Diagnosing linear solving failure

siw · November 13, 2013, 06:58

Hi,

I'm running an incompressible, external aerodynamics testcase in CFX:

Steady RANS with SST.
Air at 25 deg C material.
Isothermal for energy equation.
Velocity inlet, pressure outlet, no-slip walls for the base and body of interest and symmetry everywhere else.
High Resolution scheme (Upwind for turbulence numerics).
Physical timescale is dynamical time past the object of interest.
Double precision.

using three different ICEM Hexa meshes (same blocking topology but coarse, medium and fine mesh resolutions). The simulation with the coarse mesh ran to completion and the residuals and monitor points were OK. I'm running the exact same CFX-Pre set-up for the fine mesh and the CFX-Solver reports on the first iteration that U-Mom, V-Mom and W-Mom have failed in the linear solution by writing an F (rather than ok or OK) in the solver output text file, then CFX-Solver goes no further in the solution.

I have no idea why this has happened when the only change is the mesh resolution (the topology and quality are the same across all the meshes). There are no other error messages to help resolve this. Any recommendations on how to fix this?

Thanks

ghorrocks · November 13, 2013, 16:22

There is an FAQ on this general question:
http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

It is common for convergence to get harder as the mesh gets finer. This is because finer meshes have less numerical dissipation and therefore the flow is less damped and harder to converge. So it is common that as you refine the mesh you have to take additional measures to get convergence.

siw · November 14, 2013, 02:11

Thanks Glenn, I did read that link.

I've never had CFX fail on the first iteration before, when I've had it fail on other jobs its been due to divergence as the solution progressed.

Not sure what measures I can take in the set-up to get this working. Any suggestions?

ghorrocks · November 14, 2013, 04:17

If it fails on the first iteration then your simulation is unstable right from the start. So smaller time steps and a better initial condition are the factors I would be looking into to get it working.

siw · November 14, 2013, 06:39

I initialize the flowfield with the freestream conditions and use a physical timescale (it's a steady simulation) in based on the dynamical flow time past the body of interest. I'll reduce the timescale, not much more I can think of.

ghorrocks · November 14, 2013, 16:43

Yes, reduce the time scale. Also, using a simulation at a similar setting which did converge as an initial condition can help. Another idea is to use local time scale factor for the initial convergence.

siw · November 15, 2013, 08:55

Thanks Glenn. Drastically reducing the physical timescale has done the trick. I've always in the past been successful with a timescale of about 1/2 to 1/4 of the dynamical flow through time, as per the majority of CFX tutorials. In this case I set the timescale based on an a CFL number of about 1 on the mesh cells in the wake of the body of interest, as the above was not fine enough.

November 13, 2013, 06:58	Diagnosing linear solving failure	#1
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	Hi, I'm running an incompressible, external aerodynamics testcase in CFX: Steady RANS with SST. Air at 25 deg C material. Isothermal for energy equation. Velocity inlet, pressure outlet, no-slip walls for the base and body of interest and symmetry everywhere else. High Resolution scheme (Upwind for turbulence numerics). Physical timescale is dynamical time past the object of interest. Double precision. using three different ICEM Hexa meshes (same blocking topology but coarse, medium and fine mesh resolutions). The simulation with the coarse mesh ran to completion and the residuals and monitor points were OK. I'm running the exact same CFX-Pre set-up for the fine mesh and the CFX-Solver reports on the first iteration that U-Mom, V-Mom and W-Mom have failed in the linear solution by writing an F (rather than ok or OK) in the solver output text file, then CFX-Solver goes no further in the solution. I have no idea why this has happened when the only change is the mesh resolution (the topology and quality are the same across all the meshes). There are no other error messages to help resolve this. Any recommendations on how to fix this? Thanks

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Moving mesh	Niklas Wikstrom (Wikstrom)	OpenFOAM Running, Solving & CFD	122	June 15, 2014 06:20
Unstabil Simulation with chtMultiRegionFoam	mbay101	OpenFOAM Running, Solving & CFD	13	December 28, 2013 13:12
calculation stops after few time steps	sivakumar	OpenFOAM Running, Solving & CFD	7	March 17, 2013 06:37
Orifice Plate with a fully developed flow - Problems with convergence	jonmec	OpenFOAM Running, Solving & CFD	3	July 28, 2011 05:24
Could anybody help me see this error and give help	liugx212	OpenFOAM Running, Solving & CFD	3	January 4, 2006 18:07

November 13, 2013, 16:22		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	There is an FAQ on this general question: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F It is common for convergence to get harder as the mesh gets finer. This is because finer meshes have less numerical dissipation and therefore the flow is less damped and harder to converge. So it is common that as you refine the mesh you have to take additional measures to get convergence.

November 14, 2013, 02:11		#3
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	Thanks Glenn, I did read that link. I've never had CFX fail on the first iteration before, when I've had it fail on other jobs its been due to divergence as the solution progressed. Not sure what measures I can take in the set-up to get this working. Any suggestions?

November 14, 2013, 04:17		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	If it fails on the first iteration then your simulation is unstable right from the start. So smaller time steps and a better initial condition are the factors I would be looking into to get it working.

November 14, 2013, 06:39		#5
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	I initialize the flowfield with the freestream conditions and use a physical timescale (it's a steady simulation) in based on the dynamical flow time past the body of interest. I'll reduce the timescale, not much more I can think of.

November 14, 2013, 16:43		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	Yes, reduce the time scale. Also, using a simulation at a similar setting which did converge as an initial condition can help. Another idea is to use local time scale factor for the initial convergence.

November 15, 2013, 08:55		#7
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	Thanks Glenn. Drastically reducing the physical timescale has done the trick. I've always in the past been successful with a timescale of about 1/2 to 1/4 of the dynamical flow through time, as per the majority of CFX tutorials. In this case I set the timescale based on an a CFL number of about 1 on the mesh cells in the wake of the body of interest, as the above was not fine enough.