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

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

3 Basic Solid Modeling Extrude Options - Upon successful completion of this lesson, you will be able to: * Sketch on planes and/or planar surfaces. * Use the sketch tools to construct geometry. * Add the geometric relations or constraints. * Add/modify dimensions. * Explore the different extrude options. - The following 5 basic steps will be demonstrated throughout this exercise: * Select the sketch plane. * Activate Sketch pencil. * Sketch the profile using the sketch tools. * Define the profile with dimensions or relations. * Extrude the profile. - Be sure to review the self-test questionnaires at the end of the lesson, prior to moving to the next chapter. 3-1

4 Basic Solid Modeling Extrude Options View Orientation Hot Keys: Ctrl + 1 = Front View Ctrl + 2 = Back View Ctrl + 3 = Left View Ctrl + 4 = Right View Ctrl + 5 = Top View Ctrl + 6 = Bottom View Ctrl + 7 = Isometric View Ctrl + 8 = Normal To Selection Dimensioning Standards: ANSI Units: INCHES 3 Decimals Tools Needed: Insert Sketch Line Circle Add Geometric Relations Dimension Sketch Fillet Trim Entities Boss / Base Extrude 3-2

5 1. Starting a new Part: - From the File menu, select New / Part, or click the New icon. - Select the Part template from either the Templates or Tutorial folders. - Click OK ; a new part template is opened. 3-3

6 2. Changing the Scene: - From the View (Heads-up) toolbar, click the Apply Scene button (arrow) and select the Plain White option (arrow). - By changing the scene color to Plain White we can see better the colors of the sketch entities and sketch dimensions. - To show the Origin, click the View dropdown menu and select Origins. - The Blue Origin is the Zero position of the part and the Red Origin is the Zero position of a sketch. Blue Origin 3-4

7 3. Starting a new Sketch: - Select the Front plane from the Feature- Manager tree and click the Pencil icon to start a new sketch. - A sketch is normally created first, relations and dimensions are added after, and then it gets extruded into a 3D feature. - From the Command- Manager toolbar, select the Line command. Mouse Gesture Command Manager Toolbar OPTION: Right-Drag to display the Mouse Gesture guide and select the Line command from it. (See the Introduction section, page XVIII for details on customizing the Mouse Gesture). - Position the mouse cursor at the Red Origin point, a yellow feedback symbol appears to indicate a relation (Coincident) is going to be added automatically to the 1 st endpoint of the line. This endpoint will be locked at the zero position. Auto-Relation feedback symbol 3-5

8 4. Using the Click + Hold + Drag technique: - Click at the Origin point and hold the mouse button to start the line at point 1, drag upwards to point 2, then release the mouse button. 2 Start the line from Point 1 and drag to Point 2 The Base Sketch 1 The Base Sketch is the parent sketch of a part and is also the very first sketch in a part document. It should primarily describe the basic shape of the part, before other features can be added. - Continue adding other lines using the Click-Hold-Drag technique. - The relations like Horizontal and Vertical are added automatically to each sketch line. Other relations like Collinear and Equal are added manually. - The size and shape of the profile will be corrected in the next few steps. System Feedback While sketching the lines, watch for the System Feedback Symbols such as for Horizontal, and for Vertical Auto Relations. 3-6

9 5. Adding Geometric Relations*: - Click Add Relation under Display/Delete Relations - OR - select Tools / Relations / Add. - Select the 4 lines shown below. - Click Equal from the Add Geometric Relation dialog box. This relation makes the length of the two selected lines equal. * Geometric relations are one of the most powerful features in SolidWorks. They are used in the sketch level to control the behaviors of the sketch entities when they are moved or rotated and to keep the associations between one another. When applying geometric relations between entities, one of them should be a 2D entity and the other can either be a 2D sketch entity or a model edge, a plane, an axis, or a curve, etc. Equal Relations Adding the EQUAL relations to these lines eliminates the need to dimension each line. Geometric relations can be created manually or automatically. The next few steps in this chapter will demonstrate how geometric relations are added manually. Select the top 4 lines and click Equal relation The top 4 lines are now Equal in size. 3-7

