General Mechanical

General Mechanical

Contact Problem Between Solid and Topology Shared Surface

    • emirdegirmenli
      Subscriber

      Dear all,


      I am trying to conduct Vibro-acoustic analysis by using Acoustic ACT. to get best results, 'Share Topology' is recommended, especially bodies are contacted with the acoustic body. I modeled a musical instrument which includes solid and shell elements according to this method and  It really works, results are compatible experimental data. And next step I have been trying to add a bridge, which is the part of musical instruments where the strings are fixed, on the surface (soundboard) but I couldn't manage. When I share all geometry I couldn't select surface to contact body. If I share geometry except for bridge solid, I can select surface but 'Multiple' is written in the box and it doesn't allow contact. How can I solve this problem? Best


      Emir 


       


       


    • peteroznewman
      Subscriber

      Dear Emir,


      When Share Topology is working, the elements share nodes at common faces and there is no need for contact.


      Without Share Topology, you would use contact and it would be between the sheet and the bridge, which would be in separate components.


      I can take a closer look if you Attach the workbench project archive (and say which version of ANSYS you are using).


      Regards,


      Peter

    • emirdegirmenli
      Subscriber

      Thank you Peter, I attached archive file. I am using R18.0  version.

    • peteroznewman
      Subscriber

      When your shell elements are at the midplane and the solid elements are t/2 distance away, you have to use contact.


      There is a way to project the curves from the solid onto the shell to divide the face so the contact can be limited to the appropriate area. Below is an illustration with a 4 mm thick shell or a 2 mm gap.


    • emirdegirmenli
      Subscriber

      Thank you Peter, You are right, If I use shell element with "middle" offset type and I move it t/2 distance away, faces isn't split and I can contact bridge and soundboard. but, I have faced a different problem. all surfaces of geometry contact with air (solid) inside, so I am using share topology to contact surfaces and air as recommended for vibro-acoustic analysis. in this case, intersection mesh area is formed ;as you can see and mesh quality reduces. If I separate, they aren't bounded by using share topology. As a result, If there is any way to solve bridge and soundboard contacting problem by using shell element "bottom or top" offset type, ? think it will be very useful for vibro-acoustic analysis. Best


      Emir



       


    • peteroznewman
      Subscriber

      Emir, it is just a visual artifact that is part of rendering the shell thickness.


      In your previous model, the soundboard offset was set to bottom, so when the graphics renders the thickness it shows on the outside.


      When you changed the soundboard offset to middle, the nodes all moved out by t/2, including the air. If you uncheck on the View menu Thick Shells and Beams, you will see a clean connection of elements between the air and the soundboard. There are no new elements. Below is the image for when that is unchecked.



      Below is the image with checked.



      Below is the image if I change the soundboard thickness to 8 mm.



      I hope this clarifies the meshing.


      Best regards,


      Peter


       


       

    • maurya
      Subscriber

      hi emi 


                    how you select the shell element element  in your model i saw your  model you are working on workbench.


      there is programme itself selecting element how you can say it is shell element.


       


      regards 


      deepak

    • peteroznewman
      Subscriber

      Hi Deepak,


      Surface bodies are meshed with shell elements, solid bodies are meshed with solid elements. The distinction between surface and solid bodies is very clear in the Geometry branch of the Outline in Workbench as they use different icons.


      Regards,
      Peter

    • maurya
      Subscriber

      hello sir 


                        i agree with your point but there is solid shell element  solsh190 is there which we can use for thicker body also.


      But when i am using commands in ansys workbench to use this element it override the command and still using solid186 element.


      thank you

    • peteroznewman
      Subscriber

      Hello Deepak,


      A solsh190 element is generated in Mechanical (Workbench) by using a Mesh Control called Sweep with two specific edits: Pick Automatic Thin (or Manual Thin) and Solid Shell.


    • maurya
      Subscriber

      thank you sir 


                           i am going to try this.


       


      it works


      thank you sir


       


                         


       

Viewing 10 reply threads
  • You must be logged in to reply to this topic.