CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Divergence detected in AMG solver

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes
  • 1 Post By gfoam
  • 1 Post By yonchong
  • 1 Post By yonchong
  • 1 Post By gfoam

Reply
 
LinkBack Thread Tools Display Modes
Old   September 20, 2012, 03:16
Default Divergence detected in AMG solver
  #1
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
Hi everyone,

I'm trying to simulate a rotating machine and i'm having some dificulties to get the convergence in the solution.

I simulate the rotation using Multiple Reference Frame (MRF). The rotor has an angular velocity of 4000 rpm, and the stator is stationary.

The mesh hasnīt shown any problems when i do the mesh check.

The boundaries are defined as pressure-inlet and pressure-outlet, and the walls are the following:
-Wall-stator: The walls of the stator are defined as stationary
-Wall-rotor-static: Walls of the rotor that don`t rotate, defined as moving walls, absolute, with 0 velocity.
-Wall-rotor-dinamic: Rotating walls of the rotor, defined as moving walls, relative to adjacent cell zone, with 0 velocity.

When I do the simulation i got the following message:
Error: Divergence detected in AMG solver: epsilon
Error Object: #f

I've uploaded an screenshot of the final result (as you can see, the divergence of the continuity starts growing in the 30th iteration more or less).

Could anybody help me?

Thanks.
Attached Images
File Type: jpg Divergence.jpg (34.8 KB, 157 views)

Last edited by msatrustegui; September 20, 2012 at 06:15.
msatrustegui is offline   Reply With Quote

Old   September 20, 2012, 07:26
Default
  #2
Senior Member
 
Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 107
Rep Power: 7
gfoam is on a distinguished road
Hi:
First of all: which solver are you using? Segregated or Coupled? Which numerical schemes? First Order or higher order? What kind of initialization did you do? If you are usin second order or higher order schemes of discretization try to use first order schemes and then switch to higher order schemes. Second, if you are using standard or hybrid initialization try to use FMG initialization. Hope this helps you. Regards.
Gonzalo
gfoam is offline   Reply With Quote

Old   September 20, 2012, 07:33
Default
  #3
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
Quote:
Originally Posted by gfoam View Post
Hi:
First of all: which solver are you using? Segregated or Coupled? Which numerical schemes? First Order or higher order? What kind of initialization did you do? If you are usin second order or higher order schemes of discretization try to use first order schemes and then switch to higher order schemes. Second, if you are using standard or hybrid initialization try to use FMG initialization. Hope this helps you. Regards.
Gonzalo
Thanks for your answer.

I'm using SIMPLE method and LEAST SQUARE CELL BASED, with all the parameters in First order.

If tried with hybrid initialization and FMG initialization, but both of them got me to a similar result (the one that it's shown in the figure).

I'm a bit desperate because i started this simulation some weeks ago and it`s been imposible to get a result.

Thanks for the support.
msatrustegui is offline   Reply With Quote

Old   September 20, 2012, 08:14
Default
  #4
Senior Member
 
Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 107
Rep Power: 7
gfoam is on a distinguished road
OK, try to use a Coupled solver with the pseudo-transient algorithm and play with the timescale (rise it) if you have problems with convergence. Be carefull with it because it requieres more memory than the segregated solver. Reorder the domain to improve the memory usage. Regards
Gonzalo
msatrustegui likes this.
gfoam is offline   Reply With Quote

Old   September 20, 2012, 10:47
Default
  #5
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
Your continuity residual is going up when it is diverging which means you will have high velocity spikes in your calculation. Stop the calculation before it dies and figure out where that is occuring. You might be able to see whether it is a boundary condition problem or mesh problem or, if it occurs middle of the domain and mesh is fine, selection of solver problem.

Also you have high number of cells hitting the viscosity limiter. Check the material property you are using. Try using (incompressible) ideal gas if you are using a constant density. If the density is very much off the solution might diverge.
msatrustegui likes this.

Last edited by yonchong; September 20, 2012 at 15:23.
yonchong is offline   Reply With Quote

Old   October 2, 2012, 04:11
Default
  #6
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
I've done some changes as you recomended me. And I`ve obtained better solution, but i don't reach the convergence criteriums i've set (10-3 in all the parameters).

My final solution is shown in the picture i'm attaching. (I am now trying to solve it with Coupled method, i hope this could get me to the solution).

Thanks for the previous answers, they helped me a lot.
Attached Images
File Type: jpg convergencia_4000.jpg (48.5 KB, 132 views)
msatrustegui is offline   Reply With Quote

Old   October 2, 2012, 04:14
Default
  #7
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
Quote:
Originally Posted by yonchong View Post
Your continuity residual is going up when it is diverging which means you will have high velocity spikes in your calculation. Stop the calculation before it dies and figure out where that is occuring. You might be able to see whether it is a boundary condition problem or mesh problem or, if it occurs middle of the domain and mesh is fine, selection of solver problem.

Also you have high number of cells hitting the viscosity limiter. Check the material property you are using. Try using (incompressible) ideal gas if you are using a constant density. If the density is very much off the solution might diverge.
There was a mesh problem in an interface between two bodies, the skeweness has improved a lot. So now, if there's a problem, it must be for another reason.
msatrustegui is offline   Reply With Quote

Old   October 2, 2012, 09:16
Default
  #8
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
I see that you are using fluent 3d solver rather than 3ddp (3-d double precision). Try that. Which means when you launch the Fluent you have to select 3ddp rather than 3d.

Also once the solution has converged with the first-order discretization, rerun with the second-order discretization.

