17 Replies Latest reply on Oct 25, 2011 4:54 PM by Thimal De Alwis

    How to simulate heat transfer in Solidworks Simulation (Premium)?

    Thimal De Alwis

      Hi all,

       

      I have an assembly in Solidworks 2010, and I am trying to simulate heat transfer throughout the component using the Simulation tool.  Basically, I want to heat the top of the component at 210 C and then allow heat to flow through the component and then radiate to the external atmosphere (say at 25 C).  I am doing this in order to see how long it takes for other parts of the assembly to reach a desired target temp (say 100 C).

       

      Right now, I have defined a Thermal Study in Solidworks Simulation, and applied several thermal loads.  I defined the Initial Temperature of all exposed faces to be room temperature (25 C), and then defined the Temperature of the top face to be 210 C.  I also have a Radiation load (surface to ambient) that specifies that all exposed faces radiate to the ambient 25 C atmosphere.  However when I make a mesh and run the thermal study, the results do not seem right...my entire assembly reaches 210 C within 100 seconds (which seems unrealistically quick) and no heat seems to dissipate to the atmosphere.  Any thoughts on what I am doing wrong or defining incorrectly?

       

      - T

        • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
          Jerry Steiger

          Thimal,

           

          In most cases radiation is not the main way that heat gets lost; you need to model the heat transfer to the air. That will require you to come up with good estimates of the heat transfer coefficients on your various surfaces or to run a CFD analysis. I think the number you need is called the film coefficient, h, but it's been a long time since I did any thermal analysis.

           

          Jerry Steiger

            • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
              Anthony Botting

              I concur. It appears not enough heat is getting out of the unit. You can try something like 5 to 100 W/m^2-K as a convection coefficient on exposed-to-air surfaces (that is kind of a ball-park number I've seen used to estimate natural convection to still air). Typically, that convection coefficient (h) is tuned to give a reasonable answer (I'm assuming you have test data).  Hope that helps. -Tony B.

                • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                  Thimal De Alwis

                  In fact, I'm trying to validate test data with simulation results!!  So I am trying to avoid using test curves to calculate coefficients for the time being...

                   

                  I think the limiting factor for me is not understanding the fundamental difference between convection and radiation.  I was under the impression that radiation is when heat dissipates from a surface to the atmosphere (air, etc.), and that convection is when one body is heated by another as heat travels through some medium (air, liquid, whatever).  But you are saying that my stated application is heat transfer via convection??

                   

                  Additionally, I would like to know how to use SW to simulate heat transfer through two surfaces that are actually in physical contact?  Would this just be a surface-to-surface radiation load?

                   

                  My last question regards specifying conditions on loads.  Is it possible to specify that a certain condition is only "on" for a certain part of the study?  For example, I would like to have the top surface heated for only the first minute of a 10 minute study; after the first minute, I want the temperature to remain and dissipate to the atmosphere as the rest of the plug is doing.

                   

                  I tried using a Time Curve for this Temperature load condition, but that does not give the desired effect (I just want to specify that the temperature of the top is 210 for 0-60sec, but I do not know what the temperature is beyond 60 sec, and I want SW Simulation to solve that for me).  Any tips?

                   

                  Thanks again.

                   

                  - T

                    • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                      Jerry Steiger

                      Thimal,

                       

                      Validation usually runs the other way from simulation to test. Simlulations make lots of assumptions that may or may not be true.

                       

                      Radiation is not to the atmosphere, it is to whatever other radiating surfaces are visible to the radiating surface you are interested in. It varies with the fourth power of the absolute temperatures of the radiating surfaces. If there aren't any other radiating surfaces, then it is the sky that serves as the other surface. Unless you have a really hot body or are in a vacuum, radiation is usually not very important.

                       

                      Convection is how a solid body exchanges heat with a liquid or gas that surrounds it. It depends on material properties of the fluid, the difference in temperature between the fluid and the solid and also on the geometry of the surface. For buoyancy driven convection it is higher for a vertical surface than for a horizontal surface, lower for the bottom of a horizontal surface than the top of a horizontal surface, for example.If lf you've got a fan or pump to force the fluid to move past your object the heat flow is usually much higher.

