Making Thermal Contact Conductance a Parameter in ANSYS Mechanical 18.0 and Earlier with an APDL Command Object


padt thermal contact parameter F00 1 A support request from one of our customers recently was for the ability to make Thermal Contact Conductance, which is sort of a reciprocal of thermal resistance at the contact interface, a parameter so it can be varied in a parametric study.  Unfortunately, this property of contact regions is not exposed as a parameter in the ANSYS Mechanical window like many other quantities are.

Fortunately, with ANSYS there is almost always a way……in this case we use the capability of an APDL (ANSYS Parametric Design Language) command object within ANSYS Mechanical.  This allows us to access additional functionality that isn’t exposed in the Mechanical menus.  This is a rare occurrence in the recent versions of ANSYS, but I thought this was a good example to explain how it is done including verifying that it works.

A key capability is that user-defined parameters within a command object have a ‘magic’ set of parameter names.  These names are ARG1, ARG2, ARG3, etc.  Eric Miller of PADT explained their use in a good PADT Focus blog posting back in 2013

In this application, we want to be able to vary the value of thermal contact conductance.  A low value means less heat will flow across the boundary between parts, while a high value means more heat will flow.  The default value is a calculated high value of conductance, meaning there is little to no resistance to heat flow across the contact boundary.

In order to make this work, we need to know how the thermal contact conductance is applied.  In fact, it is a property of the contact elements.  A quick look at the ANSYS Help for the CONTA174 or similar contact elements shows that the 14th field in the Real Constants is the defined value of TCC, the thermal contact conductance.  Real Constants are properties of elements that may need to be defined or may be optional values that can be defined.  Knowing that TCC is the 14th field in the real constant set, we can now build our APDL command object.

This is what the command object looks like, including some explanatory comments.  Everything after a “!” is a comment:

! Command object to parameterize thermal contact conductance
! by Ted Harris, PADT, Inc., 3/31/2017
! Note: This is just an example. It is up to the user to create and verify
! the concept for their own application.

! From the ANSYS help, we can see that real constant TCC is the 14th real constant for
! the 17X contact elements. Therefore, we can define an APDL parameter with the desired
! TCC value and then assign that parameter to the 14th real constant value.
! We use ARG1 in the Details view for this command snippet to define and enable the
! parameter to be used for TCC.

r,cid ! tells ANSYS we are defining real constants for this contact pair
! any values left blank will not be overwritten from defaults or those
! assigned by Mechanical. R command is used for values 1-6 of the real constants
rmore,,,,,, ! values 7-12 for this real constant set
rmore,,arg1 ! This assigned value of arg1 to 14th field of real constant

! Now repeat for target side to cover symmetric contact case
r,tid ! tells ANSYS we are defining real constants for this contact pair
! any values left blank will not be overwritten from defaults or those
! assigned by Mechanical. R command is used for values 1-6 of the real constants
rmore,,,,,, ! values 7-12 for this real constant set
rmore,,arg1 ! This assigned value of arg1 to 14th field of real constant

You may have noticed the ‘cid’ and ‘tid’ labels in the command object.  These identify the integer ‘pointers’ for the contact and target element types, respectively.  They also identify the contact and target real constant set number and material property number.  So how do we know what values of integers are used by ‘cid’ and ‘tid’ for a given contact region?  That’s part of the beauty of the command object: you don’t know the values of the cid and tid variables, but you alsp don’t need to know them.  ANSYS automatically plugs in the correct integer values for each contact pair simply by us putting the magic ‘cid’ and ‘tid’ labels in the command snippet.  The top of a command object within the contact branch will automatically contain these comments at the top, which explain it:

!   Commands inserted into this file will be executed just after the contact region definition.
!   The type number for the contact type is equal to the parameter “cid”.
!   The type number for the target type is equal to the parameter “tid”.
!   The real and mat number for the asymmetric contact pair is equal to the parameter “cid”.
!   The real and mat number for the symmetric contact pair(if it exists)
! is equal to the parameter “tid”.

Next, we need to know how to implement this in ANSYS Mechanical.  We start with a model of a ball valve assembly, using some simple geometry from one of our training classes.  The idea is that hot water passes through the valve represented by a constant temperature of 125 F.  There is a heat sink represented at the OD of the ends of the valve at a constant 74 degrees.  There is also some convection on most of the outer surfaces carrying some heat away.

padt thermal contact parameter F01

The ball valve and the valve housing are separate parts and contact is used to allow heat to flow from the hotter ball valve into the cooler valve assembly:

padt thermal contact parameter F02

Here is the command snippet associated with that contact region.  The ‘magic’ is the ARG1 parameter which is given an initial value in the Details view, BEFORE the P box is checked to make it a parameter.  Wherever we need to define the value of TCC in the command object, we use the ARG1 parameter name, as shown here:

padt thermal contact parameter F03

Next, we verify that it actually works as expected.  Here I have setup a table of design points, with increasing values of TCC (ARG1).  The output parameter that is tracked is the minimum temperature on the inner surface of the valve housing, where it makes contact with the ball.  If conductance is low, little heat should flow so the housing remains cool.  If the conductance is high, more heat should flow into the housing making it hotter.  After solving all the design points in the Workbench window, we see that indeed that’s what happens:

padt thermal contact parameter F04

And here is a log scale plot showing temperature rise with increasing TCC:

padt thermal contact parameter F05

So, excluding the comments our command object is 6 lines long.  With those six lines of text as well as knowledge of how to use the ARG1 parameter, we now have thermal contact conductance which varies as a parameter.  This is a simple case and you will certainly want to test and verify for your own use.  Hopefully this helps with explaining the process and how it is done, including verification.





Get Your Ansys Products & Support from the Engineers who Contribute to this Blog.

Technical Expertise to Enable your Additive Manufacturing Success.

PADT’s Pulse Newsletter

Keep up to date on what is going on at PADT by subscribing to our newsletter.

By submitting this form, you are consenting to receive marketing emails from: . You can revoke your consent to receive emails at any time by using the SafeUnsubscribe® link, found at the bottom of every email. Emails are serviced by Constant Contact

Share this post:

Upcoming Events


2024 Arizona MedTech Conference


Optics Updates in Ansys 2024 R1 - Webinar


Connect Updates in Ansys 2024 R1 - Webinar


Structures Updates in Ansys 2024 R1 (3) - Webinar


E-Mobility and Clean Energy Summit


Fluids Updates in Ansys 2024 R1 - Webinar


2024 CEO Leadership Retreat


New Mexico Tech Summit 2024


PADT30 | Nerdtoberfest 2024

Search in PADT site

Contact Us

Most of our customers receive their support over the phone or via email. Customers who are close by can also set up a face-to-face appointment with one of our engineers.

For most locations, simply contact us: