LS Dyna

LS Dyna

Cannot calculate shape change due to wear in LS-DYNA

    • mmy3147
      Subscriber

      Hello everyone,

      I am attempting to calculate the shape change due to wear using LS-DYNA. The software's wear tool has this possibility.

      I am using the below as instructions to do the analysis.

    • Aniket
      Ansys Employee
      Ansys staff can not download/upload any files on the forum, so if you want to reach a larger audience to get answers from, please insert inline images describing your problem.
      -Aniket
      How to access Ansys help links
      Guidelines for Posting on Ansys Learning Forum
    • Reno Genest
      Ansys Employee


      Have you set SPR/MPR=2 on the *CONTACT card? Also, note that only the following contacts are supported for wear:
      *CONTACT_FORMING_SURFACE_TO_SURFACE, *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE and *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE.

      You have the following paper:

      Can you re-read the section on "Geometry change due to wear" and make sure everything is right?

      As an Ansys employee, I am not allowed to download your file to have a look.

      Let me know how it goes.

      Reno.
    • mmy3147
      Subscriber

      The paper you linked is the same paper I used and had uploaded.
      The contact is correct and SPR/MPR are set to 2 on the contact card. I have added the add_wear option and I am able to get the wear & sliding distance when I load the intfor as d3plot. So far so good.
      Looking at the section about geometry change, it states that NCYC should be more than 0 in *INTERFACE_SPRINGBACK_LSDYNA. which is the case in my input. The paper then instructs to import the dynain file after loading the k file. The issue is, for some reason *INITIAL_CONTACT_WEAR data is not recorded in the dynain file, then when I load dynain, the wear tool tells me that there is no wear data in the model.
      I have removed S=intfor in the run command, this has not helped, I have added values for *INITIAL_CONTACT_WEAR but this needs to happen node by node, and it just causes the software to read the data I input. I added multiple instances of *INTERFACE_SPRINGBACK_LSDYNA for each part set, this also did not let me write my files.
      If you want more information please let me know since at this point I am having trouble pinpointing the issue.
    • Reno Genest
      Ansys Employee


      Have you tried opening the dynain file with a text editor and make sure the *INITIAL_CONTACT_WEAR are not written?
      Also, are you using shell or solid elements? If shell elements, you have to make sure the shell normals are consistently oriented (all element normals pointing in the same direction). And the normals should point to the tool and vice versa. Can you check the normals in LS-PrePost (LSPP)?

      I am doing some tests on my side to see if I can reproduce the error. I will let you know what I find.

      Reno.
    • Reno Genest
      Ansys Employee


      With NCYC=5 on *INTERFACE_SPRINGBACK_LSDYNA, do you get meaningful wear results? Or are they very small values? I have the example from the paper and they used NCYC=10000. Maybe try with a larger value.

      Reno.
    • Reno Genest
      Ansys Employee


      There seems to be an issue with LSPP importing the dynain file into the original .k file. I tried to do it and I got the same problem as you. After importing the dynain file into the original keyword, I saved as a new .k filename and opened with a text editor and the *INITIAL_CONTACT_WEAR keywords where not there. I will check with an LSPP developer to fix it.
      In the meantime, the workaround is to open the original .k file and the dynain file in a text editor, copy and paste the *INITIAL_CONTACT_WEAR keywords from the dynain file into the original .k file and then save as a new filename (End_of_Stage_1_wear.k or something). Then, open the End_of_Stage_1_wear.k file with LSPP and go to Application and then Wear and click on compute. This should work.

      Let me know how it goes.

      Reno.


    • mmy3147
      Subscriber

      Thank you ! It appears to work! I see the deformations.
      One thing has happened however, I only see deformation on some of the parts, while there is non-zero wear depth and sliding distance on all the parts of the simulation I only got deformation on two of the parts.
      The middle part (Punch) has no deformation on it. Is it possible that it is due to the fact that I defined it as an elastic material as opposed to rigid ?


      .
    • Reno Genest
      Ansys Employee


      I did a quick test and I get wear data for parts with *MAT_001. So, you should be able to get it too. Did you define the *CONTACT_ADD_WEAR for the contact for this part? If not, you won't get wear data.

      Let me know how it goes.

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