Multigrid cycles and numerical scheme

Nkl · January 9, 2014, 10:01

Hi everyone!

My supervisor is very cryptic...a solution of one of my models is not reaching convergence after more than 10k iterations. After telling me to keep on with patience for many days, today he told me to "play with computational parameters" such as type and number of numerical scheme and multigrid cycles. Where should I look? How should I change these parameters?
Thanks in advance

Lance · January 9, 2014, 10:20

The default multigrid settings should be fine, but the choice of numerical scheme can definitely affect convergence. You'll find them under solver control...
Besides numerical schemes there are many factors affecting convergence, including mesh quality, boundary conditions, time step size, etc...

Nkl · January 9, 2014, 10:29

I have created two models and the only difference is the inlet geometry. In the second one, the one where convergence is slow, the inlet is divided in 16 circular entrances (so mass flow rate has been divided by 16). For the rest the models are identical. Where lies the problem then?
I will try to change numerical scheme, thank you!

ghorrocks · January 12, 2014, 06:56

You are probably getting a complex flow feature occurring in the difficult to converge case. Maybe shock waves getting somewhere tricky, maybe a difficult separation.

What to do is discussed in the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

And Lance is correct in that you should not fiddle with the multigrid parameters. The problem will be more fundamental - eg mesh quality, time step size, physical setup, boundary conditions.

Nkl · January 12, 2014, 08:01

Is it maybe a mistake dividing the mass flow rate by 16 because I have 16 inlets instead of only 1? I was thinking that maybe the mass flow rate is referred to the whole sum of inlets. Thanks for the advices!

ghorrocks · January 12, 2014, 17:43

The mass flow is evenly distributed over the inlet, whatever its size, and no matter how many surfaces it is spread over.

Nkl · January 13, 2014, 08:39

Thank you very much, you are far more helpful than my supervisor!
Now I have run the simulation with a physical timescale of 5s (it was 0.25s) and the correct mass flow rate. I have reached convergence after only 160 iterations and the plots seem to be ok. The only problem now lays in the yplus values, which are in the order of magnitude of e+5. This sounds strange because the mesh settings are the same I used for the model with one inlet, for which I have good yplus values (less than 100). Thank you in advance again!

ghorrocks · January 13, 2014, 17:50

As a general note: The coupled solver in CFX generally converges very quickly. For most single phase flows, if you are not converged (or at least well on the way there) by 100 iterations then something is wrong. For multiphase simulations and other simulations with tricky coupling this could be ore like 1000 iterations.

But forget about running it for 10000 iterations like you used to have to do with SIMPLE based solvers. With SIMPLE solvers if you had convergence difficulties you fiddled with the solver parameters (under relaxation, linear solver etc) to get convergence.

With CFX you almost never adjust the under relaxation or solver parameters. If you have convergence difficulties you look at your mesh quality, time step size, initial condition and double precision numerics.

Nkl · January 14, 2014, 17:48

Now that convergence is good I have one last question. My two models are identical from all points of view (fluid domain, boundary conditions, solver controls), they only differ for the geometry of inlet. When I plot the results, they are very similar. How is it possible that for my second model (with 16inlets) the yplus values are around 3000, while in the other model they are below 100??
Thanks for all the help!

ghorrocks · January 14, 2014, 17:59

Where is the high value of y+? Post an image of what you are seeing.

Nkl · January 14, 2014, 18:07

They are even around 200 000. Here is the image!

ghorrocks · January 14, 2014, 18:16

y+ is a function of mesh size and flow velocity. So either the mesh size or the flow velocity has changed. You need to use the post processor to find out which.

Also your y+ plot looks very blotchy. This is a sure sign of inadequate mesh resolution. You have not done a mesh sensitivity study, have you? If that is the case your results are little better than random numbers at the moment.

Nkl · January 14, 2014, 18:24

I have assigned face sizings, each with element size of 0.01 m. The inflation option is total thickness with 15 layers, 1.7 growth rate and a maximum thickness of 0.004 m. With orthogonal quality I have an average of 0.85. I used these settings because with the other model I achieved values of yplus lower than 100.
I have tried to increase both element size and growth rate, but yplus did not change. Should I try mesh adaptation?

ghorrocks · January 14, 2014, 18:27

But did you look at the mesh you generated?

My comment on mesh sensitivity applies to the whole mesh, not just the inflation layers. For more details see the FAQ http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F and this is an excellent description of what to do http://journaltool.asme.org/Template...umAccuracy.pdf

Nkl · January 14, 2014, 18:46

What does it mean exactly "have take a look at your mesh?". From the beginning of my simulations I have changed advection scheme from high resolution to upwind, turbulence model from k-epsilon to SST, boundary condition type from outlet to opening in order to achieve convergence. I don't understand why with the other model I have good results with the same parameters. I will try to change other parameters. Thanks for all the help!

ghorrocks · January 14, 2014, 19:05

I mean use the post processor to look at the mesh and see its quality and size. Especially compare the two simulations which you report are giving different results despite similar setups.

Also be careful of using upwind differencing. You are going to struggle to get accurate answers with that.

