode. 33. In the FeatureManager design tree, select the Binding Base Plate and click Hide/Show Components to show the part. 34. Repeat the above procedure to add pins to the Strap_Left part. 35. Save and Print your Binding assembly. 181

188 Topic 4 Final Project Multibody Parts of the Mountain Board Create the Binding Pad The Binding Pad will be made by cutting a flat piece of material to shape, then gluing it to the Binding Base Plate. This is another case where you might create two versions of this part. One would be the flat piece used for manufacturing and the other would be the part in its curved shape to be used for illustrations. You will create the curved version of the part in the context of the Binding assembly. 36. Click Insert, Component, New Part from the menu. 37. Name the new part Binding Pad your last name. Save it in the C:\Mountain Board folder. 38. The cursor changes to indicating that you need to select a plane for the first sketch. Whichever plane or face you select will become the Front plane of the new part. 39. Select the thin face shown. 40. As soon as the face is selected, you are in Edit Sketch mode, editing the new part. The FeatureManager design tree shows the part in the pink color. 41. Reorient the view to the Right View. 42. Select the six edges shown, and then click Convert Entities. 182

189 Topic 4 Final Project Multibody Parts of the Mountain Board 43. Right-click your part Binding Pad in the FeatureManager design tree and select Open Part. 44. Right-click Sketch1 and select Edit Sketch. 45. Drag one of the endpoints shown onto the other endpoint. 46. Exit the sketch. 47. In the FeatureManager design tree, select the sketch. 48. Click Insert, Curve, Composite. This will combine the six lines and arc segments into a single curve that be can use as a path for a pattern feature. 49. Click OK. 50. Create the following sketch on the Front plane. 51. Drag the corner of the sketch onto the point in the composite curve where the left end of the straight line meets the tangent arc. The sketch should be fully defined. 52. Extrude the sketch 130 mm. Click on the Reverse button for Direction1. 183

190 Topic 4 Final Project Multibody Parts of the Mountain Board You will later cut away the extra material. For now you need to make sure the extrusion will extend past the end of your Binding Base Plate. 53. Click Insert, Pattern/Mirror, Curve Driven Pattern. 54. Select CompCurve1 in the FeatureManager design tree for the direction. Enter 34 for the number of instances and 5.5 mm for the spacing. Select Tangent to curve for the Alignment method. 55. Click OK. 56. Click Insert, Pattern/Mirror, Curve Driven Pattern. 57. Select CompCurve1 in the FeatureManager design tree for the direction and Extrude1 for the Feature to Pattern. Enter 8 for the number of instances and 5.5 mm for the spacing. Select Tangent to curve for the Alignment method. Click on the Reverse button to fill in the pattern to the left. 58. Click OK. This is the full pad, ready to be trimmed. 59. Return to the Binding assembly. 60. Because the Binding Pad is different from when you left the Binding assembly, the assembly needs to be rebuilt. Click Yes. 61. The Binding Pad should completely cover the top of the Binding Base Plate. 184

191 Topic 4 Final Project Multibody Parts of the Mountain Board 62. The only part you need to use to trim the Binding Pad is the Binding Base Plate. Hide all the other parts. 63. Reorient the model to the Bottom view. 64. Create a sketch on the bottom face of the pad. Select the edge of the hole in the Binding Base Plate. 65. Click Offset Entities and create an offset 5 mm to the outside of the hole. 66. Create an Extruded Cut using the end condition Through All. Click OK. 67. Create another sketch on the bottom face of the Binding Pad. 68. Create a sketch on the bottom face of the Binding Pad that is offset 2 mm from the edges of Binding Base Plate. 69. Extrude a cut Through All. You want to cut away everything that is outside the sketch so remember to check Flip side to cut. 185

192 Topic 4 Final Project Multibody Parts of the Mountain Board 70. Return to the Binding assembly. Click to exit Edit Part. 71. Show all the parts. 72. Save and Print the assembly. 73. This completes the Binding assembly. 74. Exit SolidWorks. Click on the Forward arrow to resume the activity. 186

