Contour Flange in NX Sheet Metal

The contour flange is created on a sketch or path for creating the first base feature or secondary feature on the sheet metal. You can create sheet metal features by extruding sketch curves with a specified width. Bends are created on the sharp connections of the sketch curves. The “Contour Flange” command is used for this operation.

The Contour Flange location in NX Sheet Metal modeling

• Home Ribbon Bar => Base Group => Flange Drop-Down => “Contour Flange”
• Menu => Insert => Bend => “Contour Flange”
• Shortcut= U

Creating a main base feature by using the “Contour Flange” command:

1. Create a sketch and draw contour curves.
2. Start the “Contour Flange” command.
3. The “Contour Flange” command dialog box will open.
4. Select Curve” in the “Section” group is highlighted automatically.
   1. Select an existing sketch or curves.
   2. You can create a sketch when the “Contour Flange” command is active. Click on the “Sketch Section” icon in the dialog box to create a sketch to use in the “Contour Flange” command.
5. The preview will appear in the graphics window.
6. Check the thickness value in the “Thickness” group.
7. If you want to change the sheet metal thickness side, click on the “Reverse Direction” icon in the “Thickness” group.
8. Extrude the sheet metal by using the “Width” group. There are two width options in this group.
   1. Finite: extrudes flange at a specified width length which starts at the selected sketch.
      Specify width size by typing the width value in the dialog box or by dragging the width arrow in the graphics window.
      Change the width direction by clicking the “Reverse Direction” icon or by twice clicking to the width arrow in the graphics window.
   2. Symmetric: Extrudes the sketch in symmetric directions.
      Set the width value.
9. Click the “Ok” button to create a contour flange and close the command.

You can create contour flanges on the edge of the existing sheet metal edges.

To create flanges on the sheet metal edges by using the “Contour Flange” command:

1. Start the “Contour Flange” command.
2. The “Contour Flange” command dialog box will open.
   The contour flange method will be set as “Secondary” automatically because created sheet metal features are existing in the model such as tab
3. The “Select Curve” in the dialog box is highlighted automatically.
   Select an edge to create a sketch on it. The sketch plane will be perpendicular to the selected edge.
4. The Sketch command dialog box will open.
   Define the sketch location on the edge and orientation.
   Click “Ok”
5. The sketch application will be opened.
   The sketch origin will be the selected edge in step 3.
   Draw the contour flange section.
   Important Note: The contour flange section starting point must be at the sketch origin (selected edge at step 3)
6. Exit from the sketch.
7. Set the width option.
   1. Finite
   2. Symmetric
   3. To End
   4. Chain
8. I will create a flange on three edges of the tab. That’s because I select the “Chain” width option.
9. The “Select Edge” bar will be highlighted automatically after you select the “Chain” option.
   Select edges to create flanges on them.
10. The Preview will be shown in the graphics window.
11. Click the “Ok” button to create a contour flange and exit from the command.

Note 1:  If you can not create a contour flange and an alert box appears as “Failed to create a preview. Verify inputs.”, change the flange direction by clicking the flange direction arrow in the graphics window.