General Mechanical

General Mechanical

Modeling Snap-through behavior in the Static Structural

    • hamednik
      Subscriber

      Hello

      I have a problem modeling snap-through behavior in the static structural. I have a bi-stable structural. When I compress the structure the load increases until it reaches a maximum, then it decreases and becomes negative as shown in the below graph.

      As indicated in the energy graph, I expect that if I remove the external force or the applied displacement in point R1 and R2 the structure return to its initial configuration (A). While if we remove the force in the R3 point it will settle at the second stable configuration (C). Now, in my model, if I remove the force at point R1 it return to A configuration (as expected) but if I remove the force at point R2 the structure will continue deformation and will eventually rest at C configuration.

      I have tried different stabilization method; Constant, Reduced, Line search and Arc Length and the same behavior happens with all the method while if I do the same simulation in the Explicit Dynamics the response is as expected. I wonder if there is any way to correct this problem in Static Structural.

      My model is attached to the discussion.

      Thanks

      Hamednik

    • Ashish Khemka
      Ansys Employee
      nnI am not allowed to download the model. If you can share the snapshots of deformation and indicate what you expect then it may help me to comment further.nnRegards,nAshish Khemkan
    • peteroznewman
      Subscriber
      Hello  ,nHere is the structure at the end of step 1, a 5 mm downward displacement of the center post, then you deactivate that constraint in step 2.nHere is the structure nearly at the end of step 2. The arms on the left have passed through each other. You need to add Frictional Contact to prevent this. In Explicit Dynamics, self contact is automatically used in the simulation.nYou didn't say what version of ANYS you are using.n
    • hamednik
      Subscriber
      Hello Array nThanks for your response. Regarding the contact, I had tried frictional contact, too and it didn't hinder that arms pass through each other, I received this warning The contact status has experienced abrupt changes, check result carefully and the same problem happens.nHowever, put this aside, the main problem I have is with the results after I remove the load. As you mentioned, when I remove the load the arms continue to come down although they must return to their initial position. I have also tried this problem in the Transient Structural analysis. Surprisingly, for the same loading transient analysis predicts different but more accurate behavior. But it also has problem in predicting the behavior if I remove the force at point R3. As a summarynIf I remove the force at point R1 it returns to "A" configuration (as expected), both in Static and Transient. nIf I remove the force at point R2:nIn the Static analysis, deformation continues and structure will eventually rest at C configuration. (Which is not correct)nIn the Transient analysis, the structure will return to "A" in Transient (as expected).nIf I remove the force at point R3:nIn the Static analysis, deformation continues and structure will eventually rest at C configuration. (As expected)nIn the Transient analysis, the structure will return to point "A" and initial configuration (Which is not correct).nI have tried different stabilization method; Constant, Reduced, Line search and Arc Length and the same behavior happens with all the method. I wonder if there is any way to correct this problem in Static or Transient Structural.nI am using the ANSYS 2020R1. I have also attached my another simulation file that contains both Static and Transient.nHello Array nThanks for your response, too. You can see the screenshot in the Array response.nnArray
    • peteroznewman
      Subscriber
      Take a look at the attached 2D Plane Strain version of your model.nI replaced the Displacement with a Remote Displacement. This lets me plot both the reaction force and the reaction moment. Maybe the problem with your 3D model is the reaction moment may have changed sign at point R2 on the force reaction plot, and it was the moment that made the part continue down.n
    • hamednik
      Subscriber
      Thanks . I checked this model but actually I couldn't realize if it has solved any of the problem that I mentioned. Still, if you let the top edge to be free at point R2 (e.g. the displacement be 15mm instead of 30) it will not come back to its original position although it must.nThe contact is also still a problem, the struts penetrate into each other although a frictional contact is defined between them.n
    • peteroznewman
      Subscriber
      Hello Array ,It makes perfect sense to me that the center keeps going down in step 2 after reaching point R2 in step1. The reason is that the peak reaction force has been passed. At the start of step 2, when you deactivate the displacement constraint, the solver replaces the displacement constraint with the reaction forces, and then ramps those forces down to zero. Continuing to move down is the only direction that allows the force to be reduced to zero. An increase in force is required for the center to move up from the -15 mm point. That is not permitted in the deactivation of the constraint.nJust because there is a lower energy state on the other side of that peak doesn't mean you can get there from here. Continuing downward after deactivating the displacement at R2 is the correct behavior of the system.nIf you were in a Transient Dynamics analysis, and pushing with a force instead of a displacement, the system would snap through to the low state as soon as the peak force was passed.n
    • hamednik
      Subscriber
      Hi again nI already guess about that, too, so I also modeled it at Transient Structural. In transient structural, if we remove the force at point R2, the structure will return to “A” in Transient (as expected). In that sense, it predicts more accurate compared to the Static one. However, the problem with the transient analysis is at point R3. There we expect that the structure rest at point C (2nd stable configuration) when we remove the forces but it returns to A. In fact, for the transient structural analysis, the structure always return to point A, no matter where we deactivate the external force. I have attached the transient analysis, I appreciate it, if you can take a look at this one, too.nn
    • peteroznewman
      Subscriber
      Hello  ,nI looked at the Transient model you attached. It does not have a Force applied but a displacement.nIf you have not performed a Modal analysis prior to running a Transient Structural, then you are working without valuable knowledge of the dynamics of the problem. I recommend you first do a Modal analysis. You can influence the natural frequencies by adding a point mass to the center post, which can be helpful to slow things down.nYour questions about stable states are best addressed using Static Structural, now that you understand about which side of the peak force the system is when you let go.n
