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Need some help with the shell command!!!

JCAD

New member
I'm having problems shelling out some of my models, I am creating them using solid protrusions including sweeps, blends, and swept blends, as soon as i finish modelling and decide to shell, the model fails! i have tried to adjust the accuracy in the set-up, but this does not help, What are the rules when using the shell command, How do you experts create your models??? is the best way to use surfaces and then create protrusion from quilt? or to create the model as a surface then offset it, then join both surfaces and create a protrusion. The model shown is one i am having problems with at the moment, as you can see it is not that complex, as soon as i tell pro e to shell the model on the flat side underneath to 2mm it gives me that lovely RESOLVE message that i just love to see!!! help!

http://www.proecentral.com/uploads/images/model1.jpg
 

Israr

Active member
Your model is complex as far as shell is concerned and I would suggest you use surfaces.



Israr
 

kvision

Moderator
your model looks like it should shell. Try using a small thickness and work your way up if iy works. Assuming the model is around 12 inches in size try something like .001 or .003 and get thicker if it works until it fails.

What likely is happening is that two adjacent walls when offset the shell distance creates an area where one or the other or a common short wall disappears. This is common. to check, try using a small negative number and shell it out instead of in. Upload the file and I can check it out for oyu.
 

swcalvert

New member
I might suggest that you add some rounds to a few of the sharp corners, sometimes this adds the needed material and allows a shell to happen. Also, go backwards in your feature tree and see if you can shell there, maybe it's a later feature that is causing you problems.



Steve C
 

donha

New member
Once the shell fails, select Failed Geometry. Selecting Failed Geometry will show you where you are failing. You can possibly figure out if you need to make geometrical changes such as adding rounds or if it is physically impossible to create the shell because geometry cannot be offset.

I can see the radiused wall next to the large diameter cannot be offset. Radiusing this area might allow it to be shelled.

One of the lessons learned in Pro/E is there is more one way to do something. Sometimes it is best to try another venue.

View attachment 375
 

miked

New member
Get rid of the variable rad >shell then add it back in after.

If you add rads before shelling you should make them larger than the shell thickness.

miked
 

JCAD

New member
Cheers Guys for the advice, I made some of the rads bigger, Pro e then allowed me to shell the model, What I usually try and do is before i am ready to shell the entire model, everytime I add a new feature i then shell my model to see if that new feature causes any problems, then i delete the shell and carry on modeling, on another model i was creating all i did was create a datum curve for a swept blend trajectory, pro e wouldn't allow me after that to shell my model, work that one out???
 

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