General Mechanical

General Mechanical

Self Contact Problem

    • navidz
      Subscriber

      Hi Every one,


      I am trying to model the deformation of two cavities inside a domain that are connected with a channel to each other same as bellow:



      The material of the domain is soft, and the cavities and the channel are filled with water. After applying the forces (let say uni-axial load in the direction of channel), since the channel's diameter is very small, the channel will collapse and contact will happen there. I use the following configurations:


       


      But Whatever I am doing the contact cannot stay stable and cannot converge like:



      This is an static run. I solve the fluid part with fluent (steady) and I use system coupling. I tried different configurations like adding relaxation parameter (0.1 and 0.3), or playing with Pinball radius but nothing help this problem. I also increased the number of substeps to 10 but it changed nothing. Because of using system coupling I cannot use Auto timing steps and I have to define the problem with substeps. Also I need to have offset in my contact because this simulation is paired with fluent. This question is also very similar to other problem that I posted earlier:


      https://forum.ansys.com/forums/topic/contact-elements-pass-the-body/


      Thanks

    • Sandeep Medikonda
      Ansys Employee

      Try these, for each point below try a run:



      • Turn Trim Control off + Change Detection Method to Nodal instead of integration points.

      • You can use even more substeps 100 or even 1000 if needed

      • Normal stiffness factor: 0.1, updated each iteration, aggressive

      • Increasing Pinball radius, I understand you have tried a few values but did you try it to be as big as the initial gap between the two bodies. If yes, you can ignore this.

      • Nonlinear Stabilization: Constant, method: Energy (use default parameters)

      • Try Normal Lagrange method if nothing works, this will enforce contact very strictly without allowing for any penetration (might lead to other problems though).


        If none of these work, post plots of your Force Convergence, Analysis settings and how you are coupling in Workbench?


      Regards,


      Sandeep

    • navidz
      Subscriber

      Ok, I tried almost all of the points that you mentioned.



      • The Trime is off and I am using "Nodal-Normal to Target" detection method.

      • I am using 100 substeps.

      • Normal stiffness factor: 0.1, updated each iteration, aggressive.

      • I tried Pinball for very big numbers that are bigger than channel size and even size of the block.

      • I added nonlinear stabilizer.


      I have not tried the Normal Lagrange yet. By adding this many points, the simulations are very slow. But I could get some configuarations work but the rest are not working. Specially that the size of the channel is 50 times smaller than the spherical cavities, therefore I need a lot of elements for the whole system and when I combine it with 100 substeps, and minimum of 3 iteration in system coupling, the simulation takes a very long time.


      I use minimum iteration of 3 and maximum of 5, I use ramping in data transfer, and I only have 1 step in system coupling setting. Also:


      Project Schematic


      Analysis Setting


      Force Convergence

    • Sandeep Medikonda
      Ansys Employee

      Hi,


        First of all turn on the Auto Time-Stepping and define initial, minimum and maximum sub-steps (start with 10, 10, 100 or 1000).


        I am not surprised that it is taking longer because the settings are updating every sub-step.


        It is possible that your model is quite complex and warrants it. When you say some runs don't converge, can you specify what is it that you are changing?


        From what I understand from a structural point of view, I am assuming a soft material in between those 2 circular parts and then a small thin membrane that is in contact with this soft material? Am I correct? If not how is it loaded, in mechanical click on the static structural section of the tree which will give a summary of all the loads and the parts, Can you post an image of that that gives us an idea of loading?


        Can you detail how the channel is affecting the structural part of the simulation?


        Lastly, what are the materials you are working with, Hyper-elastic? If so, what material model are you using Neo-hookean?


      Regards,


      Sandeep

    • navidz
      Subscriber

      Hi,


      Since I am using system coupling and connecting Fluent with Structure, I cannot turn on Auto Time-Stepping. I have to define it by substeps because it is system coupling that over-write the stepping process (as far as I understood) unless it has been changed in ANSYS in the latest versions.


      Let me explain my model in more detail:


      I have a soft cubic material (using Ogden or Neo-Hookean for modeling the hyperelastic material). Inside the cube, there are two spherical cavities with radius (R_1) and (R_2). These two spherical cavities are connected with a cylindrical channel that has a radius of d and length of L. Inside the cylindrical channel and two cavities are filled with water. When I apply forces to one side of the soft cubic material, the cavities and channel will deform. But there is water inside the channel that is in-compressible and will not let the channel to deform in any shape that it wants. I use Fluent to solve for the hydro-static pressure inside the cavities (I heard that there is also a hydro-static elements in structure that I can replace but I do not know about it so I am using Fluent).


      So by different model, I meant that, I play with my variables. For example initial R_1/R_2=1 but if I increase R_2, the solution will not work. Or I can increase the length of the channel and when it is very big (L=10 R_1) it will not work. 


    • Sandeep Medikonda
      Ansys Employee

      I am not well informed on FSI simulations...So I am curious how water is being represented in your static structural simulation. Does it just transfer the pressure from fluent? But if that is the case how are contacts in play here?


      Just from a structural standpoint, try and avoid neo-hookean. It often fails to do well beyond the prescribed/fit strain limits, Also check the strains that your model is experiencing at the point of crashing. Ogden often does quite well in most cases.


      Regards,


      Sandeep

    • navidz
      Subscriber

      Yes, Fluent mainly transfers the pressure, or if needed transfer fluid from one cavity to the other one. Fluent cannot handle death of cells. In other words, when there is a contact, the elements that were filling that gap are getting zero/or negative volume. So Fluent will not be able to continue if that case happens. Therefore, you should define contact just before contact happens through offset. And in Fluent, you should tell the solver that when two surfaces that are going to have contact are getting closer than a proximity value that is bigger than offset that we defined for contact, replace the fluid with porous materials with very low conductivity. In this case fluid will barely pass the contact point and also we satisfied the contact in structure.


      I am actually trying Ogden (because it fits better to my data). Also I believe that I am far away from fit strain limits. 


      I can see in my model that contact cannot converge and it mess up the solution. And using high number of substeps will kill the simulation and will take a lot of time.

    • Bhargava Sista
      Ansys Employee

      Navidz,


      This is a challenging problem, I'd recommend you to first work on just the structural model (assume that there is no fluid in the cavity for now). This will save you a lot of time in the debugging stage. Regarding the contact settings,



      • use a pinball radius about 3x the width of the channel. Do not use a very large value (size of the block).

      • use a finer mesh at the channel, use edge sizing to control the local mesh size.

      • If you're running just the structural component, you'll have the liberty to use a variable time step as opposed to a constant time step in FSI simulation.

      • Try changing the force loading to displacement loading and see if you're still having the same issue.

      • Also, stick to one material model during the debugging stage. To be on safe side start with neo-Hookean. Ogden model, if not calibrated properly, can be unstable.


      I'd recommend you to make all the above changes in your next run and see if that resolves the contact issue. 


      P.S: are you using Fluent only to account for the hydrostatic pressure or are you interested in studying the flow properties as well? If it is just for hydrostatic pressure, then you may want to use fluid elements. Look up HSFLD242 element and see if it meets your requirements. This way you can model the entire thing in ANSYS Mechanical which will save you a lot of computational time.

    • navidz
      Subscriber

      Hi Bsista, thanks so much for your help. Yes I was using Fluent for only transferring the pressure and emphasizing the fact the since the fluid in-compressible the volume of the cavity should not change. And as you said I personally prefer to stay within structural analysis and do not use fluent but I was afraid that the contact of the channel will cause a problem for the HSFLD242 elements. Now I am trying what you said, I am only on the structure and I defined the contact with offset so that I can still use the fluid ellements. One big problem is that the ANSYS documentation for HSFLD242 is only description and I could only find one example of using this elements online at 
      https://www.simutechgroup.com/tips-and-tricks/fea-articles/158-fea-tips-tricks-ansys-hsfld242-elements


      If there is a better example, please let me know to use them. 


      I am using finer mesh but the problem is that in three dimensional problem, the number of elements increase very fast and the speed of the solution decreases dramatically (I am not sure if I am making a mistake somewhere or this is reasonable that with even 30K~40k nodes, which is not too much for 3D problem, it will take one hour for ANSYS to solve the problem). 


       

Viewing 8 reply threads
  • You must be logged in to reply to this topic.