Suppress Feature when activating Flat Pattern

[SunsetDuralite]

Hi,

 I would like Inventor to automatically suppress the Punch 'Dimple' feature when activating Flat Pattern. Is this possible?

[IgorMir]

Hi Jared;

One of the way to do it is to convert that part into iPart and in the second instance suppress the Dimple. Use that child to generate the Flat Pattern.

Cheers,

Igor.

[SunsetDuralite]

Thanks IgorMir, 

What you advised is something i could do without having to make an Ipart by simply right clicking on punch 'dimple' feature and suppressing it.

 I was thinking about some Ilogic Rule to generate the suppression when going to Flat Pattern.

Thanks

[IgorMir]

That will work too, subject - you don't need to create a drawing of the part in the unfolded state.

[johnsonshiue]

Hi! I am not sure if you are aware of the workflow to change Flat Pattern representation? Activate Flat Pattern -> right-click on it -> Edit Flat Pattern Definition -> Punch Representation -> change it to anything but "Formed Punch Features."

You will see the punch tools are removed. Is this what you were looking for?

Many thanks!

[SunsetDuralite]

Thanks johnson shiue

Yes, i want the punch tool removed when going to flat pattern, but, how can i make the 'dimple hole' feature appear in flat state in place of the punch feature?

[Curtis_W]

Hi @SunsetDuralite 

i didn’t look at the other replies so forgive me if this is duplicate info... 

but I recently looked at this workflow and posted some steps here:

https://forums.autodesk.com/t5/inventor-customization/ilogic-for-sheet-metal-gusset-suppression-in-f...

hope that helps,Curtis 

[johnsonshiue · Accepted solution]

Hi! I don't think there is a way to flatten the punch. You can remove it and retain the 2D representation or its center point.

Many thanks!

[SunsetDuralite]

Thank you Johnson,

 The 2D representation is exactly what i was looking for!

[rederle]

Hi, I have a similar issue; I'd like suppress a couple of features (ELIMINA SCHIACCIATURA TERMINALE P1 and P2) from fold part when flat pattern is activated; 

I don't need to put the flat pattern into the drawing and I don't want use ipart to manage that; 

is there a way with some ilogic rule to manage that?I attach the sample

[johnsonshiue]

Hi! As of Inventor 2021, there is only one geometric definition within a part. iPart still requires multiple members (files).

On 2022, Model States allow multiple geometric states to be defined within a part. What you want to do can be easily done on 2022 in one sheet metal ipt file.

Many thanks!

[rederle]

honestly I tried that but it didn't work; I think flat state is linked with all model state that you create

can you do this on my file attached before?