[AlexRonto]

Dear all,

I have a CHT analysis for an electric generator. I have plenty of times turned on this forum and I came up with really helpful answers. I have also read documentations, tutorials and related scientific papers, but I still can't get the results I expect from CFX.

What I want to investigate is the cooling of the machine, particularly, I want to calculate the temperatures developed at the coils. The problem is that the temperatures that CFX gives me are rather higher (about 150K difference) than the ones I measured experimentally.

My setup is like this:

4 domains:
-2 rotating steel discs with the magnets attached at their periphery (ROTORS)
-1 epoxy resin hoop between the discs which encloses (STATOR)
-24 coils (COILS)
-air at 25 C (FLUID) (so...incompressible flow with no buoyant effects)

I have a Heat Source defined as sub-domain of the COILS domain and 3 interfaces with conservative interface heat flux model at each of them:

-Solid-Solid interface between COILS and STATOR
-Fluid-Solid Interface between STATOR and AIR
-Fluid-Solid Interface between ROTORS and AIR

I am simulating only the 1/8 of the device due to symmetry conditions.

Boundaries
I have atmospheric pressure boundaries for the cylindrical fluid domain.
-Ptot=0Pa at the side faces (Openings) and
-Pstat=0Pa at the periphery side (Outlet)

Steady/Transient
I am not such interested in the transient physical phenomenon as for the steady state situation.
However, I have tried to run both steady state and transient analyses in order to get better convergence. And I did get with the transient one.

Timestepping
Due to the difference at timescales between fluid/energy equations, I initially ran a simulation with small time steps for the flow to be developed properly and then I turned off the fluid and turbulence equations through expert parameters to calculate the heat transfer.
I have tried plenty of combinations between small/big timesteps for the fluid and solid regions.

Turbulence
I am using SST and my mesh has a y+~0.05 around the stator region (where the main heat flux happens).

Convergence
My P-mass and Velocities residuals are below 10^-5.
My H-energy and T- energy residuals are below 10^-5 and the imbalances below 10^-3
The heat fluxes through each interface are balanced and with no significant difference to each other.

I am running this project for months and I am starting having headaches.... I plea for any advice on what could be the problem. Is there something about any of the above parameters that is causing the problem?

P.S.: 1)Sorry for the long post..
2) Please ask for more info if needed.

[ghorrocks]

Sorry for the long post.

Not at all, in fact this is a good post because you have explained what you are trying to do, what your problem is and what you have done to get things working. I wish more posts where as well written as this one.

I imagine the critical part of this model is the gap. While you have very fine inflation mesh in the gap (in fact probably too fine), you have filled the gap between the inflation layers with a single element. If this is a critical area of the flow this is unlikely to be accurate.

Turbulence models often have numerical roundoff problems when the y+ gets too small. If your y+ is around 0.05 then you may be getting into this problem. I would target a y+ of closer to 1.0.

[AlexRonto]

Thanks for your answer.

At the moment I am trying to create a finer mesh at the gap with a y+~1 but my PC is a bit slow for such a big mesh..So I don't have anything new for now.

However, I noticed I may have misinterpreted some things.. So just to clarify :

1) If I am interested only for the steady state condition where the Temperatures have stopped increasing, is there any reason to run a transient analysis if I could get convergence with a steady state one? It seems to me that since I want the temperatures of the heat source (COILS) it is physically impossible to simulate the phenomenon as steady state , because in this way the COILS' heat capacity, which drives the heat source's temperature rise, is left apart... ???

2) At which region of the mesh should the y+~1? At an older post at this forum I found that the y+max~1 and the y+ at any other regions should be smaller (y+<1). Is it a valid guidance?

3)Timescale: Ι suppose that if the solution is converged, the results at the end of iterations should be the same regardless of the time step I used to reach these results. So time step affects only how fast I will get the solution (apart from extreme timescale conditions where convergence may be unattainable). Is my assumption true?

[ghorrocks]

1) If the final steady state is what you want then yes, run it steady state. This will be much faster and easier than transient. But as you state, you need the full heat circuit defined for this to work - that means where the heat comes from and where it flows through and where it goes to. So you need to ensure you have the heat source, the heat path inside your model and where the heat ends up.

2) y+ = ~1 is a general guide for fine resolution of the boundary layer. Anywhere good boundary layer resolution is required you should be using a mesh resolution of this order. Note that you may also be OK to operate in the wall function regime at y+ >11. That will depend on whether wall functions are suitable for your application.

