I am trying to simulate a lap joint with a solid preloaded bolt but there are some issues. Could anyone please look into the attachment for possible sources of error?
This is just an example model. I want to use the analysis settings of this model in a slightly more complicated model.
There are several issues with your model:
1) Connection Regions should be continuous and lie on only a single part.
2) The Bolt Region should be defined by nodes as well as defining an axis along the bolt shaft. I modified your bolt by splitting it and creating a non-manifold body. The bolt region is defined by the nodes at the center of the bolt shaft and aligned with the global Y-axis.
3) Bolt preloads and non-glued connectors are not supported for the basic nonlinear solution sequence.
I've attached a Femap Neutral file with the corrections to your model that will work in linear statics.
Thank you very much for spending time on the lap joint model and responding with useful inputs.
Point no. 1 and 3 are clear.
I had posted this query as the model was not working in the advanced nonlinear static solver (sorry I forgot to mention this explicitly). And it still doesn't work after the updates suggested by you. Are there some special requirements for solid bolt preloading in SOL601 solver?
Since the meshed body was a non-manifold body, it was meshed as a single solid and there was no need to merge nodes. You could have also left the top and body of the bolt as seperate solids, meshed them and them merge the nodes at the interface. You do have control over the tolerance of locating the node in the check coincident nodes command.
For NX Nastran, you should use nodes for the definition of solid a bolt region.
You should not use all of the nodes to define the bolt region. From the NX Nastran User's Guide (you can find this using the Help > NX Nastran command):
Modeling with Solid Elements
The structure of an input file for modeling bolts with solid elements is identical to that for modeling
bolts with line elements except that:
• A mesh of CHEXA, CPENTA, and CTETRA elements are used to represent a bolt. Create the
solid element mesh such that at an intermediate position along the bolt axis the element edges
and element faces of the mesh form a cross section through the bolt. As a best practice, make
the cross section planar and normal to the axis of the bolt. Doing so will facilitate interpretation
of the results. The cross section of the mesh and the material properties associated with the
mesh should also be representative of the corresponding bolt.
• ETYPE = 2 should be specified on the BOLT bulk entries. When ETYPE = 2, the fields on the
BOLT entry are used to define the axis of the bolt and list the grid points that lie in a cross section
of the bolt.
The modeling of the bolt is the same for the Advanced Nonlinear solver.