Impeller: temperature decreasing, should be increasing
 

I am doing compressible steady state simulation of impeller which has inlet in shape of circle at the top and outlet on sides. Static inlet zone and outlet zone are attached to rotating impeller.

Pressure at inlet is around 85,000 Pa (vacuum of 15,000 Pa). Pressure is increasing towards outlet where there is atmospheric pressure (100,000 Pa). Density looks similarly (increasing)

So temperature should be increasing from inlet to outlet, because when pressure increases, so should temperature.
But in my simulation T is 300 K at inlet (the way I set), then it's falling and reaches around 294 K at boundary of impeller and lastly it increases from 294 to 300 K in outlet zone. Expected result is that temperature only increases from inlet and reaches highest value right after air exits impeller. It should increase for at least 30 K. Temperature in outlet zone should be slightly less than max T.



Do you have any idea why my temperature behaves in opposite way?

I tried changing temperature boundary conditions but temperature was never increasing towards outlet.


My boundary conditions in file /0/T are:

internalField uniform 300;


inlet has type fixedValue
walls have type zeroGradient
I tired different types for outlet:

a)
outlet
{
type inletOutlet;
value $internalField;
inletValue $internalField;
}


b)
outlet
{
type inletOutletTotalTemperature;
gamma 1.4; //heat capacity ratio (Cp/Cv), 1.40 for dry air 20°C
inletValue $internalField; //reverse flow (inlet) value
T0 $internalField; //static temperature [K]
}


c)
outlet
{
type totalTemperature;
gamma 1.4;
T0 $internalField;
}

It would help if you explain why temperature decreases - I mean generally, under what conditions temperature can decrease?
Because simulation of the same case in Fluent shows that temperature doesn't decrease from initial temp. So apparently there is some kind of heat flux exit in my case.
It really annoys me because T should increase where pressure increases according to ideal gas law, right? .. but in my simulation T decreases where pressure is higher.

I am still trying to figure out where is the problem. After reading some theory on heat transfer and reading threads about similar problem, I identified few possibilities, why my temperature falls while I expect it to increase.
1) enthalpy - maybe I have enthalpy defined as fixed, but it should be allowed to increase
2) thermal conductivity - maybe I'm loosing heat through walls or inlet or outlet because of conduction
3) convection
I think 2) and 3) are not possible because I didn't define any temperature lower than 300K.


It's probably important to mention that velocity and temperature fields look very similar in ParaView. Temperature is lower exactly where velocity is higher.


Does any of that makes sense and what should I try next?

Well, yes you are right, if there is no heat loses to the surrounding! And the impeller temperature is not less than the inlet temperature...

Anyway, I would ask for the case, cause I am interessted in the problem...

Upload the case please...

regardes

Peter

As Peter said, any kind of test case is highly appreciated. Additional information of your FOAM version would be helpful too.

I am sharing my entire case folder with you including polyMesh folder and simulation results at time=500 so size is 9 MB which is too much to upload on forum. I simplified geometry but it is still similar enough to my original geometry. Blade is a face with zero thickness. Google Drive link: https://drive.google.com/file/d/1LQy...ew?usp=sharing



The case is impeller which is rotating counter-clockwise. Air enters at the top and leaves at sides. Geometry is periodic with 7 blades so mesh is only 1/7 of impeller and it has two patches with cyclic boundary condition. Impeller itself is defined as cellZone "rotor" and this cellZone rotates (see red color on first picture). There are inlet and outlet zones which are not rotating and they are attached to rotor.

U and p look about right, but temperature drops from initial 300K but I expect it to gradually increase alongside blades from initial 300K to around 320K at the end of blades (side of impeller). Because pressure is increasing with diameter and so should temperature, right?

What do I need to change to get increase in temperature?

Hello,

The results after 500 iterations you uploded are not plausible.

Continuing calculation from the results you uploaded (500) further lets the simulation running. No divergence happends but omega is very unstable...

