17 Replies Latest reply on Oct 5, 2010 11:25 AM by Bill McEachern

    Speckled Stress Plots

    Chris Michalski

      I'm relatively new to running SW stress simulations but have been doing CFD simulations for ~6 years.  I recently encountered a bizzarre stress plot resulting from a simple thermal profile.

       

      I have a tubular heat exchanger that I have run FloWorks simulations to define the temperature fields.  I had Simulation import that temperature data and calculate the stresses resulting from thermal gradients.  I used the same procedure I have for other models that worked out as expected.

       

      I originally included the pressure data but eliminated that because I thought it might be the problem.  In the past similar modesl have come out as expected, low stress in uniform temperature unrestrained areas, higher stress in restrained areas.  The only difference is in the way I defined the fixture points on this model and they are not close to this inlet tube so I don't see how those should have caused this issue.

       

      HOWEVER, for some reason this model is generating a speckled stress plot.  Common sense says that in an unrestrained region with a uniform temperature you shouldn't have high tension and high compression intermixed, they will relieve to some middle ground.

       

      Anyone ever see anything like this and have an idea how to resolve it?  I have tried altering the mesh parameters, both standard and curvature based, smaller cells down to the point of hours to mesh and days to solve.

       

       

        • Re: Speckled Stress Plots
          Daniel Mundstock

          Hi Chris,

           

          What boundary conditions are you using in the structural simulation?

            • Re: Speckled Stress Plots
              Chris Michalski

              Daniel -

               

              All of these tubes are connected to a center mounting disc.  I have 3 points on that plate restrained vertically with respect to the top plane to prevent movement.  I have also tried a single point and fixing the oepn end of the tube - all with similar results.  I am using the Inertial Relief option as I have for all of my models.

               

              I have a plot of a similar model (a previous revision) that generates nice orderly profiles (see attached).

               

              I included an expanded view of the original query to give a bit more info and show that it's not a local phenomenon.

                • Re: Speckled Stress Plots
                  Daniel Mundstock

                  Have you tried to no use the Inertial Relief option? Just to check if it is influencing the results.

                  • Re: Speckled Stress Plots
                    Bill McEachern

                    You need to send this to support - something is busted by the looks of it.

                     

                    I recently have had Flow simulation get sort of corrupted where, in my case, I picked surfaces for a plot of say temperature and a different set of surfaces would plot than the ones I selected. Most of the time if I picked the offset option (at 0 offset) it would then plot the right surfaces. That bug is filed. However, in the same model, different analysis, I had other surfaces that would not plot correctly no matter what controls I selected and the only way I found to fix it was to re-run the model. I have no idea what was going on or why the offset option would even make a difference.Given that you have successfully done these before finger trouble seems unlikely. The plot clearly shows that what you are getting is junk and inconsistent with the temperature regime displayed. You need to send it in.

                      • Re: Speckled Stress Plots
                        Chris Michalski

                        Bill -

                         

                        um..thanks?  that wasn't what I was hoping to hear.  I have another FloWorks simulation (same revision, different boundary conditions) almost completed that hopefully will resolve the issue.

                         

                        Problem is we had to cut our support contract due to budget crunches - can I still submit a problem to SW or do I need to be on a maintenance contract?

                          • Re: Speckled Stress Plots
                            Bill McEachern

                            Not all that sure on that one. Try going to the SWX web site and see if there is a place to submit a bug and do that. I would advise though that you supply all information required to reproduce it - otherwise I doubt they will put any effort into it. If you could get a small simple file to reproduce the results it would be best.

                             

                            One thing did occur to me on this: To get this type of analysis to work properly the FEA analysis needs to be done in the same assembly/part file as the global coordinate system of that file is the key to getting the cell temps mapped into the correct locations for the structural FEA. If for any reason that between the CFD and the FEA run that any of the parts had moved relative to the global coordinate system that could produce funny looking results. You have vast differences between what appears to be adjoining elements and that seems really odd to me. You might want to plot the elemental stress and see what that looks like. I would try your technique on something simple and see if you can get this result. If so it might be a finger trouble thing, if not then something is pretty wrong with this particular analysis and you try and figure it out. Good luck.

