14 Replies Latest reply on Jul 21, 2010 9:24 AM by Keith Parker

    Static FEA Stress Analysis Error

      Hey guys,  Hope im posting this is the correct spot..Im new to this forum.


      Anways, I have a question I was hoping to get some answers on:


      Im running a Static anaylsis test on a Portable Cart we are designing to hold and move Hospital compressor/ventilator systems.


      I am trying to simulate the stress/displacement/strain and FOS of the cart due to a 200 lb load "basically a nurse pushing down on the handle as hard as she can"  along with the total weight of the ventilator it will be holding.


      However when I run the simulator, it gets 34% done and says Error:"Equilibrium is Not Achieved" "Results will be saved upto the current iteration."



      Below is a picture of the Cart and the constraints ive added to it.


      Material:  I cant specify exact material, but its a combination of Steel and aluminum


      External Loads: I have a 200 lb load normal to the bottom plane, with a 100lb load uniformially distributed over the head of the cart.


      Connections: I have Threaded Counterbore screws going up through the base into the spine (bottom)  and also connecting the handle to the head (cant see those from this view.)  I set all of the coincident interference as no penetration, and I did a contact set between the welded parts.


      Fixtures:  (THIS IS WHERE I THINK I AM HAVING ISSUES)  I fixed the bottom left corner of the base completely by selecting the Cylindrical face of the "shaft" where the casters (not shown) will attach.   Next, I selected the other 3 cylindrical shafts and added a vertical constraint.



      *IF anybody can help me out, that would be a huge help...my boss and I have tried several different ways of fixing the bottom to get the results we are looking for but arent having much luck.


        • Re: Static FEA Stress Analysis Error
          Bill McEachern

          Animate the saved result on automatic (automatically scaled deflected shape) and see what is moving. Chances are you should switch to bonded and see if that works - might get the same error. In any event you will know what is moving and then connected so it doesn't. The automatic determination of contacts requires that the surfaces being connected by whatever condition need to be coincident. Small gaps or interferences (like simplified bolts in holes) is often a source of this specific problem for less experienced users. Anyway bonded looks like the condition to use to start will anyway - it you are interested in bolt bearing stresses (not usually critical) then just do the critical connection separetely.

            • Re: Static FEA Stress Analysis Error

              I would animate the saved result, however the "equilibrium failure" denies me from seeing the results.  I set the global conditon to bonded, so originally everything that was coincident is considered bonded.


              Side note*  I previously fully fixed all 4 cylindrical edges on the base and ran the simulation.  It worked (no errors) But it didnt allow the base to move at all, which isnt what we wanted.  So I switched the fixtures to 1 corner fixed, and allowed the other 3 to only move in the verical direction...ran it again and that damn error message popped up.


              I guess what my question is, and im not sure there is an exact answer but What does that "equilibrium is not achieved" error message even mean?  Does it mean I have constrained something incorrectly, or fixed the base incorrectly?  If I could just narrow it down to one or 2 possible errors that would help alot.

                • Re: Static FEA Stress Analysis Error
                  Keith Parker

                  Ryan - I may be way off the mark here, but it looks like you're trying to determine the stability of your assembly (because it's on castors) as well as the stresses, FOS, etc.  Have you tried using bushings/springs instead of fixed constraints, as these will deflect and hence show what I think you want to see.


                  Edit:  sorry - should have written 'Spring Connectors' instead of 'bushings/springs'.  Keith.

                    • Re: Static FEA Stress Analysis Error

                      Everyone - First of all thank you for responding to my question.


                      Keith - I will eventually need to calculate the stability of the cart w/ the casters attached, along with doing a Tip test, and various others.  However what I am currently trying to accomplish is a simple static stress analysis of the Basic components of the cart.  I am looking for a way to constrain the base so that I can see the Deflection,stress, and strain applied to it from the load I mentioned previously. 


                      I fully constrained the base to get the other parts (spine, head, handle..etc) to show some movement..however the force was not applied to the base as it was forced in place.


                      If you will look at my (very bad) drawing I did on paint, it shows what I am expecting the cart to do (exagerated of course) when applied to the loads on the left.   Basically the load will be deflected down the spine and will try to pull the spine forward, creating stress on the base.  I guess I'm just having trouble placing my fixtures on the base which would allow it to deflect in that manner.


                      FEA paint pic.bmp

                    • Re: Static FEA Stress Analysis Error
                      Bill McEachern

                      you are trying to solve in a static simulation, essentially that sigma F=0. If it does not equal zero and something is moving then the smallest of forces will produce infinite displacement in the unrestrained direction. Sounds like something is not connected as the second simulation should have worked. Go the solver options and select soft springs. It may run to completion and you will be able to see what is moving. Make sure you are using the FFE solver as it will save the result if the solution terminates early. You definitely want the solution to solve in the bonded state before you go adding any no penetration contacts. Try removing the fixed holes one at a time and nail down what the issue is.

