Shell Radii Problem

[Anonymous]

I'm trying to shell the attached part and what's happening is that I have a .125 Radius on an edge and I can't make the wall thickness any larger than .12, which makes sense to me, but I need to make the wall thicker, is there a work around for that?  Meaning have the inside radius go to zero and I can put them in after with a thicker wall?  Its kind of a complex variable radius.  I appreciate any thoughts you have.

[Anonymous]

Sorry, I forgot.  Using Old fashioned 2013 Inventor Pro

[CCarreiras · Accepted solution]

Hi!

Is easy to see why you received an error, some fillets "disappear" due to the desired thickness (.125), and that will cause the error.

After aplly the .120 thickness, you can add the thickness (.005) to the interior of the part, and your problem is solved.

The thickness tool must to have the  "Automatic blend" on. The fillets will disappear, but no error will appear.

After, you can add fillets again, if you want.

[Anonymous]

This is good info. Here's my problem.  I want the thickness of the part to be .18 but the .125 radii won't allow me to do that because of the disappearing inside radius.  So I tried the thicken on all the interior faces by .06 and it gives me an error.  This will do what I want if I can get around the error.  It says The attempted operation did not produce a meaningful result.  But I see it in the display before saying ok.

[Anonymous]

Actually I just got it to work..  Not really sure how, the first times I was doing that the Join, subtract, etc.. were grayed out..  I think that should work for me.. Thank you very much!

[johnsonshiue]

Hi! You are still using Inventor 2013. I cannot provide a solution using that version. Here is a workflow you may consider. Shelling operation in Inventor usually tries to precisely offset the faces. In your case, you have a complex blend on the outside. That type of smoothness and precision may not be important for inner faces.

What you can do is to move EOP above the Fillet. Next use Thicken command to create offset surface from the side and the bottom. You will get the inner surface. Then you can create constant radius fillet on the inner surface. Lastly, use Sculpt or Split command to hollow the part.

Many thanks!