SolidWorks 2011 Parts Bible - Matt Lombard [100]
1. Open a new part using a template with inches as units. Open a sketch on the Front plane and draw a construction line starting from the origin 12 inches down (negative Y) away from the Origin.
2. Insert a sketch picture in this sketch. Use Sketch Picture 1.tif from the DVD for Chapter 6.
3. Resize the image so that the endpoints of the construction line are near the centers of the holes on the ends of the part. To move the image, just double-click it first, and then drag it. To resize it, drag the corners.
4. In the Transparency panel of the Sketch Picture PropertyManager, select the Eyedropper tool and click in the white background of the image. Make sure that the color field next to the Eyedropper tool changes to white.
5. Slide the Transparency and Matching Tolerance sliders all the way to the right, or type 1.00 in the number boxes.
6. Close the sketch, and rename it Sketch Image Front View.
7. Put the image Sketch Picture 2.tif, also from the DVD, in a sketch on the Right plane, and resize it to fit with the first image. Center it symmetrically about the Origin. Also, set the transparency to the same setting as the first image.
8. Open a new sketch, also on the Front plane, and draw two circles to match the features on the ends. Extrude them using a Mid Plane extrusion to match the image in the other direction (about 2.5 inches), as shown in Figure 6.23.
9. Open another new sketch on the Front plane and draw the tangent lines to form the web in the middle of the part. Use the automatic relations to draw the lines tangent to the two cylinders. It is easiest if you the Front View for this. Close the sketch to make a solid extrusion. Extrude this part .5 inches Mid Plane.
10. Open a new sketch on the face of the large flat web that you created in the previous step, and offset the arc edge of the larger circular boss by 2.10 inches.
Figure 6.23
Using sketch pictures
11. Change the arc to a construction arc and drag its endpoints to approximately the position shown in Figure 6.24. The endpoints of the arc are blue after you drag them. Give them a Horizontal relation, and then dimension them.
` To create the 2.10 dimension as shown, select the arc and circle with the Dimension cursor while pressing down the Shift key.
Figure 6.24
Creating an offset arc
12. Choose File⇒Properties. Make sure the Custom tab is active, and type Sketch Text in the first open box of the Property Name column. Make sure the Type is set to Text, and in the Value field, type SolidWorks. Click OK when you are done.
13. Choose Tools⇒Sketch Entities⇒Text to initiate the creation of sketch text.
14. Select the construction arc to go into the Curves window.
15. Below the Text window, click the Link to Property button. Select Sketch Text from the drop-down list. Select the Full Justify option, then click the green check mark icon to accept it.
16. Deselect the Use Document Font option, click the Font button, and then set the Units to .50 inches. Click the Bold button to make the text thicker. Click OK to exit the dialog box. Click the green check mark icon to exit the sketch text, and then exit the sketch.
17. Extrude the text to a depth of .050 inches with 3 degrees of draft. The part at this point resembles Figure 6.25.
Performance
Sketch Text is a real performance killer. The more text that you use, the longer it takes to extrude. Draft on the extrusion adds to the time required.
Figure 6.25
Creating extruded text
18. Select the flat face on the other side of the part from where you just extruded the text, and open a sketch.
19. Select the face and click the Offset button to make a set of sketch entities offset to the inside of the face by .50 inches. Remember that you may have to reverse the offset to get it to work properly.
20. Open the Line Format toolbar (right-click any toolbar other than the CommandManager and select Line Format).
21. Select all the sketch lines and change their color using the