                       

                      Conduction is the flow of heat inside and between solid bodies. It depends on the material properties and on the temperature differences. When you have two bodies touching, you have to consider things like surface roughness, so that you have a much smaller area to conduct across than you expect.

                       

                      I'm not familar at all with how SW Simulation handles thermal analysis, but I suspect that you can't solve the problem the way you are trying to do it. If you drive a temperature at a surface, you probably can't let that surfaces temperature be a driven variable at a later stage in the analysis. I also suspect that you can't put a certain heat flow on that surface and then let the heat flow become a driven variable at a later stage. Somebody who actually has experience with this type of simulation will have to help you out with that.

                       

                      Jerry Steiger

                        • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                          Regis WACHEUX

                          Thimal,

                           

                          Check the initial temperature of all the points. Are they defined ?

                          The initial condition should be that all points, including inside the model should have the intial temperature, and not only the external faces.

                           

                          To do this and be sure of the input, I run a pre-study, specify a static thermal study with only boundary condition of a heat exchange of exposed faces at 25 °C with a fictive coefficient of say h=1000.

                          The result is a mesh with all nodes having the (correct) intial temperature of 25 °C.

                          This can be verified in the graph results or exported table (node position,temperature).

                           

                          Then, create a thermal transient study with this pre-model as "input temperature", where other boundary conditions vary with time.

                           

                          >My last question regards specifying conditions on loads.  Is it possible to specify that a certain condition is only "on" for a >certain part of the study?  For example, I would like to have the top surface heated for only the first minute of a 10 minute >study; after the first minute, I want the temperature to remain and dissipate to the atmosphere as the rest of the plug is >doing.

                           

                          For that, you can run a study with 1 minute time.

                          Stop the study when the temperature load is to be stopped.

                          Then introduce a transient study with this model result as input, and other boundary conditions (heat dissipation in air where the input temperature load was), to run for the other 9 minutes.

                           

                          note1: this model sequence works if the meshes are copied from one study to the other.

                          If there are specific mesh refinement needed in the 3rd study, they must be in a way taken into account in the 1st mesh.

                           

                          note2: Similar to Anthony, I usually use h=5 to 50 W.m-2.K-1 as a convection coefficient on exposed-to-air surfaces (5 to 10 for still air like in enclosures). This gave ususally good fittings between simulation models and test results.

                           

                          note3: verify the input temperature of the top face when introducing a temperature step with a time curve (graph).

                           

                          I can provide a 3-step thermal study with these parameters if this could be needed.

                           

                          hope this helps.

                          Regis.

                          • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                            Wayne Matus

                            Jerry, So Pamela Anderson radiates?

                            Jerry Steiger wrote:

                             

                            Unless you have a really hot body or are in a vacuum, radiation is usually not very important.

                    • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                      Thimal De Alwis

                      When I try to run a mesh on my assembly now, I get the error: "Incompatible initial temperatures" before any time steps are run.  However I checked the pre-study (initial temp everywhere = 25 C) using a probe, and all values read 25 C.

                       

                      Furthermore, I tried the the same procedure on one of the sub-assemblies within the main assembly (imagine, a plug that seals the top of the tube).  When I tried running the mesh on just the plug, which contains many parts by itself, things worked fine and I was able to successfully heat the top of it and then "turn off" the heating to allow the system to cool...free of errors!!

                       

                      But when I do the same thing for the tube + plug assembly, it gives me "Incompatible initial temperatures."  I even used exactly the same faces for the convection load in both studies!  Has anyone else experienced such a problem?

                       

                      - T

                       

                      P.S.  Regis if you could explain why, in your second study, you have a temperature load set to 1 C?  I realize you are using a time-curve that gets it up to 210 in very few seconds, but I don't understand why the load still displays 1 C as the value in the FeatureTree.

                        • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                          Regis WACHEUX

                          Thimal,

                           

                          a) The mesh of the thermal pre-study must be copy/paste or drag/drop to the static study. This should solve the issue.

                          Same nodes positions will be defined.

                          Do not let run a (new) mesh computation on the 2nd study before running it.

                           

                           

                          b) The "variation with time" curve introduced is multiplied by the figure in the temperature input window.

