Question:
Our customer wants to do a Loadcase combination between two different analyses having different mesh (due to a slight geometry change), supports and loads. When he tries combining the two loadcases concerned, he gets a warning that the loadcases were solved using different mesh, BCs . . . He wants to know
1. How the combination is done in ANSYS for such type of situations, to better understand the combined results and to interpret the results at the locations where the corresponding nodes in two models are not coincident.
2. The best method to combine such type of loadcases.
Personally, I suppose that the best approach would be using the submodelling technique. I would like to have details on this method for the loadcase combination application, if applicable.
Answer:
Let me begin by reviewing for you how a finite element solution is actually done. In the beginning matrices with all of the degrees of freedom for all of the elements are created and passed to the solver for global assembly. Boundary conditions are then applied. Force type boundary conditions are added to the right hand side of the system of equations. Constraints with zero magnitude displacements reduce the size of the problem by eliminating that degree of freedom row and column from the global matrix. For constraints with non zero displacements, that displacement is multiplied by the appropriate degree of freedom column of the global matrix and the result is added to the right hand side; then that row and column are eliminated from the global matrix. In the end, the problem to be solved consists of only the unknown degrees of freedom.
If the user were then to change the constraints, not forces, the problem to be solved would be different. That is, there would be different unknown degrees of freedom and the length of the solution vector could be different. Or if the mesh were changed, the two problems could have a different element order. The program write
Question: Our customer wants to do a Loadcase combination between two different analyses having different mesh (due to a slight geometry change), supports and loads. When he tries combining the two loadcases concerned, he gets a warning that the loadcases were solved using different mesh, BCs . . . He wants to know 1. How the combination is done in ANSYS for such type of situations, to better understand the combined results and to interpret the results at the locations where the corresponding nodes in two models are not coincident. 2. The best method to combine such type of loadcases. Personally, I suppose that the best approach would be using the submodelling technique. I would like to have details on this method for the loadcase combination application, if applicable. Answer: Let me begin by reviewing for you how a finite element solution is actually done. In the beginning matrices with all of the degrees of freedom for all of the elements are created and passed to the solver for global assembly. Boundary conditions are then applied. Force type boundary conditions are added to the right hand side of the system of equations. Constraints with zero magnitude displacements reduce the size of the problem by eliminating that degree of freedom row and column from the global matrix. For constraints with non zero displacements, that displacement is multiplied by the appropriate degree of freedom column of the global matrix and the result is added to the right hand side; then that row and column are eliminated from the global matrix. In the end, the problem to be solved consists of only the unknown degrees of freedom. If the user were then to change the constraints, not forces, the problem to be solved would be different. That is, there would be different unknown degrees of freedom and the length of the solution vector could be different. Or if the mesh were changed, the two problems could have a different element order. The program writes the nodal and element solution order vectors on the results file and the load case combination marches down the solution vectors processing the results. If the solution vectors are different, the program knows that the problem has changed. Hence the message about boundary conditions, etc having changed. But that message is intended to alert the user about the change. The underlying assumption for load case combinations is that the user knows what he is doing and POST1 will attempt to accommodate the user. There is really only that one check and even that will not prevent the combination of load cases. As an example, look at the attached file. It has a different mesh and the displacements are still combined. Note in particular the y displacement of the node at Y = 0, which is supposed to be fixed in that direction. The program added the displacements but gave up processing the element results when it recognized that the element solution vectors were different. ANSYS does not inhibit the combination on the assumption that the user is aware of what is happening and how the results will be used. In reality, to check that the two finite element models are the same would require comparing every node and every element, which would slow the processing for all users to trap the few cases where the models did not match. The cost to all users would be very high for the very low benefit to the few users who attempted to combine different models. The WARNING message that we output appears to be appropriate. The ANSYS program will process the load case combination commands through the nodal and element solution vectors and if these vectors are the same, the load cases will be combined. Our best guess as to what will be happening most of the time is that results will be combined on the node by node and element by element basis so that for 2 nodes WITH THE SAME NODE NUMBER that are offset slightly, the combined result will be same as if they were actually located at the same location. We do not recommend attempting to combine load cases with different meshes. If combining load cases for slightly different meshes is required, we would recommend using the same models and import the nodes and elements for the subsequent models rather than meshing the solid models. The NBLOCK and EBLOCK commands would be particular useful for this. The nodes that must be modified could be modified in /PREP7 after the original model is read in. Using the same finite element model should result in the same solution vector and node and element order vectors. The same finite element mesh cannot be guaranteed from similar solid models. Again, if the finite elements mesh is different (different number of elements, different nodes attached to elements, etc) combining different load cases will likely not be possible. Another possibility would be to export the results to ANSYS array parameters using the *VGET command, process those results in an appropriate manner (combining, scaling, massaging, etc) and then returning the data to the database using the *VPUT command for printing and plotting. Finally, as you asked about SUBMODELING, I doubt that this is a viable option. Submodeling does not function like rezoning. In submodeling, only the boundary nodes on the submodel have displacements applied; no element results are transferred. The interior displacements and the element results are expected to be supplied during another solution. ANSYS is currently developing rezoning capability as it relates to the solution of hyperelastic and inelastic analyses. Whether rezoning will be available for load case combinations of dissimilar meshes is unknown at this time. 

