General Mechanical

General Mechanical

How to connect a rigid body with a flexible body?

    • edoardo
      Subscriber

      Hello everyone, 


      As the title says, I need help choosing the right type of connection for my system: I have a rigid body (bottom) that i need to connect to a flexible body (called middle). I cannot model the flexible body as a surface, because I need to mantain the fillet. I tried bonded connection and joint connection. I get the error that you can see in the messages in the picture. Any possibile solution?


      Thanks in advance


      Edoardo


    • peteroznewman
      Subscriber

      Hello,


      I recommend cutting at least a 10 mm margin around the red face into the rigid body and uniting that piece onto the flexible body. The reason is you don't want a boundary between flexible and rigid too near the fillet where you expect the highest stress as it may be influenced by the nearby rigid material, which is not real, it is just being used to speed up the solution. The shape of the flexible elements will be improved as well since you won't need them to come to a knife edge.


      The error is a general message about a failure to converge and is not specific to the connection between the flexible and rigid bodies. Follow the directions in other posts about how to overcome convergence failures. Under the Solution Information folder, change from 0 to 5 the number of Newton-Raphson Residual plots. Solve, and then look at these plots. They will tell you where you need smaller elements.  In your reply, show the Force Convergence Plot.


      padtinc.com overcoming-convergence-difficulties-in-ansys-workbench-mechanical-part-i


      padtinc.com overcoming-convergence-difficulties-in-ansys-workbench-mechanical-part-ii


       

    • edoardo
      Subscriber

      Hello Peter,


      I modified the geometry as you suggested:



      I bonded the faces of the flexible to the rigid body with 3 bonded contacts. I set the Detection Method to Nodal-Normal To Target and changed the Normal Stiffness Factor to 0,2 to all 3 contacts.


      Under analysis settings I used these inputs:


      neqit 75, Initial Substeps and Minimum Substeps 1000, Maximum Substeps 10000


      I get this kind of plot:



      It doesn't even converge at the first step, so It doesn't make sense to look at the max residual location right?


      How do i approach this? Thanks in advance.


       


       

    • peteroznewman
      Subscriber

      It looks like you need to do the same rigid-to-flexible treatment to the fillet on the other end of the strip.  You should just leave the Bonded Contact as the default values.  Only change them when there is a reason to do so.


      Under the Solution Information folder, Newton Raphson Residual Plots, replace 0 with 3 or 5.


      Let the solver run for just 5 iterations then Interrupt the solution.


      Now look at the 3 or 5 plots under the Solution Information folder. That will tell you where you need smaller elements.

    • edoardo
      Subscriber

      Hello Peter, I did as you said, and I found that the bigger residuals where on the lateral faces, so I modified the mesh like this:



      But Ansys can't still solve my problem:



      And the residuals look kinda like this:



      Any other suggestion? Thank you as always.


      Edoardo

    • peteroznewman
      Subscriber

      Please attach an Archive of your model so I can take a closer look. 


      Make sure to include any external files so the geometry is included in the archive. 

    • edoardo
      Subscriber

      The project I'm asking about is the G one.


      https://drive.google.com/open?id=10ek3vE1tNM2P-8YIWUi7vi41PClthMeA

    • peteroznewman
      Subscriber

      Hello Edoardo,


      I opened your file and looked at the G system.


      1. You only have one flexure. I'm not sure why you want to apply a down force on this structure.



      In your earlier models you had two or three flexures which created a hinge. I copied your geometry, rotated it around to oppose the first flexure. I united to the two copied of the top part to have a single rigid body at the top.  On the bottom, you don't need the rigid body, I just applied the fixed support to the bottom of the flexible feet.



      2. I sliced the flexure part off the foot to get two elements through the thickness of the thin part. I formed a multibody part for the flexible part so I did not need any contact elements to hold the thin part to the foot. The mesh is connected using Shared Topology.



      3. I applied a Remote Displacement, which converges more easily than a Force. I pushed the top to the side by 50 mm, but I only solved it out to 0.4 s then manually interrupted the solution to write this reply.



      4. Under Analysis Settings, I requested 100 initial substeps. This allowed the model to converge.



      5. Here is the stress result. I used a Multizone Method on the foot and a Sweep method on the flexure.



      With such a large change in thickness from the flexure to the foot, it looks like you could cut the flexure through the thick portion and add the rest of the foot portion to the rigid body. You would still maintain a blend from the thin to the thick part, but you don't need the blends to the flat plate because there is no stress there.


      Regards,
      Peter

    • edoardo
      Subscriber

      Ok thanks, I'm gonna try to replicate this approach. I have a lot to learn about Ansys.

    • edoardo
      Subscriber

      Hello Peter,


      I followed your lines and learned a lot about meshing opportunities. My model though still doesn't converge and I don't understand the cause. Maybe It's a contact problem? I made 6 bonded connection between foot faces and the top body. I'm gonna post the updated project (project H), if you could take a look at it I would appreciate it a lot. Thanks in advance https://drive.google.com/open?id=1lAGaI52USY_7PDsPXP9FdmsYOVM0Ktct


      Edoardo

    • peteroznewman
      Subscriber

      Hello Edoardo,


      I use 7zip to open zip files. It sometimes opens rar files, like it did for your first upload.  7zip cannot open this rar file.  Please create a Workbench archive .wbpz file.  You should be able to attach that to your reply.  Can your rar program write a zip file format?  I don't want to install unrar.

    • edoardo
      Subscriber

      Here you have a zip archive of it: https://drive.google.com/open?id=11uJYyrUWv4mpC6sRBAWNmzaFl5ylRKHC 


      hope it works this time.

    • peteroznewman
      Subscriber

      I made the following changes and it started converging.


      1. Made it a 2 step analysis instead of 1 step.  Each step has 100 Initial Substeps, 1 Minimum Substep.


      2. I set the Remote Displacement to 0 for step 1 and -50 for step 2.  I also set the location of the remote displacement at Z=0.


      3. I changed all the Bonded Contacts to Formulation MPC (this is probably optional).



      I only looked at the first three substeps of step 2, but it looks like it will go all the way. 
      I am solving in 2019 R2 so you might have a different result in Release 16.0.

    • edoardo
      Subscriber

      Thank you again Peter. My model converged finally. But when I look at the force convergence plot, I see this:



      So my step 1 is very long, while step 2 took very little time to solve. Can this depend on the software release?


      To make it more general, what are the steps to have a faster convergence? I thought about these:


      - Make a bigger mesh (if possible);


      - Simplify the model (if possible).


      Other things I'm missing?

    • peteroznewman
      Subscriber

      My step 1 solved in 14 iterations, so yes, it seems the 2019 R2 release is performing better than Release 16.0


      To minimize the solution time, reduce the number of equations in the model, which generally means use fewer nodes. You can do that by cutting the model geometry down to the smallest relevant piece, use symmetry when you can, convert solids to shells where you can (thin wall), convert solids to beams where you can (uniform cross-section). 


      Avoid wasting time by forcing the solver to take too many substeps. For example, if I had forced it to take 100 minimum substeps, then I would have waited for 100 iterations instead of the 14 it needed. If there is a difficult part in the middle of the load history, break the load up into 2 or 3 steps so you can have few substeps in step 1 that ends just before the difficult part, then many substeps in step 2 to get through the difficult part.  You can often let the solution control logic automatically increase the step size after it gets through the difficult part and use a 2 step solution, or break it into 3 steps. 


      A bigger mesh does reduce nodes, but you need small elements to capture high stress gradients. Big elements can cause the convergence to fail if it needs smaller elements in some location.

Viewing 14 reply threads
  • You must be logged in to reply to this topic.