193 Topic 5 Final Project Final Assembly TOPIC 5 FINAL PROJECT FINAL ASSEMBLY Objective When you have completed this topic, you will have the skills and knowledge to successfully assemble all the parts you have created for your final project into the finished mountain board. You will also create an assembly drawing of the mountain board and present the results of your designs in a realistic manner. Overview Very few of the parts designed by engineers are used by themselves. Most become part of an assembly that may then become part of a larger assembly. This is true with the final project you designed. Of all the parts you created, most are part of a subassembly that will be part of a final assembly. Three of the sub-assemblies have already been created, the Wheel Assembly, the Spring Assembly, and the Binding. You will put together the remaining subassemblies, and then create the final assembly. The final assembly will start with the Deck as it forms the foundation of the Mountain board. The final assembly should be created in an order similar to the order that will be used to assembly the actual final product. During the product design process, there are numerous requirements for output of the design details. Engineers and designers must share information and work together to satisfy the design intent. Drawings are required for the manufacture of the product. Pictures are needed for brochures and web pages to market the product. Because of this, screen prints, photorealistic prints, drawings, and image files are a must during the design process and when presenting the final results of your project. In this topic, you will complete your mountain board and create realistic models of the parts and final project. 187

194 Topic 5 Final Project Final Assembly Activity 1 Final Assembly Objective When you have completed this activity, you will have the knowledge and skills to create the assembly of all the parts you have designed to complete your final project. You will be able to: create an entire axle assembly using the completed truck, axle, wheel assembly, and spring assembly. put together all the sub-assemblies that make up the wheel assemblies. add the wheel assemblies and bindings to the deck to complete the mountain board. create an assembly drawing. Activity Directions: Final Assembly SolidWorks should be on your screen. If not, click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. Create the Axle Assembly 1. Click File, Open. Navigate to the C:\Mountain Board Training Templates. Select All Files for Files of Type. Double-click Assembly_MM template. 2. Click Insert Component and browse to locate your part, Axle your last name in the C:\Mountain Board folder. (Select Assembly for Save As Type.) 3. When the preview image appears with your cursor, move the cursor over the assembly origin until the icon appears, then click the origin. 4. Save the new file in the C:\Mountain Board folder as Axle Assembly your last name. Select Assembly for Files of Type. 5. Click Insert Component on the Assembly toolbar. 6. Click Browse and locate the part Axle Shaft in the C\Mountain Board Parts Library folder. 188

195 Topic 5 Final Project Final Assembly 7. Drop the part into the assembly. You will now add a Concentric mate: 8. Click on the cylindrical edge of the Axle Shaft. 9. Rotate the axle so you can select the inner back face. Hold the Ctrl key to select both. 10. Select Mate from the Assembly toolbar and click OK. 11. Hold down the Ctrl key and drag another copy of the Axle Shaft from the FeatureManager design tree into the graphics area. This will insert another instance of the Axle Shaft part into the assembly. 189

196 Topic 5 Final Project Final Assembly 12. Apply the same mates to this shaft. In the Coincident window, select Aligned under Mate Alignment. 13. Open the part King Pin Sleeve from the C\Mountain Board Parts Library folder. 14. Tile the two windows vertically by clicking Windows, Tile Vertically from the menu. 15. Drag the edge of the King Pin Sleeve shown to the edge of the Axle indicated. 16. When you are on the correct edge the cursor will change to the Pin in Hole. 17. Press the Tab key to reverse the orientation of the mates. When the cursor shows the Pin in Hole and the orientation is correct, drop the King Pin Sleeve. It will receive both a Concentric and Coincident mate. 18. Finish the assembly by adding two Socket Set Screws. These set screws are used to keep the axle Shafts from backing out of the axle. The set screws 190

