Basic extrusion error

Valued Contributor
Valued Contributor

Hi,

 

I want to extrude a body from a sketch drawn on a different body, but I keep getting "Zero thickness (non-manifold) body" error.  What does this mean?

 

Here is my sketch and part.  I tried the toggling include/exclude internal loops and open/close sketch options, but it didn't work.

 

ext.png

 

I want to extrude the blue sketch drawon on the fan housing.  The new protrusion should cover the hole.

10 REPLIES

Re: Basic extrusion error

Community Manager Community Manager
Community Manager

the issue is the vertex of the profile near the 66 degree dimension. It just touches the other material (neither is at a distance, nor penetrates it). As such, you will get this infinitely thin area where it touches the part. This is not supported by any system based on Parasolid (i.e. Solid Edge, NX, SolidWorks, etc.)

 

 

Dan Staples
Director, Solid Edge Product Development

Re: Basic extrusion error

Valued Contributor
Valued Contributor

The point where the two sketch lines connected, used to be on the vertical edge betweent the fan housing and the box to the right.  I removed the Point On and Connect relations and moved the end points out a bit and connected them together again.  That corner is no longer touching the other body, but I'm still getting the same error.

 

ext2.png

Re: Basic extrusion error

Community Manager Community Manager
Community Manager
Can you share the model. Would be fastest to debug that way.
Dan Staples
Director, Solid Edge Product Development

Re: Basic extrusion error

Valued Contributor
Valued Contributor

Sure.  I really appreciate your help.

Re: Basic extrusion error

Community Manager Community Manager
Community Manager

It looks like you might have a similar problem where the 9.125 and 6.000 dimension are. You appear to be missing a connect constraint there, but if you had one, then it would be "just touching" and same issue. 

Dan Staples
Director, Solid Edge Product Development

Re: Basic extrusion error

Phenom
Phenom

Hi,

 

I suggest using Multibody modeling method in this case!

 

 

BR,

Imics
http://solidedgest.wordpress.com/

Re: Basic extrusion error

Creator
Creator

Yes,

I've connected the vertex where 9.194 and 5.978 dimensions are and I could extrude the part.

 

Cheers

Re: Basic extrusion error

Valued Contributor
Valued Contributor

@Imics

 

I don't see that option on the ribbon.  Is it something I need to enable or is it something I need to buy?

 

I had no idea this limitation existed in parasolid based programs.  So If a vertex touches a body, the sketch can't be extruded, but if a side of a sketch touches a body, it can be.  I bet this drives newbies crazy.

 

Thank you all for your help and suggestions.

 

ext3.png

Re: Basic extrusion error

Phenom
Phenom

Hi,


see it as the volume must not be zero at any position.

There must not be any singularity in it.

 

And imagine the real part looking like that.

What would then will happen?

 

Yes, it breaks

 

 

 

And answering Your question:

 

There is a small icon in volume register "Add body"

Using this function You are defining another body within the same part.

You have to see it more or less like playing with builidng blocks and not melting the blocks together as it is with another extrusion.

 

So Yes, using MultiBody will solve the initial problem, but not the real problem within the part

 

 

 

regards

Wolfgang

 

 



regards
Wolfgang