Product Modelling in Solid Works

Size: px
Start display at page:

Download "Product Modelling in Solid Works"

Transcription

1 Product Modelling in Solid Works In the following exercise you will use solid works to construct the computer mouse shown opposite. In this exercise you will use a number of advanced features to achieve the complex shape shown. You will also reference the surfaces of other components in order to shape the component being modelled. Modelling the top surface The part has a contoured top surface. Before modelling any Solid geometry we will first construct this top surface. This surface will be created as a lofted construction surface passing through 3 arcs. First you will construct 3 planes. The 3 arcs will then be constructed; one on each plane, then finally a lofted construction surface will be constructed between these arcs. Using the front plane as the basis, construct 3 parallel planes to the left and right at the distances specified Plane 1: 50mm to the left Plane 2: 30mm to the right Plane 3: 80mm to the right On each plane draw arcs as follows On plane 1 construct an arc of radius 72mm with its centre on the vertical plane and 70mm below the horizontal plane or origin. Ensure the arc extends approximately 40mm to the left and right. 19/03/2013 1

2 On plane 2 and draw an arc of radius 45mm with a centre 20mm below the horizontal plane. (again extending 40mm to left and right) Finally on plane 3: draw an arc with a radius of 60mm whose centre is 50mm below the horizontal plane. Create a lofted construction surface through these curves. To do this, activate the Surfaces toolbar and then select lofted surface. This surface will later be used to define the upper top profile of the mouse. Creating the master shape. In the next step you will create the overall outline of the mouse, extrude it downward to form the base and upward to form the top. (the horizontal 60mm dimension is the dimension to corners prior to application of the 1mm fillets) First of all working on the top plane create the sketch shown opposite to define the perimeter of the mouse. Once complete select extrude. For direction 1 specify the Up To Surface option and select the lofted construction surface already created. In addition activate the draft option and specify and angle of 5 degrees. For direction 2, specify blind, a distance of 5mm and a draft angle of 8 degrees. 19/03/2013 2

3 Add a 3mm fillet to the bottom edge and a 5mm fillet to the top curved edge. This is the master which defines the overall shape of the mouse. Save the part as MASTER.SLDPRT rename the part under the name master. Splitting the mouse New we will split the mouse into two separate parts, base and top. We will then continue to add further design detail to complete both components. Working on the right hand plane, create a sketch, and draw a line level with the split line (or convert entities). Stretch the end points of this line past both ends of the mouse. Finally create an extruded construction surface, again ensuring that the construction surfaces stretches past the edges of the mouse in all directions. Select Insert Features Split from the pull down menu.. With the Trim Tools section highlighted select the extruded surface just created. Then select the [Cut Part] button. Selecting this button results in two unnamed items appearing under Resulting Bodies. Select both check boxes to indicate that you wish to keep both halves. You are now ready to save these solid bodies as separate parts. To do so expand the solid bodies folder. Now, right click on the solid body representing the base and choose insert into new part Specify the name base.sldprt. Repeat again for the top part specifying the name top.sldprt. This creates two stand alone parts which are linked back to the original master model. 19/03/2013 3

4 Modelling base detail You will now add further design detail to the base. This will include: Hollowing out to a uniform wall thickness of 2mm. Adding a lip detail around the component edges. Add bosses and counter-bored screw holes to facilitate the screws which will be used to hold the mouse together. Shelling First of all shell or thin wall the base. Specify a thickness of 2mm and select the top (split surface) as the opening or face to remove. Modelling lip detail Next we will add a lip detail around the edge. The purpose of this is to help locate both halves. Another purpose is to ensure that should a gap develop due to warpage, it will not be possible to see through the gap. This lip will be achieved by sweeping rectangular (cross section) around the inside edge (path/ drive curve). Select under Options to ensure the path (and resulting lip) follows all the way around. To do this construct a reference plane normal to the inside edge using the normal to curve feature. Then create a sketch 1mm wide by 1.5mm high. This sketch should lie between the inside and the middle of the wall thickness. Finally select Swept Extrusion the lip detail. to create Modelling bosses and screw holes Next create the bosses. These will be created by selecting the inside bottom surface and creating 3 sketches according to the dimensions shown. Use appropriate sketch relations or construction geometry to ensure that the circles are fully defined. On completing of the sketch extrude upwards by 8mm. 19/03/2013 4

5 Drafting bosses To facilitate easy removal from the injection moulding tool all vertical faces must have a taper or draft applied to them. Therefore it is necessary to draft to bosses. In this case we will apply a draft of 3 degrees to all the bosses. To draft the bosses select the draft tool form the features toolbar (or select insert features draft) For the type of draft select Neutral Plane. Specify a draft angle of 3 degrees. For the neutral plane, select the top face and for the faces to draft select the side walls. Repeat for all three bosses and finish with 1mm fillets at the base. Adding counter bores Finally add holes to accommodate the screws which will hold the mouse together. As the screws will be inserted from below counterbored holes will be required to accommodate the heads of the screw. The screw which will be used will be M4 Panhead screws (ISO 7045). This will be created later using the toolbox. To accommodate the M4 pan-head screw counterbores will be inserted from below. Working from the underside, create 3 counterbored holes. N.B. Remember to select the face first before selecting the hole wizard command. Specify the standard, type etc shown opposite. Ensure that each hole is located centrally with respect to each boss by applying the appropriate relations. If it seems that you cannot select a specific edge in order to apply a relation to, you may that by rotating the view you may be able to select it from the other side. The boss with clipping applied looks as shown below left. The completed base looks as shown on the right. 19/03/2013 5

6 Modelling Top detail You will now add further design detail to TOP.SLDPRT. This will include: Hollowing out to a uniform wall thickness of 2mm. Adding a lip detail around the component edges. Adding the bosses and threaded screw holes to receive the screws already mentioned. Adding cut-outs to accommodate the mouse buttons. Some of these details will be added now prior to assembly. Other detail will be added later after assembly enabling us to pick up on feature of other components. Open the part called TOP. SLDPRT. N.B. For clarity images will be shown with clipping plane active. Shelling Next using the shell command hollow out the part to a uniform wall thickness of 2mm. Adding lip detail In the next step you will add the lip detail. However as material was added when creating the lip on the base material will need to be taken away for this lip. This will therefore be done using a swept cut. Otherwise the procedure is the same. N.B. Because of the inside wall you will need to make a slightly larger cross section sketch to ensure that all material is removed. 19/03/2013 6

7 Adding the cut-outs for the buttons Working on the top plane, create the sketch shown opposite for the button cutouts. For the curved lines which follow the outer shape use the offset command to offset the outermost edge inwards by 5mm. Add remaining vertical lines and dimension as appropriate. Add the horizontal line and dimension so that it is 40mm from the origin or front plane. Finally trim as required to produce 3 discrete contours. When complete create an extrude cut using the through all option. Finally fillet all remaining sharp corners with a radius of 3mm. Draft edges of holes Again we need to draft vertical edges. In this case we want to maintain the lower of the hole while drafting the vertical faces outward. For this we need to use the Parting line option. For the angle specify and angle of 3 degrees. For the direction of pull select the top plane. For parting lines select the lower edge of the button openings. With face propagation set to tangent Solid Works will select the lower edge of the entire opening. Choose accept to apply the tangent. Repeat for the other two holes. For the remaining detail we will need the help of the base. For this reason we will need to assemble the mouse before we can model the next feature. 19/03/2013 7

8 Assembling the mouse Create a new assembly and insert the base component locating it at the origin by choosing accept. Next insert the top component, again choosing accept. This will insert the components at the origin will all degrees of freedom constrained. This will be denoted by the letter (f) beside the component in the feature manager. Save the assembly as mouse.sldasm. Creating an empty part within the Assy You are now ready to model the buttons. Rather than modelling separately and then inserting into the assembly, this will be designed in position or in place. This will allow us to utilise the edges of existing geometry. In this case the to hole cutouts. To design in place: Select: Insert Component New part Select the front plane in the assembly to position this new part within the assembly. Right click on the randomly named new part in the feature manager and select Rename Part. Specify the name BUTTONS. It is possible for the geometric information defining the buttons to be held within the assembly or to exist as a stand alone part file (which is usually the case). To create a stand alone Buttons part file right click on the component and select: Save Part (in External File) In the dialog which appears select the buttons File and select Same As Assembly followed by OK. This will save the BUTTONS.SLDPRT in the same folder as the other components. 19/03/2013 8

9 Creating the button geometry In order to create the button geometry you must first open the BUTTON part within the assembly. This is achieved by selecting the component in question, and then selecting the Edit Part Icon shown. Selecting the top plane open a new sketch and view normal to. Then using the CTRL key select all of the edges of one of the button openings, then select convert entities to convert in lines in the current sketch. N.B. Ensure that you select the lower rather than the upper edge. You may need to rotate the view to ensure that you get the correct edge. Repeat again for the remaining two holes. Once the sketch is complete, orientate the assembly as shown below and then select feature extrude. Change the default end condition for Blind to Offset from Surface. (This will allow you to create the buttons a specified distance above a specified surface). To specify the reference surface, activate the box and select the top surface of the mouse. In the next specify an offset distance of 1.00mm. As this offset may be above or below the surface. You may need to select to reverse the offset. The surface buttons should now look as shown protruding 1mm above the surrounding surface. N.B. Should you find difficulty with this approach an alternative approach is suggested on the next page. 19/03/2013 9

10 Alternative approach Using the offset from surface option has been a recurring problem, whereby SolidWorks will not offset upwards despite repeated attempts to do so. Should you find that this is the case you may perform the action in two steps: Extruding up to surface Offset the surface an additional 1 millimetre. To do this select, Face, Move from the Insert menu. Under the move face menu select Offset and specify a distance of 1mm. This will offset the selected surface by the specified amount stretching all attached face to maintain the integrity of the solid model. Creating the button rim You will now create a rim around the buttons to prevent them pushing though the opening in the TOP housing. To do this we will offset the button edges outward and then extrude upward until they touch the underside of the top component. While still in button editing mode, select the top plane and start a sketch. Viewing vertically downwards (normal to plane) offset the edges of the buttons outwards by 1mm. When complete, issue the extrude command. This time select the up to surface option. To select the surface, right mouse click on the top surface of the main part, choose select other and pick the underside surface. The buttons should now look as shown. 19/03/

11 Finishing the buttons We will now finish the buttons in stand alone mode. Return to assembly by clicking the assembly item at the top of the feature manager and choose Edit Assembly. Next open the buttons in stand alone mode using open part. Working on the top plane, create a sketch and draw a rectangle around the buttons. Then create an extruded cut up to 3mm below the ledge using the offset from surface option. Shelling the buttons The buttons are still quite bulky and would therefore take some time to cool after injection moulding. It is therefore necessary to thinwall or shell the components. Shelling will also reduce the quantity of material required. Shell the buttons using a wall thickness of 2mm. You can only shell one solid body at a time. As the buttons consists of three separate solid bodies you will need to shell one button at a time. Add a 3 degree draft to the upper vertical surface on the button and finish with a 0.5mm fillet to remove the sharp edge. Top component details Return to the top component and add bosses and screw holes to match with those in the base. Adding the screws To complete the mouse add three M4 x 12 Pan Head screws (ISO 7045). These will be created using the Solid Works Toolbox. To define the screws select: ISO, Bolts and screws Cross recessed screws Finally save in the current/working folder. 19/03/

12 Finish and Drafting Mouse Finally, draft the mouse creating the following: Orthographic views plan, elevation and end views. Section views and detail views Regular Isometric and exploded Isometric views Balloon references and parts list. Ensure that the standard IT-Sligo template is used for these drawings. Shown below are illustrations of each view types Orthographic views: Plan, Elevation and End views. Sections Section views should be used to show internal detail more clearly. Detail views: Create detail views of areas with small detail. E.g. seating area between buttons and top. the split line/lip detail the screw hole detail Detail views are created using: Pictorial views: Isometric and exploded views. 19/03/

Ball Valve Assembly. On completion of the assembly, we will create the exploded view as shown on the right.

