Enforced displacements from another model's results?


There is a command that seems to be designed to do exactly what I want: Model > Load > from other model results. However, I can't get it to work. The interface nodes are at the same location in both models. In the source model, they are on RBE2 elements. Could that be the problem?


I have included both the RBE2s and the nodes I want results from in a group in the source model.


The message I get is "0 elements were assigned from the source model" (rought DE>EN translation of message).


Ideally what we want is to apply all DOF from an interface in one model onto an attached component model as enforced displacements. I can do it manually but there are then 96 individual entries to be made (6 DOF x 8 nodes x 2 load cases).


Thank you for your help.


Re: Enforced displacements from another model's results?


Hi Kava,


Is the RBE (2?) element part of your sub-assembly? is it at the interface between global / local models?

be aware that slave nodes cannot be constrained and if you will apply enforced displacement you will have to fix them in every enforced direction. May be it is automatically detected by Femap when defining nodes and elements onto which you want to apply disp.


If this is the case then I suggest you to add one or two range of (plate?) elements connected to the rigid in your sub-model then apply the enforced disp and boundary conditions on them.


You should obtain the same displacement and stress level as the global model calculation. That will validate you submodeling approach.  


Personally, I prefer the Model / Load / From ouptut command and work with groups in the same model.


Post a view of the model to better understand the interface you will constrain



Seifeddine Naffoussi
SafeMecha Stress Engineering

Re: Enforced displacements from another model's results?

Siemens Phenom Siemens Phenom
Siemens Phenom

You can also create an Output Map Data Surface in the model with displacement results.  Copy it to the clipboard (from the Data Surface Editor), paste it into the model where you want to use the displacements.  In that model create an Enforced Displacement Load, and set the x, y, and z factors to 1.0, and point to that data surface.  When the Enforced Displacements are created, FEMAP will interpolate into that Data Surface and grab values.  If the nodes are in the same locations, they will match exactly.