Shelling

[rikonen]

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.

 

[CorBlimeyLimey]

I don't know why the shell doesn't work ... but suspect it has something to do "Multi-bodies". As far as I know Cadkey does not recognize multi-bodies, but SW & ProE do. If someone has a pre-multi-body version of SW perhaps they could try.

An alternative to the workaround you mentioned, would be to do a second Extrude-cut instead of the Shell. See screen capture below.




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[ctopher]

I see. It wants to shell the bottom material also. It can't, not enough mtl. Extrude-cut the square through, then shell, it will work.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP0.1 / PDMWorks 05
ctopher's home site

 

[ctopher]

...sorry, forgot, then add mtl as needed.
I hope this is what you are looking for.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP0.1 / PDMWorks 05
ctopher's home site

 

[Theophilus]

It's probably a logic problem. The software doesn't seem configured to perform a shell operation that results in multiple bodies. I tried several thicknesses to no avail. It's not a matter of the shapes, either, so I think it has something to do with resolving the shell for the two interior faces (back side of cut square and inside of rear circle).

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

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[aamoroso]

I believe it is not working because the face you are keeping will not be uniform thickness due to the square being .4 deep. You have a face of a circle that is trying to be .05 but the walls of the square are not allowing it.

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.

 

[TheTick]

I did some experiments. As far as I can tell, SW doesn't like any shells that result in multiple bodies during the shell process.

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.

I could be the world's greatest underachiever, if I could just learn to apply myself.

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[rikonen]

I am aware of the possible sink issue if it were palstic, I am a mold designer for plastics, this is simply an everyday simple example that is easily done in other packages. The shell shouldn't try to go under the square pocket because the shell is suppost to be limited by the face boundary. As posted, I did the workaround as stated in my sample. I also found it easily done with creating 2 boundaries and extruding a cut. If that's the way it needs to be done then why have the shell function at all. I have emailed the problem to my VAR and will wait to see what the answer is form SWX. It's just very unfortunate that this happened on my very first part designing with Solidworks right after I dished out the 5G's to buy it. A little discouraging to say the least.

Thanks.

 

[CorBlimeyLimey]

As you pointed out in your original post, the same problem occurs in ProE ... a much more expensive package ... and as I pointed out in my first post, both ProE & SW are smart enough to recognize multi-bodies, whereas other packages are not. However, it appears that both programs have "out-smarted" themselves this time & created a conflict/limitation with the multi-body function.

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.


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