How to define element coordinate system?

- January 3, 2020 at 12:01 am
  
  diegomagela
  Subscriber
  
  Hello all.
  
  I'm trying to simulate a composite plate with fibers varying spatially (curved fibers). For that, I'm trying to set a different coordinate system to each element in APDL, but I cannot until now. Would you know how do that? If there's another way to vary the fiber angle, I appreciate the explanation. Bellow there're the pictures that show what I'm trying to do.
  
  Regards.
- January 3, 2020 at 3:27 am
  
  BenjaminStarling
  Subscriber
  
  The workbench environment is uesful for this. If you are not committed to MAPDL I would advise switching to Mechanical. The workbench environment also has ACP which handles fibres and element orientations. I am not sure if the academic license permits use of ACP but I would highly recommend for all things composite.
  
  In short you will need to define Coordinate systems for each distinctly different orientation. For example, a rough look at your discrete grids indicates you would need about 10 different coordinate systems for that case. Then use the ESYS and/or EMODIF commands to assign the coordinate systems to the relevant elements. This gets time consuming and complicated for large models with many orientations. This is where ACP is useful as it provides GUI interfaces to create complex composites.
  
  https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v195/ans_cmd/Hlp_C_EMODIF.html
  
  https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v195/ans_cmd/Hlp_C_ESYS.html
- January 10, 2020 at 2:19 pm
  
  diegomagela
  Subscriber
  
  Thank you for the answer, Benjamin. It'll help me.
  
  I'd like to use MAPDL to do that. Can you please give me some code examples to achieve what I'm trying? I prefer to use code (script) than GUI.
  
  Thank you.
  
  Regards.
- January 11, 2020 at 11:59 pm
  
  BenjaminStarling
  Subscriber
  
  I would use an excel spreadsheet to generate three locations that are required by the CS or CSKP commands. One point is the origin, the next two define the x axis and the xy plane. Then use these locations to generate KP's. I would use KP's just to prevent numbering issues with nodes. The example below recreates the Global coordinate system using keypoints and assigns it to CS11 (created CS must be greater than the number 10).
  
  K,1,0,0,0
  
  K,2,1,0,0
  
  K,3,0,1,0
  
  CSKP,11,0,1,2,3
  
  Then once your CSYS are all created, and your model is meshed, create components with the CM command, or the component manager, that require the same ESYS. Then assign the CSYS using EMODIF.
  
  CM,nameofcomponent,elementsincomponent(these must be selected using ESEL or the GUI),elem
  
  EMODIF,nameofcomponent,ESYS,11(or number of the CSYS)
  
  repeat for as many components/ESYS that you require. This can be implemented as a do loop, but the manual work of identifying the elements and grouping them per ESYS is still required.
- February 11, 2020 at 6:38 pm
  
  diegomagela
  Subscriber
  
  Benjamin,
  
  How would be the do loop in that case?
  
  Thank you!
- September 13, 2020 at 12:52 am
  
  memo
  Subscriber
  
  Dear Benjamin,nI have a question related to this discussion and would be very thankful if you can help me with that.nI have a computational domain consisting 3D Solid elements.nI have the local coordinate systems for each of these elements stored in a matrix. Now I want to assign these local coordinate systems for each of the FE elements. Is there anyway to do this in ANSYS Mechanical?nI checked ANSYS ACP but it can only work with shell elements.nn