I am using NX Nastran 12. I have a model in which i have to use RBE3 elements to avoid adding more stiffness to the model. The problem is that i don't know how to apply constraints on the dependent node (center node) and on the same node i have to apply the force. I want to constrain the (u1,u3,u4,u5,u6=0) DOFs. Before i was using RBE2 elements and it was easy as independent node was at the center. I know of two ways. In the first way is to enable the AUTOMPC and the simultaion is running. I don't know whether it is the right way or not. The second way is to create a CBUSH element and use high stiffness values. In the second method i am getting the error which reads "USER FATAL MESSAGE 6629 (TA1BSH) BUSH ELEMENT ID = 183687 HAS INFINITESIMAL LENGTH".
I created two points on the same location to create 1D CBUSH element. But it is not working. Can anybody help me with the second method or anyother workaround?
I do not understand the problem: you want to fix to the ground the central node (dependent) of an RBE2 and then you want to apply to the same node a force? Is it correct? Because that is not sense thing: the force that you put in the system is direct discharged as reaction force. Could you explain better your problem?
Sorry for my language. So i have model with two holes. I want to use RBE3 elements on both holes to constrain the body. You can see the picture here.
So, i want to constrain DOFs of the hole 1 i.e u1,u3=0 and of hole 2 i.e u1,u2,u3,u5=0. I have to apply force on hole 1. I can not apply constraint directly on the center node of RBE 3 as it is the dependent node. My question is how to apply constrain on the RBE3 elements?
@s_gthe problem in the model of your image is that even if you apply the boundary conditions, the body is still is free in the space for 2 DoF (i.e. u4 and u6). So it is not a problem of RBE3 but only not-isostatic structure and for this reason a static analysis will always fail.
As confirmation, I also check on NX with a modal analysis and assuming a similar geometry that you sketch, and I obtain obviously 2 rigid modes around those axis.
However I ask you to add to you picture the cartesian axis in order to be sure about the orientation of the body with respect to the constraints.
Thanks for the quick answer. The picture is just an example to explain the problem. DoF u3 is fixed on both holes.
When i was running the simulation with RBE2 elements it was running successfully. Then i switched RBE2 to RBE3 elements. So, NX gave me an error and in the error message it was return that AUTOMPC must be enabled. So i enabled AUTOMPC and it worked. But i don't know if it is a right way to run the simulation or not. I know the second way which is to create CBUSH elements to apply boundary conditions. I am trying this second way but still i am not successful with this.
Firstly, take care that I modified my previous post.
Anyhow, the "AUTOMPC=ON" message appears becase you ask to the apply constraints to a dependent node (that moves according to the average movment of the structure to which it is attached). Basically this procedure is not possible, but using this particular parameter = ON, the solver keep into account to mantain in a fixed position the dependent node and therefore the calculation is performed properly.
Thus your model with RBE3 + AUTOMPC=ON is absolutelly correct!
[but I still do not understand the problem of free DOF that I highlighted in my previous post, but ok doesn't matter]
Sorry i didn't see your edited post. Thanks for the answer. Is it possible for you to show me some tutorial or something to apply boundary conditions with second method(i.e with CBUSH elements)?
I confess to you that in my opinion the usage of CBUSH as connecting element it is quite not usual and there are a lot of hidden problems such as which value of stiffness should you take for CBUSH?
In my opinion it is not a good idea use CBUSH as "spider" element like RBE2 or RBE3. Use RBE2 or RBE3!
Anyhow if you really want to use CBUSH, I suggest you to create a simple model (eg the beam with 2 holes) and create a model with RBE2, then use the same model with CBUSH with a very high value of stiffness (in comparison with the structure stiffness). If you do everithing correct, the two models should be quite similar in terms of results. Then try other simple cases in order to understand if everything work properly.
As "debugger mode", consider to use a modal solution (i.e. SOL103 response simulation or SOL103 real eigenvalues) in order to check eventual problems of DOF not constrained -> rigid modes.
Unlikelly at the moment I don't remind particular references/tutorials/videos to suggest to you on this topic, but try to search it on google. Maybe you are lucky.
Please: in case I answer to your question, consider to set the post on "acepted answer" as follow: click on top right corner->"acept as solution", in order to help other users that have a similar problem to the your. A kudo is just a form of congratulations, not an form to accepted answer!