3D Design

3D Design

How to import a composite model from APDL to workbench

    • DoubleCNg
      Subscriber
      Hello guys Can anyone tell me how to import a composite model with fiber lay-up from APDL to workbench? I have created a .cdb file but it seems like FE modeler only take the dimensions and material properties. It doesn't take any fibee lay-up at all.
    • Sean Harvey
      Ansys Employee

      Hello,


      Currently the method would be to use external model which at 19.2 can read the layup from the cdb file (sectype & secdata).  It will work for layered shells.  Now the issue is right now the student version is at 19.1 so this is not available.  If you are using an Academic license (not student) then you would use the external model  component system, not FE Modeler.  You can then link the external model to the model cell of static structural or equivalent.  In our help you can find details on external model usage.


      One other way would be to write out your model to a new cdb file w/o the layup using cdwrite in APDL.  You would have to change the secnum for all the elements.  Then you can read that mesh in using external model so you can get the mesh in Mechanical. Then in a command object in Mechanical your could copy and paste in all the sectype,secdata that has the layup from the original .cdb file and modify the elements secnum to the appropriate.  If you only have a few layups this is fairly easy. If you had dozens or hundreds, the commands would have to be able to identify which elements to update the secnum and this can take a bit more APDL.


      Let me know if this helps. Thank you.  


      Sean Harvey

    • DoubleCNg
      Subscriber
      Hi Thanks for telling me. I'm using student version so I think I will just use ACP(Pre) to create the composite since I'm modeling a 16 layers composite.
      Sorry again, I'm totally new to ANSYS. May I ask, how about fatigue analysis for composite material. It seems like the system does not allow me to run the stimulation in structural analysis. A lot of people say it is easier if you are using nCode. So, is there anyway to run a fatigue analysis for composite material other than using nCode? I do not have nCode DesignLife in my ANSYS and it keeps showing "You have chosen an invalid result for the current analysis." in structural analysis whenever I am trying to solve the stimulation.

      Regards Chu Chiat Ng
    • Sean Harvey
      Ansys Employee

      Hello,


      So, the imported plies object that comes into Mechanical from ACP (or the method I described above via cdb import in 19.2) is not compatible with the fatigue tool. Typically fatigue of composites can be much different than fatigue of metallics.   Let me explain. While some modes of failure of composite part can have S/N curve that looks similar to metallics, some do not.  In a metallic, you can have an S/N curve for a particular material and have knock down factors for size effect, surface finish, reliability, etc.  In composites, the layup and mode of failure greatly dictate what the effective "S/N" curve of the part i.e layup (not just ply) would look like so you would need an S/N curve that is unique to the material, layup, and mode of failure (tension-tension) or bearing, or short beam shear, etc.  So if you had testing that gave you an idea of say bearing failure S/N curve, one could think to use that on the macro scale, i.e. this part can see this much alternating bearing load. We can not put in a material specific S/N that would capture this macroscopic behavior that again is more of by-product of the composite layup and not the ply material.  So it is for these reasons an possibly others it is not compatible.    I hope this helps.  


      Regards,
      Sean

    • DoubleCNg
      Subscriber

      Hi, Thank you for reply again.  Regards, Chu Chiat Ng

    • Venugopalb
      Subscriber

      Hello sir!


      what is secdata & Sectype?


      I am very confused with this.


       

Viewing 5 reply threads
  • You must be logged in to reply to this topic.