    • Ashish Khemka
      Ansys Employee
      nnDid the suggestions above helped you? If yes, then I can mark the post as resolved.nnRegards,nAshish Khemkan
    • hamednik
      Subscriber
      and nThanks for your responses but the problem is not solved yet. What I like to see in my the ANSYS results is an accurate prediction of bistable configuration when force or displacement is relieved, i.e., the structure move to the closest stable configuration with minimum local energy (as shown in the top figure for potential energy) when the force or displacement is deactivated. nOn one hand, my problem is displacement driven so it makes more sense to apply displacement instead of force, on the other hand the force control will not give the negative stiffness or negative force in the Force-Displacement curve.nnRegarding the Transient Structural, I appreciate if you elaborate more on how I can use modal analysis to get more accurate results in the transient analysis. nThanksnHamedn
    • hamednik
      Subscriber
      Also, the contact problem still exist. In both analysis, as soon as I start the solution, a warning pops up:Contact status has experienced an abrupt change. Check results carefully for possible contact separation.. And when I check the results always I can see self-penetration. n
    • peteroznewman
      Subscriber
      nAs I explained earlier, your original post contains an error for the stable states of the structure and how the force relates to those states. I have a revised graph that I believe is more representative. The peak force corresponds to a peak energy. A zero force crossing corresponds to a zero tangent on the energy. So from R1 the system would return to the 1st stable config, but from both R2 and R3, the system would move to the 2nd stable config.n
    • hamednik
      Subscriber
      Thanks again for your time and response . I am not sure how you got this energy graph but I don't think it is correct actually. Two main reasons: nFirst, in the force-displacement curves (obtained from both static and transient analysis) we have three points with zero force reaction. These points indicate zero tangents (both local minima and maxima) in the energy curve so we must have not more than three zero tangent in the energy curve. But in your case we have five points.nSecond, I have fabricated this sample and experiments confirm only two stable configurations.nFor this analysis, I believe the problem with Static Analysis (as you mentioned) is that it ramps down the force when I remove the applied displacement. But I don't understand what is the problem with the Transient Analysis. It predicts more accurate results if we relieve the displacement at R2 however for R3 it doesn't work out. (you may check the files that I attached for the transient in the previous post).nI think, the problem might be the kinetic energy in the system which is not damped or stabilized. But if I change the value of structural damping to anything but zero, the solution won't converge.n
    • peteroznewman
      Subscriber
      I was just freehand sketching the energy graph and I agree it is wrong. Better to plot data!nIt's not a problem with Static analysis that it ramps down the force when you remove the applied displacement, that is exactly how it is supposed to work.nAs I explained above, in a Transient analysis, where you push down with a Force, as soon as the force passes the peak value, it will snap forward. The problem is that you are using a Displacement in a Transient analysis, then suppressing the constraint. Stop doing that. If you don't want to apply a force, you could introduce another body on a translational joint, and have that body use frictional contact to push on the center post.nYou were moving the displacement so slowly so I don't think there is any significant kinetic energy in the system. Did you perform a Modal analysis to learn the natural frequencies of the structure?n
    • hamednik
      Subscriber
      Array. I tried using another solid to apply the force, in that case the problem is the contact. I cannot understand why the contact doesn't work out in this model (although most of contacts are closed). I receive a warning Contact status has experienced an abrupt change. Check results carefully for possible contact separation. And when I check the results always I can see bodies cross each other. You may check the attached model to see if there is any wrong with my contact definitions.nRegarding the modal analysis, I performed modal analysis and obtained the natural frequency, though I don't know how I can use this data in the transient analysis. Would you mind explaining more, or introducing some reference in this regard?nThanksnArrayn
    • hamednik
      Subscriber
      nI also modeled in 3D, but the same problem persist. It seems, there is no way to make the structure stop at the second stable configuration with displacement-driven loading.n
    • peteroznewman
      Subscriber
      nI don't think your energy graphs included the buckling in the structure that occurs on the way to the bistable state.nContact is only defined between the top of the center post and the bottom of the brown pusher.n
    • hamednik
      Subscriber
      nWhat I am particularly interested to see in my analysis is the when the pusher returns. I want to see if the main structure remains stable in the second position or it will return to the initial position. I can't see this step in your video as you terminated the analysis at the end of first step.nAlso, would you mind sharing me the ANSYS files. In my analysis the contact doesn't work out as you showed in this video.nn
    • peteroznewman
      Subscriber
      Did you play the video? The pusher has gone up and doesn't touch the button at the end of the simulation where the structure is stable in the second position.nI will attach the file when I get on my other computer.n
    • hamednik
      Subscriber
      nYes. I just noticed that.nI am looking forward for the files.nThank youn
    • peteroznewman
      Subscriber
      The archive is in the attached zip.nThe model solves in 15 minutes on my 4-core computer.n
    • hamednik
      Subscriber
      Dear Peter nFollowing our discussion here. I could solve the problem thanks to your instruction and by chosing non-zero value for Damping vs Frequency. However, now I am trying on the problem from another aspect where I need to add another loadstep in which the Damping must be zero but as far as I can see, the value of damping cannot be changed in different load steps. I wonder, if there is any way to do this?The problem is simple, I need to change the value of Damping Controls at different steps but in workbench the value is the same for all load steps. I appreciate if you can help me with this.nnThanks;nHamedn
Viewing 22 reply threads
  • You must be logged in to reply to this topic.