[Far]

Dear Frends

I have simulated the NASA rotor 37 at design speed.

The turbulence model used in Spalart Allmaras (both in Fluent and CFX, beta in CFX R 12.0)

I have created two meshes
1) high quality mesh
2) bad quality mesh (only from cfx point of view as the minimum orthogonality angle is less than 20, on the other hand it satisfied all requirements of Fluent solver e.g. max skewness, cell squish index)

In short I am using two solvers (CFX and Fluent) and two meshes (one bad from CFX point of view only)

I have made the mesh Independence study for both meshes and found that the 0.7 million size produces the grid independent solution.

Now from results (see the attached Figure.) I have found interesting facts.

Results from both meshes on the Fluent almost overlap each other while the good mesh produces higher performance and bad mesh predicted the lowest performance for CFX.

Fluent results seem logical as they should be after grid Independence for both meshes, but I am confused with CFX results.

Any suggestion, advise or comment shall be highly appreciated and shall shed light on philosophy of these two widely used solvers

CFX mesh = good quality
Fluent mesh = bad quality

[ghorrocks]

but I am confused with CFX results.

I am sorry, I do not know what question you are asking. What are you confused about?

[Far]

I am confused why there is large difference in CFX simulations for both meshes, on the contrary fluent is producing same results on both meshes

[ghorrocks]

It would be risky to leap to conclusions based on a small data set like this. It may be that CFX is more sensitive to mesh quality than Fluent, but to be sure you would need to do a far more detailed check than this.

[Far]

I have also made the y plus study on this mesh (good quality mesh). My yplus is from 1 to 60. Here I have consistent results.

PS. results shown in first attachment was based on yplus 60 mesh

[Far]

what type of checks can be done to ensure that the conclusion are logical?

[ghorrocks]

It appears you are approaching mesh insensitivity, so that is good.

It depends on what conclusion you want to draw, how important it is and who you are going to tell. If it does not matter then use the results you have. If you are using this information to make expensive decisions I would contiune to explore. You have to decide how much time, effort and cost you want to spend on this issue versus the risk you are willing to take in your conclusion being wrong.

[Far]

At the moment I am running simulations on the yplus 1 mesh in the fluent to be on safe side.

Do you think it is due to fact that the fluent uses the logrithm profile for plus greater than 11.06 and linear profile for yplus less than 11.06. On the other hand CFX uses the automatic treatment.

I have still 6-9 moths and I have at-least 14-15 different plots for different models, boundary conditions and mesh densities in hand.

What can and should be done in this time limit? What is more important is the quality of results and I am willing to spend more time if required.

[ghorrocks]

I think Spalart Allmaras is still in beta for V13. This means getting details about exactly what it is doing is difficult. You will probably have to contact support for details of the approach in CFX.

[Far]

yes you are right

[Far]

i asked the CFX support but no reply. Can you suggest any further cases to run

[ghorrocks]

It is not clear to me exactly what you are trying to do. Are you trying to get as accurate an answer for your simulation as possible, or are you comparing CFX vs Fluent?

[Far]

I am trying to compare the fluent and CFX in detail so that I shall be sure in future for other turbo machinery cases. Therefore based on my data base I shall be able to clearly figure out if I am going in right or wrong direction without conducting detail study each time. You can say it best practice guide lines for company's internal use.

I am also comparing the time fluent and cfx takes on the same case with same mesh and same solver setting. e.g. I am using the coupled implicit with algebraic multi grid for fluent simulations. On the other hand CFX is also using the coupled implicit multi grid solver. It takes around 3-4 days for fluent simulation and around 12-18 hours for CFX simulation. Why this so if both solvers are same? Is this due to fact that the CFX uses vertex based control volume? I am not clear again.

This is also important that our previous cases (large data base including Fan, high pressure turbine and compressor, low pressure compressor and turbine) were run in Fluent with SA model and grid topology used corresponds to bad quality mesh as discussed earlier.

Based on my current study we shall be able to identify the source of errors from user point of view as well as the softwares and turbulence models limitations.

We are also gonna publish this study (including other test cases like: centrifugal compressor, Nozzle guide van and nasa rotor 67 and also includes the casing treatment) as well so that other can benefit form this research.

So any input will give us the direction and shall be highly valuable to everybody.

Best Regards
Far

[Far]

Originally Posted by ghorrocks

It is not clear to me exactly what you are trying to do. Are you trying to get as accurate an answer for your simulation as possible, or are you comparing CFX vs Fluent?

So I am trying to get the as accurate as possible answer for my simulations and comparing the CFX and Fluent for their strengths and weaknesses for future use.

[ghorrocks]

While CFX and Fluent have many common features, the underlying approach is very different. CFX is nodal based and has finite element like approach, whereas Fluent is based on the SIMPLE method which has been enhanced to be fully implicit.

My recommendations would be to optimise each code separately, as the different codes probably need different meshes to be mesh-independant, likewise time steps, convergence etc. Once you have got either code accurate enough for your purposes you can then compare CPU time, memory useage etc in a meaningful fashion.

[Far]

Dear

I am currently following the same path as you have just mentioned. That is to optimize each code separably.

As far as SIMPLE approach is concerned, I think CFX is also pressure based coupled solver and same option is also available in Fluent.

Do you think using the finite element like approach for CFX is the key success element? or it is the something else.

Best Regards
Far

[ghorrocks]

As far as SIMPLE approach is concerned, I think CFX is also pressure based coupled solver and same option is also available in Fluent.

Incorrect. CFX was written as a coupled solver from the beginning and you cannot run CFX in SIMPLE mode. In fact in CFX you do not have any options for pressure-momentum coupling except the coupled solver. Fluent was originally written using SIMPLE, but they have recently exhanced it to use a coupled solver.

[Far]

I have created three meshes for fluent and five meshes for CFX ranging from 0.2 million to 1.25 million. On both codes I have achieved mesh independence. After getting mesh Independence, I am comparing their results.

Even i did't stop there and carried out further mesh studies by varying the y plus, boundary conditions effect (average static pressure and static pressure), different near wall treatments (e.g. for K epsilon i tried the scalable and standard wall function and found no difference in results, although noticed some different convergence patterns).

I am in process to create another topology to run on fluent and CFX with number of nodes equal or greater than 0.7 million with controlled and optimized y plus and boundary conditions as learned from above mentioned results. (which gives mesh independent solution).

[Far]

But fluent has also option for pressure based couple solver with Algebraic multi grid. This is different than the SIMPLE method which used the segregated approach.

Can you please elaborate more why both same approaches are different?

P.S. But this solver is not as robust as CFX solver. I have no idea why this is so.

[Far]

[from section 25.9.1 of fluent user guide V 6.3] Using the Coupled algorithm enables full pressure-velocity coupling, hence it is referred to as the pressure-based coupled algorithm. This solver offers some advantages over the pressure-based segregated algorithm (SIMPLE).

[from section 25.4.3 pressure velocity coupling, fluent user guide v 6.3] The coupled algorithm solves the momentum and pressure-based continuity equations together. The full implicit coupling is achieved through an implicit discretization of pressure gradient terms in the momentum equations, and an implicit discretization of the face mass flux, including the Rhie-Chow pressure dissipation terms.

So it is clear now that the 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).

Correct me if I am wrong

Dear ghorrocks I am highly thankful to you for your time and help you are providing me. This is very useful discussion and I am learning alot (getting the insight of working of fluent and CFX)