Anyway, deleting the results you uploades and restart the sinulation from 0 delivers a divergence and the simulation crashes!

It is funny that I get diffenernt results for 500 iterations when I start it myself and compare it with yours for the same simulation :confused:

Omega explodes and a divergence happends...

Switching the turbulence off ignores the divergence problem of omega.

Well, I will ignore the turbulence in my further experimenting and continue laminar, cause that is not the main topic here.

---

Why you defindes the walls as noSlip velocity?

I am not sure, but I think the walls must be slip velocity conditions?

I could be wrong here...

---

Why you define the flow rate at the inlet as given?

Is it given at all?

ZeroGradient at the inlet delivers a different velocity/flowRate than you pre defined.

The velocity at the inlet by zeroGradient is much higher than the velocity for the given flowRate.

That could be the reason for your problem, then the pressure in this case (pre defined flowRate) is much lower than the outlet pressure.

That means vacuum as you said.

The impeller sucks without getting sufficient fluid deliverd.

Recognizing the ideal gas law, the temperature should be like that lower in the sucking sector and at the near of the blades... At least at the back side of the blades.

Later on after the plades sector, the diffuser increases the pressure again and push the temperature higher.

---

Is the rotations speed realy so high?

I still experimenting...

Regards

Peter

I never tried to run more than 500 iterations. Good to know that 500 is not enough. Now I tried to run 1000 iterations and there was no crash, but I see that residuals go crazy around 230 iterations, later they get lower but this doesn't seem good (picture attached).

Nice idea to disable turbulence. Yes, main topic is why temperature doesn't increase.
Were you able to run the simulation with turbulence set to off? When it was on, solver didn't crash, now when I have it off, solver crashes at 35 iterations.
My colleague suggested noSlip, he also uses it in Fluent. His mesh has boundary layers though - my mesh in this case is tetrahedral with no boundary layers. I'm not sure but I think noSlip is appropriate despite this.
Probably I didn't explain sufficiently the use of impeller in this case. It's goal is to generate as much vacuum as possible, not highest flow rate. Impeller/fan has low efficiency when there is no system resistance and flow rate is maximal. So operating point is not at maximum flow rate but at lower flow rate. We want maximum suction (vacuum). System resistance is caused by the filter at inlet, diffuser, housing at outlet etc. By defining mass flow rate we simulate this system resistance. The value 0.005 kg/s is only an estimate though. I know measured value of mass flow at operating point for different impeller so I chose similar number for this case geometry.
More about system resistance and operating point: http://curta.dlinkddns.com/html_tuto...s/fancurve.htm

Did you get this kind of temperatures as you mentioned? Yes, in the sucking sector they should be low, maybe even lower than 300 K because of pressure drop. Later on temperature should increase towards outlet.

Yes, rotation is really 41000 RPM and even more.

Peter, thank you so much for helping!
- Martin

Well, switching off the turbulence brings other problems with, that I am strugelling with now...

The flow is highly turbulent and my suggestion was not realy a good idea ;)

It just solves a small problem to make other...

I dont use scotch but simple here. I do that to eleminate any problem here too.

Still testing.

Regards

Peter

I usually run solver on single core to eliminate possible problems that come with parallel computing. There are 112k cells so it's calculating relatively fast even on one core.


I changed some things and solver doesn't crash anymore with turbulence off. Residuals also look good. But temperature is still too low.
thermophysicalProperties:


thermoType
{
type hePsiThermo;
mixture pureMixture;
transport const;
thermo eConst;
equationOfState perfectGas;
specie specie;
energy sensibleInternalEnergy;
}

mixture
{
specie
{
molWeight 28.966; // [ g/mol ]
}
thermodynamics
{
Cp 1006.43; // [ J/(kg K) ]
Cv 717.1; //added because of eConst
Hf 0;
}
transport
{
mu 1.845e-05;
Pr 0.71;
}
}


That is the only thing I changed, I think.

