General Mechanical

General Mechanical

Problem using results for successive transient thermal analysis

    • Carsten Bergmann

      Hi everyone,

      I imported this assembly of two parts into Ansys Mechanical. It consists of a sheet metal and a bushing

      I want to perform a transient thermal analysis with it.

      First, i want to heat the metal with internal heat Generation and then let it cool down for a defined amount of time. For this analysis i surpressed the bushing. (Is there another way to exclude parts of an assembly from an analysis, when i have to use them later on?)
      already works good and the results seem to match my measurements.


      The next step is where my problems start:


      After the defined amount of time from the previous analysis, i want to add the bushing and analyse the temperature distribution after a defined amount of time, of both parts together

      However, I‘m not able to set the temperature distribution of the sheetmetal as initial condition for the next analysis. I tried this in two different ways:

      I used the „Transfer Data to new transient thermal“ Button of the Solution.

      The Problem is, that i surpressed the bushing in the first analysis. When i unsurpress it in the second one, my results file will be cleared

      The second thing i tried, was to export the results, and then load them again. But i couldn‘t figure out how to set the exported soulution as initial condition instead of a thermal load.


      So how do i analyse the sheet metal in the first step stand alone, and then in the next step in contact with the bushing?



      Thanks already 

    • peteroznewman

      Try using Contact between the plate hole ID and the bushing OD and use Contact Step Control in single, multi-step Transient Thermal analysis.

      Step 1, Contact is disabled so no heat is conducted from the plate to the bushing.  Heat up the plate using some value for Internal Heat Generation.

      Step 2, Set the Internal Heat Generation to 0 and wait for the plate to cool off.

      Step 3, Contact is enabled and heat can begin to conduct into the bearing, wait till the End Time and examine the temperature in both parts.

      I expect you are using a Convection BC to allow the plate to cool, you would also want that on the bushing. If the Ambient temperature on the Convection BC is the same as the Environment temperature that the bushing picks up at the start of the simulation, the bushing should behave the way you want.

    • Carsten Bergmann

      That worked great, thank you!

      I had to change my settings from shared topology to bonded contact. Do i have any disadvantages regarding the accuracy of the simulation?

      Is there also a possibility to do the above analysis with shared topology?



    • peteroznewman

      Glad to hear that it worked great.

      You check the accuracy of the solution by remeshing with smaller and smaller elements to see how much the result changes.

      It may be possible to do this with shared topology. The bushing would have zero conductivity in Step 1 and 2 then in step 3 the conductivity is changed to the real value.

Viewing 3 reply threads
  • You must be logged in to reply to this topic.