In my previous post I explained how to create a table driven punch tool with the ability to add many different punch sizes.
By Default the punch is assigned a Punch ID number, which can be referenced in the drawing as a Punch Note.
Customising the Punch Note can add intelligence to that note and make annotation a breeze.
Open the iFeature (IDE) file to add more sizes
(with a sheet-metal IPT file open) Inventor Application Menu > Manage > View iFeature Catalog
Double Click on the IDE file previously created.
Select Edit Using Spread Sheet, this is where the Punch ID can be customised.
When the spread sheet is open, carry out the following;
Remove the “mm” string from Columns A, B & C
Create a formula under the PunchID column as follows;
This formula takes the values from columns A, B & C along with the text contained in “ ” to make a PunchID text string that reflects the size of the Punch.
This Column (PunchID) will be read by the Punch Notes tool in the drawing environment to create correct annotation of the punch.
Copy the Row to create as many sizes of the Punch as needed, editing the numbers in columns A, B & C as needed.
Save and Close the Excel Spread Sheet
Click on the iFeature Author Table to observe the iFeature Table
Click on “Verify” and the cells should revert from the red colour back to the default
Save and Close the IDE File.
Go ahead and use this punch in your sheet-metal part, create several sizes for comparison.
Next, create the Flat Pattern by clicking on the Create Flat Pattern icon
If you selected a simplified representation sketch during the authoring process you are able to represent the Punches as 2D Sketches on the flat pattern.
Right Mouse Button Click on the area around the flat pattern and select Edit Flat Pattern Definition.
Choose 2D Sketch Rep and Center Mark from the list on the Punch Representation TAB, then click OK
The flat pattern might look something like this.
Now that the sheet metal part includes the punch features lets create a drawing of the flat pattern.
Save and Close the Sheet Metal IPT, and create a new drawing (DWG or IDW)
Place a view of the IPT file and select the Flat Pattern view. Use the Punch Note tool to place notes associated with the sketch of the punch.
Notice how the punch direction and punch angle are part of the note by default.
To change this default behaviour, Edit the Dimension Style by Right Mouse Button clicking the note and select Edit the Dimension Style.
In this example the Punch ID <ID> (This is the data Concatenated earlier in the excel spreadsheet) is the only item left in the punch note.
With the customised punch notes in place, Save the drawing file.
You may also be interested in supplying the drawing as a DXF file.
Inventor Application Menu > Save As > Save Copy As
Make sure the save as type option has DXF selected