How to Match Parts of an Assembly

When creating a finite element mesh for a CAD assembly, the mesh on the individual parts of the assembly must be matched in order to directly and accurately transfer loads across adjoining interfaces. For example, in a heat transfer analysis, conduction between bonded parts can be simulated by matching the meshes on the parts. Conversely, in a Mechanical Event Simulation involving contact, parts may need to be kept separate so they do not behave as if they are bonded or welded.

During meshing, an automatically calculated tolerance is used to determine whether parts should be matched. For most cases, automatic part matching will be satisfactory; however, there are two cases where you may need to specify parameters for part matching:

• You want parts that are within the automatically calculated tolerance to be maintained as separate.
• The CAD model was not built with the precision needed for analysis and some parts that should be matched are not as close as the automatically calculated tolerance.

For these cases, part matching acts as a geometric construction tool. It can make sure that very small gaps between parts are maintained and it can remove gaps that should not be in the finite element model.

You can specify parameters for part matching in the CAD Solid Model environment as follows:

1. Use the "Mesh:Create Mesh..." command sequence to access the "Create Mesh" dialog.
     
2. Click on the "Details >>" button.
     
3. On the "Surface" tab, click on the "Options..." button to access the "Surface Mesh Options" dialog.
     
4. As shown in Figure 1, the method used for part matching and the tolerance value can be specified on the "Surface Mesh Options" dialog.

Figure 1: The "Surface Mesh Options" dialog enables you to specify parameters for matching the mesh on parts of a CAD assembly.

The "On-surface tolerance based on" field provides a drop-down menu with two options:

• "Fraction of mesh size" - When this option is chosen, the value in the "Tolerance value" field will be multiplied by a global geometry parameter and the product will be used during meshing to match nodes between parts.
    
• "Absolute length dimension" - When this option is chosen, the length specified in the "Tolerance value" field will be used to match nodes between parts. If you know the sizes of the gaps in the CAD assembly, it is recommended that you use this option. To match the meshes on parts, you can explicitly specify a tolerance value that is slightly larger than the smallest gap. Conversely, specifying a value that is smaller than the gap will ensure that the meshes are not matched and the gap is maintained.

After meshing, you can verify part matching in the FEA Editor environment. Use the "Editor Tools:Layer Control..." command sequence to access the "Layer Control" dialog. There, you can specify the display of lines on layer 15 of the model, which contains the lines that were modified in part matching. Thus, you can visually verify where mesh matching occurred (see Figure 2).

Figure 2: The "Layer Control" dialog enables you to visually verify part matching by highlighting lines on layer 15, which is where part matching occurs.

Part matching options provide convenience and flexibility by enabling you to control the way that the mesh is matched between parts of a CAD assembly.

For more information about part matching, see the ALGOR User's Guide.