Creating a punch tool

What's New: 2026

Punch tools are iFeatures created specifically for piercing or deforming sheet metal faces. Punch tool iFeature sketches have a specific creation requirement that separates them from standard iFeatures.

Creating a new punch tool feature, without using a pre-existing feature

  1. On a solid planar face with no other features, create a new sketch. This sketch is referred to as the punch placement sketch.

  2. Delete the sketch center point. This is important as punch tool iFeatures can have only one center point, used for placing the iFeature.

  3. Using sketch geometry, define the punch shape.

  4. Add a center point center point at the location you want to use for placing the iFeature. This is referred to as the placement point.

  5. Click Finish Sketch Finish Sketch.

  6. Use the intended feature creation tool, such as extrude-cut, emboss, etc. to create the feature.

    Note: You can define alternative sketch representations that Inventor displays to represent the punch tool when viewing the sheet metal part as a flat pattern.

  7. Continue with Creating a punch tool iFeature, below.

Using a pre-existing feature to create a punch tool feature

  1. Start a new part.
  2. Open the part containing the feature you want to have as a punch tool iFeature.
  3. Copy the feature from the existing part and paste it into the new part. This step prevents the pre-existing feature from being modified.
  4. Edit the feature sketch and eliminate extra center points other than the one to use as a placement point. If no center point exists, add one in the placement point location.
  5. Click Finish Sketch to exit the Sketch environment and update the feature.
  6. Continue with Creating a punch tool iFeature, below.

Creating a punch tool iFeature

  1. In the model browser, select the feature you just created.

    Note: You can use existing features for iFeatures. If you do, remember valid punch tools can have only one center point in the punch placement sketch.

  2. On the ribbon, click the Manage tab Author panel Extract iFeature .

  3. In the Extract iFeature dialog, select the Sheet Metal Punch iFeature option.

    If the center mark error message displays, there is an issue with the number of center points in the feature sketch, either none or too many. Resolve the issue and then create the punch iFeature.

  4. A default name is provided, right-click the name and click Rename and enter the desired name. Do not use spaces or special characters in the name. The feature name is included in the parameter name, and sometimes in equations when placing the iFeature.

  5. In the Model Browser, select one or more sketched features to extract. To extract all of the features in a part, select the base feature.

Base feature selection includes any geometrically dependent features. To delete features, use the Extract iFeature dialog box.

  1. In the Selected Feature list, double-click any parameter you want to be available to change when placing the iFeature. Or, select a parameter and click Add Add to copy it into the Size Parameters list. Add as many parameters as needed to define the iFeature when placed. Use Remove Remove to exclude parameters from the Size Parameter list.

  2. Optionally, in the Size Parameters list, click a field to modify the value for the selected parameter. The parameters and prompt are used when placing the iFeature in a model.

    • Name. Appears in the browser when you place the iFeature.
    • Value. The current value is the default. The Limit parameter restricts the new value.
    • Limit. A Drop-down menu that restricts entries in the Value box and has three options:
      • None. Places no restrictions on the parameter value.
      • Range. Lets you specify minimum and maximum values, including less than equal to, and infinity symbols. In the Minimum field, negative values allow the placed iFeature to change the depth direction or position of a sketch curve relative to an edge.
      • List. Displays values that you paste from the Clipboard or enter.
    • Prompt. Enter the text prompt that will display when the iFeature is placed on a part.

  3. Optionally, in the Position Geometry list, modify the name or prompt used for the geometry.

  4. In Manufacturing group, click in the Punch ID field to specify the punch ID if needed.

  5. Optionally, for Depth enter a Custom value, if needed. This should be defined after other size parameters.

  6. If using a simplified representation, click Select Sketch and, in the model browser, expand the iFeature node and select the sketch used to define the iFeature. Or, click any unconsumed sketch, with a single unconsumed center mark defined, that was created to simplify your punch feature in the flat pattern.

    Note: If you attempt to save a sheet metal punch iFeature without a center mark, an error message advises you to edit the sketch to add the center mark.

  7. If the iFeature will unfold for the flat pattern, select the Unfold in Flat Pattern option.

  8. Click Save.

  9. In the Save As dialog, the default folder location is the installed Catalog path. To save elsewhere, navigate to the desired folder and save the file for use with the Punch Tool command.

Parent page: About Punch Tools for Sheet Metal