General Mechanical

General Mechanical

Bond between different Profiles

    • maetha
      Subscriber

      Hey there


       


      I'm trying to model the attached geometry. My goal is to simulate the falling rock onto the structure. In a first setup I'd like to build a model which is working in static structural environment and after that with the explicit dynamic module.


      I'm having problems with the connections between the different profiles (HE, UP, IP). Is there a way to "fix" them together, as they would be one structural system? I already tried contacts between areas, which seems not to work with explicit dynamics and share topology. Latter didn't make any difference. 


      I'm using ANSYS 18.1.


      Thanks a lot!


      Maetha

    • Sandeep Medikonda
      Ansys Employee

      Hi maetha,


        I am unable to open the model due to various reasons. Can you post some snapshots of the model, tree and the details windows?  


        Have you tried using bonded contact? I am surprised that share topology didn't work. Did it work in on analysis system and not the other?


       


        Another option you would have is to use mesh connections.


      Regards,


      Sandeep

    • maetha
      Subscriber

      Hi Sandeep


      thanks for your fast response! Here are some snapshots:





       


      The shared topology didn't work in both somehow. At least that's what I'm interpreting out of the meshed geometry.


      Thanks and regards


      Maetha

    • Sandeep Medikonda
      Ansys Employee

      Maetha, 


      Are you using SpaceClaim? If so, Can you use the 'Show Contact' tool to look and make sure that the edges are being shared? Make sure to change Share Topology to 'Share' in the properties window.


      Even in mechanical, you can check this by turning on 'Edge Coloring' > 'By Connection'. This will allow you to see if the edges are being shared between components.


      ~Sandeep

    • maetha
      Subscriber

      Actually I'm using Design Modeler. In Mechanical it looks as following:


       



      Does this make sense? Anyway I'll get an solver failure with for DOF UZ at the UPE in the middle (the one there is pressure on). Why is this?


      Thanks and regards

    • Sandeep Medikonda
      Ansys Employee

      Maetha, 


      Here is the video on using share topology in Design Modeler. 



       


      Now, it looks like share topology is working here and the penetration you are seeing is because you are working with shell structures. So this is merely for visualization purposes. You can turn this off in Mechanical using View> Thick Shells and Beams.


      Coming to your error, are you able to post snapshots of your error message, you analysis settings, boundary conditions/contacts etc. so that we can debug?


      Regards,


      Sandeep


       


       

    • maetha
      Subscriber

      Thank you for the response!


      Sure, here they are: Warning and Failure



      and



      Boundary Conditions:




      Contacts:



      I hope this helps! Thank you in advane!


       

    • Sandeep Medikonda
      Ansys Employee

      Maetha,


      Unfortunately, I cannot read German :-), but I tried to get an understanding of what you are doing and for the most part, it looks fine to me.


      How far into the simulation does the model fail? Can you provide one more snapshot of your Force Convergence (In solution output change from solver out to force convergence)? Here is a very useful article on Convergence, may be looking at the newton-raphson residuals will help. Also, increase the number of sub-steps in your model?


      ~Sandeep

    • peteroznewman
      Subscriber

      Mathea,


      One way to connect those profiles is to use an Automatic Node Merge.  I used a 7 mm Tolerance Value and turned on Face/Face.



      This is the result:



      Note that one of the profiles didn't get any nodes merged at the 7 mm setting, and some of the elements are getting distorted during the merge.


      A much better way is to create a Named Selection of all the faces of the U-channels on the top and second Named Selection of all the faces of the I-beams that they rest on and make a Contact Definition between two Named Selections. When I did that, I found that some face normals are not in the same direction as their neighbors, so that needs to be accommodated to use this method.


      I suppressed your line bodies. I suppressed Fixierte Lagerung. I changed your springs from Body-Body to Body-Ground, I suppressed Körperwechselwirkung (Body Interactions) since you don't want extra complexity during the first attempt to solve.


      Hope this helps. I don't have 18.1 available at this time, I was doing this in 18.2.


      Regards,


      Peter

    • maetha
      Subscriber

      Dear Sandeep and Peter


      thank you very much for your answers!


      @Sandeep: The model fails quite in the last part of solving. Nevertheless the force convergence shows no entry.


      @Peter: I've now created those two named selections and made a contact definition between them. Furthermore I suppressed the same as you did. Unfortunately I still get the same error message. I've also created a third named selection for the lower I-profiles and connected them to the middle H-profiles, which didn't make any difference. 


      What else could it be?


      Thank you both!


      Maetha

    • peteroznewman
      Subscriber

      Maetha,


      In DesignModeler, I picked all the bodies in Oberbau and set the Shared Topology Method to Automatic.


      In Mechanical:


      I changed your groups to have 11 faces in UPE and 14 faces in HEA, the faces that touch each other, not the faces away from that plane.


      I changed your IPE to have 4 faces and created HEA2IPE with the 14 faces on the other flange of the I-beam.


      I updated the two contacts to use these two pairs of named selections and set them to use MPC contact, which is easy to visualize in the results, set the shell sides, and set a manual pinball radius. I don't know if those settings were necessary.


      I added a contact tool to show that the contacts were were closed.


      I changed it to solve with Auto Time Stepping On and set the initial substeps to 10.


      I added a Modal to make sure all the parts were attached.


      Now the Static Structural model solves (at least to 20% of the full load).



      Attached is an ANSYS 18.1 archive.


      Good luck,


      Peter

    • maetha
      Subscriber

      Thank you very much! 


      As I tried to start solving with the explicit dynamics mechanical crashes with AnsysWBU.exe not working. Is there a way to analyze the .dmp file?

    • peteroznewman
      Subscriber

      Maetha,


      I don't know how to use a .dmp file. I recommend you try Transient Dynamics for the impact of the rock with the grate.


      What is the impact velocity you have chosen for the rock?  You should move the rock in DM to be in initial contact with the grate.


      What plasticity model would you chose for the metal?


      I recommend you start a New Discussion in the Structural Mechanics area to ask new questions about the impact of the rock because this topic could be marked as solved.


      You can show your appreciation by clicking Like below the posts that are helpful.


      Regards,
      Peter

    • maetha
      Subscriber

      The impact velocity is around 20 m/s. I'll use the bilinear isotropic hardening model.


      Thanks!

Viewing 13 reply threads
  • You must be logged in to reply to this topic.