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


Thermal Contact in APDL

Thermal Contact in APDL

Thermal Contact in APDL

Hi all,

I'm relatively new to ansys apdl, and am having a lot of trouble with contact analysis in APDL Mechanical. I'm not able to correctly transfer temperatures between two bodies with contact elements in between them. I've attached an image of the problem, and also the txt file that I'm using. Unfortunately I need to use txt import, and not the gui or workbench. Any help you're able to give is really appreciated, as I've been struggling with this for weeks.

RE: Thermal Contact in APDL

Hi Benjamin,

you are using SOLID5 element with keyopt(1) = 0 so you perform coupled field analysis and UX, UY, UZ, TEMP, VOLT, MAG are your DOFs. Do you want to perform such a coupled analysis? If you are interested in thermal analysis only, change keyopt(1) to 8, in your macro ET,1,SOLID5,8 or use solid70 ET,1,SOLID70 (thermal only element).

Then you should maybe define some material properties of your contact.
If you specify thermal contact conductance for you contact via real constants

You will see results which correspond to bonded contact.

If you do not want to set material properties for the contact like TCC or emmisivity etc, use KEYOPT,cid,2,2 (MPC contact algorithm which couples the DOFs directly with constraint equations).


Petr Vymlatil (www.designtec.eu)

RE: Thermal Contact in APDL

Amazingly helpful thank you. Yes I was trying to perform structural and thermal together, as thermal expansion is a big part of the more complex model (not shown here). I'm still getting some penetration issues, but I'm now able to conduct heat through the contact. Thanks so much Petr.


RE: Thermal Contact in APDL

If you add the following to the same part as your txt (keyopt to force) than the mech/temp contact is OK and temps are OK.

Just added as per Petr Vymlatil recomendtaions a TCC contact conduction value (same as the material, 60.5), both U and TEMP DOF (keyopt(1)), and then used keyopt (5) to close or resolve any contact gaps or initial penetration.


keyo,cid,5,3		   ! close gap and penetration added
keyo,cid,8,2               ! auto create asymmetric contact (from Program Controlled setting)
keyo,cid,10,0              ! adjust contact stiffness each NR iteration (from Program Controlled setting)
keyo,cid,12,5              ! bonded always
keyo,cid,2,0               ! augmented Lagrange (from Program Controlled setting)
keyo,cid,4,0               ! on Gauss point (from Program Controlled setting)
keyo,cid,9,1               ! ignore initial gaps/penetration
keyo,cid,7,0               ! No Prediction
keyo,cid,1,1			! Both U and TEMP added
rmod,cid,14,60.5	! TCC added
!-----Apply Force----- 

RE: Thermal Contact in APDL

Thanks for your help everyone. This works great for my practice problem, but when I try to include it into my real code (transient, killed elements, and temperature dependent mat props) it fails again, and I'm not sure the issue. In the image, there is a penetrated layer below the solid, and it's at 356 K which means it's not transferring heat between the larger body.

Thanks in advance.


RE: Thermal Contact in APDL

It is because of the EKILL that probably kills elements and contacts. If you take that part (EKILL) away it works fine.

I would revise that (EKILL - in your image the grey elements I think are those inactive during that step, so you do not see the results - check the contact status if it is active that will tell if the bottom half that is not killed is in contact with the big block). Also if they are connected and there is not contact you might as well, make a compatible mesh between the parts, instead of using MPC to connect dissimilar meshes. Of course if the geometry is complex it can be hard to do that, but such a simple one it is straightforward.

It is the esel, and the esel, inve that selects the contacts/targets also and then they are killed by the subsequent ekill. Try to select the top solid5 elements differently.

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! Already a Member? Login


eBook - 10 Reasons to Choose CATIA on the Cloud
To compete in today’s fast-paced and competitive market, smaller and newer firms need a powerful platform that will enable them to compete with bigger players, without the heavy investments needed in computer hardware, software and personnel. Download Now
White Paper - Smart Manufacturing for Electronics
This white paper describes a transformative approach to electronics manufacturing made possible by the addition of Mentor Graphics to the Siemens family. It describes a completely digitalized strategy that supports both printed circuit board (PCB) and mechanical design and manufacturing, uniting the entire product lifecycle – from idea and production to customers and back. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close