Thin-Solid Meshing / Bending and Membrane Stresses 1

[ncrook]

My situation:

I'm trying to find the membrane and bending stress of a solid model (see attached image) using workbench in ANSYS 14.0.

The ANSYS help guide says that I need to use the "thin-solid meshing option" for the membrane and bending stress, and that it needs to be solved in the Mechanical APDL Solver.

From my understanding so far, I need to mesh the model in solid elements and then cover it with a thin layer of shell elements to capture the membrane and bending stress. But this doesn't seem correct according to this post:

https://forum.solidworks.com/thread/81340

I'm an engineering student (this isn't coursework) and a new user of workbench (I have some previous experience in simple APDL). Saying that, please don't hesitate to correct me because I only have a basic understanding of structural mechanics and the ANSYS software.

My questions:
-Does "to be solved in the Mechanical APDL Solver" mean that I need to go back and redo the model (geometry,loads,meshing,etc) in APDL? From what I understand workbench exports a file to the APDL solver in the background for the solution, but I'm not sure if that's what the above mentioned phrase is referring to.

-Will a shell model (no solid elements) give me the correct results for bending stresses? Can I enter in a virtual thickness/stiffness for the shell body to have the same stiffness characteristics as a solid body? I have cut the body into several parts to facilitate meshing (see attached image), but I'm not sure if that makes using shell elements more difficult....

-If a shell model won't yield the correct results, is there anyway to apply a shell layer to the outside of a solid model (in workbench or APDL)?

Thanks for your time!
Nolan

 

[rickfischer51]

To run in MAPDL, click on Static Structural in the tree, then click on Tools, Write Input File in the toolbar. This will create an input script for MAPDL. Start MAPDL, anf click on File, Read input from, and select your file. Or, at the command line, type /INPUT,filename,inp

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[spongebob007]

If you are looking to get membrane and bending stresses, I don't understand why you don't just use shell elements.

 

[corus]

The problem with solid elements is that the stresses are calculated at the integration points and extrapolated to the nodal positions at the surface. This can cause a slight error at the surface, depending on the mesh density. You can overcome that problem by 'skinning' the solid elements with thin shell elements that will calculate the stresses at the integration points, at the surface. This method though causes an error as you're adding more thickness to the solid depending on the thickness of the shell. Whether you decide to skin the solid or not won't give you the membrane and bending stresses though as the stresses at the surface could be classed as being composed of membrane, bending, and peak stresses. The best way to get the membrane and bending stresses is to put a Stress Classification Line through the solid which will calculate the membrane and linear bending stresses, devoid of any peak stress component.

 

[ncrook]

Thanks corus,rickfischer51, and spongebob007 for the responses.

@corus, The stress classification line is modeled in ANSYS workbench with the construction geometry correct? (see attachment)

@rickfischer51, My question was more if thin-solid meshing option was only available through ANSYS Classic. Since then I've found that I can input APDL commands into workbench instead of restarting from zero in classic.

@spongebob007, I've been given the requirement to use quadratic hexahedral elements for the model, which is why I didn't use shell elements. I was considering adding a thin layer of shell elements but I think corus's reply has pointed me in the right direction