Merge nodes of coplanar faces in WB 3

[castleMadrid]

How can I merge the nodes of coplanar and geometrically unique faces inorder to give me a smooth stress contour at the interface.

My model in workbench environment is supposed to be only one simple part but since I need to apply the loads on a particular portion on a face, I sliced it into two parts. I tried to use 'match faces' in the meshing tool but it required two faces on the same part.

Thanks

 

[castleMadrid]

...more information...

By the way, these two faces are actually defined as bonded contacts.

Thanks

 

[Transient1]

Can you describe the problem more clearly? Did you check the material properties of both pieces to make sure they are the same?

 

[castleMadrid]

Here is a very simplified graphical representation of my model. A cantilevered plate with bolt fixing with defined compression-only on a portion of the surface underneath. In order for me to define the BC at a certain portion of the model, I sliced the plate into two parts before importing to ANSYS WB. My problem is not about stability or achieving a solution but it is the results--I don't get a smooth stress contour at the interface of the two parts. "How can I redefine the parts as a continuous monolithic part although physically they are tw parts. (like maybe merge the nodes as can be done in classic env.)


¦¦ Force Sliced plane(to delimit BC Comp. only definition)
\/ \/ ____
,-------------,--------¦ ¦--,
¦ ¦ ¦ ¦ ¦ << plate
'-------------'----------¦ ¦---'
,----------¦ ¦---------------------
¦ ^ ¦ ¦<<Bolt
¦BC:
¦Compression
¦only
¦surface
¦
¦
Sorry for asking very siple questions. Don't worry, I have ordered the FEA book by Moaveni and also WB Tutorial and they are on their way I suppose.

 

[cbrn]

Hi,
since you used an external CAD to slice the model, you'd better slice only the face and not the entire body. That's the simplest way I see.

Regards

 

[doatis]

If you have Design Modeler, it's easy, just use the 'Form New Part' capability, which is the same as 'vglue' in the ANSYS Classic environment.

You could try inserting a command snippet to merge the nodes, but I wouldn't recommend it. The reason is because when WB tries to read in the results, the node numbers it sent out don't match what's coming back in. You would have to insert a variable to allow null results (Tools > Variable Manager).

I would try using the ceintf command instead in a command snippet. First, make a named selection out of each face, say face1 and face2. Then, use a command snippet like:

cmsel,s,face1
esln
cmsel,s,face2
cmsel,u,face1
!At this point you now have the nodes of one side and the
!elements of the other side, a requirement for ceintf
ceintf,,all
allsel,all


Should work, but will only be applicable for small displacement analyses (since the CEs aren't updated for large deflections).

Hope this helps,
Doug

 

[Transient1]

Castlemadrid,


You may find the following article from ansys.net interesting. It is a short study of Continuous
Mesh versus Bonded Contact versus Constraint Equations. It outlines the method to set these connections up in ANSYS classic, but I've found that the more you understand about how ANSYS works on the command level, the better you can make use of workbench.

http://ansys.net/tips/week24-connecting_models_tow.pdf