Flat Pattern Failure

[rttechno]

Hi Everyone,

This is a new one for me.  Take a look at the flat pattern on the attached part.  Anyone have any idea why this is happening?  Deleting and recreating the flat doesn't change it.  You can't select any of the main faces as "A-Side".  For now I'll try recreating it from scratch since it's a simple part but this is odd...

FlatFolded

Thanks,

Randy

RT Technologies

Inventor 2018.3

Windows 10 Pro 1803

Intel Core i7-8700K

32GB RAM

2x GTX 980ti

[mcgyvr]

You seem to have some ilogic happening there..

I'm not sure why you are concerned about a flat pattern in a flat part?

Yes there is an error/problems.. they may have been created because of the ilogic (that we don't have)

[rttechno]

Hi mcgyver,

The ilogic would trigger flat pattern creation in the file but this issue happens even if I create it using the button on the ribbon.  I need a flat pattern to allow automated export of the dxf.  This is the only file out of about 500 sheet metal parts in this machine that did this.

Thanks,

Randy

[jletcher]

I always need flat patterns for laser, blank size, and extra to material to be machined off.

Many many reason.

[jletcher]

I deleted your flat pattern did a rebuild and suppressed your rule on flat pattern.

Made flat and it works.

[rttechno]

Hi jletcher,

I figured out how to stop it from happening here.  Really really odd situation.  If I change the large rad at the top of the part it flattens correctly.  It looks like Inventor was seeing that top arc as flat with a bend in it.  Can anyone else reproduce that?

This dim is same as thicknessResults in this flat pattern. It sees that as the thickness.Changed the .5 top rad to .53125.Get this error. It thinks I messed with the thickness of the sheet.Delete the failed flat pattern and recreate and it works now. If I reverse the steps it faills again. Repeatable for me.

Sure looks like a bug to me.

Thanks,

Randy

[dgleis]

I opened your part, deleted the flat pattern, selected a face and created flat pattern and it worked fine.

[rttechno]

Hi dgleis,

Did you select face and export face as or select a face and hit create flat pattern?  Can you try it without selecting a face?  Based on the behaviour on my machine I'm thinking the intelligence that automatically selects the face is fooled by my arc that is the same thickness as "Thickness".  Selecting a face first may circumvent that bit of code.

Thanks,

Randy

[dgleis]

I just selected a face and clicked create flat pattern.

[TheCADWhisperer]

Is there a logical reason why you modeled as two Face features rather than as a single Face feature?

[rttechno]

Yeah, adding features as I go along.  Sometimes I make one sketch that the whole part is based off of and other times I add features as I progress.

Thanks,

Randy

[rttechno]

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@dgleiswrote:

I just selected a face and clicked create flat pattern.

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What happens if you don't select a face first?  Do you get the same error as me?

Thanks,

Randy

[TheCADWhisperer]

If I try to imagine that I am a dumb software program trying to do exactly what the designer wants - if I could think, I would be thinking, "There are two Face features, so logically the designer must be intending a Bend feature somewhere."  Unfortunately I am getting confused as to where there could be a Bend with these two Face features.

I think if you create as a single Face feature when there are no Bends, that the software will be less confused.

[dgleis]

If i don't select a face, I get the same jumbled mess you had.

[rttechno]

@TheCADWhispererwrote:

If I try to imagine that I am a dumb software program trying to do exactly what the designer wants - if I could think, I would be thinking, "There are two Face features, so logically the designer must be intending a Bend feature somewhere."  Unfortunately I am getting confused as to where there could be a Bend with these two Face features.

I think if you create as a single Face feature when there are no Bends, that the software will be less confused.

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I've attached the single face version of the file.  Same issue.  Take a look at the procedure I showed above.  What's confusing it is there is a constant thickness section that matches the "Thickness" parameter perpendicular to the actual "face".  If you alter the .5" outer rad to .53125" the issue goes away and it flat patterns as usual.  Do you never create a second face feature when you model parts?  I have to do that all the time as the part evolves.  I don't change the original sketch I add features so that it's easy to modify or eliminate them independently of the other features in the part.  I've been doing this a while and I've never heard that making a second face feature was problematic.

Thanks,

Randy

[rttechno]

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@dgleiswrote:

If i don't select a face, I get the same jumbled mess you had.

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Ok.  So it must be that the software is thinking that .25" section between the rads is a valid unfold point.  Feel like a bit of a bug I'd say.  Not that there is not a workaround for it but I can't imagine this is intentional behaviour.

Thanks,

Randy

[TheCADWhisperer]

On both parts if I delete your Flat Pattern and then click on the flat face before selecting the Flat Pattern tool - I get a valid Flat Pattern.

[rttechno]

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@TheCADWhispererwrote:

On both parts if I delete your Flat Pattern and then click on the flat face before selecting the Flat Pattern tool - I get a valid Flat Pattern.

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Yes.  That will bypass the portion of the create flat pattern code that automatically selects a face if none is selected.  What I'm saying is that there is a bug in the automatic face selection portion of the code.  I know there are many cases where it is advantageous to manually select that face but my workflow is such that the advantages of manual selection aren't worth the time it takes.

Thanks,

Randy

[TheCADWhisperer]

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@rttechnowrote:

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advantages of manual selection aren't worth the time it takes.

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Well my experience goes back to a time where it was always necessary to pre-select the face to unfold from, so it is muscle memory to me - an automatic step in the process.

I agree that it should automatically solve this one.  This is a good one for ping @johnsonshiue to take a look at.

[rttechno]

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@TheCADWhispererwrote:

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@rttechnowrote:

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advantages of manual selection aren't worth the time it takes.

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Well my experience goes back to a time where it was always necessary to pre-select the face to unfold from, so it is muscle memory to me - an automatic step in the process.

I agree that it should automatically solve this one.  This is a good one for ping @johnsonshiue to take a look at.

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Ah that makes sense.  We have automated routines that take care of flat pattern creation and a bunch of other menial, easy to forget tasks so if this doesn't work I'm in trouble....  That said, on about a 4-500 part export I think this only happened on the one part so it's a bit of an edge case.  I agree that it would be great for @johnsonshiue to look at it.  At least this one is repeatable.  Usually when I'm dealing with stuff it seems random, or at least hard to repeat (for example the right click issue of last year).  Thanks to everyone who contributed!

Randy