197 Topic 5 Final Project Final Assembly are located in the C\Mountain Board Parts Library folder as Socket Set Screw Cup Point_AM. 19. Mate each set screw using one Concentric and one Coincident mate. 20. Save and Print the assembly. Close All windows. Create the Truck Assembly 1. Click File, Open from the menu and select the Assembly_MM template in the C:\Mountain Board Training Templates folder. 2. Click Insert Component, Browse and locate the part Truck your last name in the C:\Mountain Board folder. 3. When the preview image appears with your cursor, move the cursor over the assembly origin until the pointer appears, then click the origin. 4. Save the new file as Truck Assembly your last name in the C:\Mountain Board folder. 5. Click Insert Component on the Assembly toolbar. 6. Click Browse and locate the part 8mm Threaded Insert in the C\Mountain Board Parts Library folder. Drop the part into the assembly. 191

198 Topic 5 Final Project Final Assembly 7. These inserts will actually be molded into the Truck, so there will be an exact fit. You need three coincident mates to position the insert. 8. Mate the Insert to the Truck with three Coincident mates. Mate two adjacent faces on the insert to two adjacent faces on the Truck. The third mate will be between the top of the Insert and the top face of the Truck. NOTE: Select each mating surface one at a time after selecting Mate from the toolbar. Insert three more instances of the 8mm Threaded Insert into the assembly and mate them to the three remaining hex holes. Add Mate References to the Truck bearing. 9. Open the part Bearing from the C\Mountain Board Parts Library folder. 192

199 Topic 5 Final Project Final Assembly 10. Drag a Bearing from the C\Mountain Board Parts Library by selecting Window, Tile Vertically. Select the outer front edge of the bearing and the outer edge of the bearing hole in the Truck. The Bearing will snap into position and both a Coincident and Concentric mate will be created. If the Bearing is sticking out of the hole, press the Tab key to reverse the alignment. 11. After you have placed the first Bearing, add a second bearing to the other side of the Truck. 12. Save and Print the assembly. You now have all the sub-assemblies for the mountainboard. You will first put together all the sub-assemblies that make up the wheel assemblies. Then you will add the wheel assemblies and bindings to the deck to complete the mountainboard. 13. Create a new assembly using the Assembly_MM.asmdot template. 14. If your Axle Assembly is not open, click Insert Component, Browse and locate the Axle Assembly your last name in C:\Mountain Board folder. 15. Drop the Axle Assembly on the origin of the new assembly. 16. Save the new assembly to the C:\Mountain Board folder as Truck_Axle_Wheel your last name.sldasm. 17. Insert two instances of the spring assembly in the Truck_Axle_Wheel assembly. 193

200 Topic 5 Final Project Final Assembly 18. Mate each of the Spring Assemblies to the outer holes in the Axle. The end of the Spring Assembly with the Fender Washer should be up. This is done by selecting Insert Components and then Browse to the Spring Assemblies. 19. Drag the Truck Assembly into the Truck_Axle_Wheel assembly. Select the Truck in the FeatureManager design tree to highlight it and then select Rotate Component from the Assembly toolbar. Select Free Drag under Rotate and place it in position. 20. Add a Concentric mate between the hole in the Bearing and the King Pin Sleeve. 21. Add a Coincident mate between the two faces shown to position the axle the Truck. 22. Add a Parallel mate between the two faces shown. 194

201 Topic 5 Final Project Final Assembly Add the Remaining Hardware 1. Add the King Pin and the B M Hex flange nut (located in the C\Mountain Board Parts Library folder) to the assembly. Select B18.3.3M- 10x80 SHSS--N for the King Pin configuration. 2. Add, from the Toolbox in the Design Library (on the right side of screen), two B18.3.5M -4x0.7x10 Socket FCHS-10N screws to hold the bottom of the spring assemblies to the axle. Click OK to accept default settings. 3. Open the part Adjusting Screw from the C\Mountain Board Parts Library folder. Drag two instances of the Simplified configuration of the Adjusting Screw into the Truck_Axle_Wheel assembly. 195