                           

                          Instead of having a 210°C in that cell, and a multiplying factor as time curve parameter, I better read the temperatures in the time curve.

                          FEA623(10).jpg

                          --> "Edit"

                          FEA623(11).jpg

                           

                          --> "Graph"

                          FEA623(12).jpg

                          The maximum temperature is 210°C.

                           

                           

                          just as exercise, type "10" in that cell

                          FEA623(13).jpg

                          The maximum temperature becomes 2100°C ! ...

                           

                           

                          FEA623(14).jpg

                           

                          The 1 "Celcius" written can indeed be confusing.

                           

                           

                          Regis.

                        • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                          Thimal De Alwis

                          Dear Regis,

                           

                          That makes a lot of sense.  I made the changes as you specified, and I can succesfully run a mesh on my assembly, shutting off heating after a certain time.

                           

                          However, the only problem I am facing is that the heating does not seem to transfer across the inside atmosphere to the walls of the tube.  Right now, I have a plug sitting inside the top of a tube.  The top of the plug is heated, and heat dissipates through the plug body.  However the tube and other components further down inside the tube remain at the initial temp. of 25 C.

                           

                          The only conditions I have specified so far are the temperature of the time curve (set to 210 C) for the top of the plug, and the convection at 10 W/m/K from all exposed surfaces to room temp. (25 C).  I did not specify any Contact Sets because I am approximating the "roughness" of coincident surfaces by assuming a very thin layer of air between them.  Basically, I just want to simulate the heat from my heated plug convecting across these very thin air layers to heat the walls of the tube, etc.

                           

                          Would I be better off having the parts physically coincident in my model, and then specifying contact surfaces with some thermal resistance?  This is not the way I wanted to approximate it, but I am having a hard time getting convection to work out...

                           

                          - T

                           

                          P.S.  Additionally, I was wondering if there was any way to use the study temperatures from one model as the initial temperature of another model, IF the model is slightly changed (for example, if I use some type of material that in reality changes shape with temperature).  Is this possible, or will it yell at me for having incompatible initial temps and non-matching meshes?

                           

                          P.P.S.  Is there any way to obtain the maximum/minimum temperature for just a section of the model?  I tried using a section clipping and showing the max/min values in the thermal plot, but it only shows the max/min of the entire assembly.  Sorry for having a billion questions, I am learning new things in Simulation everyday and this thread is a main reason for that

                            • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                              Regis WACHEUX

                              Thimal,

                              Try to treat the air gaps as a "solid" medium with a geometry, and fix a heat convection coefficient.

                              Air.PNG

                              However, if the air gaps are very small you would need very fine meshes and this could be computer time consuming, or even not mesh at all.

                               

                              Try to have the parts in contact, define contact sets with thermal resistance at the contact surface(s). This will have the heat to progress in your model. Although finding the correct parameters could be difficult.

                               

                              for P.S: I don't know how this can work.

                              Eventually create a static study from the thermal study, show the deformed shape, save the deformed shape as new geometry (configuration) and use it for the next temeprature input as new geometry.

                               

                              for P.P.S : For this, I need to have access to a face. if that section is always at the same place (for comparisons), I create a split of the model, or explode an assembly model. In the result graph, with exploded view, RMB select Probe Result, 'On selected entity', select the (visible) face, 'Update'. you have the nodes position and values. The min/max is in the summary section. The result can also be saved as CSV file.

                               

                              FEA623(20).jpg

                               

                              note : for a face or split face of a model, the mesher will have created nodes on that face.

                              You will get the nodes results that have been calculated.

                              For a section view, it can be that the section does not cut any node, and the nearest node value is taken, which could introduce approxmative results.

                               

                               

                              hope this helps.

                              Regis.

                            • Re: How to simulate heat transfer in Solidworks Simulation (Premium)?
                              Thimal De Alwis

                              One additional question...is there a way that Solidworks can calculate the total amount of heat that has been transferred in a transient model?  I tried using the Res Heat Flux thermal plot, but I am not sure what area they are considering when they report min/max values of W/m^2.  Additionally, the value I calculated for heat is far higher than I expected (on the order of kJ rather than J), so I am suspect of this method...

                               

                              - T