Sheet Metal Punch Tool with a Flange

[Anonymous]

Hi,

I am trying to make a punch tool in inventor for sheet metal. I noticed that for the features I could not select faces or flanges I did. I know you can extrude the same shape to get the same result but I wanted to use a face/flange so that I can retain the flat development. What is the best way around this.

To get a sense of what I am trying to make:
-square cut out
-on the bottom edge of the square I made a face that is angled at 45 degrees

It would be closest to a louver tool.

Thank you in advance for any help.

[mcgyvr]

use extrude.. I don't believe faces/flanges are supported.. The part should still flatten properly though.

[Anonymous]

mcgyvr thanks for your response!

I just tried to extrude but it doesn't flatten. I attached an example file. I used the same sketch I did for the extrusion and made a sheet metal face and it flattens properly. You can suppress the extrude and unsupress the face to try it out.

Thank you in advance for your help.

[mcgyvr · Accepted solution]

I should have said "if done properly" the extrusion will flatten.. You do not have a bend radius on that extrusion. Nor bend reliefs.. It flattens just fine then.

What version of Inventor do you have?

[Anonymous]

I have Inventor 2011, I have not added bend radius or bend reliefs to an extrusions before. When I have time I will have to look into it, if you can point me in the right direct or give me an example that would be great. Thanks for the info so far mcgyvr.

[mcgyvr · Accepted solution]

I'll give you a big hint since I don't have 2011 I can't provide the file except in step format.. (see attached) Simply place a sketch like that in the middle plane of your cutout with your extrusion having an inner radius of whatever your forming die has then an outer radius that equals inner rad+Thickness and extrude both directions. Then it will flatten. There are other ways but this is what I would do.

[Anonymous]

Hi mcgyvr,

Thanks for the tip on extruding a sheet metal flange, didn't know that was possible.

I was able to extrude a flange at an angle and I was successful in flattening the part. However, when I try to extract the iFeature, Inventor will not let me select the extrusion. When I try to select the extrusion Inventor states: "Objects taht are not supported by iFeatures will be removed from the selection."

I attached a new file that I made the extrusion which flattens, but does not let me select it as an iFeature.

I apologize if I am doing any of the steps wrong, I am new to using an exrusion as a sheet metal flange, and I am new to making an iFeature punch.

Thanks in advance for any input mcgyvr.

[JDMather · Accepted solution]

You will have to be very carefull about parent-child relationships.
Do not create the Punch tool in a way that any features will be depent on a parent that is not part or the punch.
Do not use Projected Loops.

Use variable names like Thickness or BendRadius for all dimensions.