10 6. Adding a Collinear relation**: - Select the Add Relation command again. - Select the 3 lines as shown below. - Click Collinear from the Add Geometric Relations dialog box. - Click OK. Select the bottom 3 lines and click Collinear relation The bottom 3 lines are moved to the same level. Collinear Relations Adding a Collinear relation to these lines puts them on the same height level; only one dimension is needed to drive the height of all 3 lines. ** Collinear relations can be used to constrain the geometry as follows: - Collinear between a line and another line(s) (2D and 2D). - Collinear between a line(s) to an edge of a model (2D and 3D). 3-8

11 Geometric Relations Examples Coincident Midpoint An endpoint is Coincident with a line. An endpoint is Coincident with a midpoint of a line. Tangent An arc is tangent with a line or another arc. Two circles are sharing the same center. Concentric Equal Two lines are on the same level (or Co-planar). Two circles or two lines having the same size. Tangent Collinear Vertical Two or more points are aligned vertically. Horizontal Two or more points are aligned horizontally. 3-9

12 7. Adding the horizontal dimensions: - Select from the Sketch toolbar - OR - select Insert / Dimension, and add the dimensions shown below (follow the 3 steps A, B and C). A. Click line 1 B. Click line 2 C. Place the dimension approximately here and enter.500 in. - Continue adding the horizontal dimensions as shown here. NOTE: The color of the sketch lines changes from Blue to Black, to indicate that they have been constrained with a dimension. 3-10

13 8. Adding the Vertical dimensions: - With the Smart- Dimension tool still selected, click on line 1 and line 2; place the dimension approximately as shown, and change the value to.500 in. Line 2 Line 1 A. Click line 1 B. Click line 2 - Continue adding other dimensions until the entire sketch turns into the Black color. The Status of a Sketch: The current status of a sketch is displayed in the lower right corner of the screen. Fully Defined = Black Under Defined = Blue Over Defined = Red 3-11

14 Sketch Relation Symbols 9. Hiding the Sketch Relation Symbols: - The Sketch Relation Symbols indicate which geometric relation a sketch entity has, but they get quite busy as shown. - To hide or show the Sketch Relation Symbols, go to the View menu and Click off the Sketch Relations option. Sketch Relation Symbols at a Glance Horizontal relation Equal relation Tangent relation Vertical relation Coincident relation Collinear relation 3-12

15 10. Extruding the Base: - The Extrude Boss/Base command is used to define the characteristic of a 3D linear feature. - Click from the Features toolbar - OR- select Insert / Boss Base / Extrude. - Set the following: - Direction: Blind. Reverse - Depth: 6.00 in. - Enabled Reverse direction. - Click OK. 3-13

16 11. Sketching on a Planar Face: - Select the face as indicated. - Click or select Insert/Sketch. - Click from the Sketch Tools toolbar Or select Tools / Sketch Entity / Circle. (From the View toolbar above the CommandManager, click the Isometric icon or press the shortcut keys Ctrl+7). Select the Sketch Face Planar Surfaces - A planar surface of the model can also be used as a Sketch Plane. - The Sketch will then be extruded normal to the selected surface. - Position the mouse cursor near the center of the selected face, click and drag outward to draw a circle. - While sketching the circle, the system displays the radius value next to the mouse cursor. - Dimensions are added after the profile is created. 3-14

17 - Select the Smart Dimension command and add a diameter dimension to the circle. (Click on the circle and move the mouse cursor outward, at approximately 45 degrees and place it). - To add the location dimensions click the edge of the circle and the edge of the model, place the dimension, then correct the value. - Continue adding the location dimensions as shown, to fully define the sketch. - Select the Line command and sketch the 3 lines as shown below. Snap to the hidden edge of the model when it lights up. - The color of the sketch should change to black at this point (Fully Defined). Snap to quadrant point Auto-Snap to hidden edge 3-15

18 12. Using the Trim Entities command: - Select the Trim Entities command from the Sketch toolbar (arrow). - Click the Trim to Closest option (arrow). When the pointer is hovered over the entities, this trim command highlights the entities prior to trimming to the next intersection. Trim Entities Use this command to trim, extend or delete a sketch entity. - Position the pointer over the lower portion of the circle, the portion that is going to be trimmed-off lights up. Click the mouse to trim. - The bottom portion of the circle is trimmed, leaving the sketch as one-continuous-closedprofile, suitable to extrude into a feature. - Next, we are going to look at some of the extrude options available in SolidWorks. 3-16

