14 Replies Latest reply: Apr 2, 2014 3:33 PM by Jared Conway

    Frequency Analysis Errors/Problems

    Atif Khan

      I am running a frequency analysis on Solidworks Simulation (Version 2013 SP5). The objective is to find the resonant frequencies on the assembly. The assembly model that I have is not a very large model and after simplifying the model I am down to approximately 25 parts. However the parts in question have pretty complex and small geometries. So much that I had to use 9 different types of mesh controls (Element size ranging from 0.1mm to 4mm) on a lot of surfaces. I did this since I am after more accurate results. (I have already run the test on the same model using a very average sized mesh. But the mesh looked horrible so I do not know how accurate the results were). To increase accuracy I also tried to use a finer curvature based mesh (Max Element size 20 and Min Element size 4). The resulting mesh was much better.

       

      I ran the simulation on this mesh using an FFEPlus solver for around 50 frequencies but the problem that I was facing was that the simulation was completed to approximately 18.2% in around 3 minutes and was stuck at the same place for over 2 and a half hours. I assumed that the solver might be having convergence troubles and so aborted the simulation.

       

      I tried running the simulation using the Direct Sparse solver. During the simulation I noted down the following

       

      DOF: 30251808

      Number of Nodes: 10161435

      Number of Elements: 6647214

       

      In the middle of the simulation (at approx 30%) the solver window changed and the numbers had changed to

       

      DOF: 251808

      Number of Nodes: 161,435

      Number of Elements: 47,214

       

      Is this normal? (Looking at it carefully 30251808 was reduced to 251808. The reduced DOF is just the last few digits of the original DOF. You can see the same pattern in  nodes and elements). After trying to start the simulation in the new solver window I got the following error

       

      "DSTAR has stopped working"

       

      Then I tried consulting my reseller and read a few topics on the forums here. They all advised to simplify geometry further or reduce the number of elements or try different solvers. Not wanting to compromise too much on the accuracy I used a coarser curvature based mesh (Max Element Size 30 and Min Element Size 6) and reduced the mesh control on a few surfaces and ran the mesh. It still looked pretty decent and uniform. To reduce calculation times I also reduced the number of frequencies from 50 to 30. 

       

      I tried running the simulation using the Direct Sparse solver. Again I noted down the following

       

      DOF: 26660055

      Number of Nodes: 8964094

      Number of Elements: 5855154


      Again In the middle of the simulation (at approx 30%) the solver window changed and the numbers had changed to

       

      DOF: 660056

      Number of Nodes: 964094

      Number of Elements: 55154

       

      Again I got the following error

       

      "DSTAR has stopped working"

       

      Then without changing the mesh I tried running the simulation using the FFEPlus solver. The DOF, Nodes and Elements remained unchanged. At approximately 18.2% of the simulation being completed I got the following error.

       

      "STAR has stopped working"

       

      I am not really sure now how to deal with the problem. Is there a way to get around the problem without making changes to the geometry? Or without compromising on the accuracy?

        • Re: Frequency Analysis Errors/Problems
          Shaun Densberger

          However the parts in question have pretty complex and small geometries.

           

          I can't say for certain without looking at the geometry associated with your system, but you probably don't need the small features.

           

          ...I had to use 9 different types of mesh controls (Element size ranging from 0.1mm to 4mm) on a lot of surfaces. I did this since I am after more accurate results.

           

          Displacements and frequencies are the primary solution for a finite element model (strains and stresses are a secondary), so you can typically get good results with a somewhat coarse mesh. That being said, you don't know how well your simulation has converged unless you do a coverage study (looking at how the results vary with the mesh). I would start with a coarse mesh (and simplified geometry), solve the system, record your frequencies, refine the mesh a bit, solve, record you new results, and repeat until you have the desired level of accuracy.

