Fluids

Fluids

Transient thermal analysis – Thermal interface

    • JulB
      Subscriber

      Hello,


      I am trying to simulate the temperature effect of two bonded bodies, each at different temperatures. Body 1 is at 20 degrees Celsius and Body 2 is at 100 degrees Celsius. Body 1 is the cavity with a hole in the middle where body 2 is assembled and bonded. I run the simulation for 480 seconds. The heat in the model is transferred by conduction. Convection is applied at the top surfaces of both bodies and the boundaries of body 1 that contains body 2. I have experimentally run also this arrangement, so I have points to validate the model.


      The problem that I have with the simulation results is that the temperature in the boundary increases very rapidly and this does not correspond to the reality. I have attached an example.


      Could you please advise?


      Many thanks.

    • Vishal Ganore
      Ansys Employee

      Need to know more about your geometry, how two bodies are bounded and what boundary conditions are applied in Fluent. If possible please share your project (.wbpz archive)

    • JulB
      Subscriber

      3d sketch


      Hello there,


      Thank you for your reply. I am using Ansys Workbench, steady state analysis in the beginning to apply temperatures to the two bodies and then transient analysis to apply convection and radiation to ambient applied at the top surface of the 3d assembly geometry. All the other surfaces are perfectly insulated. Please see attached sketch.


      I managed actually to reduce the temperatures in the boundary by changing the temperatures that weren't correct in the first calibration that I did but I still get a high temperature response for the first 30sec of the simulation and then the temperature decreases to the actual level that it should be as in reality.


      Let me know what you think. Is it better to run the analysis with Ansys fluent?


      Many thanks.

    • Vishal Ganore
      Ansys Employee

      Hi, 


      Following info is needed since the project file is not available:


      1. Which material are you using for these two bodies?


      2. Where are you providing temperature boundary condition? On Faces? I assume entire volume is subjected to fix temperatures. In that case, applying temperature on faces will not work. Are you patching the initial body temperatures when you initialize?


      3.  At time t=0, T1=20C, T2=100C, I assume steady state will be achieved at the end where both bodies will be at equal temperature. So your aim is to find out how the temperature of two bodies changes with respect to time before it reaches to atm temp (steady state). Is that right? 


      4. What is the value of time step used for transient analysis? Value of total time period? 


      5. Boundary condition used for convection and radiation?


       

    • JulB
      Subscriber

      Hello Vishal,


      Is there possible to communicate with you via e-mail?


       


      Many thanks.

    • Vishal Ganore
      Ansys Employee

      Any particular reason for that? Unfortunately, we are not allowed to provide 1:1 support. 

    • JulB
      Subscriber

      I wanted to share my simulation model but is confidential. I suppose this portal is seen by everybody?

    • JulB
      Subscriber

      Following your last message, please see my answers below:


      1. The material for both geometries is asphalt. They have different densities and therefore different thermal conductivity and specific heat capacities. Four values of thermal conductivities at four different temperatures are used for both geometries. These measurements are completed in the laboratory for the specific asphalt mixtures used in the model.


      2. T1=20C is applied to the whole volume of geometry 1. I have changed however lately on how I apply T2. In my latest simulation model geometry 2 has different temperatures on all its external surfaces. On this way I have much better match with my experimental results. It was happened in reality. The mix had different temperatures on its surfaces. So T2 is applied now on faces.


      What dies it mean to patch initial temperatures? Could you explain more. I do not think I am doing this and is maybe where the problem is.


      3. Yes, I want to find change of temperature with respect to time. Is it wrong to use initially steady state? I use steady state to apply T1 and T2 and then run transient analysis.


      4. Steps in total 17:


      Step time: 1 has End time:1s


      Step time: 2 has End time:10s


      Step time: 3 has End time:20s


      Step time: 4 has End time:40s


      Step time: 5 has End time:60s


      Step time: 6 has End time:80s


      Step time: 7 has End time:100s


      Step time: 8 has End time:150s


      Step time: 9 has End time:200s


      Step time: 10 has End time:250s


      Step time: 11 has End time00s


      Step time: 12 has End time50s


      Step time: 13 has End time:400s


      Step time: 14 has End time:420s


      Step time: 15 has End time:440s


      Step time: 16 has End time:460s


      Step time: 17 has End time:480s


      5. Convection and radiation is applied at the top surface of the geometry assembly shown in my last figure. Emissivity for radiation to ambient is equal to 0.967 with ambient temperature set at 21.5C as in the whole simulation model. Film coefficient value for convection is chosen from Ansys itself values (Stagnant Air - simplified Case).


      Many thanks for your help. I hope the above helps to better understand how the model is built.

    • JulB
      Subscriber

      I am sorry for steps 11 and 12. I don't know why they were converted to emoji.


      Here are the actual values:


      Step time: 11 has End time 300s


      Step time: 12 has End time 350s

    • Vishal Ganore
      Ansys Employee

      1) OK. No issues. 


      2) In order to start evaluating the transient solution, Fluent need to understand the temperature condition you have for two bodies at time = 0.



      • Body 1: You need to patch T1 (20 C) to body 1 after you initialize the solution. This means you are setting up 20C temperature to whole volume of body at t=0.

      • Body 2: If I understood correctly, looks like you have a constant temperature boundary condition at six faces of the box (temp do not change with time at faces). These faces are the source of heat generation. Means produced heat will get transferred from these faces to body 1 (out) and 2 (internally) both through conduction. Is that right? If yes, what is the initial temperature (at t=0) body 2 is suppose to have? You could patch that as well. 

      • How to patch: Initialize the case then go to patch and provide the temperature that two bodies have at t=0. After that before iteration, you could actually check the temperature contour to understand whether solver has take correction BCs.


       


      3)  Considering #2, I think run for steady state is not required here if you have correct BCs at time t=0 unless residual (only energy equation in this case) shows irrelevant fluctuation. I would initially test the case for 10 seconds to understand the simulation setup. For that, time step size could be .1 sec and total time steps = 100.

    • JulB
      Subscriber

      Hello Vishal,


      Thank you for your help.


       


      Is it possible to do patching in Ansys Workbench Transient analysis but not Fluent? I am not using or know how to build a model in Ansys Fluent.

    • etc59
      Subscriber

      Sorry for the late response here, but this question may be useful to others who run into similar issues with thermal analysis. 


      1. Did you specify a contact conductance between your bodies in your model? If you use the default conductance set by ANSYS, you may be assuming near perfect conductivity which would lead to a rapid change in temperature at your boundary.


      2. How are the bodies bonded in your experimental set-up? You can estimate the contact pressure because you are essentially performing a heat assisted force fit. Once you know the contact pressure you can calculate or approximate the conductance at the contact based on the material properties of the two bodies. This would help make your model more accurate.

    • Vishal Ganore
      Ansys Employee

       Thanks for these additional comments. Cool!

    • JulB
      Subscriber

      Hello,


      Yes you are absolutely right. I managed to accurately simulate the thermal contact between the two bodies by defining the thermal contact conductance. This parameter is significant. If, as you also mentioned, let Ansys to control thermal contact conductance then the agreement between simulated and measured data is not good at all.


       


      For Ansys Workbench, another parameter that will help to define the boundary connection between the two bodies is by using "Frictionless" type of contact and define a "Pinball Radious" larger than the gap/contact area between the two bodies even if the two bodies don't have any gap by design.  

Viewing 13 reply threads
  • You must be logged in to reply to this topic.