19 13. Extruding a Boss: - Switch to the Feature toolbar and click or select: Insert / Boss-Base / Extrude. Extrude Options Explore each extrude option to see the different results. Press Undo to go back to the original state after each one. A Using the Blind option: - When extruding with the Blind option, the following conditions are required: * Direction * Depth dimension - Drag the direction arrow on the preview graphics to define the direction, then enter a dimension for the depth. Direction & Depth Blind Condition B Using the Through All option: - When the Through All option is selected, the system automatically extrudes the sketch to the length of the part, normal to the sketch plane. Through All Condition 3-17

20 C Using the Up To Next option: - With the Up To Next option selected, the system extrudes the sketch to the very next set of surface(s), and blends it to match. Up To Next Condition D Using the Up To Vertex option: - This option extrudes the sketch from its plane to a vertex, specified by the user, to define its depth. Select a Vertex Up To Vertex Condition E Using the Up To Surface option: Select a Surface - This option extrudes the sketch from its plane to a single surface, to define its depth. Up To Surface Condition 3-18

21 F Using the Offset From Surface option: - This option extrudes the sketch from its plane to a selected face, then offsets at a specified distance. Select a surface to offset from & enter a distance. Offset From Surface Condition G Using the Up To Body option: - This option extrudes the sketch from its sketch plane to a specified body. Select a Solid Body to extrude to. (optional) Up To Body Condition - The Up To Body option can also be used in assemblies or multi-body parts. - The Up To Body option works with either a solid body or a surface body. It is also useful when making extrusions in an assembly to extend a sketch to an uneven surface. 3-19

22 H Using the Mid Plane option: - This option extrudes the sketch from its plane equally in both directions. - Enter the Total Depth dimension when using the Mid-Plane option. Mid Plane Condition - After you are done exploring all the extrude options, change the final condition to: Through All - Click OK. - The system extrudes the circle to the outer most surface as the result of the Through All end condition. 3-20

23 - The extra material between the first and the second extruded features is removed automatically. - Unless the Merge Result checkbox is cleared, all interferences will be detected and removed. Extrude summary: * The Extrude Boss/Base command is used to add thickness to a sketch and to define the characteristic of a 3D feature. * A sketch can be extruded in both directions at the same time, from its sketch plane. * A sketch can also be extruded as a solid or a thin feature. 3-21

24 14. Adding the model fillets by Lasso*: - Fillet/Round creates a rounded internal or external face on the part. You can fillet all edges of a face, select sets of faces, edges, or edge loops. - The radius value stays in effect until you change it. Therefore, you can select any number of edges or faces in the same operation. - Click or select Insert / Features / Fillet/Round. Stop here Start here - Enter.125 in. for radius value. - Click-Hold the mouse approximately at the "Start here" position and drag the pointer around the entire model to select all of its edges. - Click OK. * To set the Lasso Selection as the default, go to: Tools / Options / Display Selection / Default Bulk Selection Method / Lasso (arrow). 3-22

25 * In the Training Files folder, in the Built Parts folder you will also find copies of the parts, assemblies, and drawings that were created for cross referencing or reviewing purposes. Fillet (adds material) * Fillets and Rounds: Using the same Fillet command, SolidWorks knows whether to add material (Fillet) or remove material (Round) to the faces adjacent to the selected edge. 15. Saving your work: - Select File / Save As. - Change the file type to Part file (.sldprt). - Enter Extrude Options for the name of the file. Round (removes material) Fillet - Click Save. Round 3-23

26 1. To open a new sketch, first you must select a plane from the FeatureManager tree. a. True b. False 2. Geometric relations can be used only in the assembly environments. a. True b. False 3. The current status of a sketch is displayed in the lower right area of the screen as: Under defined, Fully defined, or Over defined. a. True b. False 4. Once a feature is extruded, its extrude direction cannot be changed. a. True b. False 5. A planar face can also be used as a sketch plane. a. True b. False 6. The Equal relation only works for Lines, not Circles or Arcs. a. True b. False 7. After a dimension is created, its value cannot be changed. a. True b. False 8. When the UP TO SURFACE option is selected, you have to choose a surface as an endcondition to extrude up to. a. True b. False 9. UP TO VERTEX is not a valid Extrude option. a. True b. False 3-24

