Ansys Learning Forum › Forums › Discuss Simulation › General Mechanical › MPC Joints Shared Between Bodies › Reply To: MPC Joints Shared Between Bodies

You can have two types of models to understand the performance of this structure. The model you have is a “System” model. It correctly predicts deformation and dynamics results such as first mode frequency or harmonic response. You can improve this model by removing some joints and replacing them with shared topology and you may be successful eliminating the MPC warning. You might not see the results change significantly because the constraints are not in conflict. However, the system model lacks the fine detail of how the weld beads hold the structure together and this model is not helpful in evaluating the stress in the welds. For that you need a “Detailed” model.

To construct a Detailed model, open the geometry in a CAD system such as SpaceClaim where an I-beam will be idealized as three surfaces instead of a line and a square tube will be idealized as four surfaces instead of a line. Now you have many more faces and edges to keep weld beads separated from each other. A simpler detailed model can use Joints to represent where each weld bead holds two parts together to extract the forces going through the weld bead. In this way, you may be able to build the model where there are only two entities in each joint, one for the Reference side and one for the Mobile side. You may need to add connection bodies as described above to keep the welds separated. If that proves difficult or deviates too far from the actual build, you may need to build a “Breakout” model, which is a third type of model.

Say three tubes come together and one complex 3D weld wraps around the intersection of the three tubes. To evaluate the stresses in that area, open the geometry in CAD and create a plane normal to each tube axis at least 4 tube diameters back from the intersection of the tubes. Create a solid model of the tube sections and the blend that represents the weld. Assuming this is a full penetration weld, there is just a single solid body. That body has a Tet mesh on it. The same 3 planes are setup in the Detailed model and the method in this discussion is used to extract the displacements occurring on each plane and those become the loads going into the Breakout model. In that way, you will have an accurate evaluation of stress in that complex weld. Ansys has a way to automate the transfer of loads from a global model to a local Breakout model, it is called Submodeling.