Defining a Punch Tool in Inventor R5

by Elise Moss

This is an excerpt from Inventor R5 Fundamentals: Conquering the Rubicon, available from Schroff Development Corporation <www.sdcacad.com>, reprinted by permission.

File: New Sheet Metal Part using inches

Estimated Time: 15 minutes

This exercise reviews the following tools:

• Create iFeature

• Rotate

• Modifying Dimension

Create a sketch of a rectangle that is 10 x 6 units.

In this case, we will create a punch for an IEC320 cutout. An IEC320 is an industry standard power connector. You can look on the back of your computer's tower case and find what the connector looks like.

Create the sketch shown. (This is a cut-out pattern for a panel cutout for an IEC320 female power connecter.) 

Use a coincident constraint between the vertical center line and the circle. We only put ONE circle center point for our punch tool because Inventor only allows a single hole defined for each punch tool. 

You do not need to locate this sketch precisely on the metal because this is going to be converted to a punch tool.

Highlight the IEC320 cut in the browser and select the ‘Create iFeature’ tool.

Select the 0.140 dimension.  

Press the Insert Arrow to add it as a Size Parameter. Change the Prompt to read ‘Enter Hole Diameter’.

Select the 1.570 dimension. 

Press the Insert Arrow to add it as a Size Parameter. Change the Prompt to read ‘Enter Distance Between Holes’.

Select the 0.160 dimension. 

Press the Insert Arrow to add it as a Size Parameter. Change the Prompt to read ‘Enter Fillet Radius’.

Select the 0.980 dimension.

Press the Insert Arrow to add it as a Size Parameter. Change the Prompt to read ‘Enter Width’.

Select the 1.280 dimension.

Press the Insert Arrow to add it as a Size Parameter. Change the Prompt to read ‘Enter Length’.

Press ‘Save’.

Locate the file away from Inventor in your work folder.

Save the file as ‘iec320-fem’. Press ‘Save’.

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