Hello,

I am simulating a complex flow configuration (wall jet) from what I have experimental data. I have used the RANS turbulence models from CFX (even the models in beta version, as Algebraic Stress Models), but I am not satisfied with the results. LES and its derivates are out of question, because there are limited computational resources available.

I would like to use the v2-f turbulence model, that some papers I read say has better agreement with experimental data in my case. But as this model is not available in CFX, I will have to implement the new model using User Fortran.

Have someone experience with turbulence model implementation using User Fortran? It is a problem that the v2-f model has 4 equation to solve, and the standart models in CFX only 2 or 7 equations? The CFX manual have not helped a lot in this case.

I am a experienced CFX user, but I never used User Fortran before. Any help will be appreciated.

V2-f is available as an add-on for Fluent, an other option to writing user fortran could be asking to see if the same v2f could be added to CFX.

Dear flga and Amadou,

A third option: try to understand why the current turbulence models (either in CFX or Fluent) do not give the results you expect/observe in the experiments..

There are more turbulence models out there than I could to keep track.. The main issue is to improve a few of the best models, and not chase for the holy grail..

I would contact ANSYS CFX support, and explain the features of your particular setup and why current turbulence models in CFX do not provide the correct answer. Otherwise, you will need to implement not only v2-f but a few other ones before you are convinced as which one is better for your application..

Opaque

SST generally performs better than V2-F, and V2-F requires licensing from a 3rd party, so there has been little motivation to implement it in CFX. Try SST instead.

-Robin

Thank you all for the answers.

I agree with you, Opaque, that I need to understand why the current implemented turbulence models don´t work with my problem. But the functionality of the CEL in CFX is too much limited, and I can´t investigate further without programming with User Fortran.

An example: the Cmu constant, used to calculate the eddy viscosity, can´t be substituted for a expression, only for another constant value via CEL. That is just one problem I faced.

I would like it was different, but I think that the only way to have control of the turbulence models is to programming the models myself. Problem is that I don´t have experience with this kind of programming. If one of you could help me with that, I would be very grateful.

Flga,

I'm trying to implement my own transition correlation in CFX using fortran. I think you'll need to use fortran to interact with cmu after each iteration. You need to take the following steps.

1 - try the fortran based tutorials in CFX, such as the air conditioning tutorial to get a feel of how it works etc.

2 - Your fortran is called by a user routine which is called by a user function, which links in to CEL expression. The arguments in the expression can be used in the fortran code.

3 - Spend quite a bit of time reading the cfx manuals. They are not the best for when you want to do something non-trivial, but the basic information is there is you are prepared to look at it.

Hope this helps

Adam

Hi Flga,

you are right on with the limitations of cel. The real downside of the design in CFX is that since CEL is so easy and can do quite a few things, nobody (either users or CFX people) have exercised the user Fortran. When you get to something that you cannot do with CEL you are screwed!!!

I really hope the future merged Ansys products adopt the flexibility seen in the fluent udf's which can do all kinds of things....CEL is just too limited for serious work...and as Adam points out it will take serious work to learn and read the documents. I would be reluctant to undertake this unless you have an example of something similar to start.

As for V2F vs SST vs. RKE, etc. all models are wrong but some are useful. The sales guys at CFX will say SST is better because Menter works for them....I have seen good and bad results with all models. If you know your category of problems and pick a trubulence model with which you have done some validation and you control other parameters such as mesh, domain, boundary conditions for turbulence quantities, etc...you will be better off than switching to some miracle model.

Regards,

Bak_Flow

Thank you, guys. The comments were very useful!

I wish I could do all with CEL... but as I have no choice, I will learn how to do with Fortran.

As Bak_Flow said, some people like to point out always a "miraculous" turbulence model. But to make a decision comparing the different models out there is not that easy too!

flga

Why are you "screwed" when you can't do something in CEL?

Can you give a specific example of something which is fundamentally difficult to implement in user FORTRAN?

Or, maybe you can you give a specific example of what is flexible in Fluent's UDFs that cannot be done in User FORTRAN or CEL?

I'll give a CFX exammple that is not so hard. Implementing a turbulence model generally does not require CFX User FORTRAN. This can easily be done with AVs+User Defined Wall Functions+CEL.

Hi HekLer,

Thank you for the input. It appears that you have experience implementing turbulence models in CFX.

I have a specific question. Do you know if it is possible to access the velocity gradients using CEL? I have tried, but I can't make it works.

Thanks

flga

Dear flga,

Up to ANSYS CFX 10.0, you can only access Gradient's them via a User Fortran wrapper function, and then use them in CEL expressions.

For 11.0, you can access the gradient components of each scalar/tensor/vector component individually via CEL.

Anything else you need to implement v2-F via CEL? Have you thought about

- linearization for the k, v2, epsilon, and f equations?

- What about boundary conditions on walls?

- Or how to properly treat the kinetic energy production term near the boundaries in a consistent manner as CFX treat the momemtum equation?

- Any subtle limiters for v2-f that are not clearly explained in Durbin's papers?

It is not trivial to implement, even in your own source code.

Best of luck,

Opaque

Not to mention that probably not everything about v2-f is published either. I hightly doubt someone could implement it identically to the published model on their own and expect it to actually work.

The custom production term treatment at the wall is a good point too... basically the turbulence models don't work in the CFX solver unless you do it this way, which is not published anywhere either.

Hi opaque,

I was not expecting it to be easy to implement a new turbulence models in CFX. And I am aware too that the v2-f model is complex and the documentation is poor. But I have first to convince myself that it is out of my reach to put this model in CFX... and I am not convinced yet

I have a specific question regarding the access to the gradients via CEL using the new CFX 11. I have here the beta version in my computer, build 2006.07.13-23.13, and in the etc\VARIABLES file I found the new gradient operator, but it appears not to work. I can write the expression in CFX-Pre, but I got a error message in CFX-Solver. Am I using the correct syntax (Velocity u.Gradient X)?

Thank you for all the help!

Dear flga,

Your syntax is correct; however, the access to Gradient became available after preview 6. If you are getting the error:

'Vector operators are not supported yet'

you are using an old beta solver..You must use the latest beta/preview version.. The ANSYS CFX solver build date must be either October or November.

Recall that you can always access them via User Fortran in 10.0.

Opaque

Hi Opaque,

I've checked, and the version I have from the CFX-11 beta is from September. I will ask Ansys for the new beta version.

Thank you!

flga