The dreaded "The attempted operation did not produce a meaningful result"

[johnPGNFG]

Would anybody like to take a look at this part and see if they can figure out the cause of this error?  If you edit any feature, then click "ok" (even without changing anything on the feature), you'll get the error.  There's some problem with updating the flat pattern.  If I delete the flat pattern and recreate it, this problem goes away.  If these were my own parts, I would recreate the flat pattern, carry on, and leave it to "Only the Inventor gods know what was causing that error."  The problem is, these parts aren't mine. I wrote a plugin for some others that export parts out of inventor into a different software.  When the code analyzes the part, it has to modify the part(same effect as editing a feature), thus causing the code to crash.  I need some way to check the part for the error but I need to know what is causing it first.  I'm using version 2023  

[kacper.suchomski · Accepted solution]

Hi

In version 2024, the problem is fixed. There is no error message.

But the reason lies in the wrong design method.

The base should be made using Contour Flange, not Extrude. Then there would be no problem, because the zero radius can be defined in this tool. And now Inventor doesn't understand radius 0 because it's not officially defined in the feature, it's just a result of forcing the sketch.

[Curtis_Waguespack]

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@johnPGNFG wrote:

  I need some way to check the part for the error but I need to know what is causing it first.  I'm using version 2023  

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Hi @johnPGNFG,

Does your plugin save the file after it does it thing? If not you could it delete the flat pattern with code after opening it, then do your magic, and then close the file without saving changes.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Frederick_Law · Accepted solution]

k = 0.001

Bend rad = 0

Someone didn't know how to setup sheet metal and cheating dimension to get what they want?

[johnPGNFG]

I do not save but I do look at sketches created on the flat pattern to see if there are any textblocks or sketchlines visible.  If there are some that exist, these would be exported as "etch" operations.  So, if I delete the flat pattern, the sketches created on the flat pattern go with it.

Last resort is to check the flat pattern for these "etch" operations, delete the flat pattern, recreate it, then once exported, if the part had "etch" operations, let the user know some elements disappeared.

[Curtis_Waguespack · Accepted solution]

Hi @johnPGNFG 

I think @Frederick_Law  has the answer. I changed the Bend Radius to 0.01 and it fixed the error, but the flat is not correct.

Your code might just need to check the BendRadius to make sure it is not zero, etc.

[johnPGNFG]

@kacper.suchomski  @Frederick_Law @Curtis_Waguespack 

Thanks guys, that clears it up.  I'll delete and recreate the flat pattern in the code and alert the user that they programmed their part with a 0 bend radius.

I appreciate the help!

[kacper.suchomski]

Zero bend radius has been possible in Inventor for several years.
The important thing is that you define it so that Inventor can work with it.
You can design such a geometry, but you have to do it with sheet metal tools, not with Extrude, as I mentioned in the first comment.
Another thing is that such geometry is unlikely in reality, and the model should be adapted to the production technology, as @Frederick_Law  mentioned.

[Frederick_Law]

Zero Bend Radius:

Let me know when Inventor can make ZPM.

[kacper.suchomski]

@Frederick_Law , Od kilku lat

Edit: You are right, it is made with minimal cosmetic value.

[Curtis_Waguespack]

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@kacper.suchomski wrote:

You can design such a geometry, but you have to do it with sheet metal tools, not with Extrude, as I mentioned in the first comment.

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@kacper.suchomski,

Using extrude and bend is not the best practice, but it is not technically wrong, and it can work if the bend radius and Kfactor are set correctly. See the attached version of this part which flattens correctly.

[Curtis_Waguespack]

@johnPGNFG 

This might worth looking at also:

https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/flat-pattern-export-check/m-p/673071...