Ball Valve Assembly. On completion of the assembly, we will create the exploded view as shown on the right. Ball Valve Assembly Supplied are the main components of a ball valve. In this exercise you will assemble the valve as shown below Left. (N.B. Socket head cap screws are not supplied these will be created

More information

Engineering Technology

Engineering Technology Engineering Technology Introduction to Parametric Modelling Engineering Technology 1 See Saw Exercise Part 1 Base Commands used New Part This lesson includes Sketching, Extruded Boss/Base, Hole Wizard,

More information

SolidWorks 95 User s Guide

SolidWorks 95 User s Guide SolidWorks 95 User s Guide Disclaimer: The following User Guide was extracted from SolidWorks 95 Help files and was not originally distributed in this format. All content 1995, SolidWorks Corporation Contents

More information

SOLIDWORKS 2016 Basic Tools

SOLIDWORKS 2016 Basic Tools SOLIDWORKS 2016 Basic Tools Getting Started with Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

More information

SolidWorks Part I - Basic Tools SDC. Includes. Parts, Assemblies and Drawings. Paul Tran CSWE, CSWI

SolidWorks Part I - Basic Tools SDC. Includes. Parts, Assemblies and Drawings. Paul Tran CSWE, CSWI SolidWorks 2015 Part I - Basic Tools Includes CSWA Preparation Material Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered

More information

Engineering & Computer Graphics Workbook Using SolidWorks 2014

Engineering & Computer Graphics Workbook Using SolidWorks 2014 Engineering & Computer Graphics Workbook Using SolidWorks 2014 Ronald E. Barr Thomas J. Krueger Davor Juricic SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

More information

AEROPLANE. Create a New Folder in your chosen location called Aeroplane. The four parts that make up the project will be saved here.

AEROPLANE. Create a New Folder in your chosen location called Aeroplane. The four parts that make up the project will be saved here. AEROPLANE Prerequisite Knowledge Previous knowledge of the following commands is required to complete this lesson. Sketching (Line, Rectangle, Arc, Add Relations, Dimensioning), Extrude, Assemblies and

More information

Digital Camera Exercise

Digital Camera Exercise Commands Used New Part This lesson includes Sketching, Extruded Boss/Base, Extruded Cut, Fillet, Chamfer and Text. Click File, New on the standard toolbar. Select Part from the New SolidWorks Document

More information

Engineering & Computer Graphics Workbook Using SOLIDWORKS

Engineering & Computer Graphics Workbook Using SOLIDWORKS Engineering & Computer Graphics Workbook Using SOLIDWORKS 2017 Ronald E. Barr Thomas J. Krueger Davor Juricic SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

More information

Part 8: The Front Cover

Part 8: The Front Cover Part 8: The Front Cover 4 Earpiece cuts and housing Lens cut and housing Microphone cut and housing The front cover is similar to the back cover in that it is a shelled protrusion with screw posts extruding

More information

Introduction to Circular Pattern Flower Pot

Introduction to Circular Pattern Flower Pot Prerequisite Knowledge Previous knowledge of the sketching commands Line, Circle, Add Relations, Smart Dimension is required to complete this lesson. Previous examples of Revolved Boss/Base, Cut Extrude,

More information

Beginner s Guide to SolidWorks Alejandro Reyes, MSME Certified SolidWorks Professional and Instructor SDC PUBLICATIONS

Beginner s Guide to SolidWorks Alejandro Reyes, MSME Certified SolidWorks Professional and Instructor SDC PUBLICATIONS Beginner s Guide to SolidWorks 2008 Alejandro Reyes, MSME Certified SolidWorks Professional and Instructor SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com Part Modeling

More information

Introduction to Autodesk Inventor for F1 in Schools (Australian Version)

Introduction to Autodesk Inventor for F1 in Schools (Australian Version) Introduction to Autodesk Inventor for F1 in Schools (Australian Version) F1 in Schools race car In this course you will be introduced to Autodesk Inventor, which is the centerpiece of Autodesk s Digital

More information

Part Design Fundamentals

Part Design Fundamentals Part Design Fundamentals 1 Course Presentation Objectives of the course In this course you will learn basic methods to create and modify solids features and parts Targeted audience New CATIA V5 Users 1

More information

Below are the desired outcomes and usage competencies based on the completion of Project 4.

Below are the desired outcomes and usage competencies based on the completion of Project 4. Engineering Design with SolidWorks Project 4 Below are the desired outcomes and usage competencies based on the completion of Project 4. Project Desired Outcomes: An understanding of the customer s requirements

More information

Engineering Design. with SolidWorks A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling

Engineering Design. with SolidWorks A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling INSIDE: MultiMedia CD An audio/visual presentation of the tutorial projects Engineering Design with SolidWorks 2010 A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling Introductory Level

More information

Sheet metal tutorial. To set the bend radius Right click on the first sheet metal icon in the command manager and specify a bend radius or 1mm.

Sheet metal tutorial. To set the bend radius Right click on the first sheet metal icon in the command manager and specify a bend radius or 1mm. Sheet metal tutorial In the following tutorial you will cover the basic features of the Solid Works sheet metal tool by modelling the component shown opposite. Activating Sheet metal mode Sheet metal components

More information

From the above fig. After sketching the path and profile select the sweep command First select the profile from property manager tree And then select

From the above fig. After sketching the path and profile select the sweep command First select the profile from property manager tree And then select Chapter 5 In sweep command there is a) Two sketch profiles b) Two path c) One sketch profile and one path The sweep profile is used to create threads springs circular things and difficult geometry. For

More information

SolidWorks Navigation

SolidWorks Navigation SolidWorks Basics SolidWorks Navigation Command Bar Feature Tree Model Window Simple Box Select the Front plane Create a new sketch Create a Center Rectangle from the origin Smart Dimension the length

More information

10/14/2010. Chevy Malibu. Vehicle Design with Solidworks. Start SolidWorks Create a New SolidWorks Document. Miles, Rowardo B

10/14/2010. Chevy Malibu. Vehicle Design with Solidworks. Start SolidWorks Create a New SolidWorks Document. Miles, Rowardo B Chevy Malibu Vehicle Design with Solidworks Start SolidWorks Create a New SolidWorks Document Miles, Rowardo B 1 Click: Part and then OK Now you are ready to make a Part. 2 Right Toolbar: Document Properties:

More information

Introducing SolidWorks

Introducing SolidWorks Introducing SolidWorks SAAST Robotics 2008 SolidWorks Software Visually-based 3-D Mechanical design software Engineers and Designers use it to: Quickly sketch out ideas Experiment with features, dimensions

More information

SOLIDWORKS 2015 and Engineering Graphics

SOLIDWORKS 2015 and Engineering Graphics SOLIDWORKS 2015 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

Basic Features. In this lesson you will learn how to create basic CATIA features. Lesson Contents: CATIA V5 Fundamentals- Lesson 3: Basic Features

Basic Features. In this lesson you will learn how to create basic CATIA features. Lesson Contents: CATIA V5 Fundamentals- Lesson 3: Basic Features Basic Features In this lesson you will learn how to create basic CATIA features. Lesson Contents: Case Study: Basic Features Design Intent Stages in the Process Determine a Suitable Base Feature Create

More information

Activity 1 Modeling a Plastic Part

Activity 1 Modeling a Plastic Part Activity 1 Modeling a Plastic Part In this activity, you will model a plastic part. When completed, your plastic part should look like the following two illustrations. While building this model, take time

More information

Shaft Hanger - SolidWorks

Shaft Hanger - SolidWorks ME-430 INTRODUCTION TO COMPUTER AIDED DESIGN Shaft Hanger - SolidWorks BY: DR. HERLI SURJANHATA ASSIGNMENT Submit TWO isometric views of the Shaft Hanger with your report, 1. Shaded view of the trimetric

More information

Engineering Design with SolidWorks A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling. David C. Planchard & Marie P.

Engineering Design with SolidWorks A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling. David C. Planchard & Marie P. Engineering Design with SolidWorks 2003 A Step-by-Step Project Based Approach Utilizing 3D Solid Modeling David C. Planchard & Marie P. Planchard SDC PUBLICATIONS www.schroff.com www.schroff-europe.com

More information

SDC. SolidWorks Tutorial 2001Plus. A Competency Project Based Approach Utilizing 3D Solid Modeling. David C. Planchard & Marie P.

SDC. SolidWorks Tutorial 2001Plus. A Competency Project Based Approach Utilizing 3D Solid Modeling. David C. Planchard & Marie P. 2001Plus A Competency Project Based Approach Utilizing 3D Solid Modeling David C. Planchard & Marie P. Planchard SDC PUBLICATIONS www.schroff.com www.schroff-europe.com Project 2 Below are the desired

More information

SolidWorks. SolidWorks Workbook Advanced Modeling. Version 2009

SolidWorks. SolidWorks Workbook Advanced Modeling. Version 2009 SolidWorks SolidWorks Workbook Advanced Modeling Version 2009 SolidWorks Europe 53, Avenue de l Europe Immeuble DSP 13090 AIX-EN-PROVENCE, France Tel: +33 (0)4 13 10 80 20 Fax: +33 (0)4 13 10 80 21 Email:

More information

Spatula. Spatula SW 2015 Design & Communication Graphics Page 1

Spatula. Spatula SW 2015 Design & Communication Graphics Page 1 Spatula Introduction: The model shown in the picture is made of three parts, - the base, the washer and the handle. The base requires the use of Spline and Style Spline command, Slot command and Mirror

More information

and Engineering Graphics

and Engineering Graphics SOLIDWORKS 2018 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

Autodesk Inventor. In Engineering Design & Drafting. By Edward Locke

Autodesk Inventor. In Engineering Design & Drafting. By Edward Locke Autodesk Inventor In Engineering Design & Drafting By Edward Locke Engineering Design Drafting Essentials Working Drawings: Orthographic Projection Views (multi-view, auxiliary view, details and sections)

More information

Hydro Hull. Chapter 21. Boat. A. Save as "HYDRO". Step 1. Open your HULL MID PLANE file (Chapter 2).