January 9, 2014, 10:01	Multigrid cycles and numerical scheme	#1
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	Hi everyone! My supervisor is very cryptic...a solution of one of my models is not reaching convergence after more than 10k iterations. After telling me to keep on with patience for many days, today he told me to "play with computational parameters" such as type and number of numerical scheme and multigrid cycles. Where should I look? How should I change these parameters? Thanks in advance

January 9, 2014, 10:20		#2
Lance Senior Member Lance Join Date: Mar 2009 Posts: 669 Rep Power: 22	The default multigrid settings should be fine, but the choice of numerical scheme can definitely affect convergence. You'll find them under solver control... Besides numerical schemes there are many factors affecting convergence, including mesh quality, boundary conditions, time step size, etc...

January 9, 2014, 10:29		#3
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	I have created two models and the only difference is the inlet geometry. In the second one, the one where convergence is slow, the inlet is divided in 16 circular entrances (so mass flow rate has been divided by 16). For the rest the models are identical. Where lies the problem then? I will try to change numerical scheme, thank you!

January 12, 2014, 06:56		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	You are probably getting a complex flow feature occurring in the difficult to converge case. Maybe shock waves getting somewhere tricky, maybe a difficult separation. What to do is discussed in the FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria And Lance is correct in that you should not fiddle with the multigrid parameters. The problem will be more fundamental - eg mesh quality, time step size, physical setup, boundary conditions.

January 12, 2014, 08:01		#5
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	Is it maybe a mistake dividing the mass flow rate by 16 because I have 16 inlets instead of only 1? I was thinking that maybe the mass flow rate is referred to the whole sum of inlets. Thanks for the advices!

January 12, 2014, 17:43		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	The mass flow is evenly distributed over the inlet, whatever its size, and no matter how many surfaces it is spread over.

January 13, 2014, 08:39		#7
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	Thank you very much, you are far more helpful than my supervisor! Now I have run the simulation with a physical timescale of 5s (it was 0.25s) and the correct mass flow rate. I have reached convergence after only 160 iterations and the plots seem to be ok. The only problem now lays in the yplus values, which are in the order of magnitude of e+5. This sounds strange because the mesh settings are the same I used for the model with one inlet, for which I have good yplus values (less than 100). Thank you in advance again!

January 13, 2014, 17:50		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	As a general note: The coupled solver in CFX generally converges very quickly. For most single phase flows, if you are not converged (or at least well on the way there) by 100 iterations then something is wrong. For multiphase simulations and other simulations with tricky coupling this could be ore like 1000 iterations. But forget about running it for 10000 iterations like you used to have to do with SIMPLE based solvers. With SIMPLE solvers if you had convergence difficulties you fiddled with the solver parameters (under relaxation, linear solver etc) to get convergence. With CFX you almost never adjust the under relaxation or solver parameters. If you have convergence difficulties you look at your mesh quality, time step size, initial condition and double precision numerics.

January 14, 2014, 17:48		#9
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	Now that convergence is good I have one last question. My two models are identical from all points of view (fluid domain, boundary conditions, solver controls), they only differ for the geometry of inlet. When I plot the results, they are very similar. How is it possible that for my second model (with 16inlets) the yplus values are around 3000, while in the other model they are below 100?? Thanks for all the help!

January 14, 2014, 17:59		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	Where is the high value of y+? Post an image of what you are seeing.

January 14, 2014, 18:16		#12
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	y+ is a function of mesh size and flow velocity. So either the mesh size or the flow velocity has changed. You need to use the post processor to find out which. Also your y+ plot looks very blotchy. This is a sure sign of inadequate mesh resolution. You have not done a mesh sensitivity study, have you? If that is the case your results are little better than random numbers at the moment.

January 14, 2014, 18:24		#13
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	I have assigned face sizings, each with element size of 0.01 m. The inflation option is total thickness with 15 layers, 1.7 growth rate and a maximum thickness of 0.004 m. With orthogonal quality I have an average of 0.85. I used these settings because with the other model I achieved values of yplus lower than 100. I have tried to increase both element size and growth rate, but yplus did not change. Should I try mesh adaptation?

January 14, 2014, 18:27		#14
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	But did you look at the mesh you generated? My comment on mesh sensitivity applies to the whole mesh, not just the inflation layers. For more details see the FAQ http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F and this is an excellent description of what to do http://journaltool.asme.org/Template...umAccuracy.pdf

January 14, 2014, 18:46		#15
Nkl Member Nikola Join Date: Sep 2013 Location: Madrid, Spain Posts: 60 Rep Power: 13	What does it mean exactly "have take a look at your mesh?". From the beginning of my simulations I have changed advection scheme from high resolution to upwind, turbulence model from k-epsilon to SST, boundary condition type from outlet to opening in order to achieve convergence. I don't understand why with the other model I have good results with the same parameters. I will try to change other parameters. Thanks for all the help!

January 14, 2014, 19:05		#16
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	I mean use the post processor to look at the mesh and see its quality and size. Especially compare the two simulations which you report are giving different results despite similar setups. Also be careful of using upwind differencing. You are going to struggle to get accurate answers with that.