                              • Re: Speckled Stress Plots
                                Chris Michalski

                                how much does the STAR.exe hit your hard drive?  since I've just started stress simulations in the past few months I'm used to FloWorks using an entire core continually, I'm always processor speed limited.  STAR only hits for maybe 0.20% every 10 seconds which just seems like a crawl in comparison.

                                 

                                Does that sound right?  It seems to be vastly underutilizing the processor.  Granted, it is running 21GB of RAM and Page File (12GB physical RAM).  Is there anyway to speed things up?  If I add more page files on other partitions can I at least make it appear that I'm making progress?

                                 

                                For similar models (i.e. same geometry and Flow data and only revising the mesh from .138" to .135") the mesh time is similar but the solve times are vastly different.  I was hoping that with tweaking the mesh I'd eliminate the odd spots because the high stress spots corresponded with jumps in the mesh.

                                  • Re: Speckled Stress Plots
                                    Bill McEachern

                                    If you can't get the job to run in core it will take a really long time to solve. So it works like this, if you run in core it runs really fast, as soon as you cross the threshold to not being able to hold the whole job in core you drop to a crawl. Floworks requires the entire job to run in core or it won't even solve correctly. You can vastly reduce memory requirements by using the FFE solver. The sparse solver is a memory hog of enormous proportions by comparison. The FFE solver doesn't handle all analysis but since you are transferring results from flow you are probably running an entirely solid element mesh which is the FFE's solvers sweet spot. And if there are not great differences in stiffnesses in the materials used in the model (probably your case given as it looks like an all metallic structure) it should run at comparable speeds to a sparse solution running in core, maybe even faster. If you are already running an FFE solution and still consuming 21GB of RAM you probably hold the world record for the biggest SolidWorks simulation model ever attempted - assuming nothing much else is running on the machine. How many DOF (degrees of freedom) are being reported in the solver window when it is solving? Even if you are using the sparse solver the model size seems crazy big. The FFE solver would drop your memory requirements by a very large factor like say 5-10 if I had to guess.

                                      • Re: Speckled Stress Plots
                                        Chris Michalski

                                        I'm pretty sure that FFE is the default solver I'm set to.

                                         

                                        It's an entirely solid model, I'm only analyzing the thermal strain induced stresses in the one part (solve the entire model in FloWorks, then disable all but 1 part.)  I'm only concerned about the stresses in the one part (of course the most complicated one).

                                         

                                        There are 7,473,407 Nodes, 4,596,624 Elements, and 22,420,221 Degrees of Freedom.  Because it's a tubular structure I can't really reduce resolution due to the tube thickness.  I might be able to look into revising the mesh so I have lower resolution in the straight tube section and increase mesh density at the u-turn ends.

                                         

                                        Your comment about the speed dropping when you cross the threshold would be the reason that such a small change in mesh sizes causes such a drastic increase in solve time.  I'm just too much of an engineer, I keep thinking I live in a linear world.  So that means that Solidworks is itself a non-linear solver? sounds like there's a step function in there ha ha

                                          • Re: Speckled Stress Plots
                                            Bill McEachern

                                            well, 22 million DOF is non trivial and is the largest problem I have ever heard of being tackled with SWX Simulation. I would get more RAM - if your existing board with 6 slots can handle 4 GB DIMMS then go get some of those if your mobo can handle that. or a new box - say a dual core box that has lots of slots for cheap RAM a Supermicro workstation would cost say $5k or so with moderate processors & 24 GB of RAM.

                                             

                                            You could always explore ways to use shell elements and assume the through thickness temp variation is zero...there might be ways to fool that one into happening. Haven't ever tried it. Say take the temps into a thermal study add a shell elements to that and see if you can get the temps to the shells and then do the structural once you have that done. Might be a way......

                            • Re: Speckled Stress Plots
                              Derek Bishop

                              I've seen it before. Make sure the mesh between the two studies are identical. Copy the mesh across from one study to the other.