General Mechanical

General Mechanical

Definition of force to simulate an indentation

    • garazilizaso
      Subscriber

      Hi,

       

      I am trying to simulate an indentation. I know I want to apply a 2N force in a specific axis (z), in order to provoke the simulation. The issue I'm having is that I don't want to define the displacement because I want the force to be the one that moves the indenter into the piece of substrate. The substrate is fixed in two of its sides. If I define a displacement as z being free, y = 0mm and x = 0mm, it says that the boundary conditions are invalid.

       

      My aim is to define a for of 2N in order to create a creep (keeping the force constant during a period in order to have a constant indentation during that time) in the indentation. Can somebody help?

    • peteroznewman
      Subscriber

      Please reply with a sketch of the parts and the boundary conditions.

      If the substrate is a cube where the +Z face is going to be indented, then you can use a Fixed Support on the two XZ sides of the cube.

      On the flat back end of the indenter, insert a Translational Joint. Apply a Joint Load of 2N.  The tip of the indenter should have a small radius at the tip, not a perfectly sharp tip. That tip should be exactly tangent to the cube so that the frictional contact between the indenter and cube is initally closed. Insert a Contact Tool to verify the Initial Contact Status.

    • garazilizaso
      Subscriber

      The substrate is a rectangular prism, with a non-homogeneous surface, but the tip is exactly tangent for sure. The indenter already has a small radius at the tip. The Fixed Support is defined by experimental data, so that cannot be varied. I have created a Translational Joint, but still the message of invalid boundary conditions appears. In the next picture you can see the boundary conditions, being the force application in the z axis. 

    • peteroznewman
      Subscriber

      For load step 1, the force starts at 0 N at t=0, and the force ramps up to 2 N at t=1 s.

      For load step 2, the force can stay constant at 2 N while the creep occurs until t=2 s .

      For load step 3, the force can ramp down to 0 N until t=3 s.

      Reply with an image of the Coordinate System under the Translational Joint and make sure the Joint X axis is pointing along the global Z axis.

    • garazilizaso
      Subscriber

      Okay so right now the X is not pointing along the global z axis, how can I turn it around? Should I be changing the global one? In the previous try, I managed to make the movement in the z axis and not in the x, that is why maybe it didn't work?

    • peteroznewman
      Subscriber

      Click on the + sign next to the Translational Joint to show the Reference Coordinate System then click on that.

      The Ribbon will show a Coordinate System menu, click on the Rotate Y button and type 90.

    • garazilizaso
      Subscriber

      I insert you a photo of my interface. The boundary conditions are still invalid. Can you spot what's wrong?

    • peteroznewman
      Subscriber

       

      The Translational Joint shown is a Body-Body joint. That is wrong.  Delete that Joint.

      Create a new Translational joint, but select Body-Ground in the Details window. Then make sure the Reference Coordinate System has the X axis pointing down.

      Once that joint is created, add the Joint Load.

      Under Analysis Settings, turn on Auto TIme Stepping.

      Set the Initial and Minimum Substeps to 100 and the Maximum Substeps to 10000.

      Turn on Large Deflection.

      Under the Connections folder add a Contact Tool and Generate Initial Contact Status and check the result to make sure the contact is closed.

      What kind of material model do you have for the bone?

       

    • garazilizaso
      Subscriber

      The boundary conditions are still invalid. I have changed what you said. What could be the problem?

    • peteroznewman
      Subscriber

      Why is the Translational Joint showing Multiple entities?  There should be just one flat circular face at the top of the indenter.

      You don't show what the Fixed Supports are Scoped to.

    • garazilizaso
      Subscriber

       

      Okay so I have changed it to the flat circular surface:

      The fixed support are the following:

      Still, invalid boundary conditions

    • garazilizaso
      Subscriber

      One of the problems is that I cannot suprress the displacement, but that is exactly what I want to do. I want to control de movement with the force. How shall I do it?

    • peteroznewman
      Subscriber

      You have a Force Reaction output request in your Solution branch with a ? on it.  Delete that.

