cyclone LES simulation prob: ERROR # 004100018
 

Dear all,
I am simulating a cyclone separator by LES. (Ansys cfx 14)
I could run the program for 5m/s inlet velocity but for 10m/s, it faied due to following error. (time step is 0.001s)

"ERROR 004100018 has occurred in subroutine FINMES. Message: Fatal overflow in linear solver. "

I know this is because my simulation is diverged.

Then I used a finer mesh, firstly it was 533,867 nodes and now 4,290,589. With 533,867 grids it failed after 3,549 time loops but now with 4,290,589 grids) fails within 2 loops.

Another fact is that I could run both 5m/s and 10m/s with attached geometry (Before.png) and all errors came with new geometry (After.png).

Can anybody help me?

I am working with this for 2 weeks, but cannot fix.

Thanks.
Sakura.

Have you tried using the solution from the 5 m/s case as an initial condition for the 10 m/s case? Check your grid quality (see CFX manual for recommended ranges for various parameters). Are you using auto timescale or physical timescale? Either way try reducing time step or timescale factor for better stability. Does it work using first order upwind for advection?

Need to some details - steady state or transient? Any multiphase stuff or other complexities? If transient what time stepping are you using?

Dear Chris,
Thanks for the reply.

I used same initial conditions both two cases except inlet velocity. For both simulations, initial conditions were taken from steady state simulation.

Mesh quality for 5m/s(533,867 nodes)

Histogram of Quality values
0.95 -> 1.0 : 380419 (21.234%)
0.9 -> 0.95 : 446649 (24.931%)
0.85 -> 0.9 : 115125 (6.426%)
0.8 -> 0.85 : 89766 (5.011%)
0.75 -> 0.8 : 76967 (4.296%)
0.7 -> 0.75 : 81695 (4.560%)
0.65 -> 0.7 : 74305 (4.148%)
0.6 -> 0.65 : 75083 (4.191%)
0.55 -> 0.6 : 80359 (4.485%)
0.5 -> 0.55 : 88292 (4.928%)
0.45 -> 0.5 : 98672 (5.508%)
0.4 -> 0.45 : 76947 (4.295%)
0.35 -> 0.4 : 60994 (3.405%)
0.3 -> 0.35 : 43099 (2.406%)
0.25 -> 0.3 : 1833 (0.102%)
0.2 -> 0.25 : 808 (0.045%)
0.15 -> 0.2 : 398 (0.022%)
0.1 -> 0.15 : 132 (0.007%)
0.05 -> 0.1 : 9 (0.001%)
0.0 -> 0.05 : 0 (0.000%)

Mesh quality for 10m/s(4,290,589 nodes)

Histogram of Quality values
0.95 -> 1.0 : 1289467 (14.098%)
0.9 -> 0.95 : 824662 (9.016%)
0.85 -> 0.9 : 421565 (4.609%)
0.8 -> 0.85 : 482698 (5.277%)
0.75 -> 0.8 : 526351 (5.755%)
0.7 -> 0.75 : 602196 (6.584%)
0.65 -> 0.7 : 641481 (7.013%)
0.6 -> 0.65 : 685583 (7.495%)
0.55 -> 0.6 : 729671 (7.977%)
0.5 -> 0.55 : 673423 (7.362%)
0.45 -> 0.5 : 642011 (7.019%)
0.4 -> 0.45 : 589060 (6.440%)
0.35 -> 0.4 : 521825 (5.705%)
0.3 -> 0.35 : 366581 (4.008%)
0.25 -> 0.3 : 49234 (0.538%)
0.2 -> 0.25 : 19569 (0.214%)
0.15 -> 0.2 : 10634 (0.116%)
0.1 -> 0.15 : 9591 (0.105%)
0.05 -> 0.1 : 8453 (0.092%)
0.0 -> 0.05 : 52699 (0.576%)

I think mesh quality is fine.

I am using automatic time steps and it is 0.001s. By this time steps also, it runs a longer time (total simulation time is 10s).

The advection scheme is central difference.

Dear Glenn,

Thanks for the reply.
It is a transient simulation and I used LES. Single phase flow only. The time step is 0.001s and simulation time is 10s.

****
Only this problem occurred after the geometric modification as shown in After.png. Geometry in Before.png worked properly for both cases with 533,867 nodes.

I'm not sure about the mesh quality. Overall it is fine but there are a number of really bad quality cells. I would try to smooth those out.

Dear Chris,
This mesh quality I have obtained by 50 smooth steps upto 0.3 for both cases. When I tried to give a smaller mesh size than this ICEM CFD stuck. Do you think I should increase the smoothing steps?
Thanks a lot for your kind assistance.

In ICEM I usually delete the volume elements and smooth the surface mesh very well first alternating Laplace smoothing on and off for about 10 iterations each until it stops improving. Then I regenerate the volume mesh and smooth it with something like you said above. It's not a bad idea to try more steps to see if it improves more. Another thing to consider is deleting unnecessary vertices in your model because ICEM always places a mesh node on vertices and won't move it during smoothing. This can cause difficulties in getting a good quality.

Also should note that the first volume mesh is generated using Robust to get a good surface mesh. The second time I use Quick (Delaunay) for the final volume mesh. Robust doesn't give a good volume mesh for CFD.

There are some good videos on YouTube by Simon Pereira describing best meshing practices for ICEM. www.youtube.com/user/ansysinc

Why did you choose that? Any reason or did you just guess?

Very often these errors are caused by too large a time step. I strongly recommend you change to adaptive time stepping, homing in on 3-5 coeff loops per iteration. Then the solver can find its own time step size.

Dear Glenn,

I selected this time step after trying from 0.5s to smaller time step. For larger time steps solver crashed due to,

Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG

Current Directory : /FLOW/NAMEMAP
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created.
+--------------------------------------------------------------------+
End of solution stage.

This could fix by using a smaller time step, 0.001s.

Thank you very much for your advice, I will work on that too, changing the time steps to adaptive.

Dear Chris,

Thanks a lot for advises. I am trying to improve the mesh quality now.

And the cool thing about adaptive time steppign is that when you improve the mesh quality, it will automatically increase the time step as convergence will be faster on a better mesh.

DES formulation will give the best results + easy to setup
>> right.. physical timestep "play" will give you flexibility AND >> do not forget to activate the imbalance charts AND >> do static first and use the results as input for transient.

Dear All,
Thank you very much for your great helps. Your advises and suggestions strongly help me to clear the way.

Dear Dmitry,
I would like to know how to activate imbalance charts?

To activate imbalance charts in solver manager, click button for "New Monitor" and check off the equations you want to show the imbalance for under the main title "IMBALANCE". In CFX-Pre you can also set up a conservation target under solver control which will cause the solver to continue iterating until a certain minimum imbalance level is achieved. Pretty cool so you don't have to watch it necessarily.