By the way, you are using standard K-epsilon turbulence model but unless you have a particular reason the Realizable k-epsilon should be a better option for you.
msatrustegui likes this.
yonchong is offline   Reply With Quote

Old   October 2, 2012, 14:43
Default
  #9
Senior Member
 
Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 107
Rep Power: 7
gfoam is on a distinguished road
Quote:
Originally Posted by msatrustegui View Post
I've done some changes as you recomended me. And I`ve obtained better solution, but i don't reach the convergence criteriums i've set (10-3 in all the parameters).

My final solution is shown in the picture i'm attaching. (I am now trying to solve it with Coupled method, i hope this could get me to the solution).

Thanks for the previous answers, they helped me a lot.
Hi, did you try raising the timescale factor? Because doing that you can filter some structures in the fluid flow that aren't inestationary. Another thing you ca try is using lower URF's. Regarding the turbulence model, I always have convergence problems with RNG k-e o Std k-e, may be your values at the ilet and outlet are too low and this may cause that your simulation does't converge to a better level. I hope this helps you.
Gonzalo
msatrustegui likes this.
gfoam is offline   Reply With Quote

Old   October 11, 2012, 07:38
Default
  #10
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
Hi,

I've tried with double precision, but it still do not converge. I also tried with Standard k-epsilon and realizable, but both of them get me to a similar solution.

The thing is that my model is a machine rotating at 4000 rpm. To see the convergence, i change the rotating velocity to 100 rpm and it converged. But when i raise the velocity (even to 200 rpm) it doesn't converge. It stays near the convergence with 200 rpm.

With 4000 rpm i got 100 m/s in some cells, should it be a problem of air compresibility?

Does anyone have an idea?

Thanks for the support.

PD: Sorry for my english.
msatrustegui is offline   Reply With Quote

Old   October 11, 2012, 11:26
Default
  #11
Senior Member
 
Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 107
Rep Power: 7
gfoam is on a distinguished road
Quote:
Originally Posted by msatrustegui View Post
Hi,

I've tried with double precision, but it still do not converge. I also tried with Standard k-epsilon and realizable, but both of them get me to a similar solution.

The thing is that my model is a machine rotating at 4000 rpm. To see the convergence, i change the rotating velocity to 100 rpm and it converged. But when i raise the velocity (even to 200 rpm) it doesn't converge. It stays near the convergence with 200 rpm.

With 4000 rpm i got 100 m/s in some cells, should it be a problem of air compresibility?

Does anyone have an idea?

Thanks for the support.

PD: Sorry for my english.
Hi:
mmmmm, 4000rpm is a lot for me. What's the external radius of your compressor? With it you can calculate the velocity at the tip of the blades and vectorially adding the inlet velocity you can calculate the total velocity at these points and whit the local properties of the air calculate the mach number and decide either if the flow is compressible or not. with regard with your convergence problem, what is the minimal Orthogonal Quality of your mesh? There exis big diferences betwen adyacent cell sizes? If you're using BL meshes, firs try to get a converged solution with a mesh without it or a coarse mesh, then interpolate the data to the finner mesh. Regards
Gonzalo
gfoam is offline   Reply With Quote

Old   October 11, 2012, 11:32
Default
  #12
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
Quote:
Originally Posted by gfoam View Post
Hi:
mmmmm, 4000rpm is a lot for me. What's the external radius of your compressor? With it you can calculate the velocity at the tip of the blades and vectorially adding the inlet velocity you can calculate the total velocity at these points and whit the local properties of the air calculate the mach number and decide either if the flow is compressible or not. with regard with your convergence problem, what is the minimal Orthogonal Quality of your mesh? There exis big diferences betwen adyacent cell sizes? If you're using BL meshes, firs try to get a converged solution with a mesh without it or a coarse mesh, then interpolate the data to the finner mesh. Regards
Gonzalo
I've done some calculations and the air should be near 0.3 match number in some places of the machine...

The max skeweness is 0.94 (in a few cells), with a skeweness average of 0.24 more or less. I think the mesh is not the problem, but i will check it again to be sure.

Should i put the air in a compresible state?

Thanks for your answer
msatrustegui is offline   Reply With Quote

Old   October 11, 2012, 11:36
Default
  #13
Senior Member
 
Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 107
Rep Power: 7
gfoam is on a distinguished road
I don't think so, one more thing: what is the turbulence level and the lenght scale you're using at the inlet?
gfoam is offline   Reply With Quote

Old   October 11, 2012, 11:37
Default
  #14
Member
 
Marco
Join Date: Aug 2012
Location: Spain
Posts: 41
Rep Power: 4
msatrustegui is on a distinguished road
Quote:
Originally Posted by gfoam View Post
I don't think so, one more thing: what is the turbulence level and the lenght scale you're using at the inlet?
Intensity: 5%
And length scale: 0.01 m
msatrustegui is offline   Reply With Quote

Old   October 11, 2012, 11:52
Default
  #15
Senior Member
 
Gonzalo
Join Date: Mar 2011
Location: Argentina
Posts: 107
Rep Power: 7
gfoam is on a distinguished road
One thing you can do is run the case until it diverges, then stops it and make contours of velocity and p and look for zones where exits singularities. Then you can try to refine the mesh on that zones or improve the quality. I don't know, it's a little difficult to see what is happening without more specifications. Sorry I can't help you.
Gonzalo
gfoam is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Quarter Burner mesh with periosic condition SamCanuck FLUENT 2 August 31, 2011 11:34
ERROR: divergence detected in AMG solver black mamba Main CFD Forum 0 April 19, 2010 15:15
divergence detected in AMG solver !!! yansheng FLUENT 0 September 27, 2007 11:22
DIVERGENCE detected in AMG solver ENTHALPY MANOJKUMAR FLUENT 2 December 25, 2005 10:54
divergence detected in AMG solver: Shekhar Jain FLUENT 1 September 18, 2003 09:31


All times are GMT -4. The time now is 13:03.