Auto vs Corner Relief in SolidWorks Sheet Metal

Article by Andrew Lidstone, CSWE updated December 20, 2010

Article

Sheet Metal functionality within SolidWorks provides designers with powerful tools to create accurate, formable models of their designs.  However, a common point of confusion when using sheet metal functions is the difference between the auto relief and corner treatment tools.

 

 

Auto Relief

When starting a sheet metal part by creating a base flange feature, one of the initial parameters, along with Sheet Metal Gauge and Bend Allowance, are the Auto Relief settings.  This parameter will determine how SolidWorks will create relief cuts as they are needed in the sheet metal body. There are three relief types available, Rectangular, Obround and Tear.

Rectangular Auto Relief

Rectangular Auto Relief

Selecting a Rectangular or Obround relief allows the user to specify the Relief Ratio.  The width of the relief cut and the depth it extends past the bend will be determined by (relief ratio) * (part thickness).   The value of the Relief Ratio must be between 0.05 and 2.0. The higher the value, the larger the size of the relief cut added during insertion of bends.  Once the base flange feature is created, this setting will be available by editing the Sheet Metal feature in the FeatureManager design tree.

Obround Auto Relief

Obround Auto Relief

If a partial edge flange is added to a base flange with the “Material Inside” option selected under “Flange Position” then SolidWorks will apply the specified relief cuts so that the bend can be correctly created.  When creating an Edge Flange feature, the Auto Relief settings that were previously set in the Sheet Metal feature can be overridden by checking “Custom Relief Type”.

Tear Auto Relief

Tear Auto Relief

The Auto Relief settings do not have any impact on the corner treatment of the sheet metal part.

 

Corner Relief

Corner Reliefs can be added to a sheet metal part from within the part’s flattened state.  With the flat pattern activated select Insert > Sheet Metal > Corner Trim or select it from the Corner button on the Command Manager Toolbar.  Individual corners can be selected or “Collect all corners” can be used.

Rectangular Corner Relief

There are three corner relief types available, Circular, Square and Bend Waist.  Selecting “Centered on bend lines” for either the Circular or Square reliefs will position the cut over the center of the bend.  The size of the relief cut can be set as either a set dimension or as a ratio to the material thickness.

Circular Corner Relief

Circular Corner Relief

Applying a corner relief under the Corner-Trim command will only apply the feature within the flat pattern, the corner treatment will not be visible on the formed part in SolidWorks.

Corner Treatments On Flat Pattern

Corner Treatments On Flat Pattern

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Andrew Lidstone, CSWE

Andrew is a SOLIDWORKS Elite Applications Engineer and is based in our Dartmouth, Nova Scotia office.