Hydro Hull. Chapter 21. Boat. A. Save as HYDRO. Step 1. Open your HULL MID PLANE file (Chapter 2). Chapter 21 Boat Hydro Hull A. Save as "HYDRO". Step 1. Open your HULL MID PLANE file (Chapter 2). Step 2. Click File Menu > Save As. Step 3. Key-in HYDRO for the filename and press ENTER. B. Delete Loft1,

More information

Using Siemens NX 11 Software. The connecting rod

Using Siemens NX 11 Software. The connecting rod Using Siemens NX 11 Software The connecting rod Based on a Catia tutorial written by Loïc Stefanski. At the end of this manual, you should obtain the following part: 1 Introduction. Start NX 11 and open

More information

Introduction to Sheet Metal Features SolidWorks 2009

Introduction to Sheet Metal Features SolidWorks 2009 SolidWorks 2009 Table of Contents Introduction to Sheet Metal Features Base Flange Method Magazine File.. 3 Envelopment & Development of Surfaces.. 14 Development of Transition Pieces.. 23 Conversion to

More information

Model House Exercise-( Extrude)

Model House Exercise-( Extrude) -( Extrude) Prerequisite knowledge Focus of the lesson Commands Used This lesson requires an understanding of using the sketch commands including Inserting a new sketch Adding sketch geometry Understanding

More information

Toothbrush Holder. A drawing of the sheet metal part will also be created.

Toothbrush Holder. A drawing of the sheet metal part will also be created. Prerequisite Knowledge Previous knowledge of the following commands is required to complete this lesson; Sketch (Line, Centerline, Circle, Add Relations, Smart Dimension,), Extrude Boss/Base, and Edit

More information

Starting a 3D Modeling Part File

Starting a 3D Modeling Part File 1 How to Create a 3D Model and Corresponding 2D Drawing with Dimensions, GDT (Geometric Dimensioning and Tolerance) Symbols and Title Block in SolidWorks 2013-2014 By Edward Locke This tutorial will introduce

More information

Module 1G: Creating a Circle-Based Cylindrical Sheet-metal Lateral Piece with an Overlaying Lateral Edge Seam And Dove-Tail Seams on the Top Edge

Module 1G: Creating a Circle-Based Cylindrical Sheet-metal Lateral Piece with an Overlaying Lateral Edge Seam And Dove-Tail Seams on the Top Edge Inventor (10) Module 1G: 1G- 1 Module 1G: Creating a Circle-Based Cylindrical Sheet-metal Lateral Piece with an Overlaying Lateral Edge Seam And Dove-Tail Seams on the Top Edge In Module 1A, we have explored

More information

Copyrighted. Material. Copyrighted. Material. Copyrighted. Material. Copyrighted. Material

Copyrighted. Material. Copyrighted. Material. Copyrighted. Material. Copyrighted. Material ENGINEERING & COMPUTER GRAPHICS WORKBOOK Using SolidWorks 2005 Ronald E. Barr Thomas J. Krueger Theodore A. Aanstoos Davor Juricic SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com

More information

IT, Sligo. Equations Tutorial

IT, Sligo. Equations Tutorial Equations Tutorial Parametric Modelling: SolidWorks is a parametric modelling system where parameters, such as dimensions and relations, are used to create and control the geometry of the modelled part.

More information

Modeling Basic Mechanical Components #1 Tie-Wrap Clip

Modeling Basic Mechanical Components #1 Tie-Wrap Clip Modeling Basic Mechanical Components #1 Tie-Wrap Clip This tutorial is about modeling simple and basic mechanical components with 3D Mechanical CAD programs, specifically one called Alibre Xpress, a freely

More information

Siemens NX11 tutorials. The angled part

Siemens NX11 tutorials. The angled part Siemens NX11 tutorials The angled part Adaptation to NX 11 from notes from a seminar Drive-to-trial organized by IBM and GDTech. This tutorial will help you design the mechanical presented in the figure

More information

Anchor Block Draft Tutorial

Anchor Block Draft Tutorial Anchor Block Draft Tutorial In the following tutorial you will create a drawing of the anchor block shown. The tutorial covers such topics as creating: Orthographic views Section views Auxiliary views

More information

SolidWorks Design & Technology

SolidWorks Design & Technology SolidWorks Design & Technology Training Course at PHSG Ex 5. Lego man Working with part files 8mm At first glance the Lego man looks complicated but I hope you will see that if you approach a project one

More information

Alternatively, the solid section can be made with open line sketch and adding thickness by Thicken Sketch.

Alternatively, the solid section can be made with open line sketch and adding thickness by Thicken Sketch. Sketcher All feature creation begins with two-dimensional drawing in the sketcher and then adding the third dimension in some way. The sketcher has many menus to help create various types of sketches.

More information

SOLIDWORKS 2018 Basic Tools

SOLIDWORKS 2018 Basic Tools SOLIDWORKS 2018 Basic Tools Getting Started with Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

More information

Copyrighted. Material. Copyrighted. Material. Copyrighted. Material. Copyrighted. Material

Copyrighted. Material. Copyrighted. Material. Copyrighted. Material. Copyrighted. Material ENGINEERING & COMPUTER GRAPHICS WORKBOOK Using SolidWorks 2008 Ronald E. Barr Thomas J. Krueger Theodore A. Aanstoos Davor Juricic SDC PUBLICATIONS Schroff Development Corporation www.schroff.com Better

More information

SOLIDWORKS 2018 Intermediate Skills

SOLIDWORKS 2018 Intermediate Skills SOLIDWORKS 2018 Intermediate Skills Expanding on Solids, Surfaces, Multibodies, Configurations, Drawings, Sheet Metal and Assemblies Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices.

