Hey people,

I noticed something interesting running a problem in both CFX and FLUENT. I use a unstructured mesh for a T pipe junction, a mixing type one, with flow inlets from the branch and from the main header pipe. I use the same mesh for both the cases. I use k-epsilon turbulence model. I have run the cases with both coarse and finer meshes.

Now, here is what I noticed, and here is where I need your help. I believe CFX is better than FLUENT, called me biased if you would. From the CFX results when I plot the pressure (static) and the density through the centerline of main header pipe. I notice that the density follows the same trend as the pressure. Which actually makes sense. The higher the pressure there, the denser the gas in the region.

But when I do the same with FLUENT, I find that the density does not follow, the same trend as the static pressure. I mean for most parts, it behaves in the same way as results from CFX, but near the juntion, the density increases abnormally, whereas the pressure doesn't rise. And by the way, the pressure curve on the centerline is almost similar from both CFX and FLUENT.

Is it safe to conclude that density will follow the same trend as seen from the results of CFX? or will I be wrong, is there some phenomenon I am missing? Is FLUENT doing something erroneous or is the fault CFX's?

And yes, I seem to have a good 18-20% difference in total pressure values on the centerline. And I use similar properties for the fluid for both CFX and FLUENT.

Thanking You

Regards

As for Cfx,you can define ideal gas eqn,redlich kwong eqn with aungier corrections(latest one),u can get the required parameters for RW eqn from pollings book of physical props.

And as u r saying that rho is varying with st pressure in cfx,which is the result of these eqns of state,and try to keep const values of viscosity and th cond as long as they really doesn't affect the solution purpose.

And at the corners of the tee u really need a fine mesh,try using hex grid with low y+ values. Abt fluent, put the question in fluent forum and ask for the definition of eqn of state.

Thanks Pankaj.

Yes, for my final mesh I do use low Y+ , using inflation for CFX. Since I cannot use the .gtm CFXmesh in FLUENT, I did not test it in FLUENT.

But maybe I am missing something.....I couldn't still understand, if my assumption is right that density varies with respect to static pressure ? Or does it have a complex relationship w.r.t pressure? I really couldn't find any publications as such that truely plot change in density through centerlines, neither did I find any mention of it in the litereture.

Hi,

Is your simulations mesh-independent? If not then the results could be anything and a comparison is meaningless.

Regards, Glenn

Assumption of variable Density totally depends on your case, i.e. the fluid you r considering must be compressible(u will find density-pressure relations in any thermodynamics book).

and as Glenn said your comparison for two diff mesh is really meaningless.

Very interesting examination. Let's get more of that.

Being a former CFX user and a current FLUENT user I know that the default values in CFX is "ideal gas" with density varying with pressure and temperature. FLUENT uses constant gas specification as default. Are you sure you have changed it to the proper settings in FLUENT? What about Differencing scheme? Default CFX uses "higher resolution" and FLUENT only 1st order.

BTW you should be able to export a CFX mesh into FLUENT. Go to CFX Solver and choose Tools / Export and set the output format as CGNS. That should work.

Maybe you could share some more information and plots with us.

What about reaching convergence? Which one is the fastest? What about comparison with experiments? Which one is the most accurate?

-Dr. Flow Squad http://tinyurl.com/2gkjh8

This may be obvious, but are you sure your Fluent simulation is fully converged? Is the mass balance over your domain ok?

Bart

Hi Omer,

Comparisons such as this are useful, but you need to take care to ensure the codes are set up as similarly as possible. Check that your boundary conditions, fluid properties and equation of state are the same. For equation of state, keep it simple (i.e. ideal gas) and make sure compressibility is turned on in FLUENT and that you are solving the Total Energy Equation in CFX. For each code, check for grid convergence by running a sequence of similar grids until the solution no longer changes. Running the exact same grid is not necessary and is, in fact, irrelevant since CFX is node centered and Fluent is cell centered, what is more important is the relative use of resources (memory, cpu time, etc.) to get the same accuracy.

As for the pressure vs. density problem in FLUENT, I suspect your solution is not converged. Convergence criteria are differnt between CFX and FLUENT, so pick an appropriate convergence level for each code.

Keep us up to date on your progress.

Best regards, Robin

Anything new? Keep us posted! -Dr. Flow Squad http://tinyurl.com/2gkjh8

Thanks a lot Glenn, Bart, Flow, Robin and Pankaj. All of your suggestions make sense and I am working on with them, starting right now.

Sorry, couldn't reply faster than this, I was travelling.

No need to use the same grid, that makes sense. All I need is convergent grids on both. I have mesh convergence with CFX, I might just use the final mesh in FLUENT to start with. If that doesn't work, I would start from scratch in FLUENT.

Yes, My setup in both cases is similar, I also changed the compressible methane gas properties in CFX to match those in FLUENT.

Sadly, I don't have experimental data to test the accuracy of the results, nevertheless I have validated CFX results for a similar case with a different cross-sectional area.