202 Topic 5 Final Project Final Assembly 4. Mate each Adjusting Screw with a Concentric and Distance mate as shown. 5. Set the distance mate to 10 mm. Add the Wheel Assembly To complete this assembly, you only need to add two wheel assemblies and a lock nut on each axle shaft. 6. Click Insert, Component, Existing Part/Assembly from the menu. 7. Click Browse and locate the Wheel Assembly your last name in the C:\Mountain Board folder. Insert two instances of the Wheel Assembly into the Truck_Axle_Wheel assembly. 8. You will need two mates to position each of the wheel assemblies. Add a Concentric mate between the inside face of one of the wheel bearings and the cylindrical face of the Axle Shaft. *Note: Make sure that the valve stems are facing out. 9. The Axle Shaft has a step face. When assembled, the wheel is pushed onto the shaft until the face of the bearing is stopped by the step. 196

203 Topic 5 Final Project Final Assembly 10. Add a Coincident mate between this stepped face and the side of the bearing. TIP: To select the stepped face, you will have to zoom in close as the face is only.5 mm wide. 11. Finish the assembly by adding a B MHex jam nut, M10 x 1.5 to each axle Shaft to hold on the wheels. You need to select this jam nut from the Toolbox in the Design Library (right side of screen). Select ANSI, Metric, Hex Jam Nut. In the dialog box, change the size to M Save and Print the assembly. 197

204 Topic 5 Final Project Final Assembly Add the Bindings to the Deck You only created one binding for the left foot. You could make a right footed version of each part individually, or you can create all the right handed parts in a single operation in the assembly. 1. Create a new assembly using the Assembly_MM template. 2. Insert the Deck part and Mate it to the origin. 3. Save the assembly as Mountainboard your last name.sldasm in the C:\Mountain Board folder. This will be your top level assembly. 4. Click Insert Components and then Browse. Locate your Binding assembly in the C:\Mountain Board folder and click Open. 5. Drop the Binding assembly into the Mountainboard assembly. There are no SmartMates, so you can place the Binding anywhere. 6. Add a Coincident mate between the bottom of the Binding Anchor and the planar face where the binding will rest. 7. Add a Coincident mate between the Front plane of the Deck and the Right plane of the Binding Anchor. You will have to expand the tree in the Drawing area to select the planes. You may have to switch the mate alignment to match the view below. 198

205 Topic 5 Final Project Final Assembly 8. Add a Tangent mate between the back end surface of one of the racetrack shaped holes in the Binding Anchor and the appropriate mounting hole in the Deck. 9. Switch between Aligned and Anti-Aligned to center the slot over the hole. Insert a Mirrored Binding 10. The second binding will be a mirror image of the first binding. Some of the parts will need to be mirrored, others will not. 11. Click Insert, Mirror Components from the menu. 12. Select the Right plane of the Deck as the Mirror plane. 199

206 Topic 5 Final Project Final Assembly 13. Select the Binding Assembly in the fly-out FeatureManager design tree for the Components to Mirror. 14. Select the following components in the Components to Mirror box: Binding Assembly Binding Base Plate Strap Assembly Strap_right Strap_left Foam_Pad Binding Pad 15. Select Recreate mates to new components located at the bottom of the Mirror Components window to the left of the screen. Click the Next arrow. 16. The mirrored components are new parts that must be named. The default is to add Mirror as a prefix to the existing file names so that the mirrored assembly of Binding will be MirrorBinding. 17. Click Next. 18. If you need to reorient components, you can do it now. Select Preview mirrored components and Preview instanced components at the bottom of the Mirror Components window to see the preview of the new assembly. 19. Click OK. 20. A List of Mates dialog box appears stating that some of the mates could not be created automatically. You will have to fix this manually. Click OK. 21. The mirrored binding has been created. The new binding is not mated to the Deck, so you will have to do it manually. 200

207 Topic 5 Final Project Final Assembly 22. Add the three mates between the Binding Anchor and the Deck that were used to mate the original Binding. Add the Wheel Assemblies The last major assembly to be added will be the wheel assemblies. 23. Insert one instance of the Truck_Axle_Wheel assembly into the Mountainboard assembly. 24. Mate the top face of the Truck to the mounting face on the bottom of the Deck with a Coincident mate as shown. 25. Add Concentric mates between the two holes in the Truck and the corresponding holes in the Deck. Make sure the Truck is oriented so that the rounded face is near the end of the Deck. *Note: If you get a mate error when adding the second Concentric mate, check the positioning dimensions of the holes both the Deck and the Truck. They must be exactly the same or the two Concentric mates will fight for control. 201

