Why does my Sheet Metal Drawing have the wrong Flat Pattern View?

Problem

When creating drawings of sheet metal parts, you may find that the flat-pattern view will instead show a different view of the part.

This issue is caused by the flattened configuration being created by changing by changing the configuration to the FLAT-PATTERN state. Instead, you should enable the flattened configuration by using the flatten tool. While using the improper configuration, if you un-flatten the sheet metal part it will break the way the SOLIDWORKS drawing file views the flatten state. 

Solution 1: Correcting the flatten configuration

Follow the below steps to correct the flat-pattern configuration to properly return to the flatten state

1) Open the part file within SOLIDWORKS

2) Enable the FLAT-PATTERN configuration within the configuration tab (the Flatten tool will likely be un-toggled)

3) If the Flatten tool is un-toggled, re-enable it so the sheet metal returns to the flattened state

4) Toggle back to the Default configuration

5) Open the drawing file and refresh the view pallet to update the flat-pattern view

Solution 2: Creating a new FLAT-PATTERN configuration

If the above steps do not correct the issue, then the FLAT-PATTERN configuration must be re-made in order for the drawing file to properly create a flat-pattern view within the view pallets.

1) Within the configuration tab of the feature manager tree right click the parts name and choose "Add Configuration." Any name for the configuration is okay at this point; it can be renamed later.

2) Enable the new configuration and select the Flatten tool within the Sheet Metal tab, then refresh the view pallet within the SOLIDWORKS drawing file. This will generate a new FLAT-PATTERN configuration for the part within this configuration.

3) Within the configuration tab of the feature manager tree delete the original default configuration by right clicking the configuration name and selecting delete. You can also re-name the newly created configuration to Default if you wish to by modifying the properties of the configuration. 

4) Return to the drawing file of this sheet metal part and refresh the view pallet. The flat-pattern view will return to the flattened state.

For further technical support, please contact Hawk Ridge Systems at 877.266.4469 for the U.S. or 866.587.6803 for Canada and support@hawkridgesys.com.