                  • Re: Static FEA Stress Analysis Error
                    Stephen Burke

                    "Equilibrium is Not Achieved" means that SW could not find a solution due to a lack of stability or incorrect connections/contacts.

                    I think you need to look at your connections and contacts.
                    Omit any bolt connections and no penetration contacts you have setup and do a first pass run.

                    • Re: Static FEA Stress Analysis Error

                      Here is a picture of the bottom of the base, showing you the cylindrical faces Im picking to constrain along with my current constraints.  



                      The top 2 and bottom left holes are vertically constrained while the bottom right hole is completely fixed.  Now shouldnt that allow the base to bend due to the load?  I just dont understand how switching from 4 fixed points to 1 fixed point and 3 vertical constraints screws up the simulation so much



                      FEA bottom.bmp

                        • Re: Static FEA Stress Analysis Error
                          Keith Parker

                          Ok thanks for clarification.  What happens when you apply just the one fixed constraint?  Also, perhaps your first analysis is ok with your four fixed hole constraints because the base isn't deflecting as it's good & stiff!

                            • Re: Static FEA Stress Analysis Error

                              Lol I wish that was the case with the base..but unfortunately I am expecting it to light up like a christmas tree once I got all the constraints properly placed.


                              I will try fixing just one corner though and see what happens.  Ill let you know (may take a few hours..)

                                • Re: Static FEA Stress Analysis Error

                                  Hi Ryan,


                                  With complex models, I have had Simulation complain that the model is inadequately restrained and "fixed" the problem by simply using a finer mesh.  This does not always work however.


                                  If you can't get your model to work, I suggest that you simplify all or part of your assembly, find rigid body/reaction forces with the simplified model, then apply those forces to your individual parts.  This is often quicker than using a bunch of contacts and connectors, which really slow down the analysis.




                            • Re: Static FEA Stress Analysis Error

                              base FEA example pic.JPG




                              I have successfully Constrained the base in order to get translation on the back end.  However this only works when I apply a vertical load.  When I try to apply a load at an angle or horizontaly (Above Pic)  a "large" displacement error appears and the solver fails.  Any ideas on how to constrain it so that it runs error free?

                                • Re: Static FEA Stress Analysis Error

                                  Hi Ryan,


                                  You are definitely moving in the right direction by simplifying your problem to a study with just the base.


                                  I'm sort of concerned about your "On cylindrical faces" restraint.  It says z=0mm?  I would check that restraint.  You want 0 displacement in the AXIAL direction to simulate the casters holding up the cart.  On your diagram, it looks like Y is the axial direction.  Perhaps I am wrong.


                                  The other thing that seems fishy to me is the virtual wall constraint.  You never mentioned that before.  Virtual wall works like a "no penetration" contact set, with the bonus that you can define an entire geometric plane as the "no penetration" source and pick any body geometry as the target.  It would be nice to know how you applied that virtual wall constraint.  They can be tricky.  It could be the right thing to use in the final analysis, though.


                                  Whenever I get "large displacement" errors, I turn on a setting in the solver options called "inertial relief."  This crazy wacked-out feature simulates something like the following problem:  You're standing on a skateboard on a flat surface, and you're not moving.  Someone runs up and body-slams you in the direction of the front of your skateboard.  What is the static displacement?  It applies an inertial force equal to the unbalanced force (the body slam) and solves the displacement that way.  It doesn't give you real results for scenarios that are static in reality (like your nurse's cart), BUT!  What it does for you is show you what flew away.  Then you can properly constrain it.  REMEMBER to turn it off after you've fixed your problem and before you run the solver for real.  It's a serious waste of time, because you will still get wacky results.


                                  Good luck!

                                  David Fletcher

                                • Re: Static FEA Stress Analysis Error



                                  Thanks for your response.  It was very helpful.   Let me try to answer some of the questions you may have.  The following pic is an exagerated displacement of the base when a vertical load only is applied.  This is what I am thinking the base is pretty much supposed to look like for the most part.


                                  I was trying to figure out a way to keep the 4 Caster shafts stable while allowing the rest of the base to bend and shift.  For that reason I restricted the movement of the cylidrical faces in the Z direction with the Cylindrical restraint.  I then used a virtual wall with the bottom edge of the cylinder shaft as my geometry.  My thinking was that with those 2 constraints I would keep the base from moving in the Z direction only at the 4 edges I selected in the virtual wall, while the rest of the base could go below the VW.


                                  What I really would like to do is make it so that only one caster is locked and the rest of the base is free to move as it pleases.  This is because I believe if a Load is applied to the far handle of the cart it will create a torque at the back of the base and try to pull the back casters away from the base.  Unfortunately I've tried several different constraint combos to do this and cant get a combination that works. 


                                  base FEA example.JPG