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Shell Fail on surfaced part
Posted: Sat Oct 09, 2021 2:51 pm
by RCD Machine
Hi all!
I have a project I'm working on for a customer that involves some compound curves that are a little outside my comfort zone. The part has to be shelled as pretty much the last operation, but it fails to shell, giving me the following error:
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Error Shell1 The shell operation failed to complete. One of the faces may offset into an adjacent face, a small face may need to be eliminated, or one of the faces may have a radius of curvature which is smaller than the shell thickness. Please use Tools Check to find the minimum radius of curvature on appropriate faces. If possible, eliminate any unintended small faces or edges.
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I've been beating my head over this one for two days, so it must be something obvious that I'm just missing.
Can someone take a look at this model and suggest what the problem is?
https://1drv.ms/u/s!AtfE2uFNgBOWhxbdFpS ... u?e=88zJhe
THANKS!!!
Re: Shell Fail on surfaced part
Posted: Sat Oct 09, 2021 5:43 pm
by matt
2 things. First, what thickness shell do you want to create?
Second, that lip on the bottom would probably be best placed after the shell.
I was able to shell it with Solid Edge at 0.055".
The tools in Solid Edge say that the tightest curvature is 0.039, so theoretically, that should be where it fails. You might have to use some different tactics like shell before you put the fillets on, or use offset faces to shell manually, or ... there are a bunch of ways to skin that cat.
Re: Shell Fail on surfaced part
Posted: Sat Oct 09, 2021 5:54 pm
by zxys001
RCD Machine wrote: ↑Sat Oct 09, 2021 2:51 pm
Hi all!
I have a project I'm working on for a customer that involves some compound curves that are a little outside my comfort zone. The part has to be shelled as pretty much the last operation, but it fails to shell, giving me the following error:
____________________________________________________________________________________
Error Shell1 The shell operation failed to complete. One of the faces may offset into an adjacent face, a small face may need to be eliminated, or one of the faces may have a radius of curvature which is smaller than the shell thickness. Please use Tools Check to find the minimum radius of curvature on appropriate faces. If possible, eliminate any unintended small faces or edges.
____________________________________________________________________________________
I've been beating my head over this one for two days, so it must be something obvious that I'm just missing.
Can someone take a look at this model and suggest what the problem is?
https://1drv.ms/u/s!AtfE2uFNgBOWhxbdFpS ... u?e=88zJhe
THANKS!!!
..your mrc is only .034" ... you'll need .11 min
Or,.. rollback before bossextrude3 and it will work (images)
Re: Shell Fail on surfaced part
Posted: Sat Oct 09, 2021 8:20 pm
by Maha Nadarasa
@RCD Machine
Do you want a symmetrical or asymmetrical part? Because I found this part is not symmetry at this location. That means opposite side does not have this line.
Re: Shell Fail on surfaced part
Posted: Sun Oct 10, 2021 1:13 am
by Maha Nadarasa
Try this
Re: Shell Fail on surfaced part
Posted: Sun Oct 10, 2021 9:01 pm
by Lucas
The problem is in the Fillet 63. The edges are too close, and when you fillet them they will overlap. Then the Shell cannot use them properly.
Moving Fillet 63 to the end and suppressing 79:
I would suggest to make a new part:
- change those Sweeps to Loft/Boundary - for a better fillet finishing and no need to trim them
- the first Boss sketch fully defined - and the arcs with tangency in the connection points
- remove all Cut features, there is not need to have them and it would be easier to make changes
- make the design with just two Fillet features, one for those sweeps and other for the border
Re: Shell Fail on surfaced part
Posted: Mon Oct 11, 2021 1:56 pm
by zxys001
Lucas wrote: ↑Sun Oct 10, 2021 9:01 pm
The problem is in the Fillet 63. The edges are too close, and when you fillet them they will overlap. Then the Shell cannot use them properly.
Moving Fillet 63 to the end and suppressing 79:
image.png
image.png
I would suggest to make a new part:
- change those Sweeps to Loft/Boundary - for a better fillet finishing and no need to trim them
- the first Boss sketch fully defined - and the arcs with tangency in the connection points
- remove all Cut features, there is not need to have them and it would be easier to make changes
- make the design with just two Fillet features, one for those sweeps and other for the border
..agree... this should be redone.. since it's symmetrical, focus on 1/2 and mirror
Re: Shell Fail on surfaced part
Posted: Mon Oct 11, 2021 2:00 pm
by zxys001
Nice.. much cleaner!
Re: Shell Fail on surfaced part
Posted: Mon Oct 11, 2021 2:29 pm
by Maha Nadarasa
zxys001 wrote: ↑Mon Oct 11, 2021 2:00 pm
Nice.. much cleaner!
Thanks for the comment. If shell fails, it is a issue with underlaying geometry that is the reason, I model it from scratch.