SolidWorks 2011 Parts Bible - Matt Lombard [291]
4. After the Base Flange has been created, edit the Sheet Metal feature, and change the default bend radius to .050 inches.
5. Click one of the 14-inch edges and then select the Line tool from the Sketch toolbar. This is a shortcut to creating a plane perpendicular to the end of the edge and opening a new sketch on the plane. This is useful in other situations in addition to working with sheet metal. Draw a sketch similar to that shown in Figure 21.51. The arc overrides the default inside bend radius setting and directly controls that particular bend.
6. With the sketch still active, click the Miter Flange button on the Sheet Metal toolbar. Use the settings shown in the image to the right in Figure 21.52. Select three edges as shown. Remember to select the edges on the same side of the Base Flange. In particular, notice the Start/End Offset settings. Click OK when you are satisfied with the settings.
Figure 21.51
The sketch to start a Miter Flange
Figure 21.52
Specifying the Miter Flange settings
7. Select the remaining edge that is not touched by the Miter Flange, and click the Edge Flange tool on the Sheet Metal toolbar. Click the top point of one end of the Miter Flange to establish the flange length using the Up To Vertex end condition.
8. Click the Edit Flange Profile button in the PropertyManager, and manually pull the sketch back from the ends of the flange. Add dimensions to make the flange 3 inches from the corner on the left side, and 5 inches from the corner on the right side, as shown in Figure 21.53; otherwise, use the default settings for the flange. Click OK to accept the feature when you are satisfied with the settings.
Figure 21.53
Creating an Edge Flange
9. Select the inside edge of the top of the Edge Flange that you have just created and initiate a Hem feature. Use the settings Material Inside, Closed Hem, with a length of .25 inches, and make the material go toward the inside of the box. The settings and preview of the feature are shown in Figure 21.54.
Figure 21.54
Creating a hem
10. Create a second Edge Flange the same height as the first, just to the right of the first flange, as seen from the point of view used in Figure 21.48. Edit the flange profile and pull the new flange away from the existing flange. Add a dimension to make the new flange 2 inches wide. Click OK when you are satisfied with the settings.
11. Open a sketch on the inside face of the new Edge Flange and draw a line across the flange .75 inches from the end.
12. Create a Jog feature with the settings shown in Figure 21.55. Make sure to set a custom bend radius by deselecting the Use default radius option and entering .025 inches. If you do not set the custom radius, you may get a warning that the jog distance is less than a minimum jog value. Be careful when selecting the fixed face to select the side of the line with the largest area, or the face you want to remain where it is while the rest of the part bends and moves around it.
Figure 21.55
Creating a jog
13. From the DVD, in the folder for Chapter 21, find the part named Chapter 21 – Cross Break.sldprt. Copy this file to a folder in the library that you have established outside of your SolidWorks installation folder, called Forming Tools.
14. Make sure that this folder appears in the Design Library. You may have to press F5 or click the Refresh button at the top of the Task pane. When the folder appears, right-click the folder and select the check mark next to Forming Tools Folder.
15. When the file has been copied and the folder has been assigned as a Forming Tool folder, drag the Chapter 21 – Cross Break part from the folder and onto the big flat face of the sheet metal part. You will be put into a sketch that looks like Figure 21.56.
Figure 21.56
Placing a forming tool
16. Once you have dropped the feature into the sketch, drag the Origin of the sketch onto the Origin of the part, and then click Finish. Notice that the cross break is