general errors with part

[AnthonyHarris90842]

I have this tube that was derived from a multi body part.
I Have attached the model and the drawing.
The part wont allow me to extrude as per the image attached and get rid of the countersunk holes as I thought that might be the problem with the part.
I tried converting it to a sheet metal part and it wont flatten.
I did a drawing of it and there is a problem with it trying to section. See image.
Could it be a modeling error or a software glitch.

[SBix26]

I don't know what the problem is with the file.  But I tried using Delete Face with Heal to remove the holes (very easy to use window select with Delete Face), and this "fixed" the file.  After the Delete Face operation, the model could be converted to sheet metal and generates a flat pattern easily, as well as a section view in a drawing.

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Sam B
Inventor Pro 2022.1 | Windows 10 Home 20H2
LinkedIn

[johnsonshiue]

Hi Anthony,

The tube may look Ok but the data is very poor. You can press Ctrl+F7 to check the body sanity. Quite a few face loop issues are reported.

To repair the body, go to Modify section -> expand the panel -> Copy Object -> pick the solid body -> copy it to Repair Environment. After that, enter the environment -> Find Errors -> Heal Errors.

After that, the body will be healthy.

Convert it to sheet metal (Thickness = 6mm). And, the flat pattern can be made.

Many thanks!

[AnthonyHarris90842]

Hi Johnson

I did what you said and it healed the part.
I still cant get a flat pattern as it says flat patterns don't work on multi body parts. I attached the part again.
Also my question is that it is not a very complex part and why would Inventor generate a part with so many errors then in the first place.
I attached the base part from where it is derived and maybe you can trace a reason for such a bad part.
Thank you so much for your help

[AnthonyHarris90842]

Hi Sbix26

But I dont want the holes removed.
Also again why does Inventor generate such a bad part

[AnthonyHarris90842]

Hi Johnson

I just picked up that the healed body is 4mm longer than the original.
I then had to move face to return it to it original length
Why would that happen?

Part attached

[JDMather]

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@AnthonyHarris90842 wrote:

Also again why does Inventor generate such a bad part

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Sheet metal part Attached.

[johnsonshiue]

Hi Anthony,

Flat Pattern is only supported in a sheet metal part with only one single solid body. When there are multiple solid bodies, Flat Pattern cannot be created. You will need to use Make Components to push individual solids to individual parts. Then create flat pattern there.

My proposed workflow was to copy the body -> Heal Errors -> delete the original body.

Many thanks!

[johnsonshiue]

Hi Anthony,

It looks like the added length may have come from the original derive part after the update.

Many thanks!

[AnthonyHarris90842]

Ok if I delete the original body then the healed body doesnt update when I change the master multi body part that its derived from?

[AnthonyHarris90842]

Hi JD

I can do a part like this on its own but my modeling starts with a multi body part where this part was derived from.
Also I opened your part and then ran through the steps and it gives an error at Rectangular pattern 2

[AnthonyHarris90842]

Hi Johnson
That weird as I didn't change the part at all.
Just trying to get it to behave the way its supposed to.
Anyway I sent you the original multi body part.
Were you able to find out why Inventor generated such a bad part?

[JDMather]

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@AnthonyHarris90842 wrote:
Hi JD

I can do a part like this on its own but my modeling starts with a multi body part where this part was derived from.
Also I opened your part and then ran through the steps and it gives an error at Rectangular pattern 2

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I guess the lesson here is for the most robust sheet metal - create as sheet metal.

I am not getting error that you report - can you show Screencast or at least screen shot of the error?

Also, are you aware that in your original design you do not have the holes at 25mm from the edge?

(Not sure if this was intended or an oversight.)

[johnsonshiue]

Hi Anthony,

Could you tell me which part is the original derive source part?

Many thanks!

[AnthonyHarris90842]

Cage master

[AnthonyHarris90842]

The 25 is intentional.

[johnsonshiue · Accepted solution]

Hi Anthony,

Many thanks for sharing the info! I took a quick look. The bad body in CAGE MASTER.ipt is actually caused by Chamfer5, Preserve All Features option. If it is turned off, the body will check good. This is a bug for sure. I will follow up with the project team. But, for geometry specific issue like this, it will be hard to find a good solution.

Thanks again!

[AnthonyHarris90842]

Ok so Inventor is the problem here.
I hope you and your team can get it fixed.
Thank you very much for all your trouble