27 Exercise: Extrude Boss & Extrude Cut NOTE: In an exercise, there will be less step-by-step instruction than those in the lessons, which will give you a chance to apply what you have learned in the previous lesson to build the model on your own. 1. Dimensions are in inches, 3 decimal places. 2. Use Mid-Plane end condition for the Base feature. 3. The part is symmetrical about the Front plane. 4. Use the instructions on the following pages if needed. Origin 4X.060 X

28 1. Starting with the base sketch: - Select the Front plane and open a new sketch. - Starting at the top left corner, using the line command, sketch the profile below. Origin Parallel - Add the dimensions shown. - Add the Parallel relation to fully define the sketch. - Extrude Boss/Base with Mid Plane and in depth. 3-26

29 2. Adding the through holes: - Select the face as indicated and click the Normal-To button. - This command rotates the part normal to the screen. Select this face and click the Normal-To button - The hot-key for this command is Ctrl Open a new sketch and draw a centerline that starts from the origin point. - Sketch 2 circles on either side of the centerline. - Add the diameter and location dimensions shown. Push Escape when done. Both circles are Symmetric about the Centerline - Hold the Control key and select both circles and the centerline, then click the Symmetric relation on the properties tree. 3-27

30 - Create an extruded cut using the Through- All condition. 3. Adding the upper cut: - Select the upper face and click the Sketch pencil to open a new sketch. - Sketch a centerline that starts at the Origin. - Sketch a rectangle as shown. Both lines are Symmetric about the Centerline - Add the dimensions and relations as indicated. - Create an extruded cut using the Up-To-Vertex condition (up-to-surface also works). - Select the Vertex indicated. Select Vertex - Click OK. 3-28

31 4. Adding the lower cut: - Select the lower face of the part and open a new sketch. - Sketch a rectangle on this face. - Add a Collinear and an Equal relations to the lines and the edges as noted. - Extrude a cut using the Through All condition. The line is Collinear and Equal with the edge on both sides. 5. Adding a chamfer: - Click Chamfer under the Fillet button. Select 4 edges - Enter.060 for depth. - Select the 4 circular edges of the 2 holes. - Click OK. 6. Saving your work: - Click File / Save As. - Enter Extrudes_Exe1 for the file name. - Select a location to save the file. - Click Save. 3-29

32 Using the Search Commands: The Search Commands lets you find and run commands from SolidWorks Search or locate commands in the user interface. These features make it easy to find and run any SolidWorks command: - The results are filtered as you type and typically find the command you need within a few keystrokes. - When you run a command from the results list for a query, Search Commands remembers that command and places it at the top of the results list when you type the same query again. - Search shortcuts lets you assign simple and familiar keystroke sequences to Commands you use regularly. 3-30

33 1. Search Commands in Feature Mode: - The example below shows how you might use Search Commands to find and run the Lasso Selection command in the Feature Mode. - With the part still open, start typing the command Lasso Selection in Search Commands. As soon as you type the first few letters of the word Lasso, the results list displays only those commands that include the character sequence "lasso", and Lasso Selection appears near the top of the results list. - Click Show Command Location, a red arrow indicates the command in the user interface. 3-31

34 2. Search Commands in Sketch Mode: - The example below shows how you might use Search Commands to find and run the Dynamic Mirror command in the Sketch Mode. - Using the same part, open a new sketch on the side face of the model as noted. Sketch face - Start typing the command Dynamic Mirror in Search Commands. As soon as you type the first few letters of the word Dynamic, the results list displays only those commands that include the character sequence "dyna", and Dynamic command appears near the top of the results list. 3-32

35 - Click Show Command Location, a red arrow indicates the command in the user interface. - Additionally, a Search Shortcut can be assigned to any command to help find it more quickly (see Customize Keyboard in the SolidWorks Help for more info): 1. Click Tools / Customize, and select the Keyboard tab. 2. Navigate to the command to which you want to assign a search shortcut. 3. In the Search Shortcut column for the command, type the shortcut letter you want to use, then click OK. - Save and close all documents. 3-33

36 SolidWorks 2015 l Basic Tools l Basic Solid Modeling 3-34

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