25 Replies Latest reply on May 16, 2012 7:24 AM by Chris Michalski

    heat conduction in solids problem

    Daniel Cox

      I am having trouble with a flow simulation for a school senior design project.  Flow simulation is doing exactly what I need so far, but whenever I check the "heat conduction in solids" box under "General Settings" the simulation jumps from 15 minutes to over 24 hours.  Flow Simulation does a great job of showing the fluid flow lines and temperatures around the solids in my model but I need to see the heat gradient inside the solids as well.  Can Solidworks do this?

       

      My goal is to have a heat flux surface plot over a solid that has two different air flows around it.

       

      EDIT:  Uploaded the assembly.

       

      Message was edited by: Daniel Cox

        • Re: heat conduction in solids problem
          Chris Michalski

          you've likely got too fine of a mesh and/or there is a large change in temperature from initial conditions to equilibrium.

           

          Try generating some local meshes to increase precision where you need it and avoid it where you don't.

           

          Then refine the initial conditions of the solids to give it a head start towards the equilibrium temperatures.

           

          If it is taking 15 minutes for only fluid flow you either have a large/complext model or you have the mesh set way too fine.

            • Re: heat conduction in solids problem
              Daniel Cox

              There is indeed a large change in temperature.  I am trying to determine the steady state temperature of a plate with one side mated to a body held at 60 degrees F and the other side exposed to 700 degree F exaust. 

               

              The mesh is set to a value of 3 in General Settings.   

               

              How do I generate local meshes?

                • Re: heat conduction in solids problem
                  Chris Michalski

                  so you need a fine resolution in the solid but not the gas around it?

                   

                  to make a local mesh you need to define a solid that is the volume in which the mesh will be refined - I typically make a part slightly larger than the intended volume, say 10% larger in each dimension.

                   

                  In component control you disable that part - this way it does not attach solid properties to it for the simulation.  Then Flow Simulation -> Insert -> Local Initial Mesh.

                   

                  I never use the automatic settings, none of my models are adequately served by that, so I can't say what level of resolution to attempt.  I'd drop the overall resolution by a level or two and when you insert the local mesh increase that by the same to start.  Generate the mesh without solving and look at the size of the mesh for the solid relative to the fluid.

                   

                   

                  Have you taken classes in CFD or is this just trial and error hoping for an answer that looks right?  (Most times) CFD will give you the correct answer, the details are in making sure you ask it the question that you intend to (and knowing the difference between the two).

                    • Re: heat conduction in solids problem
                      Daniel Cox

                      Yes that is what I need.  Are you saying I should create a new part around the part in question in order to define a volume?  Can I just create a large cube and place it around the plate I am analyzing?  

                       

                      By "disable" do you mean hide the part?  I'm not sure I know what you mean. 

                       

                      This is mostly trial and error.  I have taken fluid dynamics, finite element analysis and Solidworks classes but none of them have really prepared me for this.  I appreciate the help.

                        • Re: heat conduction in solids problem
                          Chris Michalski

                          yes, create a similar part that is larger then add it to the assembly.

                           

                          In the Flow Simulation menu there is a sub-menu called "component control" - use this to disable the new part.  Hiding it only means you can't see it, it is still there.  If you supress it then you can't use it at all, if you disable it that simply means it isn't a solid (think of it as a wireframe).

                           

                          what is your Sr design project?

                            • Re: heat conduction in solids problem
                              Daniel Cox

                              Ok I will implement this tonight and let you know how it goes.  It seems like I must be doing something really wrong to make the simulation last so many hours.

                               

                              Our project is to model the heat gradient on the surface of a plate that is near hot exaust from a jet engine.  The exaust vent in the model is only a few inches away.  It blows hot air at an angle so that one side of the plate is hotter than the other.  Once we figure out how to model heat transfer inside the plate we will create a few variations of the plate and try to reduce the heat flux on the surface.

