Beams Modeling Bolts “Behavior” Options
Beams Modeling Bolts “Behavior” Options
(OP)
In Ansys, when the bolted joint is modelled by using Beam Elements, there is options of defining the Beams as, Deformable, Rigid and Beam.
If I understand correctly, this is the area stiffness, where Beam is connected to the members of the joint, that is at bolt head and nut interfaces.
"Deformable" means the interface area stiffness will be true.
"Rigid" means, the interface area is rigid and it is not the structure true stiffness.
"Beam" I am not sure, what this behavior means. In the Deformable and Rigid behavior, the beam stiffness is true, that is from Beam cross section and material assigned to Beam. What this truly means?
Thanks for sharing of your knowledge.
If I understand correctly, this is the area stiffness, where Beam is connected to the members of the joint, that is at bolt head and nut interfaces.
"Deformable" means the interface area stiffness will be true.
"Rigid" means, the interface area is rigid and it is not the structure true stiffness.
"Beam" I am not sure, what this behavior means. In the Deformable and Rigid behavior, the beam stiffness is true, that is from Beam cross section and material assigned to Beam. What this truly means?
Thanks for sharing of your knowledge.
Talk To Other Members
RE: Beams Modeling Bolts “Behavior” Options
Beam connections connect end points of beam element to washer/bolt or nut head surface in contact with clamping plate. Multipoint constraints (MPC) are used for this connection which connects master node to slave nodes using rigid links.
Rigid behaviour is like RBE2 connection or (kinematic coupling in abaqus) wherein the master node drives and slave nodes are driven. That's why the shape of bolt hole remains constant
Deformable is like RBE3 connection or (distributing coupling in abaqus) wherein the master node displacement is weighted average of slave nodes which are independent nodes and hence bolt hole may become oval or distort from circular shape due to master/slave node displacements.
Beam is like connecting the master node to slave nodes by using beams with custom defined beam material and beam cross section. This might be useful in getting distribution of forces from bolt beam end node/master node to slave nodes.
IMO, use rigid behaviour if you are really not interested in beam hole behaviour and just want quick check. You can gain some insight from deformable behaviour but then its better to use solid bolt modelling.
RE: Beams Modeling Bolts “Behavior” Options
The modeling of Bolt Beam connection to Head/Nut Interfaces through beams of certain cross sections gives the forces/displacement determination in ANSYS Workbench, I am not sure at this point, what will be usage of it. NASTRAN RBEs, ANSYS MPC Contact Algorithm are efficient ways of modeling the connections.
In NX, the MPC Forces/Reactions can be requested in results output request which gives the loads going through a MPC connection.
Again, Thanks for the valuable reply.