           

          I ran the simulation on this mesh using an FFEPlus solver for around 50 frequencies but the problem that I was facing was that the simulation was completed to approximately 18.2% in around 3 minutes and was stuck at the same place for over 2 and a half hours. I assumed that the solver might be having convergence troubles and so aborted the simulation. I tried running the simulation using the Direct Sparse solver. I tried running the simulation using the Direct Sparse solver. During the simulation I noted down the following

           

          DOF: 30251808

          Number of Nodes: 10161435

          Number of Elements: 6647214

           

           

          While it is true that different solvers are better depending on the size of the problem, I think the main issue is the fact that you have over 30 million DOF; that's huge....really huge. I don't know why SW would end up changing the number of DOF, so this is all speculation, but it might be a memory issue. How much memory does your system have?

           

          Then I tried consulting my reseller and read a few topics on the forums here. They all advised to simplify geometry further or reduce the number of elements or try different solvers. Not wanting to compromise too much on the accuracy I used a coarser curvature based mesh (Max Element Size 30 and Min Element Size 6) and reduced the mesh control on a few surfaces and ran the mesh. It still looked pretty decent and uniform. To reduce calculation times I also reduced the number of frequencies from 50 to 30.

           

          I tried running the simulation using the Direct Sparse solver. Again I noted down the following

           

          DOF: 26660055

          Number of Nodes: 8964094

          Number of Elements: 5855154

           

          26 million DOF is still a very big model (for example, I think NEi Nastran 64-bit can only do something like 25 million DOF)...we need to go smaller....

           

          I am not really sure now how to deal with the problem. Is there a way to get around the problem without making changes to the geometry? Or without compromising on the accuracy?

           

          You need to start with a coarser mesh and simpler geometry. Again, I can't say for certain without seeing your model, but these small features probably don't have a meaningful effect on your results. Start with a basic model (geometry and mesh) and work towards a more complicated one.

           

          Can you post a picture of your assembly, as well as a picture of it with your current mesh?

            • Re: Frequency Analysis Errors/Problems
              Atif Khan

              Thank you very much for the reply Shaun. Your help is much appreciated.

               

              Some small geometry are necessary and are part of the system. Other geometry are intended to give the assembly an advantage in environmental tests. It should be seen when I run linear dynamic analysis. There are some geometries that I can remove. So I will try and simplify the model further. I have attached the PDF's of our assembly. Hope this helps

               

              "Displacements and frequencies are the primary solution for a finite element model (strains and stresses are a secondary), so you can typically get good results with a somewhat coarse mesh."

               

              You are absolutely right but even though my objective now is just to check the resonant frequencies. I had intended to configure the mesh such that I could converge the Mass Participation Factor too. That is the reason I had started out with high number of frequencies. To save time I had intended to use the same mesh for when I carried out linear dynamic analysis. In that study checking stresses will become more important.

               

              You have recommended the "bottom to top" approach where I start off with a coarse mesh and then work up to a finer mesh. But what do you think about "top to bottom" approach where you do exactly the opposite? Do you think that it is a good idea?

               

              I have about 90GB worth of space left on my hard drive.

               

              What is the maximum DOF that solidworks simulation can handle? Any idea?

               


                • Re: Frequency Analysis Errors/Problems
                  Shaun Densberger

                  Some small geometry are necessary and are part of the system. Other geometry are intended to give the assembly an advantage in environmental tests. It should be seen when I run linear dynamic analysis. There are some geometries that I can remove. So I will try and simplify the model further.

                   

                  I agree that the geometry is part of the system, but will it add a meaningful effect to the system's performance? For example, all of those heat-sink fins (I'm assuming); do you feel that have a meaningful impact on the results your after? It's hard for me to say yes or no because I don't have the intimate knowledge of the design that you do. Just remember that (roughly) if you double the number of DOFs in your system, you quadruple the time required to solve.

