3D Design

3D Design

Add same element type to several geometry

    • Sarah
      Subscriber
      Hello all. I’m modeling random fiber inside concrete ( still in trials period). Let’s say I have 30 fiber and I need to use Link180 for all. Now I add command window for each to add the element type. Since I’m trying several options, it is really hard to keep doing that. Anyway I can do this in groups or in “bulk” for all fiber geometry?
      Thank you
    • peteroznewman
      Subscriber

      Hello Sarah,


      Here is a long discussion on how to create a large number of random fibers into DesignModeler for reinforcement of concrete.


      The conclusion is that you can take a spreadsheet and read in bulk the coordinates of the endpoints of 30 fibers and they will become line bodies.


      Regards,


      Peter

    • Sarah
      Subscriber

      Peter,


      thank you for forwarding me to this discussion, it is helpful to see what is already available. I wrote my own matlab code and I have all points for lines. I'm asking about assigning "Link180" to each. Will that happened automatically, because I assign it now by inserting "command" for each one.


      Thank you

    • peteroznewman
      Subscriber

      Sarah,


      If you put a command object under each line body in Workbench, then you can assign the LINK180 element to that body.  You can verify that it is working by using Tools > Write Input File in Mechanical and examining the contents of the file created.


      Regards,


      Peter

    • sk_cheah
      Subscriber

      Hi Sarah,


      Hopefully this analysis snippet is what you are after:


      /prep7
      !!! Setup for LINK180
      area = 3.1414
      et, 1010, 180
      sectype, 1010, link
      secdata, area

      !!! Selects all beam188 elements for conversion to link180
      esel, s, ename,, 188
      emodif, all, type, 1010
      emodif, all, secnum, 1010

      !!! Revert back to solution
      /solu
      alls

      Kind regards,
      Jason

    • Sarah
      Subscriber

      Peter, 


      write input file is gray and I can open it. but looking at the forum you referred made me thinking: what is the way you used to connect fiber with concrete as you mention there previously?


      Appreciate your help

    • Sarah
      Subscriber

      Jason,


      thank you for the code, that is exactly what I'm looking for. But where should I add this command in the tree? 


      Regards


      Sahar

    • sk_cheah
      Subscriber

      Sahar,


      Please see last slide in this presentation. Add the command snippet to the Solution Processor as pictured on the right of that slide.


      Kind regards,
      Jason

    • Sarah
      Subscriber

      Thank you Jason, That is way easier than copying the command fifty times

    • peteroznewman
      Subscriber

       Sarah,


      Slide 5 in Jason's link shows that you have to click on Solution, then the Write Input File will not be grey.


      One way I know how to use line bodies that lie randomly within a solid volume as reinforcements is in the Explicit Dynamics solver where the Body Interactions tab allows the line bodies to be called out as type = Reinforcement.


      This is rather elegant. The line bodies are meshed independently of the mesh of the solid volume. It is the solver that figures out which nodes of the line body is inside an element of the solid body, and connects those nodes to the intersecting solid elements.  Below is a bit of the ANSYS help section.


      2.6.2.2.4. Reinforcement Type


      This body interaction type is used to apply discrete reinforcement to solid bodies. All line bodies scoped to the object will be flagged as potential discrete reinforcing bodies in the solver. On initialization of the solver, all elements of the line bodies scoped to the object which are contained within any solid body in the model will be converted to discrete reinforcement. Elements which lie outside all volume bodies will remain as standard line body elements.


      The implicit solver used in Static Structural has a different way of dealing with reinforcement. I recall making sure the line body mesh shared nodes with the solid body mesh. Maybe some one else will comment on other methods available.


      Regards,


      Peter

    • Sarah
      Subscriber

      Thank you Peter.

    • jackhero
      Subscriber

      @Sarah


      Could you please share the matlab code which you have used to model the fibers reinforcement? I am also working on the design and modeling of fibers in concrete in ANSYS workbench. I would like to follow your updates/progress in this matter.


      Thank you

    • Emad64
      Subscriber

      Hi Sarah and Jason,


      Can you please decode the command, or suggest me a command to convert all solid186 to solid65.


      Thank you.

    • walkdenp
      Subscriber

      Please could you repost the link to the presentation? the link in the comment doesn't work.

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