I am running a frequency analysis on Solidworks Simulation (Version 2013 SP5). The objective is to find the resonant frequencies on the assembly. The assembly model that I have is not a very large model and after simplifying the model I am down to approximately 25 parts. However the parts in question have pretty complex and small geometries. So much that I had to use 9 different types of mesh controls (Element size ranging from 0.1mm to 4mm) on a lot of surfaces. I did this since I am after more accurate results. (I have already run the test on the same model using a very average sized mesh. But the mesh looked horrible so I do not know how accurate the results were). To increase accuracy I also tried to use a finer curvature based mesh (Max Element size 20 and Min Element size 4). The resulting mesh was much better.

I ran the simulation on this mesh using an FFEPlus solver for around 50 frequencies but the problem that I was facing was that the simulation was completed to approximately 18.2% in around 3 minutes and was stuck at the same place for over 2 and a half hours. I assumed that the solver might be having convergence troubles and so aborted the simulation.

I tried running the simulation using the Direct Sparse solver. During the simulation I noted down the following

DOF: 30251808

Number of Nodes: 10161435

Number of Elements: 6647214

In the middle of the simulation (at approx 30%) the solver window changed and the numbers had changed to

DOF: 251808

Number of Nodes: 161,435

Number of Elements: 47,214

Is this normal? (Looking at it carefully 30251808 was reduced to 251808. The reduced DOF is just the last few digits of the original DOF. You can see the same pattern in nodes and elements). After trying to start the simulation in the new solver window I got the following error

"DSTAR has stopped working"

Then I tried consulting my reseller and read a few topics on the forums here. They all advised to simplify geometry further or reduce the number of elements or try different solvers. Not wanting to compromise too much on the accuracy I used a coarser curvature based mesh (Max Element Size 30 and Min Element Size 6) and reduced the mesh control on a few surfaces and ran the mesh. It still looked pretty decent and uniform. To reduce calculation times I also reduced the number of frequencies from 50 to 30.

I tried running the simulation using the Direct Sparse solver. Again I noted down the following

DOF: 26660055

Number of Nodes: 8964094

Number of Elements: 5855154

Again In the middle of the simulation (at approx 30%) the solver window changed and the numbers had changed to

DOF: 660056

Number of Nodes: 964094

Number of Elements: 55154

Again I got the following error

"DSTAR has stopped working"

Then without changing the mesh I tried running the simulation using the FFEPlus solver. The DOF, Nodes and Elements remained unchanged. At approximately 18.2% of the simulation being completed I got the following error.

"STAR has stopped working"

I am not really sure now how to deal with the problem. Is there a way to get around the problem without making changes to the geometry? Or without compromising on the accuracy?

However the parts in question have pretty complex and small geometries.

I can't say for certain without looking at the geometry associated with your system, but you probably don't need the small features.

...I had to use 9 different types of mesh controls (Element size ranging from 0.1mm to 4mm) on a lot of surfaces. I did this since I am after more accurate results.

Displacements and frequencies are the primary solution for a finite element model (strains and stresses are a secondary), so you can typically get good results with a somewhat coarse mesh. That being said, you don't know how well your simulation has converged unless you do a coverage study (looking at how the results vary with the mesh). I would start with a coarse mesh (and simplified geometry), solve the system, record your frequencies, refine the mesh a bit, solve, record you new results, and repeat until you have the desired level of accuracy.

I ran the simulation on this mesh using an FFEPlus solver for around 50 frequencies but the problem that I was facing was that the simulation was completed to approximately 18.2% in around 3 minutes and was stuck at the same place for over 2 and a half hours. I assumed that the solver might be having convergence troubles and so aborted the simulation. I tried running the simulation using the Direct Sparse solver. I tried running the simulation using the Direct Sparse solver. During the simulation I noted down the following

DOF: 30251808

Number of Nodes: 10161435

Number of Elements: 6647214

While it is true that different solvers are better depending on the size of the problem, I think the main issue is the fact that you have over 30 million DOF; that's huge....really huge. I don't know why SW would end up changing the number of DOF, so this is all speculation, but it might be a memory issue. How much memory does your system have?

Then I tried consulting my reseller and read a few topics on the forums here. They all advised to simplify geometry further or reduce the number of elements or try different solvers. Not wanting to compromise too much on the accuracy I used a coarser curvature based mesh (Max Element Size 30 and Min Element Size 6) and reduced the mesh control on a few surfaces and ran the mesh. It still looked pretty decent and uniform. To reduce calculation times I also reduced the number of frequencies from 50 to 30.

I tried running the simulation using the Direct Sparse solver. Again I noted down the following

DOF: 26660055

Number of Nodes: 8964094

Number of Elements: 5855154

26 million DOF is still a very big model (for example, I think NEi Nastran 64-bit can only do something like 25 million DOF)...we need to go smaller....

I am not really sure now how to deal with the problem. Is there a way to get around the problem without making changes to the geometry? Or without compromising on the accuracy?

You need to start with a coarser mesh and simpler geometry. Again, I can't say for certain without seeing your model, but these small features probably don't have a meaningful effect on your results. Start with a basic model (geometry and mesh) and work towards a more complicated one.

Can you post a picture of your assembly, as well as a picture of it with your current mesh?