                   

                  I have attached the PDF's of our assembly. Hope this helps

                   

                  Mother of God.png

                  All jokes aside, that's way too much. After a quick look over the images your posted I would recommend removing:

                   

                  1. The counter-sinks for the fasteners.
                  2. The handle.
                  3. The sets of four smaller holes around the larger holes.
                  4. The hexagon indents.
                  5. The recessed features on the sides, top, and bottom.
                  6. Those gray rod things on the back.
                  7. Those two black pieces with the u-shape on the bottom that are on the front.
                  8. Probably the heat-sinks.
                  9. Definitely the small indents on top of some of the heat sinks.

                   

                  There are probably additional things on the inside that you can remove, but I'd need to see. Out of curiosity, how long does that take to mesh?

                   

                  You are absolutely right but even though my objective now is just to check the resonant frequencies. I had intended to configure the mesh such that I could converge the Mass Participation Factor too. That is the reason I had started out with high number of frequencies. To save time I had intended to use the same mesh for when I carried out linear dynamic analysis. In that study checking stresses will become more important.

                   

                  Very true (although the MPF should converge just as easily as the frequencies); if your end goal is accuracy stresses, then you'll need a good mesh. However, since you're doing dynamics, this is going to be rather lengthy. Sadly, SW Simulation doesn't calculate stresses when you do a modal analysis (aka frequency analysis), so you're going to have to be re-running the modal and dynamic analysis a lot. Also keep in mind that the point of FEA is to help guide your in the right direction and get you in the ball-park; it's not meant to exactly predict every little detail.

                   

                  You have recommended the "bottom to top" approach where I start off with a coarse mesh and then work up to a finer mesh. But what do you think about "top to bottom" approach where you do exactly the opposite? Do you think that it is a good idea?

                   

                  I don't think the "top to bottom" approach is a good idea. If there is an issue with your model (meshing, solving, characteristics of the solution, etc) then you're going to waste significantly more time starting with a fine mesh and moving to a coarse. Building an efficient and robust finite element model is easiest to achive when you start simple and work your way up (especially if you don't have much experience as an analyst).

                   

                  I have about 90GB worth of space left on my hard drive.

                   

                  When I asked about how much memory you had, I was referring to volatile memory (your computers RAM).

                   

                  What is the maximum DOF that solidworks simulation can handle? Any idea?

                   

                  Have no clue to be honest. Even it SW can handle +20 million DOF, I think your machine might not be able to. A rough rule of thumb is that you need about 1 GB of solver memory per 1 million DOF, but this can be 2X or 3X more depending on the circumstances.

                   

                  Without knowing all of the intimate details of your design, I strongly suggest that you start with a simple model and work your way up. If you want to get into the specifics for why you think you need certain features, then we can do that. However, I think you have way too much detail in your model that will not add anything meaningful to your results. In fact, I think that all of the detail that you have in your model is preventing you from getting the model to solve in the first place.

                    • Re: Frequency Analysis Errors/Problems
                      Atif Khan

                      Again thank you very much for the detailed explanation.

                       

                      I agree that the geometry is part of the system, but will it add a meaningful effect to the system's performance? For example, all of those heat-sink fins (I'm assuming); do you feel that have a meaningful impact on the results your after?

                       

                      It may not have too much of an impact for frequency analysis. But when I start linear dynamic analysis they will definitely be important. The heat sink area is actually of concern since I know they are susceptible to breaking. So during linear dynamic analysis I want to make sure that the area is not under a lot of stress and where the stress concentrations are so that I can reinforce them in some way. Those depressions also play a role in increasing stiffness such that they can withstand stresses caused by vibration, shock and other environmental stresses.

                       

                      LOL at the reaction.

                       

                      As you have advised I have removed

                       

                      1. CSK's and their corresponding thread holes.

                      2. The Handle

                      3. The small holes (both internal and external)

                      4. The gray rod things (LOL)

                      5. The two black pieces

                      6. The screw holes on the heat sinks.

                       

                      Extra Measures for Quick Solution

                       

                      7. Removed some mesh control parameters and removed a lot of surfaces under mesh control

                      8. Used Remote Mass to define the internal modules and had already excluded a lot of other internal modules from the analysis. 

