The feature failed to cut the body

[Lapuo]

I opened file and after CTRL+Q feature tree is red and yellow.
First error is with cut extrude option and it says "the feature cant cut the body" .
I cant add any new features because of same error.
Same file on another PC - no errors
Any ideas what went wrong?
Pc's have same confogurations and same SW settings.
SW 20221 SP3

[SPerman]

Try flipping the direction. The arrow indicating cut direction is pointed away from the body.

image.png (7.72 KiB) Viewed 6141 times

[bnemec]

Try flipping the direction. The arrow indicating cut direction is pointed away from the body.



image.png

... because in these terribly ambiguous situations that is the most helpful direction to cut.

[Lapuo]

Sketch is on the other side (face which is not visible)so direction is ok.
Anyhow it does not work in any direction no matter what depth i choose.

[AlexLachance]

remove "link to thickness" and select "through all".

Should fix your issue IMO

[Lapuo]

I tried , with all possible options.
I tried to recreate feature.
SW says NO

[AlexLachance]

Oh, excuse me, I hadn't read that it works on one PC and doesn't on another.

Have you tried resetting the SolidWorks registry and then reloading SolidWorks settings?

[Lapuo]

Yeah i probably should.
Not me , but my IT

[AlexLachance]

Yeah i probably should.
Not me , but my IT

Alin, or Javelin Tech, has a very nice summary of how to process, if you ever feel like doing it yourself.

https://www.javelin-tech.com/blog/2019/ ... -registry/

If that doesn't work, I'd look to see if you're running the same driver for your graphic card. Perhaps you have a faulty driver and the other one has the approved one.

[SPerman]

Oh, excuse me, I hadn't read that it works on one PC and doesn't on another.

Have you tried resetting the SolidWorks registry and then reloading SolidWorks settings?

I missed that as well. My only suggestion would be to reach out to your VAR.

[bnemec]

Oh, excuse me, I hadn't read that it works on one PC and doesn't on another.

Have you tried resetting the SolidWorks registry and then reloading SolidWorks settings?

I missed as well. It's just habit to assume that SW flipped the cut direction.

On the problem PC, can you try logging in as a different windows user? When the behavior seems to be local to one PC I ask that user to test same thing on another PC and the user from a PC that doesn't replicate the problem to try it on the problem PC. Then I know if it's the user's roaming profile or PC.

[RichGergely]

Has one computer got verification on rebuild active and the other doesn't?

[Lapuo]

Has one computer got verification on rebuild active and the other doesn't?

As i said , all settings are the same.
PC is same.
Driver is same.

We will try to reset settings (i dont have any permissions , so that is why IT must), and probably we will contact our VAR

[zxys001]

Are you sure the sketch is closed? As a test, try to extrude it.

[AlexLachance]

Are you sure the sketch is closed? As a test, try to extrude it.

I can vouch it's closed. Sketch lines do not have the same thickness for open profiles. They become "as thick" as construction lines.

[Lapuo]

I can vouch it's closed. Sketch lines do not have the same thickness for open profiles. They become "as thick" as construction lines.

Yes , and i dont believe it would work on another PC if sketch is open

[SPerman]

I don't do much sheet metal work, so these are just guesses. Is there an add-in that could be missing from one computer? Or a feature that isn't turned on?

[Ömür Tokman]

have you tried normal cut?

[Lapuo]

have you tried normal cut?
2022-06-03_14-38-14.png

Yes.
Unfortunately it wont work.
Biggest suprise to me is why this part is loaded normally at PC's of my colleague who have exactly same settings as me, and on my PC it shows red feature tree.

[AlexLachance]

Yes.
Unfortunately it wont work.
Biggest suprise to me is why this part is loaded normally at PC's of my colleague who have exactly same settings as me, and on my PC it shows red feature tree.

Have you tried @bnemec's suggestion of trying on your PC with a different user then yours..?

[Lapuo]

I tried , and no success

[bradb]

Been following this to see what the outcome is. I'm not an IT guy put this is my $.02.If you have logged into the other users PC as you and it works, has the other user logged into your PC as themself and what is the outcome? If it works on yours with the other user logged in there is something in the settings. If it doesn't work there is something in the registry.

