Methods to add rotation dof to solid with ABAQUS, MSC NASTRAN and SAMCEF

[AACING]

Hello !
For my internship, I am doing a benchmark on thermal and thermomechanical analysis, particularly on mapping of thermal results. For this purpose, I am asked to establish a list of ways to add rotation dof to solids with ABAQUS, MSC NASTRAN and SAMCEF that could be compatible with thermomechanical cases (mainly the addition of thermal expansion). As of now, I have tested/selected the ones listed below :
-adding a perpendicular shell through SAMCEF sticking/MSC NASTRAN glue contact/ ABAQUS TIE, beam links or coincident nodes inside the volume,
-APS macro with SAMCEF (not tested but suggested by my tutors).

NB: the use of shells is standard procedure in the company.

I am considering :
-MSC NASTRAN RBE3,
—MSC NASTRAN GAP/CGAP
-adding a beam/rigid element linked to the solid the same way as the shells,
— ABAQUS shell to solid coupling,
— ABAQUS Rigid body constraint,
— ABAQUS General contact,
— ABAQUS Coupling constraint.

Does anyone have any remarks or other ideas regarding this topic?

Thank you in advance for your help !
A.

 

[rb1957]

I've never heard of a 3D solid element having rotational freedoms at its nodes. 3D solids are formulated for translational freedoms. Moments are reacted over multiple elements. I guess you could use an RBE to create a point moment ...

"Wir hoffen, dass dieses Mal alles gut gehen wird!"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[SWComposites]

Google "transition from solid elements to shell elements" - there is lots of info out there

 

[GVDR]

Rotation DOF have no meaning for 3D solid elements. These DOF exist in 1D and 2D elements as a mean to simplify the small dimensions. You can see them as the way of connecting the mesh nodes to the shallow structure section orientation.
ABAQUS has a shell to solid feature but it is rather defined to connect a shell with a normal in the same plane.

How I would do this in ABAQUS: keep the first layer of your plate elements in contact as 3D. This 3D layer can be connected with a TIE to your solid, then do a solid to shell connection in your plate between the 3D layer in contact and the remaining.

How I would do that in other softwares as lower level -- in fact I developed specific tools to do this in our SDT software at SDTools:
- add rigid elements linked to the plate membrane to represent the plate skin (and therefore assess the plate thickness trace on the solid for the connection)
- use the master nodes of the rigid elements to do a node-to-surface tie on the 3D solid.
That way, the rigid elements will transfer the section induced momentum to the shell rotation DOF.

Now for a thermal analysis in your case, I would first check the plate thermal expansion behavior in the thickness direction, and how this interacts with the connection. I am not sure any code formulation is equivalent on this point.