Hi Saimohan,

So you have two pairs of faces which are connected by contacts. One of these pairs shall now be connected by merged nodes? Recently I had the same problem; this is what worked for me:

I created a small gab between the faces that shall be connected by contacts. The gab has to be as small as possible (1E-3 mm or so). Than you can select both bodies in the DM and "Form New Part". This causes a connection by shared nodes except at the face which has the gab. In Mechanical, you can insert a frictional contact. If the gab is small enough, the mash shall not be influenced. In the Post Processor you can use the contact tool to find out if the contact works and if pressure of frictional stress appears.

I hope this helps.

Marco

Thanks Marco, I understand what you said. how you created small gab (i assume gap)? by crating small volume between faces and removing that volume from original volume ??

You are right, gap.

I was able to slice the volume and delete a part. Otherwise, I would extrude the surface and subtract it from the original volume.

If this does not work, you can use APDL: You can glue the surfaces with "AGLUE" command so both volumes share this surface, but then you have to create the contact by APDL, too.

can you please tell me how to use AGLUE command in design modeller... ??

Sorry, I forgot to say that this would be the alternative way in ANSYS Classic, or in Mechanical, but the generation of the contacts by APDL in the Workbench might be tricky. I have only done that in Classic.

You can use "Form New Part"  in DM to connect  the both bodies

thanks for your suggestions... but the problem is i cant use form new part feature. that will generate continuous mesh at the whole interface. but i want same nodes at some part of the interface and in other part of interface i want mesh which don't has common nodes at interface....

Like shown in fig, i want common nodes at three interfaces and i dont want common nodes at fourth interface... for this i cant form four bodies into part.

Hi Saimohan

I think you can use form new par separately e.g (S1+S2 ), (S1+S3) and(S3+S4) in this case the three glue interfaces got common nodes without the forth one.

hope this will be useful.  

@Rzgar, I don't think this works, because all volumes will be in one part with your procedure. there won't be three parts.

As mentioned above, I solved this problem for investigation of a welding seam by creating a small gap between solid 4 and 2. If this gap is suffient large (1E-6m ?), there will be no common nodes in this interface but you can still create a frictional contact in mechanical. If the gap is sufficient small, the mesh at this interface will not be influenced due to mesh defeaturing (no elements of 1E-6m? length).

@Rzgar, Like marco said, we can not include one solid in different parts... if s1 in one part, we cannot add s1 in another part. So, removing small gap seems to be good option for this problem. So Marco, You created gap with 1e-6m ?

(edited from can to can not)

I used 1E-7m. For smaller values the DM was not able to slice the solid, for lager values the contact did not close, but you might have to play a little with this value.

Maybe you have to play a little with the element size and the contact description, but you can visualice the contact force or the pressure/friction within the contact to ensure that load transmitted. Thus, the contact is within one part between two volumes.

But as far as I know, this option only generates imprints of the surface like the boolean or body operation "imprint". This causes to split the surfaces but when the surfaces are meshed, each one is meshed individually. So there are (at least at the edges) two nodes at the same location. (You can see this if you hide each surface individually in Mechanical.) These can be merged by NUMMRG,NODE,TOL (at least in APDL). In WB, these volumes are then connected by contacts. These contacts lead to better results than without imprint, but you still need contacts. Or is there an option within the meshing tool I yust don't know?

If you use the automatic option, an impring is generated and one of these double faces is deleated. Thus, both both volumes share one surface. If this surface is meshed both volumnes share the same nodes and no contacts are needed at all. This is the same like the APDL command VGLUE.

Dear salvatore, can you please explain about what you said for this particular problem ???

But the imprint function does not merge nodes. It only imprints the surfaces. You can force the nodes to be at the same position by "Match Control" tool in mechanical but you still need contacts at each interface. No nodes are merged. Only if you set the shared topology to automatic, nodes are merged and multiple bodies share a single surface.

Look at:

http://www.ansys.com/staticassets/ANSYS%20UK/staticassets/Presentations/2013%20User%20Conference%20Presentations/Track2%20-%201620%20DM-AM%20Tips%20n%20Tricks%20AW.pdf

and "Conformal Meshing Between Parts" in the ANSYS Help.

if you are using shell element you can use mesh connection for merge the bodies.

WITH VIRTUAL TOPOLOGY

I hope this video will be helpful: https://www.youtube.com/watch?v=npbLyVoS9M4

(mesh edit --> insert node merge group --> connect mesh)