      Delete the Fixed Supports and create fresh copies of them. Do you still have Invalid BC error?

    • garazilizaso
      Subscriber

      Okay! No BC error! But now, how will I be able to analyse the force reaction output? I am interested on seeing how the force varies through out the indentation

    • peteroznewman
      Subscriber

      You specified the force in the Joint Load as a function of time: [(0,0),(1,2),(2,2),(3,0)]. You can add a Probe of the Reaction Force of the Fixed Support and have Ansys plot it.

      You could plot the Displacement of the Indenter as a function of time and see how the displacement changes in the 1 second while the Force is a constant value of 2 N to see how much the material creeps.

    • garazilizaso
      Subscriber

      Now the problem is that it doesn't converge... Even if I change the substeps and the 0N force to a really small one.

    • peteroznewman
      Subscriber

      You need to provide a lot more detail to make some progress on a convergence issue. What is the exact error message?  Look in the Solution Output and search for the error and show some of the lines of text above that.

      If you can share your model, I can take a look at it. First delete the mesh in Mechanical, then save the Project, then use File Archive in Workbench to create a .wbpz file. Put that file on a sharing site such as Google Drive, OneDrive or Jumpshare.com so anyone can download it.  Reply with the link to that file.

    • garazilizaso
      Subscriber

       

       

      You can access to it now. Feel free to change whatever you feel like and send back any improvement you are able to make. Thank you so much

       

    • peteroznewman
      Subscriber

      The first problem I see is that the Indenter does not start out touching the bone.

      Bonded Contact is on the tip so that the Static Structural model can start. If you don’t have initial contact and have a force driving the indenter, there is no solution if there is no initial contact.

      After I delete the Bonded Contact, I ran a Contact Tool to get the Initial Contact Status on the Frictional contact.

      You can see there is a 25 micron gap.

      A quick and easy fix for that is to use “Adjust to Touch” in the contact details and it will close that gap automatically by moving the contact surface by that amount. But it might not move it along the Z axis, it finds the smallest distance and moves it in that direction.

      Mechanical issued a warning.

      The solver issued a warning.

      *** WARNING ***                         CP =       7.656   TIME= 09:01:01
       Meshes made up of 10 percent or more of SOLID185 tetrahedra are not recommended.

      You should consider following that advice, however the model will take longer to solve.

      You have 4 steps, but no load is applied in Step 1.  I reconfigured the steps like this:

      Finally, under Analysis Settings, you must have Large Deflection turned on.

      It is solving now with those changes and I will report back later.

      Regards,

      Peter

       

    • peteroznewman
      Subscriber

      With those changes, the models runs to the end in 141 iterations.

      Because Adjust to Touch was used instead of moving the indenter into contact, there will always be a 25 micron visual gap between the indenter and the bone.

    • garazilizaso
      Subscriber

      Thank you so much. I have made those changes and I'm running the model. Would you mind if you share with me your model just in case?

    • peteroznewman
      Subscriber

      If you make the same changes I made, you will get the same result. If will send mine if you get stuck, but let's see what happens first. There may be an easy fix if it doesn't work on the first try.

    • garazilizaso
      Subscriber

       

      It worked! Thank you so much Peter

      Now the thing is I want to make multiple cycles. So 5 cycles of 2N loadings, and that did not converge. Should something be changed when loading multiple times?

    • peteroznewman
      Subscriber

      Hi Garazi,

      I applied 20 N for 200 seconds using the same brief ramp on and ramp off times as before. I got some meaningful deformation at the end. Can you use longer times instead of cycles?

      Look in the Solution Output text near the end and see what it says. Depending on what it says, different corrective actions would be used. If you would like to have a live video chat, I can meet to go over the solution output with you on Google Meet or Skype. Reply with your email address and I will contact you. You can delete your email address as soon as I have it.

    • garazilizaso
      Subscriber

       

      That would be so nice. My email is: 

       

    • peteroznewman
      Subscriber

      Okay, you can edit your previous reply. I got it.

Viewing 25 reply threads
  • You must be logged in to reply to this topic.