Dear all,
I am using the user subroutine (UMAT/VUMAT) to define the constitutive relation. However, this constitutive relation includes only in-plane membrane components. When I am using the membrane element, the simulation runs alright; but I have to include the out-of-plane bending behaviour using the shell element. I have assigned the section properties with the transverse stiffness, but it does not work. Any suggestions?
For implicit simulations, you can use an UGENS user subroutine,
http://abaqus.software.polimi.it/v6.14/books/sub/default.htm
Apparently, an explicit version of this subroutine also exist (VUGEN), (see for example : http://www.sciencedirect.com/science/article/pii/S2212827117304067).
Kind regards,
Hi Eduardo Guzman,
Thanks for your answer.
For Abaqus/Standard, UGENS (rather than UGEN) is the subroutine to define the shell section behaviour.
However, for Abaqus/Explicit, there is no VUGENS. As far as I understand, there is no user-defined subroutine available in Abaqus/Explicit to define the shell section behaviour. I guess VUEL is required to define a new type of element to include the bending component.
Anyway, thanks for your kind suggestion. ^_^ Also, you are warmly welcome to give some further suggestions.
Best regards,
Shuai
Hi All,
This might be late but in case anyone else still exploring methods on the same front. You can have membrane elements and shell elements sharing the same nodes to form a "hybrid shell" in Abaqus. Make two mesh parts (one with shell elements and one with membrane elements) and then merge them in the assembly (Merge/Cut). Select the options "Merge mesh", "Merge nodes", uncheck "remove duplicate elements". In the input file, you can specify the shell elements to be "bending only" so the in-plane behavior of the model is dominated by your membrane elements.
- Badges
- Science topic
- Similar topics
- Engineering
- Chemical Engineering
- Membranes