3) For a steady state run you are correct. A converged solution is independent of the time step size used to get there. This is not completely correct - some flows bifurcate - but that is beyond the scope of this discussion

[AlexRonto]

Hi again,

I used a different turbulence model and a finer mesh at the gap, so the mass flow rate increased and the coils' temperature decreased, but not sufficiently.

So I am reconsidering the thermal aspect of the analysis. I am setting up a steady state thermal analysis according to this

Originally Posted by ghorrocks

1) If the final steady state is what you want then yes, run it steady state. This will be much faster and easier than transient. But as you state, you need the full heat circuit defined for this to work - that means where the heat comes from and where it flows through and where it goes to. So you need to ensure you have the heat source, the heat path inside your model and where the heat ends up.

Question 1: Since I use Conservative Interface Flux condition why is it necessary to define the flow path? Isn't it obvious for CFX that the heat generated will all (steady state, conservative interface) be transferred through the interface to the adjacent domain?

So let's say that the COILS domain has a Heat Source of 100W. In order to define the heat path I define the following Energy sources at the interfaces:

COILS/STATOR coilside -100W
COILS/STATOR statorside 100W
STATOR/FLUID statorside -100W
STATOR/FLUID fluidside 100W

Question 2: Should I use Boundary conditions instead of Interfaces and replace the Energy sources with Heat Fluxes? What would be the difference in the physical meaning of heat transfer?

Question 3: Should I also define the amount of heat coming out of the fluid domain from its boundaries? In this case, I do not know the heat flow passing through each boundary so I suppose I need a transient analysis..


I am trying to ensure that my "thermal settings" are OK, so that I decide that the problem is at the "flow setting"

Cheers!

[ghorrocks]

By defining the heat path I mean you need something to define the heat source and sink, and something to bound the temperature field.

For example: If you have an adiabatic box and put a 100W heat source in it there is no steady state solution to this. The temperature will just increase in time forever and no steady state solution exists.

For example2: If you have an adiabatic box and put a 100W heat source and a -100W heat sink in it, it still will not work. This is because with numerical methods there is always approximations which means the heat in and heat out will not exactly match. There will always be some tiny amount as an imbalance. This tiny imbalance then means the temperature always changes and again there is no steady state solution.

For example 3: Pipe flow where the fluid enters at 25C, passes a 100W heat source and goes out an exit. This case will have a steady state solution as there are heat sources (the inlet and the 100W source), somewhere for the heat to go (out the exit), and the temperature is bounded (the inlet is 25C).

Your comment in Q1 is not correct. You do not need to define the heat flows through the interfaces, the interface calculates it. So only use a heat source where the heat is entering the simulation domain and let CFX handle how the heat flows from there.

Q2: No, see previous comment.

Q3: The normal approach is that you know the temperature of the fluid at the inlet and you know the heat being added in the domain. Then you can just use outlet boundaries at the fluid exit and these require no specification of thermal conditions as the fluid inside the domain simply flows out the domain at whatever temperature it is. But I do not know if this setup is suitable for your application.

[AlexRonto]

I really appreciate your help Glenn. You were pretty clear.

As I said, first of all I want to check that my model has a physically and numerically valid thermal set-up.. The fluid temperatures are bounded at the Inlet and Outlet (Tin=296K Tout=not specified). At the output file I notice that the Heat Flux is passing through each interface and is equal to the energy source I have specified (896000W/m^3) at the coils subdomain. So I suppose that it is a good sign that my model is defined properly.

It seems that I have to focus on the fluid models, turbulence etc in the pursuit of a proper combination of these settings that will give me a bigger mass flow and a higher Heat Transfer Coefficient after all.

Best Regards,
Alex

[ghorrocks]

You seem to be on the right track. Once you have confirmed that the simulation has the correct fundamental setup you need to check that the simulation is accurate. Mesh size, time step size and convergence criteria are the normal things to check here. This FAQ has some further comments: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[evcelica]

Just a quick thought here: You are using Air at 25C, but I'm guessing this thing gets pretty hot? Are constant properties for air applicable here?

[AlexRonto]

Originally Posted by evcelica

Just a quick thought here: You are using Air at 25C, but I'm guessing this thing gets pretty hot? Are constant properties for air applicable here?

Hi Erik,
thank you for your comment.

The compressibility issue is the next thing I'm planning to deal with at my setup. The air heats up to 120C in about 14 min which corresponds in about 25% density drop. I don't know if it is a significant value for the flow and heat transfer development, but from searching through publications which deal with a similar project (electric generator cooling) I have noticed that it is a common practice to consider the air's density as constant. Besides, the incompressibility makes the heat flow set up and the timescale strategy more simple.

I will try to set up a new model with air as Ideal Gas and the buoyancy effects included as well and I hope it will work better.