                      9. Reduced number of frequencies to 5.

                       

                      After doing all that I am down to

                       

                      DOF: 17651019

                      Nodes: 5946113

                      Elements: 3810846

                       

                      Almost half the original value. Running simulation now with FFEPlus solver to see what happens. If it does not work will try the Direct Sparse and if that does not work then I will have to go for a more coarser mesh.

                       

                      Out of curiosity, how long does that take to mesh?

                       

                      The model that I sent you the photo of took me around 6/7 hours to mesh. Most of my time was spent in applying mesh control. The solidworks mesher finished it in about 5 minutes.

                       

                      Also keep in mind that the point of FEA is to help guide your in the right direction and get you in the ball-park; it's not meant to exactly predict every little detail.

                       

                      I understand that but our company puts a lot of weight behind FEA simulation results. So I try and get the results as accurate as possible. 

                       

                      I have about 32GB worth of RAM on my computer. I hope it is enough. According to the Task Manager I am using about 14.8GB worth of RAM.

                       

                      Thank you very much for the interest that you are taking and for all your help and advice.


                        • Re: Frequency Analysis Errors/Problems
                          Shaun Densberger

                          I understand that but our company puts a lot of weight behind FEA simulation results. So I try and get the results as accurate as possible.

                           

                          Doing this has the potential to result in FEA having a negative impact on the engineering process and the final product. There are a number of different areas within an analysis that add error to your solution. You need have a solid understanding of each area and how to go about reducing or bounding the error, otherwise you're results are somewhat worthless. You can do the most detailed analysis here and get beautiful convergence on your results, but if you're system is very non-linear (and you're using linear dynamics), then you're results can be irrelevant. While your company might put a lot of weight behind FEA results, that doesn't mean they should be. Remember: "FEA makes a good engineer great, and a bad engineer dangerous."

                           

                          I have about 32GB worth of RAM on my computer. I hope it is enough. According to the Task Manager I am using about 14.8GB worth of RAM.

                           

                          It should be, but it might be worth it to up your virtural memory just to be safe.

                        • Re: Frequency Analysis Errors/Problems
                          Atif Khan

                          Ok so I started the simulation on a friday evening and ran the simulation over the weekend and according to some of my colleagues who were here on sunday it finished on a late sunday morning (around 44 hours). Not too bad I guess given the intensity of the problem.

                           

                          Now we know that FFEPlus Solver can handle 17.5 million DOF.

                           

                          I have good MPF values in the X Direction (0.71). The MPF in the Y direction is really poor (0.045). The Z direction seems better than Y but well below the recommended limit (0.28).

                           

                          I think my next step would be to try and converge the MPF. Will raise number of frequencies to around 25. Might try the Direct Sparse Solver this time to see if it can solve the problem quickly.

                           

                          A quick question. For faster simulations do you require more processing power from the CPU or more RAM? I might be able to convince my management to invest some more in one of these.

                            • Re: Frequency Analysis Errors/Problems
                              Shaun Densberger

                              Ok so I started the simulation on a friday evening and ran the simulation over the weekend and according to some of my colleagues who were here on sunday it finished on a late sunday morning (around 44 hours). Not too bad I guess given the intensity of the problem.

                               

                              I think you need to go simpler...at 44 hours per modal run, this is going to take you a really, really, really long time to get good result.

                               

                              I have good MPF values in the X Direction (0.71). The MPF in the Y direction is really poor (0.045). The Z direction seems better than Y but well below the recommended limit (0.28).

                               

                              71% MPF is a little on the low side. Most of the dynamic analysis work I do is seismic, and you typically want a MPF of 90% (some standards say 80% is OK, but most say 90%).

                               

                              I think my next step would be to try and converge the MPF. Will raise number of frequencies to around 25. Might try the Direct Sparse Solver this time to see if it can solve the problem quickly.

                               

                              This is what you should do, although with 44 hours worth of run time, this is going to take you a long, long time. Stick with FFEPlus for your solver; it becomes faster than Direct Sparse around 100k DOF and becomes more efficient the larger the problem gets.

