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 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 unflatten the sheet metal part, it will break the way the SOLIDWORKS drawing file views the flattened state. 

Solution 1: Correcting the flattened configuration

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

1) Open the part file within SOLIDWORKS

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

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 palette 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 part's 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 palette 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 rename 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 palette. 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.