[kastarkas]

Hello Friends,

Back after a long time.

I have a centrifugal pump geometry for which i have done 3 levels of mesh sensitivity(1.8M,2.5 M and 4.6 Million Mesh). ALL these were successful in solving.

I use MRF Frozen Rotor and k-o SST as my turbulence model with medium turblence intensity and a conservation target for imbalances as 1%. All the solver numerics are of 2nd order (High Resolution). Following exactly the same things for the previous setups. All the Boundary conditions(Mass flow inlet and opening pressure at exit), and setting up remain the same.

Expecting a mesh independent solution in the next level, i refined the mesh to 6.2 M unstructured tetrahedral Mesh with all the quality requirements met as usual in ICEM.

First, I met with floating point error at 103rd iteration.I searched the whole thing and narrowed my focus on timescale. (since Physics was right and mesh is ok, running in parallel and double precision too)

I reduced it to 1/3 rd and even below ..i met with total divergence at say 20 to 40 iteratoins again.

I FIND DIVERGENCE WITH MY TURBULENCE PARAMETERS ALONE and THE P-MASS PARAMETERS ARE SEEN TO BE RAPIDLY CONVERGING AS WELL.

I have attached the images of the residual plots and ccl here with.

Attachment 51763

6.2 mesh p mass.JPG

k e divergence.JPG

k o divergence.JPG

p mass convergence in k e model.JPG

I know this have been discussed N no of times, but everyone found a way out in the issues where i had no problem at all.

Any sort of help is appreciated to sort this out.

Regards.

[ghorrocks]

It is common for convergence to be harder to achieve as you refine the mesh. Finer meshes have less numerical dissipation, so the flow is less damped - and this allows little flow instabilities (such as vortex shedding off bluff bodies) to start moving about and causing problems for steady state simulations.

The general FAQ on this issue is here: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

But in your case it is highly likely that small flow instabilities are causing problems for a steady state simulation. To overcome this you increase physical time step size, but you have said that you have already had to decrease time step size to achieve convergence. You can probably overcome this impasse by improving mesh quality - and improvements in mesh quality you can achieve will help in this situation.

If that does not work then your only option is to run it transient and march it out to steady state. This will increase simulation time dramatically, but is likely to be successful. And if you are doing this just to check grid convergence then you only have to do it once so hopefully that is manageable.

[kastarkas]

True that Glenn. Thank you so much.

I thought so ....but as you said, the problem is i dont have a steady solution to beef up the transient solutions.....even in parallel it takes time..I can do upto 4 processors...

I l look once upon slowly to improve the mesh quality and aspect ratios...(its above 0.2 and 0.3, i l try to get more..)

Parallely I l update about the convergence in transient setup.

Thank you again.

[kastarkas]

Hello Glenn,

I improved the mesh quality once again and mesh size to some 7.4 Million and it ran smoothly for only a closer convergence of 1.5E-4 to 1.3E-4.

(In between i tried a transient one with an initialisation override, but still got diverged and then only i confirmed to move to the meshing part)

Anyway Thankyou glenn for that.

My next Doubt is :

REF : http://www.cfd-online.com/Forums/cfx...searching.html

I have an expression/function which is to be volume integrated in CFD post;
The expression consists of scalar shear stress (dyn visc. * shear strain rate)and these terms has some exponents in the expression as in the REF;

The results which i need for my further calculations are the ones which i get after volume integrating the above said expression.

Now i find an increase in its values (volume integrals of my expression) along with increase in elements of my mesh;

I started from a 1.8 Million Mesh to now I am at almost 7.4 Million; (all the other functions like pressure, velocity, have reached an independent solution way back;

How will expressions like these be mesh independent ? Am i expected to move further with more elements ?

Thank you all and Any help is really insightful .

[bparrelli]

When you refine the mesh more and more close to the walls, you will sometimes get flow reversals within the boundary layer due to round-off errors in the turbulence models. I have seen this in CFX turbomachinery problems many times, and it is mainly due to the aspect ratios of the prism elements near the walls becoming too large (squished rectangles). If you want to achieve a grid independent solution this way, you have to refine the mesh equally in all directions. Do you have access to Turbogrid? If so, I would recommend it trying it for this problem, because it is very easy to refine the mesh evenly in all directions, if grid-independence is what you are after. Best of luck!

[ghorrocks]

kastarkas: I do not understand your second question, but if you have not achieved mesh insensitive results by 7.3M nodes then you might have to go finer. Brian's point is important - you don't want to refine the mesh but reduce mesh quality. When I do mesh sensitivity studies I generally halve the mesh element length in all directions. This keeps the aspect ratio of the elements about the same. It also means that each refinement step increases the number of nodes by a factor of 5-10, so the models get very big very quickly.

[kastarkas]

Wow for the replies.
Thanks a lot Brian

Brian, I do not have access to T grid and i l see to it about the possibility of access. I got your point. yeah seems, that may also be the case. I l think about that and update. I already reached 7.3M. Let me try more.

Thanks a lot. I will update.

[kastarkas]

Thank you for the help Glenn . Yeah, i too can do that,and probably my next step would be to almost halve the element size or even a bit less that. I l try that.

But Glenn,

I just have an expression : D= A*((Scalar Shear)^B));
[Scalar shear = Dyn Viscosity*SHear Strain Rate]

I do need to have say X=vol int (D); THis is an index ;
(seperately for both my rotating and stationary domains)

I was asking that, as i moved from 1M mesh to 7.4M mesh , X is also increasing ;
BUt thats fine, and let it increase; But I am doing all of this only to reach a final constant value of this particular index which i expect to remain same at larger no of mesh also;
As this involves volume integral, obviously more no of elements will give more accuracy. But i find a rise like say 20 to 30 % in very mesh steps of mine (ie. @2.4M mesh, then 4.6M Mesh it was.. etc)
As my next steps in increasing the mesh size is a bit larger (ie, say 10M or something) , i needed to clarify this before i start doing .

[ghorrocks]

As a general rule, derivatives increase noise, integrals decrease noise. Your function D uses the shear strain rate which is a derivative twice over (once in space, once in time). Fortunately you ease the situation a little by then integrating it over the domain. It is a crude and simplistic way to look at it, but that is two derivative steps and one integration so you have a net of one derivative step. This means your function will amplify noise.

So you can expect that this function is going to be noisy and sensitive to error. This means it will be hard to get grid independant answers for it and the normal flow variables like velocity and pressure will have converged long before your function does.

[kastarkas]

Yes true that only glenn, we have a net effect of one derivative to amplify those errors.

So whats next, I actually dont know;
A diplomatic desicion is required here i guess. I cannot edit or bring a change in the model though. I l see to it apart anyway.

I think, then i have to stop somewhere !

Truly Clueless !

Thanks a lot again Glenn. I l update back right here.