                               

                              A quick question. For faster simulations do you require more processing power from the CPU or more RAM? I might be able to convince my management to invest some more in one of these.

                               

                              Both. RAM is the cheapest to upgrade, but make sure to check how much memory your motherboard can support before you buy more. For the processor, both core speed and number of cores matter, but core speed will effect all parts of an analysis (while the number of cores will only effect certain parts of the analysis). It'd be worth your time to dig around in the forums for some more information on this (it's been brought up a couple of times). This thread is a good place to start.

                                • Re: Frequency Analysis Errors/Problems
                                  Atif Khan

                                  Thank you very much for all your help and advice.

                                   

                                  I will try and simplify it further. Will reduce mesh control on a few more surfaces. Suppress some more features and try and reduce the DOF number. I might reduce the global mesh size too. However I am worried that reducing global mesh size might adversely affect MPF convergence since MPF increase primarily depends on two factors (Increase in number of freqencies and Mesh refinement).

                                   

                                  Will keep this thread updated. Currently I am running the simulation for 25 frequencies using the Direct Sparse Solver. Been around 24 hours.

                                   

                                  Thank you for posting the thread. It was very helpful. Some of those guys have beast like systems.

                                    • Re: Frequency Analysis Errors/Problems
                                      Jared Conway

                                      simulation can handle millions of DOF but it will take a long time to solve

                                      i would recommend going with shaun's recommendation to start simple

                                      get the outside box to solve, use the right mesh, use the right idealization and then go from there

                                      your reseller should be able to give some guidance here to get your solve time down

                                      the solve time might also be cuased by inappropriate contacts..etc because frequency can solve pretty quickly

                                      if you watn to move this to linear dynamic eventually, you're going to have to get the DOF down

                                      if you're interested in some feedback directly, feel free to contact us at jared@hawkridgesys.com

                                    • Re: Frequency Analysis Errors/Problems
                                      Atif Khan

                                      An update to the situation.

                                       

                                      The Direct Sparse solver failed. I guess it could not handle that many DOF. I got the STAR error again.

                                       

                                      Removed the indents on all sides now to try and simplify the solution. Did some further simplifications and removed some more surfaces from mesh control.

                                       

                                      Now I am down to

                                       

                                      DOF:10432824

                                      Nodes: 3482605

                                      Elements: 2263308

                                       

                                      Using the FFEPlus Solver now to run the simulation. Lets see what happens now. 

                                        • Re: Frequency Analysis Errors/Problems
                                          Jared Conway

                                          still going to be a bear of a problem to solve

                                          would recommend you go with the start simple technique and build up to the larger problem unless you have a lot of experience with simulation. you'll learn a lot about your problem and the software going through it. also you're going to get much faster solve times if it is setup appropriately. and likely won't take any hit on accuracy.

                                          the fact that the direct sparse solver fails, tells me almost for sure that it is a contact/connection problem.

                                            • Re: Frequency Analysis Errors/Problems
                                              Atif Khan

                                              Aplogies for the late reply. Extended weekend break here. So the simulation is completed. Took me quite a while almost 2 days. Was monitoring remotely from home. I was surprised to see that it took me almost the same amount of time as my previous simulation. But then again I was running the simulation for 25 frequencies to try and converge MPF.

                                               

                                              Got good values for MPF in X and Z Direction

                                               

                                              X=0.84

                                              Y=0.24

                                              Z=0.77

                                               

                                              I guess given the times the best approach would be to just run with a not so coarse not so fine global mesh size and forget about mesh control. Any mesh errors due to small parts will just have to go with an incompatible mesh.

                                               

                                              Funny thing is I have already tried running the simulation with a coarser mesh with most of the parts and features included and without putting in remote masses and it had worked earlier (Simulations were taking only about 1/2 hours) but when I tried mesh control you could then see the problems. I suppose I took the advice from the simulation manual (2 rows of high quality elements on each face) too seriously.