This was a post to a message on a Meshing Problem that I am reposting here. https://forum.solidworks.com/message/110194#110194
When you add parts or place model into an assembly, the default mesh size that is calculated changes from before (when there were fewer parts). Try using automatic trials to fix the problem by successively reducing the mesh size by a factor < 1. If that still fails, try applying manual mesh controls to individual components or faces. There is also a nice option in the mesh control for a component mesh control to mesh it as if the mesh size was dependent on itself only.
The other comments above are helpful also. Here are some meshing tips that I compiled before:
Here are the order of tips to use to overcoming meshing problems:
1) First if the standard mesher fails for the default mesh size, then I suggest doing one of two things: (a) try meshing using the auto looping technique, or (b) look at the failure diagnostics to determine where it failed to give a clue as to why.
2) If you did the auto looping in step 1 as suggested and it still fails, then this time at least check the failure diagnostics.
3) Did you check interference? If there is interference, then: (a) fix the geometry, (b) create a cavity in one part so that they are not interfering but be wary of small geometry made by this feature, or (c) make it an incompatible mesh.
4) Does the geometry have some other issues like sliver areas or super small faces that are a a result of imported geometry? Can it be repaired easily? These are good questions to ask at this point but wait until you try more before doing the harder task of fixing the model.
5) Set a mesh control for the part or parts that failed and use the sliding bar for "Component significance" towards the right to High. The left end of the slider corresponds to using the default global element size of the assembly (f=0), and the right end of the slider corresponds to using the default element size if the component is meshed independently (f=1). The program calculates the element size (Ei) for component i from the equation: Ei = G - (G-Ci)*f. G is the global element size; Ci is the component size for component i; and f is the slider factor as described above.
6) Set mesh controls on individual features of the parts. Just as a recommendation for what I use for the ratio and number of layers, I think 1.25 and 4 does a better job and looks a bit smoother than the default 1.5 and 3.
7) Open the failing part or parts individually and try to mesh them by themselves. If it automatically meshes with the default, then try to find the largest mesh size that works. If the default size does not work, then use auto looping to find one that does. You may have to use feature-based mesh controls here as well. Make note of the mesh size(s) when it does mesh successfully, so that you can use this as the mesh size for a component (or feature) mesh control back in the assembly.
8) After trying 1-7 and it still fails, maybe there is a problem with how the parts are touching. Consider sliver faces or bad geometry that may be created by the mesher automatically imprinting one surface onto another. Get a better visualization of this by creating a split line if possible. You may be required now at this point to create an Incompatible mesh and create bonded contact sets semi-automatically by using the "Find Contact Sets" command.
9) If all else fails, then with your incompatible mesh, use the "Alternate" or curvature-based mesher. The alternate mesher uses the Global Size value to define maximum element size and the Tolerance value for the minimum element size. The minimum element size is used for boundaries with the highest curvature. The maximum element size is used for boundaries with lowest curvature.
Continuing on with the meshing tips, one addition:
1a) You may find in the failure diagnostics that it will tell you to either change the element size and/or raise or lower the tolerance value. Changing the element size has the effect of also changing the tolerance which sometimes is the deciding factor. You can also manually change the tolerance size to something other than the default 5% of the global element size.
First, it is important to understand how meshing is performed. After preparing the geometry by imprinting touching faces and breaking up faces into logical sub-surfaces, a surface mesh is created for each face independently.
Next, the tolerance value is used in knitting the surfaces together to create a water-tight solid, so you want to have a reasonable size tolerance value to be able to knit surfaces together (5% by default). Do not increase the tolerance value too large, but up to 25-30% of the global element size is fine. The surface meshing technology was developed in-house which is typically done for any FEA code. If there is only a Shell mesh, then the meshing stops at this point.
For a Solid mesh, it continues by filling in the volume with solid tet elements and again uses the tolerance value to determine whether elements should be collapsed or not. Here you want to have a reasonably small tolerance size so that elements are not collapsed unnecessarily. If the mesher fails in the volume filling phase, you will want to decrease the tolerance down to about 1% or sometimes smaller. The volume mesher is done by a third-party meshing product called TetMesh-GHS3D from a company in France called Distene; again this is the typical scenario used by many FEA codes.
So you have two opposing concepts that fight for raising and lowering the Tolerance value.
Here are tips on when and how to change the tolerance value:
(a) If the tolerance is too large, it will collapse nodes and create bad element shapes causing the mesh to fail. If you have features like a fillet radius or wall thickness that is smaller than the tolerance value, then decrease the tolerance to something at least half the size of the smallest feature.
(b) Be careful that you don't make it too too small or you will run into the problem of having the surface mesh not able to knit itself together to create a water-tight solid for volume meshing. Look for mesh failures coming up during the final stage of meshing a part where it is filling in the volume.
(c) The tolerance is a global value and so you should also consider the smallest mesh control size that was defined. Also as mentioned before, consider the smallest geometry feature. Make use of the SolidWorks tool "Check" for information about short edges, minimum radius of curvature and other min/max features.
(d) If the solver fails because there are not enough restraints or parts are ripping apart from one another when they should be bonded by a global contact condition, typically when working with a shells or a mixed mesh, then either your Tolerance is not large enough or you should define a Local contact set as bonded.
My favorite new values are: (0.5)^(1/4) and (0.5)^(1/3), which are approximately 0.8409 and 0.7937, respectively. Why?
Well, when I set my automatic mesh trials options, these values bring me to half the original global mesh size in 4 steps (or 3 steps). To quarter in 8 steps (or 6), to 1/8 in 12 steps (or 9), to 1/16 in 16 steps (or 12), and so on.
See below image for settings:
Copyright © 2010 Dassault Systèmes SolidWorks Corp. All rights reserved.
Do not distribute or reproduce without the written consent of Dassault Systèmes SolidWorks Corp.