I also assume your IT dept has given you the standard reply of "have you tried rebooting it" to get it to work.

Seriously though, this is my biggest complaint with this, the software knows there is a problem preventing a function but won't to tell me what or where it is so I can attempt to fix it.

[Lapuo]

Been following this to see what the outcome is. I'm not an IT guy put this is my $.02.If you have logged into the other users PC as you and it works, has the other user logged into your PC as themself and what is the outcome? If it works on yours with the other user logged in there is something in the settings. If it doesn't work there is something in the registry.

I also assume your IT dept has given you the standard reply of "have you tried rebooting it" to get it to work.

Seriously though, this is my biggest complaint with this, the software knows there is a problem preventing a function but won't to tell me what or where it is so I can attempt to fix it.

So , i tried to log in on another PC and it works.
On my PC it does not work (with different users)
You are right about IT , and i gave up because i recreated part from scratch.
I am leaving company (and this kind of job) at the end of this week , so , to be honest , it does not matter to me anymore.

[zxys001]

So , i tried to log in on another PC and it works.
On my PC it does not work (with different users)
You are right about IT , and i gave up because i recreated part from scratch.
I am leaving company (and this kind of job) at the end of this week , so , to be honest , it does not matter to me anymore.

Hi Lapuo,
Just to confirm (again) is/was the "verification on rebuild" option on your and the other computer turned on (see image).

[DanPihlaja]

Hi Lapuo,
Just to confirm (again) is/was the "verification on rebuild" option on your and the other computer turned on (see image).

That is a great question. I forgot about that and remember an issue from old where that effected different people.

Again! I wish that this check box was checked by default!

[Lapuo]

Good point,but It is checked on both computers.

[Lapuo]

So , i found something interesting.
When i supressed one of the features (closed corner) everything worked - all errors were "fixed" and i could recreate new ones.
I tried to edit feature , and i noticed that gap was 0.01 mm. After i changed it to 0.1mm everything worked.

0.01 is still a gap but when it is so small than corner is overlapping and i guess that was reason why this body was not valid to SW.

Still does not explain why everything is working at another pc, but i am little bit happy i found something.
Maybe until end of the week we can see what the route of the problem is

[DanPihlaja]

So , i found something interesting.
When i supressed one of the features (closed corner) everything worked - all errors were "fixed" and i could recreate new ones.
I tried to edit feature , and i noticed that gap was 0.01 mm. After i changed it to 0.1mm everything worked.
image.png

0.01 is still a gap but when it is so small than corner is overlapping and i guess that was reason why this body was not valid to SW.
image.png

Still does not explain why everything is working at another pc, but i am little bit happy i found something.
Maybe until end of the week we can see what the route of the problem is

Run a check on the part:

And see what you get for invalid stuff.

[zxys001]

So , i found something interesting.
When i supressed one of the features (closed corner) everything worked - all errors were "fixed" and i could recreate new ones.
I tried to edit feature , and i noticed that gap was 0.01 mm. After i changed it to 0.1mm everything worked.
image.png

0.01 is still a gap but when it is so small than corner is overlapping and i guess that was reason why this body was not valid to SW.
image.png

Still does not explain why everything is working at another pc, but i am little bit happy i found something.
Maybe until end of the week we can see what the route of the problem is

Glad you found the something, that overlap is imho the problem which triggers the other .01mm to fault.
As @DanPihlaja shows there are ways also to do detailed checking.
It is odd that the other computer does not do this though.
Short edges and close vertices also have issues... sheetmetal does some strange transitions so also look at the settings for rips?

[bradb]

Going back to the works on one but not the other almost makes me think there is a system accuracy / tolerance / limit setting someplace that's causing it. Long ago we used to run into that with files from different CAD systems.

[bnemec]

Going back to the works on one but not the other almost makes me think there is a system accuracy / tolerance / limit setting someplace that's causing it. Long ago we used to run into that with files from different CAD systems.

Save your SW user settings and then:

https://www.javelin-tech.com/blog/2019/ ... -registry/