[gikamc]

Hello!

I am simulating a multi-stage Axial Turbine in CFX.

I want to calculate Local Heat Transfer Coefficients along stator and rotor blades' surfaces so as to use them as an input for a FEA model. My purpose is to make HTC mesh independent by specifying my own reference temperature rather than the default one which is based on the nearest cell to the surface.

HTC = q / (Twall - Tref)

CFD code calculates the q (heat flux per unit area) and T wall and uses Tref as the reference value.

So as far as I've studied the FAQ (https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F) about calculating heat transfer coefficent in CFX I found it difficult to understand what is the right approach to get the local HTCs for my model.

1. Will I have just to specify the expert parameter <tbulk for htc> as a massflowaverage temperature of the whole Turbine (for all stages) ? (I think it's is a rough approach).

2. Is the adiabatic the appropriate boundary condition for stator and rotor blades' surfaces?

3. Should I use a different Tbulk for each and every distinct domain (stator/rotor blade) and how can i do it ?

4. Is there another suggestion for that task ?

Thank you in advance!

[ghorrocks]

1) I answered this in your other thread. A bit of maths means you can evaluate HTC for any tbulk you want.
2) Not if heat transfer is significant, and I can't see why you are bothering with HTC unless heat transfer is significant. This makes HTC=0.
3) See other thread. You cannot do it directly but you can work it out.
4) Only that you need to be sure of what you are doing. Your Q2 seems to contradict everything else, so better sort that out before doing anything else.

[gikamc]

Dear Glenn Horrocks,

Thank you kindly for your reply.

1. My purpose is to extract HTC and Temperature Field so as to import them as Temperature Load and Convective Heat Transfer respectively to my FEM model.

2. I started by running a simulation with adiabatic boundary conditions (heat flux = 0) at stator/rotor surfaces. I noticed that by plotting heat flux in CFD-Post the value is 0 as expected from the equation: h = q/(Tw-Tref).

But "Wall Temperature Heat Flux" was specified other than 0. From what I've studied so far about "Wall Temperature Heat Flux" I found that it is specified based on an equation like q = f(y+) (function of y+ parameter) and it is not connected with Newtons Law of Cooling. Is that correct ? Is that the case for Wall Temperature too ?

3. I was thinking about running a second case which will use the temperature field from adiabatic simulation as the Fixed Wall Temperature boundary condition so as to let heat flux per unit area to be computed by CFX solver and to let me account for Heat Transfer and especially HTC. My questions are:

- Is this possible to specify such a boundary a boundary condition in CFX-Pre?

- Will then HTC be a std variable provided by CFX to plot it directly to CFD-Post or do I have to wright a CEL Expression for HTC ? If so, the equation will be HTC = q / (Tw - Tref) where Tw will be the results from adiabatic simulation (specified now as boundary conditions) and Tref the tbulk for each and every domain ?

I think it is a good chance to wright the complete procedure to help me and others' futural implementations.

Again, thank you for your time to reply in my threads!

[ghorrocks]

It has been a while since I looked at the precise definition of those variables, so you will have to work that out for yourself.

3a) I don't understand how this helps. You are still specifying a HTC.

If you do not know the conditions at the boundary then you cannot put a boundary condition there. In this case you should move the boundary further out so this wall condition is internal to the simulation. So if you model the wall as a heat transfer solid then you do not need to specify anything at the wall boundary and CFX works everything out as it is internal to the simulation. You could then map these results over to your FEM model without jumping through hoops like you are currently considering.

3b) It is a standard variable, isn't it?

I think it is a good chance to wright the complete procedure to help me and others' futural implementations.

Please do not have unrealistic expectations. We will answer direct questions, but nobody has the time to write a complete procedure.

[gikamc]

Originally Posted by ghorrocks

Please do not have unrealistic expectations. We will answer direct questions, but nobody has the time to write a complete procedure.

Actually I was refering to myself about writing that procedure if i finally figure it out, excuse me for not claryfing that properly.


So do I have to specify a solid domain for blades of interest with proper material assignment (thermal conductivity) and create interfaces between solid and fluid based on conservative interface flux? Is that what you recommended ?


Thank you for your reply!

