×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Merge nodes of coplanar faces in WB
3

Merge nodes of coplanar faces in WB

Merge nodes of coplanar faces in WB

(OP)
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

RE: Merge nodes of coplanar faces in WB

(OP)
...more information...

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

Thanks

RE: Merge nodes of coplanar faces in WB

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

RE: Merge nodes of coplanar faces in WB

(OP)
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.

RE: Merge nodes of coplanar faces in WB

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

RE: Merge nodes of coplanar faces in WB

2
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

RE: Merge nodes of coplanar faces in WB

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources