[Far]

This can also be seen here Section 25.4.3

http://my.fit.edu/itresources/manual...8.htm#sec-pbcs

and section 25.9.1

http://my.fit.edu/itresources/manual...021.htm#177653

[ghorrocks]

fluent has also coupled pressure based AMG solver similar to CFX. This is different (3rd option as solver choice) than density based (implicit and explicit) and pressure based segregated option (SIMPLE, SIMPLEC and PISO)

You are correct.

[Far]

But why fluent is also so slow as compared to CFX and Fluent is also not as robut as CFX.

Any comments? I am not grasping that if same solver is available is both softwares then what is making determined effect in convergence. Fluent is way behind CFX in this aspect.

One more thing, instead of higher resolution advection scheme i have used the beta = 1 which means i have forced CFX to use the 2nd order scheme. There is difference in result between default option of higher resolution scheme and forced 2nd order scheme. Why?

Best Regards
Far

[ghorrocks]

Your question is now delving into the depths of CFX and Fluent and as they are both commercial software these details are not public.

All I can say is refer to the software documentation and you will see the different underlying approach of CFX being node centred with a FE-like approach and Fluent is cell centred with a Finite volume/SIMPLE approach.

The default high res scheme has flux limiters in it. If you used the hybrid scheme with blend factor =1 you are using second order differencing everywhere regardless.

[Far]

Your question is now delving into the depths of CFX and Fluent and as they are both commercial software these details are not public.

This means any body will never be able to identify what is happing inside black box? Do you think in this way we can do the meaningful research?

I have seen many papers in good journals where authors have used the one of commercial softwares and they got them published. It shows that they are accepted as what they (commercial CFD codes) are?

All I can say is refer to the software documentation and you will see the different underlying approach of CFX being node centred with a FE-like approach and Fluent is cell centred with a Finite volume/SIMPLE approach.

But at the end of discretization process we get the one matrix involving all unknowns at all nodes (in implicit approach). Once they are converted to algebraic equations (matrix) now it is responsibility of solver to solve it. The solver can be Guass siedel, ADI or any advance type.

Do you think with widely available literature with lots of options for solver for more than couple of decades, one solver can be very fast (CFX) and other too slow (Fluent). After all commercial products needs to be highly competitive. Otherwise they wont be able to survive.

Best Regards
Far

[ghorrocks]

Do you think in this way we can do the meaningful research?

CFX and Fluent is commercial software. They are there to make a profit. They cannot release their source code, or bits of thier approach which are commercial secrets or they will loose their competitve advantage. Welcome to the real world, it is profit before research.

Note your comparison for CFX and Fluent is for your case only. CFX is known to be good for steady state flows, especially with rotating components. Fluent is especially good at transient flows. Gross generalisations, but generally true.

[Far]

Note your comparison for CFX and Fluent is for your case only

To generalize the conclusion I have already obtained the low speed centrifugal compressor geometry by NASA and its LES data is also available with me. More over I am also building the geometry of rotor and stator of stage 35 by NASA. Also working on T 106 profile. These are the small portions of large separate projects at my university (co supervised by me)

. CFX is known to be good for steady state flows, especially with rotating components. Fluent is especially good at transient flows. Gross generalisations, but generally true.

Very true. It is also my experience that CFX is very much specialized in solving the rotating components and fluent is general type solver which gives you the solution by any means with unlimited time and never diverges.

Yesterday I simulated the case with two U bands connected by two diffusers and one converging nozzle (sort of wind tunnel). And further aid to complexity I have no clear picture of boundary conditions as such. CFX diverged in few iterations, on the other hand Fluent continued to solve and finally after two days it is on the path of converging with physics seems to be reasonable.

I would like to give one comment about CFX : It has limiters every where like in turbulence model (production limiter , shear stress limiter, curvature correction, blending functions limit the KW and KE model behavior), limiter in advection scheme and many more.

Thanks ghorrocks for discussion. It is very much interesting and informative. I have further questions to ask about plotting the turbulence quantities in CFD post and shall post in new thread.

Best Regards
Far

[ghorrocks]

I would like to give one comment about CFX : It has limiters every where

Again, a gross generalisation but I think you will find Fluent with its SIMPLE based approach has more limiters and under-relaxation than CFX does. That is why CFX can be harder to converge than CFX, but you have to be more careful with Fluent that you have not under-relaxed your simulation to death.

[Far]

I run the three cases with same mesh (good quality mesh) in fluent and CFX as follows


1. Fluent 2nd order advection scheme

2. CFX with high resolution scheme

3. CFX with 2nd order scheme

before writing details about the results I would like to mention that Fluent puts the limiter on the gradient (delta phi) and on the other hand CFX uses the gradient as average of integration points. But CFX has the limiter on the flux which fluent does not have. And it is interesting that both mention that they use the boundedness principle by barth and jesperson (forgive me if spelling of authors is wrong)

Now we come to results: I am getting qualitatively same results but having convergence difficulties with case 1 and 3 that is CFX and Fluent with 2nd order upwind scheme.

I am wondering why 2nd order scheme has difficulties and on the other hand CFX says it try to keep the beta as close to 1 as possible (which apparently says it tries hard to have 2nd order accuracy)

[ghorrocks]

There may only be small isolated regions where the second order scheme is a problem, and it is only there that the high res scheme is reducing beta.

Have a look at the residuals and beta values in the post processor and I bet high residuals correspond to low beta.

[Far]

Dear ghorrocks

I am unable to find the beta in cfd post.

