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SolidWorks Tips & Tricks sponsored by ProFab Lite V3.5Custom Relief Type When you create an Edge Flange or a Miter Flange that does not go the full length of the edge you select, you have the opportunity to specify a Custom Relief at the short end. To do this, let’s create a new Part document. Then from the Sheet Metal CommandManager, create a base flange using the Base-Flange/Tab command. Make the base flange 12.00 by 8.00 and set the material thickness to '0.048'.
This same feature exists for both the Edge Flange and the Miter Flange. This tutorial will use the Edge flange. Select the Edge Flange button from the Sheet Metal CommandManager. Select an edge on the Base Flange where you want to create the Edge Flange.
In the Feature Manager, set the Flange Length to '2.00'. Make certain the Flange Position is not set to Bend Outside. The Bend Outside option does not require a relief notch. For this tutorial, use Material Inside. Also, make certain the Offset check box is not checked. Next pick the Edit Flange Profile button at the top of the PropertyManager. Change the view to Normal To. If the Profile Sketch dialog box is on top of the part, place the cursor at the top of the dialog box, press and hold the left mouse button and drag the dialog box away from the part. Now place the tip of the cursor on the black vertical line on the left side of the sketch. Press and hold the left mouse button, then drag the line to the right. Use the Smart Dimension command to add a dimension of '5.00' to the width of the flange.
Click the Back button in the Profile Sketch dialog box to close the dialog and exit the sketch. If you should pick the Finish button, just right click on Edge-Flange1 in the FeatureManager design tree and pick Edit Feature from the menu. At the bottom of the PropertyManager, you will find Custom Relief Type. Check the box to the left of it to expand it. You may have to scroll down on the PropertyManager to see it.
The default is to use the relief ratio. Just uncheck the Use relief ratio check box and it will update the PropertyManager to allow the input of a Width and Depth.
Pull down the Relief Type menu (where it says Rectangle) and pick Obround. Then, enter the Width of '0.125' and a Depth of '0.00'. The PropertyManager should now look like the image below.
Click the OK button, the green check mark, to close the PropertyManager and create the flange. If need be, change the view orientation to Isometric so you can see the flange with the relief notch.
That’s it! Adjust the style and dimensions to suit your tooling, especially if you are manufacturing the part on a punch press. To learn more about sheet metal part creation, click here.
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