Shelling
Shelling
(OP)
this is probably a very easy question to answer but I'm a little puzzled as to why I can't shell out a part. Here's my example:
I draw a 4.00 diameter circle and extrude it .500
I then create a 2.5" square using the face as my sketch plane and extrude cut down into the part .400" (this can be any shape)
Now I want to shell out the remaining amount of the face to .05 and all I get is errors.
I am familiar with working in solids using cadkey for many years and shelling like this is common and no problem, is it because of the parametrics that make this shell not work or is it the way I'm doing it?
Any help would be greatly appreciated.
I worked around it by making my cut through rather than blind, then created the shell, made boundary from edges on bottom cut and extruded the bottom back up to make my part. I don't know if this is the way I'll need to do it all the time but I'm hoping someone will give me the answer.
This is an example I've posted on two other forums (cadchat, solidworks) and seems to be a real problem not just an inexperience problem. does anyone know why this may not work? I'll add that I tried it in Pro Engineer with similar results. That leads me to believe it's a parametric issue that I'm not yet familiar with.
Thanks.
I draw a 4.00 diameter circle and extrude it .500
I then create a 2.5" square using the face as my sketch plane and extrude cut down into the part .400" (this can be any shape)
Now I want to shell out the remaining amount of the face to .05 and all I get is errors.
I am familiar with working in solids using cadkey for many years and shelling like this is common and no problem, is it because of the parametrics that make this shell not work or is it the way I'm doing it?
Any help would be greatly appreciated.
I worked around it by making my cut through rather than blind, then created the shell, made boundary from edges on bottom cut and extruded the bottom back up to make my part. I don't know if this is the way I'll need to do it all the time but I'm hoping someone will give me the answer.
This is an example I've posted on two other forums (cadchat, solidworks) and seems to be a real problem not just an inexperience problem. does anyone know why this may not work? I'll add that I tried it in Pro Engineer with similar results. That leads me to believe it's a parametric issue that I'm not yet familiar with.
Thanks.






RE: Shelling
An alternative to the workaround you mentioned, would be to do a second Extrude-cut instead of the Shell. See screen capture below.
[url=http://www.imageshack.us][img=http:
Eng-Tips.com Forum Policies FAQ731-376
Making the best use of this Forum. FAQ559-716
How to get answers to your SW questions. FAQ559-1091
Helpful SW websites every user should be aware of. FAQ559-520
RE: Shelling
Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP0.1 / PDMWorks 05
ctopher's home site
RE: Shelling
I hope this is what you are looking for.
Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP0.1 / PDMWorks 05
ctopher's home site
RE: Shelling
The faces collide at zero thickness at 0.050", so that's a logic problem. Thinner and thicker shells still do not work--strange, but probably a result of the multi-body conflict primarily with the thinner walls and another collision of surfaces with the thicker walls.
Perhaps you could send the problem to your VAR and get the reasons behind the behavior beyond what I've posted. I think it's some sort of logic problem (contradictions cannot exist).
Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.
RE: Shelling
Having said that, the only way to achieve the goal is multiple features, one is the Circle extruded, two shell to .05, three sketch the square and use thin extrude.
If this were a plastic injection molded part, there would be sink marks on the face of the circle where the square is due to the non-uniform thickness of material where the walls of the square are. SolidWorks is perfoming the shell feature exactly as it should work, it will not allow a non-uniform thickness for a single face in shell command.
RE: Shelling
Your model temporarily results in a split body (before the two parts would be reunited because they intersect).
Sounds like a limitation to be lived with until SW fixes. Do us all a favor, call your VAR and make sure this is reported.
http://www.EsoxRepublic.com-SolidWorks API VB programming help
RE: Shelling
Thanks.
RE: Shelling
If you Shell from the underside of the part you describe, you will see that it works the way it is intended to.
Also if you create a square instead of a round as the first feature & then Shell on various faces (other than the top) you will see that it also works as intended.
As TheTick suggests ... report this to you VAR, so that they can submit it to SW as a bug/limitaiion which needs to be fixed. I also suggest you encourage others to do the same to their VARs.
Eng-Tips.com Forum Policies FAQ731-376
Making the best use of this Forum. FAQ559-716
How to get answers to your SW questions. FAQ559-1091
Helpful SW websites every user should be aware of. FAQ559-520