[ghorrocks]

They are the variables velocity u.beta.

[Far]

They are the variables velocity u.beta.

Thanks ghorrocks for your help.

I want to make one correction to my last post regarding the advection scheme. Both fluent and CFX uses the the gradient limiter based on the principles by barth and jesperson but with different formulation. Correct me if I took it wrongly.

Today I had simulated the case with 2nd order scheme (bad quality mesh, in CFX. And to my surprise the pressure ratio is comparable to the coarse mesh results and efficiency is equivalent to fine mesh results. On the other hand with high resolution scheme I have consistent trends that is pressure ratio and efficiency is lower for coarse mesh and higher for fine mesh.

Any idea why results deteriorate with 2nd order scheme? More over is it true that the high resolution scheme is equivalent to 3/4 of 2nd order scheme?

PS: I had created the three meshes for bad quality mesh :- coarse, medium and fine and found that the medium and fine mesh gives the mesh independent results. For good quality mesh, five mesh level are created : coarse, medium, fine (both fine have 0.7 million nodes), very fine, ultra fine. again medium and fine mesh provides me the mesh independence.

[BalanceChen]

Hi Far, I am doing the similar job as code checking with rotor 37, but i am lack of the experimental data of the rotor performance, do you get one? If so, would you please send me a copy, my e-mail is: chenml03@gmail.com, thanks a lot.
Best regards,
BalanceChen

[Far]

I will be more than happy to share info/knowledge with any one including you. You will receive data in mail today

[BalanceChen]

You are so kind, Far, thank you again~

[Far]

After having large data created by me and my fellows and discussion at this forum, I would like to give the concluding remarks on this topic as per my understanding:

First I would like to say that both flow solvers tend to provide the similar results if the mesh is of good quality and has appropriate no.of nodes and yplus values.

Thereforethe first and the most important rule is to make, in any simulation of turbo machinery in particular and external flows in general, high quality mesh with all appropriate parameters e.g. yplus.

Now lets come to the difference

1. CFX has good turbulence models, although after merger with ANSYS all model seems to be incorporated in Fluent as well. Therefore this point does not make any difference any more.

2. Solution time : yes this is big factor where fluent is lagging behind CFX. In my estimate Fluent takes at least 3 days and CFX takes 12-18 hrs for same case (1 million nodes with 4 GB RAM).

3. Scaling : This means with increasing no. of nodes iteration time should not increase. CFX does provide this feature.
For example if you r running a case with 0.5 million mesh size and CFX is taking 12 hrs and fluent is taking 36 hrs. Now you double the mesh size from 0.5 million to 1.0 million. In this case CFX again takes 12 hrs but fluent may take 48 or more hrs. I am assuming you have enough computational resources.

4. Memory management. With CFX you can run 50% higher no of nodes on the same computer. In other words with fluent you can handle 1.0 million and CFX will go up to 1.5 million. Assuming 1.0 million nodes is the limit of your computer for fluent.


I would like to mention again: Fluent and CFX have very little difference in results, the most important thing is the mesh.Therefore instead of solver one should put more emphasis on acquiring the good skill on high end meshing sofwares (GRID PRO is my first choice and then comes ICEM CFD and GRIDGEN)

Any further comments regarding your experience with CFD in and these codes will be highly valuable and appreciated

Best Regards
Far

[ghorrocks]

Your comment that CFX has the same simulation time when you increase mesh size is unusual. CFX usually scales linearly with mesh size (as long as the model remains happy and converging similarly).

Did you use the coupled solver in Fluent? I would imagine the segregated solver in fluent will use far less memory, and much less than CFX. So the coupled solver in fluent uses more memory than the coupled solver in CFX, I did not know that but it makes sense.

Your other comments agree with my estimations of the strengths and weaknesses of the codes relative to each other.

[Far]

Your comment that CFX has the same simulation time when you increase mesh size is unusual. CFX usually scales linearly with mesh size (as long as the model remains happy and converging similarly).

Yes you are right. I usually put the solution on system in evening at 1700 hrs and when I come back at 9 am in morning I use to see the converged solution on CFX but ..... I see more no of iteration for coarse mesh and low number of iteration for fine mesh . Which does mean CFX scales linearly. But in both cases I have the converged solution in the morning therefore I had that perception.

Did you use the coupled solver in Fluent? I would imagine the segregated solver in fluent will use far less memory, and much less than CFX. So the coupled solver in fluent uses more memory than the coupled solver in CFX, I did not know that but it makes sense.

Yes segregated solver uses the less memory, according to our rough estimate half to that of the coupled solver of Fluent. It should be noted that CFX has no segregated solver.

When I started to learn CFD I did try the segregated solver, but based on our experience (me and my adviser) with both (segregated and coupled) solvers we tend to prefer the coupled solver due to its robustness with minimum interaction . Frankly speaking afterwards we did not use the segregated solver due to our that experience. Moreover since we working on the transonic compressors and turbines, we believe that the coupling between the pressure and velocity is strong, therefore segregated approach may introduce errors.

Best Regards
Far

[ghorrocks]

Well, the segregated solver does not introduce errors - it just has a looser coupling between the momentum and pressure/mass equation and therefore if the coupling is tricky it makes convergence more difficult. A properly converged segregated solver will be as accurate as a equivalently converged coupled solver.

Segregated solvers iterate much faster, so for cases where the tight coupling is not so important they are superior. For instance you will find segregated solvers often out-perform coupled solvers in transient simulations.