208 Topic 5 Final Project Final Assembly 26. Add another instance of the Truck_Axle_Wheel assembly to the Mountainboard assembly and mate it to the other end of the Deck. 27. Save and Print the assembly. Add fasteners The only remaining tasks to complete the assembly are to add the fasteners that hold the Bindings and Trucks to the Deck. 1. Open the part Tee_Nut from the C:\Mountain Board Parts Library folder. 2. Drag four instances of the Tee_nut into the assembly. 3. Using SmartMates, drag the edge shown, while holding down the Alt key, into the proper hole. Use the Tab key to reverse the direction of the Tee_nut so that the shaft goes into the hole. 4. Reorient the model so you can see the tops of the four Tee_nuts. *Note: It will be easier to insert the screws in the next step if you hide the Binding Strap assembly. 5. Click the pushpin in the Design Library to keep it open. Expand Toolbox, then Ansi Inch, then Bolts and Screws by clicking the plus sign next to each. Select Machine Screws. 202

209 Topic 5 Final Project Final Assembly 6. Hold down the Ctrl key and select the top circular edge of each of the four Tee_nuts. In the lower pane of the Design Library, right-click the Truss Head Screw and select Insert Into Assembly. 7. Select: Size - 1/4-20 Length Drive Type - Cross Thread Length Thread Display - Simplified 8. Click OK. All four Truss Head Screws will be inserted. 203

210 Topic 5 Final Project Final Assembly 9. Add Tee_nuts and Truss Head Screws to the other MirrorBinding. *Note: When you insert the Truss Head Screws you will be asked if you would like to create new copies or to use the existing copies of the parts, use the existing parts. 10. Use Toolbox to add 8-32 x inch Truss Head Screws and 8 32 Machine Screw Nut Hex to the eight locations to hold the Truck to the Deck. 11. Save and Print the assembly. 12. Create a Drawing of the Mountainboard on a B-size sheet. Include an assembled view. 13. Insert the B-size printer paper into the printer and Print the drawing. 14. Save and Close all open documents. 15. Exit SolidWorks. Click on the Forward arrow to resume the activity 204

211 Topic 5 Final Project Final Assembly Activity 2 Presenting the Results Objective When you have completed this activity, you will have the knowledge and skills to display your model as the built part would appear if it existed. You will add material, lighting, decals, and scenery and output your results to the printer. You will be able to: demonstrate advanced features in PhotoWorks. create a photorealistic rendering of your model. apply decals, lighting, and scenery to your model. Activity Directions: Final Rendering SolidWorks should be on your screen. If not, click on the Application Launch button and choose SolidWorks from the menu. Follow the directions below to complete the activity. Use the Render Wizard 1. Open your part Axle your last name from the C:\Mountain Board folder. 2. Orient the model to the Isometric view. 3. Activate PhotoWork by clicking Tools, Add-Ins from the Main menu. Check PhotoWorks. Click OK from the Add-Ins box 4. Click PhotoWorks, Render Wizard. The Render Wizard lists three basic steps to create the first rendering: Apply material Select a scene Render the image 5. Click Next. Select an appearance. The wizard instructs you to choose an appearance from the Appearances Editor. The Appearances Editor will open in the PropertyManager and the Task Pane will open to the Appearances/PhotoWorks tab. Appearances affect the way a surface reacts to light. They may be applied to parts, features or faces. Appearances are of two general types, Procedural and Textures. 6. To apply material to the part, click PhotoWorks, Appearance. 205

