How do you determine what is an appropriate size mesh for your assemblies?

Is there a rule of thumb or some other means that you use to determine a comfortable mesh size?

How do you determine what is an appropriate size mesh for your assemblies?

Is there a rule of thumb or some other means that you use to determine a comfortable mesh size?

One way to do this automatically is to use an adaptive mesh (RMB on Study 1 in FM and select Properties). This works by running a study, locating high error (energy inequalities) and refining the mesh in those areas. It is not true error but it tends to refine in the best places (typically where there is high stress, but watch out for discontinuities)

One thing to watch out for though is that this option is only available for solid elements only. I'm assuming that if you're working with an assembly, you are simplifying your components into shell bodies to reduce your solve time.

Also, I get an error before the third iteration that says mesh adaptation failed. What can cause this error?

Try adding mesh constraints to areas of interest. Mesh failure in an adaptive mesh is common. I am not familiar with the methods that adaptive meshes use so I don't know about the rigid bodies. After the second mesh was generated, the first mesh was erased. Re-run the study using this second mesh without remeshing (turn off adaptive). This should give you an idea of how to best mesh an assembly.

FEA is as much an art as a science. Typically the smaller the mesh the more accurate the results, but a mesh with 1,000,000 nodes can be pretty strenuous for a desktop computer that you wish to continue using while the study is going (these studies can take hours to solve, if not days). Read up on FEA or mabe take Solidworks' Simulation class. Experience will tell you how to build your study as far as your hardware and time constraints.

Thanks for all the help. I am starting my senior year in ME at IPFW on Monday, and I am taking the course on FEA this fall. Hopefully it will help me out, but I doubt it. I think the class is focused on theory not application.

For whatever reason the mesh on the second h-adaptive loop has some parts meshed with an incompatible mesh.

I am supposed to have a new computer here at work on monday, so hopefully it will be able to handle a fine enough mesh to satisify without messing with the adaptive methods.

Nate Sieger wrote:

One thing to watch out for though is that this option is only available for solid elements only. I'm assuming that if you're working with an assembly, you are simplifying your components into shell bodies to reduce your solve time.

Thank you Nate! I've been searching and searching for why I didn't have the option to run with adaptive meshing...

If a part is in bending, you want a miniumum of three mesh elements across the depth. If a part is in tension or compression alone then a single element span may work okay.

Generally I run a very coarse mesh to check the model is working properly (constraints, applied loads, displacements are in the magnitude expected etc). Then refinement is done in the areas of interest.

Usually there are three reasons I will run an FEA simulation.

1. To backup hand calculations.

2. To investigate the effects of geometry too complex for easy hand calculations.

3. To provide a pretty picture to show a client where problem areas lie.

Number 2 in this list is the one where I most often need a refined mesh.

Yes I concur and do what Dougal says. Get a Hand Calc done first to estimate and provide upper and lower bounds. Then just make a coarse mesh and get the model to run (this is often the biggest challenge). Once you get it running, look for gradients (in stress, displacement, strain energy, or whatever your criteria are). The object is (usually) to capture the gradients as accurately as you can (through convergence studies), while minimizing the number of elements needed in the overall model (so as not to strain computing resources). If looking at stress, you may see "singularities", or unreasonably high values at corners and contact points and contact edges. I often plot the Element Stress (using the high order elements), and determine if values are reasonable - then attempt to capture the gradients by localized refinement. As you approach convergence, the Element Stress should theoretically approach the Nodal Stress, but plots of nodal stress can look incorrect (i.e., sometimes you need to 'gloss over' unreasonable nodal stress values and discover a singularity is there - then just plot the Element Stress).

You can also do a stress error plot (right click on results > new stress plot> Stress Error:ERR) This shows the change across elements as the force flows through them, expressed as a percentage. If the change is high, I have seen meshes with over 1000% variance, you may consider refining that area. Typically it is only worth doing if there is a high stress in that particular area, It should not matter that much if the stresses are too low to be concerned with. I try to aim for less than %100 in most highly streses areas.

I will typically start with a very coarse mesh, and only refine in the areas that show both high stresses and too high a stress error plot. This tends to drop the total time spent running simulation drastically compared starting with a fine mesh, or just modifying overall mesh sizes.

Start with a lower resolution mesh, something has a reasonable distribution of elements. From there, depending on what you're looking for, you should be able to refine your mesh in the critical areas so you can converge on an accurate solution. In short, convergence determines the appropriate mesh size, so for large assemblies, focus on the critical areas and leave the rest as low resolution. This is best done by splitting geometry near the regions of analysis so you can refine that local region instead of selecting the entire component of the assembly to refine the mesh for. I hope that helps.