More information

Assembly Receiver/Hitch/Ball/Pin to use for CAD LAB 5A and 5B:

Assembly Receiver/Hitch/Ball/Pin to use for CAD LAB 5A and 5B: MECH 130 CAD LAB 5 SPRING 2017 due Friday, April 21, 2016 at 4:30 PM All of LAB 5 s hardcopies will be working drawing layouts. Do not print out from the part file. We will be using the ME130DRAW drawing

More information

Introduction to Revolve - A Glass

Introduction to Revolve - A Glass Introduction to Revolve - A Glass Design & Communication Graphics 1 Object Analysis sheet Design & Communication Graphics 2 Prerequisite Knowledge Previous knowledge of the following commands are required

More information

Teach Yourself UG NX Step-by-Step

Teach Yourself UG NX Step-by-Step Teach Yourself UG NX Step-by-Step By Hui Zhang Ph.D., P.Eng. www.geocities.com/zhanghui1998 Table of Contents Chapter 1 Introduction... 1 1.1 UG NX User Interface... 1 1.2 Solid Modeling Fundamentals...

More information

SOLIDWORKS 2017 Basic Tools

SOLIDWORKS 2017 Basic Tools SOLIDWORKS 2017 Basic Tools Getting Started with Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org)

More information

LABORATORY MANUAL COMPUTER AIDED DESIGN LAB

LABORATORY MANUAL COMPUTER AIDED DESIGN LAB LABORATORY MANUAL COMPUTER AIDED DESIGN LAB Sr. No 1 2 3 Experiment Title Setting up of drawing environment by setting drawing limits, drawing units, naming the drawing, naming layers, setting line types

More information

Solidworks: Lesson 4 Assembly Basics and Toolbox. UCF Engineering

Solidworks: Lesson 4 Assembly Basics and Toolbox. UCF Engineering Solidworks: Lesson 4 Assembly Basics and Toolbox UCF Engineering Solidworks We have now completed the basic features of part modeling and it is now time to begin constructing more complex models in the

More information

Advance Dimensioning and Base Feature Options

Advance Dimensioning and Base Feature Options Chapter 4 Advance Dimensioning and Base Feature Options Learning Objectives After completing this chapter you will be able to: Dimension the sketch using the autodimension sketch tool. Dimension the sketch

More information

Dual clip mould In the following exercise you will create a full 2 cavity mould of your dual clip mould component.

Dual clip mould In the following exercise you will create a full 2 cavity mould of your dual clip mould component. Dual clip mould 2018 In the following exercise you will create a full 2 cavity mould of your dual clip mould component. The mould is required to be a 2 cavity mould and must contain all the necessary detail

More information

Lesson 10: Loft Features

Lesson 10: Loft Features 10 Goals of This Lesson Your students will be able to create the following part: profiles chisel This lesson plan corresponds to the Loft Features chapter of SolidWorks Getting Started. SolidWorks Student

More information

J. La Favre Fusion 360 Lesson 2 April 19, 2017

J. La Favre Fusion 360 Lesson 2 April 19, 2017 In this lesson, you will create a round plate with 12 counter-bored holes to fit 6-32 socket head screws. A counter-bored hole has two diameters, one to fit the threaded part of the screw and the other

More information

Quick Start for Autodesk Inventor

Quick Start for Autodesk Inventor Quick Start for Autodesk Inventor Autodesk Inventor Professional is a 3D mechanical design tool with powerful solid modeling capabilities and an intuitive interface. In this lesson, you use a typical workflow

More information

Lesson 6 2D Sketch Panel Tools

Lesson 6 2D Sketch Panel Tools Lesson 6 2D Sketch Panel Tools Inventor s Sketch Tool Bar contains tools for creating the basic geometry to create features and parts. On the surface, the Geometry tools look fairly standard: line, circle,

More information

Module 1H: Creating an Ellipse-Based Cylindrical Sheet-metal Lateral Piece

Module 1H: Creating an Ellipse-Based Cylindrical Sheet-metal Lateral Piece Inventor (10) Module 1H: 1H- 1 Module 1H: Creating an Ellipse-Based Cylindrical Sheet-metal Lateral Piece In this Module, we will learn how to create an ellipse-based cylindrical sheetmetal lateral piece

More information

Computer Aided Design Module 2. Lesson Toblerone Bar

Computer Aided Design Module 2. Lesson Toblerone Bar Computer Aided Design Module 2 Lesson Toblerone Bar Lesson? Toblerone Bar New Commands used: Polygon, Add Relations, Smart Dimension, Extrude Boss/Base (Mid Plane), Fillet, Line, Extrude-Cut, Linear Pattern

More information

Essentials of SOLIDWORKS 2015 (4+ Days) * Ve-I Bonus! * File Management + SimulationXpress

Essentials of SOLIDWORKS 2015 (4+ Days) * Ve-I Bonus! * File Management + SimulationXpress Essentials of SOLIDWORKS 2015 (4+ Days) * Ve-I Bonus! * File Management + SimulationXpress Overview What is SOLIDWORKS? Interface Tour View Manipulation Provides some background info on the SOLIDWORKS

More information

Datum Tutorial Part: Cutter

Datum Tutorial Part: Cutter Datum Tutorial Part: Cutter Objective: Learn to apply Datums in different ways Directions 1. Datum Axis Creation a. First we need to create a center axis for the cutter b. Model Tab > Datum > Select Axis

More information

Inventor-Parts-Tutorial By: Dor Ashur

Inventor-Parts-Tutorial By: Dor Ashur Inventor-Parts-Tutorial By: Dor Ashur For Assignment: http://www.maelabs.ucsd.edu/mae3/assignments/cad/inventor_parts.pdf Open Autodesk Inventor: Start-> All Programs -> Autodesk -> Autodesk Inventor 2010

More information

SolidWorks 2013 Part I - Basic Tools

SolidWorks 2013 Part I - Basic Tools SolidWorks 2013 Part I - Basic Tools Parts, Assemblies and Drawings Paul Tran CSWE, CSWI Supplemental Files SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com