                                • Re: heat conduction in solids problem
                                  Bill McEachern

                                  You could just pick the part you are interested in for hte mesh control and just not diable it if you only want the higher resolution inthe solid. The cell growth rules will make the mesh in the neighboring fluid a bit more refined and will drop off quite quickly. If you don't need the extra fluid cells this is less work, Chris's way  way works fine too..

                                  • Re: heat conduction in solids problem
                                    Chris Michalski

                                    is the one side truly held at 60deg? i.e. is it water cooled with a high flowrate?  If you mean it is exposed to air at 60deg that makes a huge difference.

                                     

                                    Part of the problem may be that with a thin plate it is going to take a low of cooling to maintain such a drastic temperature gradient and therefore take a long time to solve for the gradient.

                                    • Re: heat conduction in solids problem
                                      Rich Bayless

                                      Hello,

                                       

                                      this problem sounded familiar.  take a look at:

                                       

                                      https://forum.solidworks.com/message/136406#136406

                                       

                                      Feel free to post your model.  Use 'Pack and Go' under 'File' to create a zip file of you model.

                                       

                                      Which version of SW are you using?

                                       

                                      Rich.

                                      • Re: heat conduction in solids problem
                                        Bill McEachern

                                        I haven't read all the posts so forgive me if I am not on target. You can really speed up a heat transfer calc by using flow freezing but it is a tad risky depending on the problem. Risky in the sense you can get a seriously wrong answer but it works great for hte right type of problem - which this sounds like. When it is invoked it holds the convective terms (flow) constant and allows the diffusive processes (heat diffusion in this case) to advance quite quickly. I would use the default sttings and give it a rip. Check out the help from the menu. It is under calculation control options, advanced as I recall. Use the periodic settings. if the your flow only goals are settling down by 0.25 travels then go with the defaults. If not, use however many travels is required so the flow part of the problem has more or less settled down (the convective terms).

                                      • Re: heat conduction in solids problem
                                        Daniel Cox

                                        I created a very fine mesh around my panel and set the rest of the mesh to be rather low resolution.  The mesh calculations took 2 or 3 minutes but the simulation itself still blew up.  I uploaded the assembly (without any initial meshes) in case you want to look at it yourself.  It is in Solidworks 2010 format. 

                              • Re: heat conduction in solids problem
                                Daniel Cox

                                Does anyone else have any advice?  I've tried creating local meshes but the simulation still won't finish.  The file is up as well if anyone wants to take a look. 

                                  • Re: heat conduction in solids problem
                                    Rich Bayless

                                    Hello Dan,

                                     

                                    I ran the model as-is, see attached screenshots.  1.3 million cells, predicted run time about 60 hours.  Only one warning.

                                     

                                    Supersonic flow, external study, conduction, 1.3 million cells, seems to me that 60 hours may not be unreasonable.

                                     

                                    Suppressing the 'initial mesh' and using automatic meshing, set to 1, gives 350k cells, predicted run time of 15 hours.

                                     

                                    Reducing the computational domain manually, brought the cell count down to 170k cells, predicted run time of 9 hours.

                                     

                                    Rich.

                                      • Re: heat conduction in solids problem
                                        Chris Michalski

                                        Rich -

                                         

                                        on a slight tangent - you say "Supersonic flow, external study, conduction, 1.3 million cells..."  Does the supersonic flow result in longer solve times typically?

                                         

                                        I've got a series of models (external, conduction, and radiation) I've been running lately with 1.4M cells that clocks in at a repeatable 24 hours in Flow2009.  I know radiation adds time because it has to solve the resulting rays at each iteration but I didn't realize that supersonic has a noticeable impact on solve time.  How much of a factor is it?  I could see things being less stable and requiring more iterations to settle out but does the calculation algorithm actually take longer?

                                          • Re: heat conduction in solids problem
                                            Rich Bayless

                                            Hello Chris,

                                             

                                            Honestly, the models I've done for work don't require the supersonic option, so I don't have direct experience with supersonic modeling time.  I'm assuming that turning on the supersonic option will require more solution time, which is why they make it an option.

