Thermal Stress Results From Your CFD Simulations

After performing a conjugate heat transfer (CHT) simulation in ANSYS Fluent or ANSYS CFX software, you may be interested in the thermal stresses generated in your model. ANSYS Workbench 13.0 makes it easy to perform this type of analysis by transferring the volumetric temperature field from your CFD solution and applying it as a body temperature load in a static structural system.

In the Workbench project schematic you simply need to link the solution cell of your Fluent or CFX analysis to the setup cell of a static structural analysis.

The geometry cells are typically shared between the two systems but there’s no requirement to do so. The CHT bodies in your CFD analysis do need to overlap with the solid bodies in your structural system to enable accurate load mapping.

In the structural setup you’ll now see an imported load object. A right-click on this object allows you to import a pressure or body temperature load from the CFD solution. For a thermal stress analysis import a body temperature load.

In the details view for the imported body temperature you’ll be prompted for the structural body to which to map the temperature load and the CFD domain to use as the source. You can then update the imported load object to view the mapped temperature load and some diagnostics about the mapping process.

Make sure you check those diagnostics. So what do you do if some nodes were not mapped correctly? Well the mapping is actually performed in the background using ANSYS CFD-Post and there’s an interpolation tolerance setting in CFD-Post that’s used by the mapping process. To adjust this setting launch CFD-Post and go to “Edit > Options > CFD-Post”. You’ll see the interpolation tolerance which defaults to 0.5, which means 0.5 percent of the CFD domain extent. If you change this and close CFD-Post, it gets saved in your preferences and will be used when mapping data to your structural simulation. Increasing this value should help map structural nodes that lay outside of the CFD mesh (due to a course mesh on a curved surface for example). Decreasing this value may help the mapping around sharp corners.

Lastly, since the mapping is performed in CFD-Post, MAPDL users can perform the mapping manually too. I won’t provide all the details here, but the main steps are:

  • Write out a CDB file containing the solid mesh.
  • Load the CFD results in CFD-Post and import the CDB file.
  • Export a load file containing BF commands with the mapped temperature from CFD-Post.
  • Read the load file into MAPDL.

Feel free to follow up to this blog post if you want more details on this approach.

If you’re looking for more information on fluid structure interaction then consider the ANSYS CFX Fluid Structure Interaction (FSI) 2-day training course. Further information can be found in the Training Center at ansys.com. Classes are typically scheduled on request.  Also watch for the upcoming Fluent FSI training course in the New Year. This will include 1-way and 2-way FSI between Fluent and ANSYS Mechanical using version 14.0.  I’ll have more to say on Fluent–Mechanical FSI in future blog posts.

7 thoughts on “Thermal Stress Results From Your CFD Simulations

  1. I am using ANSYS Workbench 2.0 Version 13.0.0 with the mechanical package. I am doing a thermal-stress optimization of a cooling channel and I am wondering how I can make the ambient temperature of the convection inside the channel change when the dimensions of the channel change.

    Thank you

  2. You can link a geometry dimension with the ambient temperature using parameters. In your Static Structural analysis click in the check-box to the left of Ambient Temperature; you’ll see a “P” symbol shown and on the Project Schematic you’ll now have a Parameter Set. Next edit the geometry and find the dimension(s) that controls how the channel changes. Click on the check-box next to these dimension(s) to also make these parameters. Now double-click on the Parameter Set to edit. In the Outline of All Parameters table select the Convection Ambient Temperature parameter, then lower down in the Properties table you can write an Expression. Your geometry parameters will have labels such as P2, P3, etc. An example of an expression to enter is: 15 [C] * (P2/30). In the Table of Design Points you can enter new values for the geometry parameters to allow you to run through a series of design points. Be sure to click the “Exported” check box in the Table of Design Points if you want to retain all the results files. Hope this helps!

  3. Hi Michael, I found this message very useful. Thank you for your post.
    I am planning to do similar thing for stress calculation for my transient problem. There is slight more complexity in my CFD domain which is expanding with time. How should I take care of this changing domain, if I want to do one way coupling?
    Thanks & best regards,
    Ravindra

    • Hi Ravindra,
      there are a few potential approaches here, but it does depend on the details of your case, so let me ask a few questions first:
      – What variable do you want to transfer? Volumetric temperature, surface temperature/convection coefficient or surface forces?
      – Are you using CFX or Fluent?
      – Is it practical to run the structural solver using the same time step size as you will use for the CFD solver?
      Regards,
      Mike

  4. Hi Michael.
    I was doing a simple coupled thermal-structural case in which the temperature field is solved in a solid material. And the solution is linked to structural solver.
    I am using ansys workbench, and for the thermal boundary condition I need to use spatial varying heat flow. Unfortunately this is not possible in Ansys workbench as only some boundary types are available with spatially varying condition.
    Can you tell me How I can define a spatial varying heat flow? Should I change the steady state thermal solver with another one like Fluent or CFX?
    Thanks in advance.

    • Take a look at the External Data component in Workbench. You’ll need a text file that defines x,y,z locations and the Heat Flux at those locations. That file can be read into External Data and then connected to the thermal analysis.

Comments are closed.