More information

Solid Part Four A Bracket Made by Mirroring

Solid Part Four A Bracket Made by Mirroring C h a p t e r 5 Solid Part Four A Bracket Made by Mirroring This chapter will cover the following to World Class standards: Sketch of a Solid Problem Draw a Series of Lines Finish the 2D Sketch Extrude

More information

Feature-Based Modeling and Optional Advanced Modeling. ENGR 1182 SolidWorks 05

Feature-Based Modeling and Optional Advanced Modeling. ENGR 1182 SolidWorks 05 Feature-Based Modeling and Optional Advanced Modeling ENGR 1182 SolidWorks 05 Today s Objectives Feature-Based Modeling (comprised of 2 sections as shown below) 1. Breaking it down into features Creating

More information

SolidWorks Part I - Basic Tools SDC. Includes. Parts, Assemblies and Drawings. Paul Tran CSWE, CSWI

SolidWorks Part I - Basic Tools SDC. Includes. Parts, Assemblies and Drawings. Paul Tran CSWE, CSWI SolidWorks 2015 Part I - Basic Tools Includes CSWA Preparation Material Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered

More information

SolidWorks 2014 Part I - Basic Tools

SolidWorks 2014 Part I - Basic Tools SolidWorks 2014 Part I - Basic Tools Parts, Assemblies and Drawings Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit

More information

Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated)

Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated) Inventor (5) Module 2: 2-1 Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated) In this tutorial, we will learn how to build a 3D model

More information

To start a new drawing Select File New then from the dialog box, which appears select Normal.dft followed by OK.

To start a new drawing Select File New then from the dialog box, which appears select Normal.dft followed by OK. Draft Tutorial This tutorial provides step-by-step instructions for the detailing of a drawing of the anchor block shown opposite. As you create this drawing, you will use the following drafting techniques:

More information

1. Creating geometry based on sketches 2. Using sketch lines as reference 3. Using sketches to drive changes in geometry

1. Creating geometry based on sketches 2. Using sketch lines as reference 3. Using sketches to drive changes in geometry 4.1: Modeling 3D Modeling is a key process of getting your ideas from a concept to a read- for- manufacture state, making it core foundation of the product development process. In Fusion 360, there are

More information

Introduction to Parametric Modeling AEROPLANE. Design & Communication Graphics 1

Introduction to Parametric Modeling AEROPLANE. Design & Communication Graphics 1 AEROPLANE Design & Communication Graphics 1 Object Analysis sheet Design & Communication Graphics 2 Aeroplane Assembly The part files for this assembly are saved in the folder titled Aeroplane. Open an

More information

Activity Bracket

Activity Bracket Activity 1.5.6 Bracket Introduction Studying how an object is fastened is not something you do every day. But, just for fun, consider looking at how your desk or your locker is held together. Most likely,

More information

Part Design. Sketcher - Basic 1 13,0600,1488,1586(SP6)

Part Design. Sketcher - Basic 1 13,0600,1488,1586(SP6) Part Design Sketcher - Basic 1 13,0600,1488,1586(SP6) In this exercise, we will learn the foundation of the Sketcher and its basic functions. The Sketcher is a tool used to create two-dimensional (2D)

More information

1. Open the Feature Modeling demo part file on the EEIC website. Ask student about which constraints needed to Fully Define.

1. Open the Feature Modeling demo part file on the EEIC website. Ask student about which constraints needed to Fully Define. BLUE boxed notes are intended as aids to the lecturer RED boxed notes are comments that the lecturer could make Control + Click HERE to view enlarged IMAGE and Construction Strategy he following set of

More information

Understanding Projection Systems

Understanding Projection Systems Understanding Projection Systems A Point: A point has no dimensions, a theoretical location that has neither length, width nor height. A point shows an exact location in space. It is important to understand

More information

Module 2.1, 2.2 Review. EF101 Analysis & Skills Module 2.3. Sketched Features and Operations. On-line Help Two Locations

Module 2.1, 2.2 Review. EF101 Analysis & Skills Module 2.3. Sketched Features and Operations. On-line Help Two Locations EF101 Analysis & Skills Module 2.3 Engineering Graphics Revolved Features Placed Features Work Features Module 2.1, 2.2 Review What are the three types of operations for adding features to the base feature?

More information

Module 1C: Adding Dovetail Seams to Curved Edges on A Flat Sheet-Metal Piece

Module 1C: Adding Dovetail Seams to Curved Edges on A Flat Sheet-Metal Piece 1 Module 1C: Adding Dovetail Seams to Curved Edges on A Flat Sheet-Metal Piece In this Module, we will explore the method of adding dovetail seams to curved edges such as the circumferential edge of a

More information

Cube in a cube Fusion 360 tutorial

Cube in a cube Fusion 360 tutorial Cube in a cube Fusion 360 tutorial n Before using these instructions, it is helpful to watch this video screencast of the CAD drawing actually being done in the software. Click to link to the video tutorial.

More information

SOLIDWORKS 2018 Intermediate Skills

SOLIDWORKS 2018 Intermediate Skills SOLIDWORKS 2018 Intermediate Skills Expanding on Solids, Surfaces, Multibodies, Configurations, Drawings, Sheet Metal and Assemblies Paul Tran CSWE, CSWI SDC PUBLICATIONS Better Textbooks. Lower Prices.

More information

Made Easy. Jason Pancoast Engineering Manager

Made Easy. Jason Pancoast Engineering Manager 3D Sketching Made Easy Jason Pancoast Engineering Manager Today I have taught you to sketch in 3D. It s as easy as counting ONE, TWO, FIVE...er...THREE! When your sketch only lives in Y and in X, Adding

More information

for Solidworks TRAINING GUIDE LESSON-9-CAD

for Solidworks TRAINING GUIDE LESSON-9-CAD for Solidworks TRAINING GUIDE LESSON-9-CAD Mastercam for SolidWorks Training Guide Objectives You will create the geometry for SolidWorks-Lesson-9 using SolidWorks 3D CAD software. You will be working

More information

1. Create a 2D sketch 2. Create geometry in a sketch 3. Use constraints to position geometry 4. Use dimensions to set the size of geometry

1. Create a 2D sketch 2. Create geometry in a sketch 3. Use constraints to position geometry 4. Use dimensions to set the size of geometry 2.1: Sketching Many features that you create in Fusion 360 start with a 2D sketch. In order to create intelligent and predictable designs, a good understanding of how to create sketches and how to apply

More information

How to Build a Game Console. David Hunt, PE

How to Build a Game Console. David Hunt, PE How to Build a Game Console David Hunt, PE davidhunt@outdrs.net Covering: Drafts Fillets Shells Patterns o Linear o Circular Using made-for-the-purpose sketches to define reference geometry Using reference

More information

< Then click on this icon on the vertical tool bar that pops up on the left side.

< Then click on this icon on the vertical tool bar that pops up on the left side. Pipe Cavity Tutorial Introduction The CADMAX Solid Master Tutorial is a great way to learn about the benefits of feature-based parametric solid modeling with CADMAX. We have assembled several typical parts

More information

CAD Tutorial 24: Step by Step Guide

CAD Tutorial 24: Step by Step Guide CAD TUTORIAL 24: Step by step CAD Tutorial 24: Step by Step Guide Level of Difficulty Time Approximately 40 50 minutes Lesson Objectives To understand the basic tools used in SketchUp. To understand the

More information

SolidWorks Training. Introductory course for staff and students from the School of Physics and Astronomy

SolidWorks Training. Introductory course for staff and students from the School of Physics and Astronomy SolidWorks Training Introductory course for staff and students from the School of Physics and Astronomy i) Introductory presentation SolidWorks Training ii) The SolidWorks GUI The SolidWorks Graphical

More information

CATIA Instructor-led Live Online Training Program

CATIA Instructor-led Live Online Training Program Course Outline Introduction & Understanding to CATIA Environment Introduction & Understanding to CATIA interface Starting new file Understand the Sketcher workbench of CATIA V5 Start a new file in the

More information

Wireless Mouse Surfaces

Wireless Mouse Surfaces Wireless Mouse Surfaces Design & Communication Graphics Table of Contents Table of Contents... 1 Introduction 2 Mouse Body. 3 Edge Cut.12 Centre Cut....14 Wheel Opening.. 15 Wheel Location.. 16 Laser..

More information

Draft Analysis Tools 1 Tuula Höök, Tampere University of Technology

Draft Analysis Tools 1 Tuula Höök, Tampere University of Technology Draft Analysis Tools 1 Tuula Höök, Tampere University of Technology What is new in this exercise? - Draft analysis tool - Undercut analysis tool - Drafting faces with a neutral plane - Modifications to

More information

Clock Exercise (Inserting Planes)

Clock Exercise (Inserting Planes) Clock Exercise (Inserting Planes) Prerequisite Knowledge To complete this exercise you will need to be familiar with Sketching, Applying relations, Extrude Boss/ Base, Extrude cut, Applying Textures, Renaming

More information

Drawing and Assembling

Drawing and Assembling Youth Explore Trades Skills Description In this activity the six sides of a die will be drawn and then assembled together. The intent is to understand how constraints are used to lock individual parts

More information

Modeling an Airframe Tutorial

Modeling an Airframe Tutorial EAA SOLIDWORKS University p 1/11 Difficulty: Intermediate Time: 1 hour As an Intermediate Tutorial, it is assumed that you have completed the Quick Start Tutorial and know how to sketch in 2D and 3D. If

More information

Alibre Design Tutorial: Loft, Extrude, & Revolve Cut Loft-Tube-1

Alibre Design Tutorial: Loft, Extrude, & Revolve Cut Loft-Tube-1 Alibre Design Tutorial: Loft, Extrude, & Revolve Cut Loft-Tube-1 Part Tutorial Exercise 5: Loft-Tube-1 [Complete] In this Exercise, We will set System Parameters first, then part options. Then, in sketch

More information

The project focuses on the design for a Pencil holder, but could be adapted to any simple assembly.

The project focuses on the design for a Pencil holder, but could be adapted to any simple assembly. Introduction - Teacher Notes Fig 1. The project focuses on the design for a Pencil holder, but could be adapted to any simple assembly. Pro/DESKTOP enables pupils (and teachers) to communicate and model

More information

Drawing a Living Room and Family Room Floorplan

Drawing a Living Room and Family Room Floorplan Appendix C Drawing a Living Room and Family Room Floorplan In this chapter, you will learn the following to World Class standards: Draw a Living Room and Family Room Floorplan Draw the Walls and Stairs

More information

Kitchen and Bath Design Tutorial

Kitchen and Bath Design Tutorial Kitchen and Bath Design Tutorial This tutorial continues where the Interior Design Tutorial left off. You should save this tutorial using a new name to archive your previous work. The tools and techniques

More information

Parametric Modeling. with. Autodesk Inventor Randy H. Shih. Oregon Institute of Technology SDC

Parametric Modeling. with. Autodesk Inventor Randy H. Shih. Oregon Institute of Technology SDC Parametric Modeling with Autodesk Inventor 2009 Randy H. Shih Oregon Institute of Technology SDC PUBLICATIONS Schroff Development Corporation www.schroff.com Better Textbooks. Lower Prices. iii Table of

More information