7 Replies Latest reply on Jun 6, 2017 6:26 AM by Joe Galliera

    Conduction Temperature Discontinuities in Flow Simulation without contact resistance

    John Bankert

      Hello,

       

      I am new to flow simulation, but have used Solidworks Simulation for a few years.  I am noticing some non-physical results when I look at temperature cut plots of mating solids.  To illustrate the results I made a simple simulation.  The setup is:

       

      1) Two discs mated together without any contact impedance between them

      2) External air flow, 1 m/s in plane with the discs.

      3) Volumetric Heat source(1 W) imparted on one disc.

      4) Material of the disc with the heat source has a conductivity of 1 W/mK

      5) Material of the disc without the heat source has a conductivity of 100000 W/mK

      6) 4 mesh elements through the thickness of the discs

      7) Ambient temp 21 C

       

       

      In the attached file "Single_Heat_Source_Compare.png", the temperature profile of a cut plot through the center of the discs is seen.  There is a clear discontinuity in the temperature at the junction between the two discs.  Unless I had specified a contact resistance, the second body's interface should should the same temperature as the mating part, and then the heat should diffuse appropriately.   In Solidworks Simulation thermal analysis, when you have two materials of different conductivities bonded together, as far as the solver is concerned they are a single body, and the impedance value simply changes between cells that belong to one part vs. another.  As such, a continuous solution is shown in Solidworks Simulation where the heat diffuses through the cells closest to the mating part.  As far as I understand, when there is no specified contact impedance between parts, there should never be a discrete temperature drop at the boundary.

       

      Is there something I could have set up wrong to cause this?  Is the flow simulation program solving the mesh in a different way than I am imagining?  Thanks for the help!

       

      P.S., out of curiosity I ran a simulation with power dumped into both discs, and the same issue happened.  I have attached some images showing another example with a completely different model (still no contact impedance), as well as some 1 D numerical integrations I did in matlab to illustrate how it should look with and without contact impedance for mated materials of different conductivities.  It bothers me that I am seeing these results and it makes me question the model I have.

       

      Thanks!

       

      -John

       

      Message was edited by: John Bankert Updated matlab plots

        • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
          Matthew King

          Hi John,

           

          Looking at the Single_Heat_Source_Compare screenshot, it appears that the computational region is confined to just the solid bodies.  Are you sure you have the study setup as an external flow?  I was able to duplicate your two disc example with a 10" diameter and 1" thick (you didn't give dimensions in explanation).  I'm lazy so I used predefined materials I had in my library, glass for heated disc and aluminum for passive disc.  Thermal conductivities are still ~100000:1.  I get the following result with no sign of a discontinuity at the interface. 

           

          If you specified internal flow, it could be possible that simulation assumes each solids boundary as perfectly insulated.

          Disc Example.png

            • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
              Siavash Khajehhasani

              Good work Matthew! Just as a side note, as long as the default solid is selected while the heat conduction is solid is checked, no matter for internal or external flows, flow sim assumes all walls are the default material unless specified as different solid material.

              Cheers,

              - Siavash

              • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
                John Bankert

                Matthew,

                 

                Thanks for looking into this.  I did have my comp domain set up close to the body.  I re-ran it and still got a discontinuity.  I would be interested to see what would happen if you changed the scale on your result so that the lowest temperature was say, 303 K.

                 

                In the attached ("fixed_comp_domain.png"), I show an XY-plot through the center of the parts with a clear jump in temperature at the interface.  I wonder if this is really just something with the way the results are averaged and interpolated.  I used two vastly different conductivities because this exacerbates the effect (I assume by encouraging the high conductivity material to be isothermal), but it is still observed when I make both discs the same material (see attached "same conductivity.png").  