                                             

                                            Probably got myself in trouble with assumptions......

                                             

                                            Rich.

                                              • Re: heat conduction in solids problem
                                                Chris Michalski

                                                I think everytime it told me I needed it I used that as an indicator that I'd screwed something up in my setup.

                                                 

                                                I've never used it to know so I figured I'd ask and put that in my "things that might be useful to know someday" memory.  You know, just in case I get lucky and when I meet Alex Trabek the Final Jeopardy category is Solidworks Flow Simulation

                                            • Re: heat conduction in solids problem
                                              Daniel Cox

                                              Thanks for looking at it, Rich.  I was hoping there would be another solution besides reducing the mesh size but it looks like that is the issue after all. 

                                               

                                              I will simply have to make do with a smaller, less fine mesh. 

                                               

                                              Is the "supersonic flow" option necessary immediately after mach 1?  What about 1.2 or 1.5?  

                                                • Re: heat conduction in solids problem
                                                  Rich Bayless

                                                  Hello Daniel,

                                                   

                                                  If you want to reduce the cell count, you could try changing from an external study to an internal study.  External studies always seem to default to a high cell count, which is why I reduced the computational domain manually.  Add an 'enclosure' to mimic a wind tunnel, such as a cylindrical tube or a rectangular tube.  Add an inlet lid and an outlet lid and set your boundary conditions.  Let us know what you find out.

                                                   

                                                  Rich.

                                                    • Re: heat conduction in solids problem
                                                      Daniel Cox

                                                      The wind tunnel idea is working great. I still had to reduce the cell count manually but the results are more consistent.  I'm not getting insane max mach number values anymore.  On the external study previously there would be certain cells with mach 5 air flow and above even though the inlets are mach 0.85 and 0.91.  Convergence is faster as well.

                                              • Re: heat conduction in solids problem
                                                Shahrul 88

                                                Hi All, sorry for interrupt..

                                                 

                                                I'm using solidworks to do convection heat transfer in the microcomputer. The problem is my understanding on the number of iterations.

                                                 

                                                2 simulations are done through 2 different setting on the iteration:

                                                       1) goals convergence (result obtained as in Pic 1 attached - stop at iteration 56)

                                                       2) maximum iterations = 42 (result obtained as in Pic 2 attached - stop at iteration 42)

                                                 

                                                How do I explain about the differences of data ( in this case temperature) at iteration 20 and iteration 30??

                                                For goals convergence; what is mean by goal convergence?? is it equilibrium state/ condition??

                                                 

                                                This number of iterations are not explained about time, am I right?

                                                 

                                                Thanks

                                                 

                                                Pic 1.JPG

                                                 

                                                 

                                                Pic 2.JPG

                                                  • Re: heat conduction in solids problem
                                                    Chris Michalski

                                                    Shahrul -

                                                     

                                                    For all pratical purposes these runs are the same, I have seen much more variation run to run in my models.  Did you change anything in the model? (e.g. mesh settings?)

                                                     

                                                    Goals convergence lets you tell FlowSimulation what values are critical.  If you are looking specifically for the temperature of one component in a large assembly, you can let Flow stop the simulation when that part has stabilized, even if other parts are not completely stabilized.

                                                     

                                                    When you setup your model you set goals - these are the conditions that Flow makes sure have converged, otherwise the simulation will run for a set number of iterations/travels (either not long enough to converge or longer than necessary wasting time).  If you rerun that simulation with goals and click the Goals Table icon while it is solving it will show the value of each goal and which goals have converged.  Goal convergence simply means that the change in that parameter (max temp, min velocity, etc) has stabilized and the change from one iteration to the next is insignificant.  If all of the goals are not converged it has not found the steady state solution yet.  It is much better to set goals than to manually select a limit to the # of iterations.

                                                     

                                                    (In the future start a new thread for a new question, it makes it simpler.)