Learning Forum

[LCP]

Hello all,

I am trying to simulate a vessel with fibers. These fibers can change their primary orientation in each element. Therefore, I am trying to give each element their own local coordinate system in Mechanical APDL. I have found that I can use the CS command to assign a local coord. system through the element nodes. However, I have also found that just one of these coord systems can be used during the simulation. Is it also possible to assign a coord system to each element, and that during the simulation the (e.g.) stresses are calculated for each element in their own coordinate system?

Regards,

[Sean Harvey]

You can create a local coordinate system using one of the several commands such as cs, then use the emodif command to modif the element to use that local coordinate system (change the esys of element). You can loop over your elements in a *do loop to do this in an automated fashion too. You end up with a local CS for each element,which is fine.
Once you solve the model, you just use the rsys,solu command so that when you plot or list stresses such as using plnsol or prnsol, they are reported in the element coordinate system.
One comment. If you are trying to simulate a vessel with fibers, if you have a layup of composite instead of just a single material (or smeared equivlalent material), you can use the sectype, secdata to define the layup, use the emodif to modify the esys (this will be your reference direction), and use emodif at same time to modify secnum (layup of the element). You then use rsys, solu along with shell command for top,bot, mid, and layer command in post to post-process layer by layer.
I hope this answers your question.
Regards Sean