                 

                Additionally, to show that this causes absolute temperature answers to be incorrect, I did a test where I removed the flow, added a third body set to 20.05 C, then injected 1 W of power on the surface opposite of the body (see attached "no_convection_example.png").  The diameter of the discs is 2", the thickness is 0.1".  The ambient fluid temperature is 20.05 C.  Again using K=1 W/mK and K=100000 W/mk for the two bodies.  Analytically, the impedance through the thickness of these two discs is 31.8mK/W, and so the temperature rise from injecting 1 W of power should have been 31.8 mK maximum (if anything less because of conduction through the air to the sinking part, but this effect should be negligible).  However, the simulation results showed a temperature rise of 1.22 K (see "no_convection_example_sim.png").  I exported this model and attached it if anyone cares to look to see if something is set up wrong.

                 

                Anyway, thanks for looking into this!

                 

                -John

                  • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
                    Bill McEachern

                    couple things to consider:

                    1. in flow you have a finite volume scheme - things are evaluated at the cell centers (integration pts)  not at the boundary nodes as they don't really  have boundary nodes. In an FEA calc though the temperature variable is analogous to a displacement and is evaluated directly at the nodes. A finer discretization may help.
                    2. Try putting a control plane at the boundary between the two discs. The cut cell approx may have some impact on how things get distributed though I suspect not.
                    • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
                      Matthew King

                      I see your model is actually setup as a three disc stack.  Bottom is the thermal pad generating your 1W power, middle is the super conductor, and top is an epoxy.  In your initial conditions you set the temperature of the entire epoxy volume to 20.05degC.  I believe this is your problem.  You should remove this and set the temperature of 20.05 to the ambient conditions in the general settings.

                       

                      I removed the VS Temperature 1 boundary condition and reran your simulation.  Looks much better now.

                      2017-06-01 09_55_36-Document1 - Microsoft Word.png

                        • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
                          John Bankert

                          Matthew,

                           

                          The 3-disc model I uploaded was just an example for comparing analytical results to the simulation result.  I couldn't find a way to set the temperature of a surface so I did it using a whole new body.  The other simulations where I observed this behavior were done with only two bodies and no VS Temperature conditions.

                           

                          Some of the strange results, like seeing 3 different slopes through the bottom disc in your plot (second half of plot), appear to be the result of mesh density.  That effect was not present when I vastly refined the mesh.

                           

                          Additionally, thinking about Bills comment about interpolating from the center of the cell, that seems important in answering this question:

                          I know very little about CFD meshes and how the software handles them, but this seems like an answer to the question, and I am less worried about it now.

                           

                          That being said, it is a little concerning that the analytical result of simple conduction did not match the simulation result by an order of magnitude (see zip file from my last comment).  That is a different question for another time I suppose.

                           

                           

                          Thanks all!

                           

                          EDIT:

                               "That being said, it is a little concerning that the analytical result of simple conduction did not match the simulation result by an order of      magnitude (see zip file from my last comment).  That is a different question for another time I suppose."

                           

                          I rushed this calculation and forgot a unit conversion.  The result of +1.22 K as seen in simulation was almost exact (analytical result is +1.25 K).  Thank you all for helping me with my concerns. 

                            • Re: Conduction Temperature Discontinuities in Flow Simulation without contact resistance
                              Joe Galliera

                              John, SOLIDWORKS Flow Simulation (SWFS) solves the CFD problem based on the principles of the finite volume (FV) method, and it is no different from other finite volume solvers in that regard.  Reading up on the FV method might be helpful for you to understand its foundations.  The program has some really good documentation on its methods, such as its Technical Reference, that are already on your hard drive.  Ask your reseller how to find or access this document.

                              One additional thing that I will add is that the concept of a single cell per fluid region or solid body doesn't necessarily hold true in how SWFS handles its mesh; they have shifted this paradigm to a multi-control volume solver approach to treating the mesh cells.  You will notice this in your images where there are mesh cells that span multiple bodies whether they be fluid-solid or solid-solid boundaries.  You can read up more on this in a whitepaper that SOLIDWORKS had published with the help of the developers called "Advanced Boundary Cartesion Meshing Technology in SOLIDWORKS Flow Simulation."  The discussion of paradigm shift is specifically on pages 11-12 of that document.