CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Divergence detected in AMG solver (http://www.cfd-online.com/Forums/fluent/107203-divergence-detected-amg-solver.html)

msatrustegui September 20, 2012 03:16

Divergence detected in AMG solver
 
1 Attachment(s)
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.

gfoam September 20, 2012 07:26

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

msatrustegui September 20, 2012 07:33

Quote:

Originally Posted by gfoam (Post 382743)
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.

gfoam September 20, 2012 08:14

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

yonchong September 20, 2012 10:47

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 October 2, 2012 04:11

1 Attachment(s)
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.

msatrustegui October 2, 2012 04:14

Quote:

Originally Posted by yonchong (Post 382795)
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.

yonchong October 2, 2012 09:16

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.

gfoam October 2, 2012 14:43

Quote:

Originally Posted by msatrustegui (Post 384464)
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 October 11, 2012 07:38

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.

gfoam October 11, 2012 11:26

Quote:

Originally Posted by msatrustegui (Post 386141)
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

msatrustegui October 11, 2012 11:32

Quote:

Originally Posted by gfoam (Post 386174)
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

gfoam October 11, 2012 11:36

I don't think so, one more thing: what is the turbulence level and the lenght scale you're using at the inlet?

msatrustegui October 11, 2012 11:37

Quote:

Originally Posted by gfoam (Post 386177)
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

gfoam October 11, 2012 11:52

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


All times are GMT -4. The time now is 12:45.