[ghorrocks]

If you are planning to write the procedure yourself then that is good and we would welcome it

Yes. If making the simulation domain larger means that you can place a boundary condition in a location where you can more accurately describe the conditions, or alternately make the boundary conditions far enough away that its effect on the area of interest is small. So if you include the solid object, and make the troublesome wall boundary entirely inside the simulation then that make simplify things and make it more accurate. The penalty is a larger simulation, of course.

[gikamc]

Finally, I set fluid solid interfaces to make the walls internal to the solution as suggested. I enabled for each fluid solid interface Heat Transfer with conservative interface fluxes. I noticed that when I use the previous solution (with adiabatic walls) as initial condition for the second one, residuals are decreasing straight away giving me the solution even in 10 iterations.

But, I've tried to solve the case separately (without the initial conditions from the previous run) and I noticed that residuals regarding Heat Transfer in Solid Region of one particular blade tend to increase while for the other blade they are decreasing. I tried to refine the mesh of that particular solid domain to see what happens and I noticed that divergence comes faster. Could you please refer to possible causes of that? Can I trust the solution with initial conditions from my previous run?

Also, I can't find HTC as a standard variable in CFD-Post. I only find Wall HTC that I think it is computed based on y+ value.

Please have a look at the attached image below for the energy equation:
https://ibb.co/8dNRz3W

Thank you!

[ghorrocks]

This is a common problem with conjugate heat transfer (CHT) simulations. The problem is the time scale for the fluid equations is much faster than the time scale for the heat equations. This means that it converges quickly in terms of residuals, but the heat equation has not converged yet and does not have conservation of heat.

The fix in a steady state simulation is to use "Local solid time scale factor" of probably 1000 or maybe higher. This accelerates the heat equation relative to the fluid equations so the converge at similar rates.

A second part of the fix is to include imbalances as part of your convergence criteria. This means you will also be checking for global conservation before you declare a result converged.

[gikamc]

Your advice helps me a lot to figure out what I have to do in my model. I have already seen your useful comment in other threads as well. Seems like most of us who are involved in CHT kinda simulations face that particular problem.

As I said before, firstly, I run a case with adiabatic walls for Blades and Vanes.

Then I specified a high quality mesh with hexaherdal elements for the solid phase and that is for the creation of mesh for solid CHT Interfaces for the targeted blades that I specified in CFX-Pre. Then I've chosen Conservative Internal Flux for Intefaces and in Additional Interface Models ticked the Heat Transfer option to account for heat transfer interaction between the CFD-Mesh and Solid Mesh. (I didn't specified Thin Wall or Thermal Contact Resistance)

Just for updating, I would like to inform you that running the simulation with Solid Time Steps specified as 100, 1000, 10000, 50000 didn't work in my case. (That's the cause for my late reply!) The solution came with a specification of initial conditions from my previous run (with adiabatic walls).

Residuals reached the specified value (10e-4 I' ve found somewhere that it is ok for turbomachinery applications) and I attach the imbalances. Though, I didn't find Global Imbalances in my results file.

Secondly, I transfered my data in a thermal analysis. For the temperature is pretty straightforward, but for the convective heat transfer coefficient I followed the exact procedure as in the attached link of another thread:
loading of heat trsf coefficient

Thank you for your help so far!

[ghorrocks]

For CHT simulations the imbalances are critical - you really need to check those to see if you are converged and add imbalances as a convergence criteria of if your imbalances are not good it will continue solving.

You can get the imbalances from the solver manager, or at the end of the output file.

[gikamc]

I didn't find the term "Global Imbalances" but i've found Noramlised Imbalances for each domain, I forgot to attach it previously

https://ibb.co/dMhcj1x

[gikamc]

Finally, I imported loads for temperature and convection coefficient from CFD analysis to Thermal Analysis.

I specified the reference ambient temperature for the calculation of HTC as the VolumeAve(Temperature)@Each blade Domain but the results for HTC look not reasonable at all. In most nodes at Blade Surface HTC is 0.

Do I really have to specify convection boundary condition as soon as I made the solid blade internal to my CHT simulation ?

Is temperature the only result that i have to map in Thermal Analysis after my CHT simulation ?

Thank you in advance!

[jcoelho5]

If anyone have time, please check my post
heat flux coefficient with wallHeatTransfCoeff

I am having some problems using wallHeatTransfCoeff utility in OpenFOAM