212 Topic 5 Final Project Final Assembly 7. The Appearnace/PhotoWorks Pane lists all the materials that are available to be applied to the model. 8. Click the plus sign to the left of the Metal folder, and then select the sub-folder Aluminum. 9. In the material selection area, located polished aluminum. Drag the material polished aluminum into the graphics area. This applies the material to the entire part. Click OK. 10. Click Next in the Wizard. Select a scene The next task is to apply a scene. The Scene Editor opens in its own window. PhotoWorks scenes are made up of the things you see in the rendering that are not the model. They can be thought of as a virtual box or sphere around the model. Scenes are composed of backgrounds, foreground effects, and scenery. 11. To select a scene, click the plus sign next to the Presentation Scenes folder. 12. Select the scene Factory Background. 206

213 Topic 5 Final Project Final Assembly 13. Click Apply. 14. Click Next on the Render Wizard. Render The final instruction summarizes the process. The Render Wizard will close the Scene Editor and render the model. 15. Click Finish to close the Render Wizard. 16. The Axle will be rendered. Examine the rendering; you should be able to see the reflections of the holes on the flat surfaces of the model. 17. The Render Wizard led you through the steps to add material and a scene to the model, but it didn t change the default lighting. You can improve the rendering by adding some additional light. 18. Proper lighting can greatly enhance the quality of the rendering. The same principles used by photographers work well in PhotoWorks. Add a Fill Light The default lighting has only one Directional light. As you are looking at the computer monitor, the default light is coming in over your left shoulder. You will add a second directional light over your right shoulder, and then adjust the intensity of the two lights. 19. The model will only stay rendered if it is not moved. To clear the rendering, move the model, then change the view back to Isometric. 20. In the FeatureManager design tree, right-click the Lights, Cameras and Scene folder and select Show Lights. 21. Double-click light Directional2. Enter deg for Longitude, and 6.12 deg for Latitude for the Light Position. Click OK. 22. Adjust the brightness to Click Render on the PhotoWorks toolbar. 24. Save the Axle. You will now print the Axle using the printer paper (small). 25. Select Tools, Options, and then click on the Document Properties. Select Unit, Unit System. Click the MMGS Radio button and then click OK. 207

214 Topic 5 Final Project Final Assembly 26. Click PhotoWorks, Page Setup. The PhotoWorks Page Setup allows you to size and position the image that will be printed. 27. Select Landscape orientation. 28. Make sure Fixed aspect ratio is selected so you do not distort the image when you change its size. 29. Select Center. This will automatically center the image on the printed page. 30. Type 200 mm for the Width, the Height will automatically adjust to a value of around 170 mm to maintain the aspect ratio. 31. The actual value of the height is determined by the proportions of your graphics area. 32. Clear Use rendered image quality for printing. The rendered image on your screen is only 72 or 96 dpi (dots per inch), if you use this quality for your print, it will be very grainy. 33. Adjust the Quality slider to 300 dpi. Click OK. 34. Click PhotoWorks, Print to render the image and send it to the printer. Note that this will take much longer than when you render to the screen. 35. Close the Axle. Texture Materials Texture materials are like elastic wallpaper. They are applied to the outside of the model. They can be stretched and rotated to completely cover all the surfaces. You will add a texture material to the Deck, and then customize it. 1. Open the part Deck your last name from the C:\Mountain Board folder. 2. Click Appearance on the PhotoWorks toolbar. 3. Select the appearance carbon fiber dyneema plain in the plastics, composite folder. Hodl the Alt key and drag the appearance into the graphics area. 4. Click OK. 208

215 Topic 5 Final Project Final Assembly 5. Click Apply and Close. 6. Render the model. This is more interesting, but maybe not what you are looking for. Examine the other materials in the Appearance Editor to see if there is something better than this pattern. Decals 7. Decals are separate files, just like texture materials. They are made with essentially the same procedure used to create texture materials. 8. Click New Decal on the PhotoWorks toolbar. The Decal Editor opens. 9. Under Image file path, click Browse. 10. Navigate to the C:\Mountain Board Parts Library\Decal Images folder. Select the file SolidWorks.jpg, and then click Open. 11. Click Save Decal. Save the decal file as SolidWorks your last name.p2d to the C:\Mountain Board folder. Click Save. 12. Click Yes to have PhotoWorks open the Decals folder in the Decal Editor. 13. The Decal Editor will show the image. In the graphics area, zoom in on the area shown and select the face indicated. 14. The Preview shows the decal on the selected face. Select the Mapping tab in the Decal Editor. 15. Notice that the colors used in the Preview correspond to the color shown in the Mapping tab indicating: Width - Blue Height - Magenta 209