Hallo,


I made the following:

- Used your Simulation that you uploaded as default plattform

- Changed the walls from noSlip to slip

- Adding a reference pressure at the inlet to the pressure

as in the simulation:

/tutorials/compressible/rhoSimpleFoam/squareBend/p/

I do not know why this is nececcery. Maybe somebody could comment to that.

The simulation that you uploaded runs now very stable.

Tubulence is on!

Still experimenting.

https://drive.google.com/file/d/1MJ-...ew?usp=sharing

Regards

Peter

Update after a long time. I tried literally anything but I couldn't get correct temperature with solver rhoSimpleFoam. I managed to get good enough velocity, turbulent energy and pressure, even efficiency, but temperature is just wrong.
Then I learned that there are two kinds of solvers, pressure-based and density-based solvers. So I tried density-based solver steadyCompressibleMRFFoam from foam-extend-4.0 and now I get correct temperature field! Temperature is increasing from inlet to outlet from 300 to around 315 K.
I'm not exactly sure what is the reason, but apparently only density-based solvers can correctly calculate temperature in such cases, where air intake is not sufficient so density drops and pressure drops (vacuum).
Or the reason could be that I am dealing with very high rotating speeds (45000 RPM) and air velocity goes over 120 m/s (0.35 Mach) and density-based solvers handle that better.

Same issue for chtMultiRegionFoam, OpenFOAM 7
 

The case file is attached.

The temperature drops below 300K, although I defined all initial temperature to be 300K.

The physics here is to push incompressible fluid through a small gap, so the temperature should not drop at all. It is supposed to be increasing due to the viscous heating.:confused:

Appreciate any help.

Gonna submit a bug report as well.

Btw, I have tried to refine the mesh, and it seems only get worse, the temperature can reduce from 300K to 70+K. Strange.

Also, found a bug report: https://bugs.openfoam.org/view.php?id=1339

bug report submitted here:
https://bugs.openfoam.org/view.php?id=3506

Hello charlliemarshalll!

cht_solver was in the past two solvers, that has been merged in one (since OF5.0 I think...).

A transient and a steadyState...

If ddtScheme is euler, then the case is transient, as in your case!

If ddtScheme is steadyState, then the case is steady state!

Now,

If the case is transient, as in your case, then the pressure by definition is absolute to be defined.

For atmoapherical pressure as example, you define the pressure to be 1e5 pa.


In the case you uploaded you need to:

Change the pressure to be 1e5 pa

Please apply those changes and give a feedback if you still have a probleme running the case.

Regards

Peter

Hello peterhess!!!

Thank you so much for the suggestion.

I have configured p_rgh of both internal field and outlet to 1e5.

The problem is still there. I also noticed that there is a large pressure oscillation roughly from -3e6 to 3e5, and interestingly, it seems the pressure oscillation only occurs on the left domain (near inlet) and there seems to be no oscillation on the right domain (near outlet).

The test case is attached.

Thanks for the insight. Perhaps I should try the steadyState first of all.

Best,

Charlie

Running checkMesh shows that the:

Overall domain bounding box (-17.78 0 -0.24624772) (17.78 5.64 0.24624772)

In x direction as example, You have more than 35 m (m and not mm).

Is that right or you need to rescale the mesh?

if you mean mm please rescale the mesh and retry...

If the dimensions are right, then I could imagine that you need much more cells than about 60 000 Cells...

Is pr number for water so high? 7.56 is a good number :)

Reducing the velocity at inlet to 0.01 and decreasing deltaT to 1e-6 let the simulation at least run!


Regards

Peter

Thanks for the insight.

I have scaled down the geometry to 1/100, and reduced Prandtl Number (I originally tried to simulate silicone oil, that is why it was so high). Reduced inlet velocity to 0.0001. Yet it still diverges.

Just thinking that maybe it requires a code level improvement.

Here is the working case!

https://drive.google.com/file/d/1maj...ew?usp=sharing