Hi There fellow users.
Does anyone know how to create a rigid element between the holes of two lugs? to simulate a pin joint for example?
You can use the Custom Tools / Meshing :
Spider Curves : select two curves and Femap will create a RBE2 with a master node located at the center of the circle (if hole)
Spider Nodes : select nodes and hit ok ==> RBE2 created
Spider Surfaces : for solid mesh, select two surfaces and Femap will create a RBE2.
Note1: The slave nodes of the RBE2 created by these API script will have rotational DOF free.
You will be able to update this using Modify / Update Elements / Rigid DOF...
Note2: You could also create a RBE2 using Model / Element or ctrl+E under Type select Rigid.
Note3: RBE2 Master node have always 6DOF defined. You can only play with the slave nodes DOF.
Note4: a Slave Node could not be constrained.
Note5: You can also use the Custom Tools / Meshing / Hole to Hole Fastener. This will create two RBE2 + Beam element. Before using it, you need to create and activate a beam property which represent your pin...
If I well understood your problem then you want to check the Lugs under the load transefered by your pin. (feasible manually)
If the load is applied along Z-axis then create a spider (RBE2) for each hole (pick only 7 nodes on the -Z side of your hole) and then create an RBE3 connecting the two RBE2 master nodes and apply your load on the RBE3 slave node.
It will also better to use two CBUSH elements between each RBE2 / RBE3 interface to extract forces...
I have a similar situation in which I am trying to transmit a load from a node into a structure using RBE2 elements. In your diagram is the CBUSH element placed between the RBE3 elements and the RBE2 elements?
Great thank you!
One more thing how does changing the stiffness of the CBUSH element influence the results of the analysis? What I mean by this is does a stiffer CBUSH element or a CBUSH element with minimal stiffness help in transferring the applied load?
You should control how stiff the connection needs to be. If you need to model a bearing and have some stiffeness values from vendor for example then you can enter these stiffenesses directly in the CBUSH property. To model a fastener, a stiffness of 1E+12 N/m is generally used and of course will rigidly transfer the loads. You can use the Femap Freebody to verify if forces and moments are correctly transferred to the rest of your structure.
I am trying to extract the forces at RBE2 elements.
I saw Seif mention that the user cannot extract the forces at RBE2 elements and that is why you need CBUSH element.
However, if the "MPCFORCE" card is set "ON" in the NASTRAN input file shouldn't the forces at the RBE2 elements be available.
I went to the Analyses -> Edit -> Output -> Checked on the Force Balance, Constraint Force and Equation Force.
Let me know your thoughts on this issue.