216 Topic 5 Final Project Final Assembly Offset Horizontal - Red Offset Vertical - Green 16. Make sure Fixed aspect ratio is selected. Enter deg for Rotation Angle. Press Enter. 17. The preview will show that the decal has been rotated to the correct orientation. 18. Adjust the size and position of the decal by entering the following values. Watch the preview as you enter the values. Horizontal Location: 10 mm Width: 50 mm 19. Click OK. Render the model. The decal is located and sized correctly. Now let s use only the black ellipse and the image inside of it. To remove the image outside of the ellipse, you will use a mask. 20. Right-click the decal in the RenderManager and select Edit. 21. Select the Image tab. Select Image mask file. Click Browse and locate the file SolidWorks-mask.jpg in the C:\Mountain Board Parts Library\Decal Images folder. The image mask is a black and while image that will be overlaid on the decal image. Where the mask is white, the decal will show through. Where the mask is black, the decal will not show. The Resulting image shows that all the area with the pink and white cross hatch will be masked out. Only the black ellipse and the image inside of it will be placed on your model. 22. Click OK. 23. Render the model. The tan area has now been masked out leaving only the ellipse and the image inside. The decal is a little dull as it takes on the reflective properties of the material on which it is applied. 24. In the RenderManager, right-click the decal SolidWorks and select Edit. 25. Select the Illumination tab. 210

217 Topic 5 Final Project Final Assembly 26. For Material type, select Constant from the list. Click OK. 27. Render the model. The decal now stands out as its reflective characteristics are now different from the Deck. 28. Save and Close the Deck. Adding Materials to Assembly Components You will add materials to all the remaining components of the mountain board. Add materials to the Spring Assembly 1. Open the Spring Assembly your last name from the C:\Mountain Board folder. 2. In the FeatureManager design tree select the part Spring. 3. Click Material on the PhotoWorks toolbar. 4. Apply the material chromium plate from the metals, chrome folder. 5. Use the same procedure to apply the other materials to the parts in this assembly: Fender Washer - metal, steel, brushed steel Spring Dampener - plastics, high gloss, white high gloss plastic (change color to yellow) Spring Retainer - plastics, high gloss, white high gloss plastic (change color to black) *Note: You can apply the material to one Spring Retainer, then select the second Spring Retainer, right-click the material and select Attach to Selection. 6. Render the model. 7. Click Scene on the PhotoWorks toolbar. 8. Select the Studio Scenes folder and the Light Cards studio. Click Apply and Close. 9. Change the view to Trimetric by clicking Trimetric on the Standard Views toolbar. 10. Render the model. Save and Close the Spring Assembly. Add materials to the Wheel Assembly 211

218 Topic 5 Final Project Final Assembly 11. Open the Wheel Assembly. 12. Apply the following materials: Tire rubber, matte, matte rubber Bearings, nuts and bolts - metals, steel, stainless steel 13. Open the Wheel Hub in its own window by right-clicking the Wheel Hub in either the graphics area or FeatureManager design tree and selecting Open Part. 14. Apply the appearance polished plastic1 from the plastics, high gloss folder to the entire part. The default color should be gray. 15. In the FeatureManager design tree select the two features Text and CirPattern Add the material polished plastic1. Select the Color/Image tab and change the color to red. 17. Render the part to check your work. 18. Save the part. Return to the Wheel Assembly by clicking Window and selecting Wheel Assembly from the list. 19. Open the Inner Tube in its own window. Zoom in on the valve stem and cap area. 20. Select the three yellow surfaces shown. 21. Apply the appearance polished brass from the metals, brass folder. 22. Select all the visible faces of the valve stem cap. 23. Apply the material polished plastic1 from the plastics, high gloss folder. 24. Change the color to black. 212

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