Hello fellow pioneers,
I encountered a rather strange issue in Abaqus. I am modeling contact interactions among shell elements. In this application, it is critical to apply thickness to the shell elements properly so contact can be modeled accurately. However, I am noticing abaqus assigning a thickness (1.192) to the shell elements by itself. I tried using *NODAL THICKNESS keyword to assign thickness to the nodes yet abaqus ignores that. I am attaching an inp file that replicates my problem.
This input file does not assign any thickness to the shell elements in part-2. If you run the model, the .msg file will show abaqus adjusted spacing of the parts to eliminate overclosure (which should not exist). In the odb after the simulation, you will see the shell has a section thickness (STH) of 1.192. However, you will not find this number mentioned anywhere in the input file.
Any thoughts on this issue are welcome. Thanks in advance.
Hi Yunpei Yang,
Unfortunately, I don't know how Abaqus calculates shell thickness for Shell General Section. But I tried estimating it via stiffness matrix D. According to plate theory, h=sqrt(12*D44/D11)=sqrt(12*100/898)=1.156 which is close to STH= 1.192.
Hi Victor J. Аdlucky ,
Thank you very much for the comment. You are absolutely correct. I changed the bending stiffness on the shell general section definition, both the STH and the overclosure adjustment changed as a result.
A few more things I have noticed in these tests:
1. Thickness for shell general section is handled differently in Abaqus/Standard and Abaqus/Explicit. In Abaqus/Standard, the *Nodal thickness keyword can assign arbitrary thickness to the shell general sections. Section thickness (STH) is not available as output. In Abaqus/Explicit, shell general section thickness is (very likely) calculated from the shell stiffness matrix. Section thickness is available as output. This is somewhat inconvenient since the shell general section is useful in uncoupling the in-plane and bending properties of a shell.
2. To overcome this. One can use a coupled shell membrane by having shell and membrane elements sharing the same nodes. Assign thickness to the membrane elements accordingly. Set shell elements to bending only. Then assign the contact interaction to membrane elements. This way the shell can have uncoupled in-plane and bending behavior as well as correct thickness for contact modeling.
I have a few test cases for anyone interested in this topic:
Cont_Tst_Imp.inp: a single element shell contacting a rigid shell in Abaqus/Standard. Thickness of deformable shell is controlled by the *Nodal thickness keyword.
Cont_Tst_Exp.inp: similar model but in Abaqus explicit. Coupled shell membrane. Contact interaction applied to membrane elements. Contact thickness is correct.
Cont_Tst_Exp_2.inp: similar model but in Abaqus explicit. Coupled shell membrane. Contact interaction applied to shell elements. Overclosure adjustment caused the shell to move far away from the rigid shell. (bending only caused the shell element to have a very low in plane stiffness, which then caused it to have very high thickness (~300))
- Badges
- Science topic