General Mechanical

General Mechanical

Non linear analysis- doesn’t converge

    • neomale89
      Subscriber

      Hello,


      I am trying to perform an analysis on a fuel tank which is been secured to the structure with the help of the straps. For the initial setup, I have not provided any material properties and also no hydrostatic load. I have also suppressed a few members to reduce the solving time. Attaching the archived model prepared in 18.2. Please help. 

    • Sandeep Medikonda
      Ansys Employee

      Hi,


      Can you provide snapshots of your setup (boundary conditions), materials, model etc?


      I am probably missing something but how can it solve without any materials or loads?


      Regards,
      Sandeep

    • neomale89
      Subscriber

      Hello Sandeep,


      it has by default stainless steel assigned to all components. Here is the screenshot. I have also attached archived model of it.


       


    • neomale89
      Subscriber

    • peteroznewman
      Subscriber

      Hello neomale,


      I set the number of steps to 1, since you only have one load, gravity. However, the solver will not converge in 26 iterations with 100 substeps. If you look at the NR Force Residual, all the points are around the brown strap. 



      Here is a closeup on the geometry



      Here is the mesh



      Here is a better mesh made by putting a Sizing Mesh Control on the 8 edges at the bottom of the strap.



      While you are in the area, you can also add a Sizing control to the face of the solid part that the strap holds onto. That was too coarsely meshed also.



      While a better mesh (on all four straps and Tee bolts) will allow the convergence to continue, it would be ideal to midsurface the straps. Do you want to do that while you are fixing the next issue?


      The next issue that prevents convergence is the interference between the large light grey sidewall and the darker grey strap backer. The solver is trying to resolve that interference. Do you want to resolve it in the geometry editor and get rid of that interference?  Then the model should converge.



      Regards,
      Peter

    • neomale89
      Subscriber

      Thanks, Peter. I will try to resolve the model again by implementing the suggestions above. Just one question, what are the substeps required in this case? How do we decide the number of substeps?

    • Sandeep Medikonda
      Ansys Employee

      What are the errors?


      If the materials are not a problem. It is very likely coming from the contacts.


      Also, what are your analysis settings?


      I see that you did a modal analysis. Remove the Fixed support and perform an unconstrained modal analysis, what do you observe for the first 6 modes? Is something flying away? Try the methods listed here to debug.


      Regards,
      Sandeep
      Guidelines on the Student Community

    • neomale89
      Subscriber

      Sandeep,


      I tried the modal analysis without any constraint, nothing is flying but still, 4-6 modes are not coming zero.

    • peteroznewman
      Subscriber

      Neomale, you did a great job and hit all the right points trying to get this model running.



      • NR Residuals

      • Modal check for contacts

      • Contact Tool

      • Substeps

      • Simplifying loads to get something to converge


      You just need to learn to respond to NR Residuals with a mesh refinement and you will be a bit more capable

    • peteroznewman
      Subscriber

       One idea to save you some time in the Geometry editor fixing the interference. Just remove that one strap face (actually 4 faces) from the contact definition so that the solver is not checking the faces that penetrate the tank. All the other faces of the strap that wrap around the tank are fine.

    • peteroznewman
      Subscriber

      I implemented the idea from my last post.
      Now the NR Force Residual shows a problem on the No Separation contact.



      Here is the No Separation contact.



      I don't understand why a No Separation contact is used here.


      Why not use a Bonded Contact so that the Tee bolt stays at its current location on that midsurface plate?


      Regards,
      Peter

    • neomale89
      Subscriber

      Hello Peter,


       


      yes I faced the same problem, the idea behind that was once the initial model is finalized, I want to put the initial tension in the belt to hold the tank steady. So I used no-separation to allow the movement along the axis of T bolt. I am not sure if this is the right approach.


      So what I did was, I converted the following contact as bonded. I am still running the model, so can't comment on the results.



       

    • peteroznewman
      Subscriber

      I converted the No Separation to Bonded and found the next problem is that there is a large interference of the top of the strap with the tank.



      It's best to check for interference in the CAD system before you bring the geometry over for modeling.


      Regards,
      Peter

    • neomale89
      Subscriber

      Ohh, I didn't really see that. So what will be the best method to fix that? Should I go back in CAD model and fix that or is there any way of doing it in ANSYS workbench?

    • peteroznewman
      Subscriber

      All your geometry is in SpaceClaim, so you could try to use the Move tool to move those faces of that part up, while leaving the faces around the Tee bolt in place. This is complicated because there is the strap and the pad under the strap that both have to move. What if you just delete the pad from the model, and just have a strap?


      You might have more control in the native CAD but then you will break a lot more of the model in Mechanical.

    • neomale89
      Subscriber

      Good morning Peter,


      So what I did is that I didn't make changes in the interference geometry and changed the contact formulation to the pure penalty, It converged.


       


      Now I have introduced the material properties as shown below:



       


      So, I want to know if it will be ok to use the pure penalty formulation with neoprene?


      Also, if I want to introduce the tension in the belt, what will be the right way to do that? Right now what I am doing is applying force at the bottom of T- bolt, I don't know if it is right or wrong?


    • neomale89
      Subscriber

      Ohh, so the image up there is blurry, adding more information the belt inside is steel, outside strap is neoprene and tank is steel.

    • peteroznewman
      Subscriber

      Pure Penalty is a good contact formulation, it takes a little longer than the Default formulation, but if the Default fails, that is an excellent reason to try Pure Penalty.  It's good for steel or neoprene.


      Applying force to the T-bolt is good as long as it has freedom to move. If you changed the No Separation contacts between the T-bolt and the plate with the hole in it to Bonded Contact, then the T-bolt can no longer slide and the Force is not tensioning the strap.  Instead of No Separation Contact, suppress that and insert a Translation Joint between the T-bolt and the plate with the hole. Make sure the X axis points along the length of the T-bolt. You then apply a Joint Load of Force to the Joint.


      Regards,
      Peter

Viewing 17 reply threads
  • You must be logged in to reply to this topic.