Derive not working as expected

[DavidTunnard]

Hi all.

Can't get the derive function to work as expected. Doesn't seem to be working like it used to. Im trying to subtract the blocks to leave me with the mould in the centre but it keeps coming up with errors or leaving chunks of material in the model. Please see pictures. The material left from the holes is fine, its the large chunks of material that is the problem.

Any help appreciated.

[mechielvanvalen]

In my Inventor i don't have the red dot in the status. If you set it on the yellow dots can you place you're block?

[DavidTunnard]

No. If you leave them as yellow then they will be kept as part of the new part.

I want to subtract all but one (the epoxy model) form the part.

[SBix26]

Post your data set.  It's nearly impossible to diagnose without the files.

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Sam B
Inventor Pro 2021.1.1 | Windows 10 Home 2004
LinkedIn

[j.palmeL29YX]

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@mechielvanvalen wrote:

In my Inventor i don't have the red dot in the status.

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You must not use the derive style of the third button.

>>example<<

[j.palmeL29YX]

The cylinder and the blocks end at the same plane (theoretically). This may cause problems (only a guessing). If you increase the length of the cylinder a little, do you get a better result?

[DavidTunnard]

sure, see attached

[DavidTunnard]

Good suggestion, but I just tried extending the cylinder another 10mm away from the block at both ends and I get the same result unfortunately.

[mechielvanvalen · Accepted solution]

Is this what you need? 

I made a shrinkwrap from you're assembly and loaded in to the expoxy model as a derived part.

Then i used the combine tool to make the mould blok as one solid body, and used the combined feature again to get the form in the epoxy model.

[mechielvanvalen]

i changed the circel to a rectangle, see result

 

[johnsonshiue · Accepted solution]

Hi! I think there is a geometry specific Derive Boolean bug here. Somehow the order of performing the Boolean matters. Here is a simple workaround without changing any geometry.

1) Derive the assembly as a multi-solid body part.

2) Combine -> pick the cylinder as the base body -> pick the blocks as tools -> Cut.

It will work.

Many thanks!

[DavidTunnard]

I just tried this method but it did not work for me. It left me with square blocks of material at either end again. Strange. I've never had this problem before. Only on the 2021 release.

[DavidTunnard]

Yes! This workflow works! I think I would go with @mechielvanvalen  Shrinkwrap method though as the  I can keep the epoxy model as a separate part from the multibody part file of the mould blocks. 

Either way the key is to use the combine feature and not the derive feature.

Thanks for the help everyone. Really appreciate it!

[johnsonshiue]

Hi David,

Do you have a set of older files showing that it worked before but fails now? I tried using the assembly you attached here on prior releases (2016 to 2021) via STEP roundtripping. They all work including 2021. Something seems to be specific to this 2021 files. If you have example showing pass success, please send it to me directly johnson.shiue@autodesk.com. It may be a regression defect.

Many thanks!

[david.tunnard]

HI John,

Yes OK. Will send some over when I get some time.

The only thing I can think That I have done differently in this data set is that all the mould blocks were modelled as a multibody part. Previously I think I have modelled one half, and then either taken that part file into an assembly or derived it and made necessary changes to the mirrored half. Then I'd assemble them all together and do the final derive/cut operation.