General Mechanical

General Mechanical

ACP Composite Flat Plate warping

    • MicrofractureMan
      Subscriber

      Hey!


      I'm doing a simple analysis of a flat composite plate (carbon fiber - data from a datasheet). I am fixing one edge and applying a purely tensile force on the other side. From CLT, and from just a general intuition, I expect that the flat plate should stretch in the tensile direction. However, I am getting most of my deflection in the Y direction (upwards in my coordinate system). I suspect something is wrong with my setup, but can't quite put my finger on it. I've attached pictures with setup and deformation results, as well as the archived project. I am getting a correct force reaction at the fixed support, as well as 0 displacement there, which checks out.


      Currently the plies are oriented [0/45/-45/90/-45/45/0] (odd symmetry), for an unidirectional fiber.


      Any help is appreciated.


      Thanks,


      MicrofractureMan


       



       



    • Arnopov
      Subscriber
      Hi,I had the same issue, and ended up here. Frustrating that nobody commented.nAnyway, I think I worked it out:the constraint and load are applied on edges, BUT the composite plate has a real meaningful thickness, even with shell elements, AND the edges is not centered on the stack, but is at one end. That creates a bending moment. In fact it's possible to replicate that warping with an isotropic material loaded on edges, it will warp too (might have to turn on weak springs on)nI'm pretty sure that this scenario was purely for a learning experiment, but in case it does matter, possible workaround are:n1/ create a solid model in ACP, and then load on facesn2/ Symmetrise the layup stack with an aditional OSS pointing in the opposite direction (with your stack, that would mean dividing your center 90 into two I think.n3/ Apply sensible constraints on the side edges ? (haven't tried that last one)n
    • April Wang
      Ansys Employee
      Another tip to add here is, one can go to ACP-post, create a sampling point, and plot the through thickness stressnFor example, in this case the s1 is in bending patternn
    • MicrofractureMan
      Subscriber
      Thanks for the comments! I did end up creating a solid model instead, and that seemed to fix it. I think it was indeed creating a moment from being applied off-center, maybe only the top nodes were having a load applied to them, while the other side might have had all nodes fixed. It was, like you said, just a playing around with ANSYS and ACP model, so that I could move on to a model that I require for research. nAs for the sampling point, that's something I've never used before, I'll definitely start using it now, it seems incredibly helpful. nThanks to both of you for answering and sorry for not replying until now!n
Viewing 3 reply threads
  • You must be logged in to reply to this topic.