Convective heat transfer issues in CFX
 

Hello.

Computed task is: hydrodynamics and heat transfer of the flow in circular pipe with uniform wall heat flux.

Modelled liquid: water (density=1000 kg/m3, thermalconductivity=0.6 W/(m*K), heat capacity=4200 J/(kg*K), dyn. viscosity=0.0009 Pa*s).

Length of the pipe: x/d=200 gauges.

Main thermohydraulic parameters: Re=100000, Gr=~3.5e7, Pr=6.3.

Mesh about 500000 elements with average y+~10 (computed by CFX).

Turbulent model: k-omega SST with standart parameters.

Boundary conditions: Inlet - constant velocity = 9 m/s, constant temperature = 300 K; Outlet - relative pressure = 0 Pa; Wall - Wall Heat Flux = 100000 W/m2.

Reference pressure = 1 atm.

Used CFD codes: CFX & FLUENT.

Results:

Dimensionless heat transfer coefficient (Nu) computed by:
CFX 16.2 - 2447;
FLUENT 16.2 - 640;
Petukhov equation (semi-empirical equation for constant wall heat flux condictions in the circular pipe flow) - 575.

Nu=alpha*d/lambda;
alpha=Qwall/(Twall-Tliquid) where Twall - average wall temperature at selected cross-section, Tliquid - mass-weighted averaged temperature of liquid in selected cross-section

Selected cross section was about x/d=170.

So. Anyone know why I have obtained so big error in CFX?

You have provided no details about how you did these models so I have no idea why you are getting a difference. You better work through the issues discussed on the accuracy FAQ before doing anything else: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

But I can assure you there is no inherent inaccuracy in CFX relative to Fluent. When configured correctly CFX can give very accurate answers.

In the case of CFX simulation, you can see how well your system convergences by monitoring the residuals and imbalances plot. Sometimes posting these diagrams helps. Another recommendation is to switch wall back to adiabatic and use it as a heat source (again in W/m^2). For me boundary heat flux does not work correctly.

It should be noted that i' m a beginner so don't take me too much into consideration.

Personally, I am not a fan of Nusselt number comparisons since they are plagued with details such as: reference temperature, characteristic length, empirical correlations, etc..

I would check the basics first, and if those pass, you can narrow down why the heat transfer coefficient is different between the calculations.

First test: Energy conservation (first law)

For flow in a circular pipe with uniform heat flux boundary conditions, there are two back of the envelop calculations that MUST pass.

If you plot T_bulk along the length of the pipe, it must be linear.

Notice in the equation above, there are no subtleties when evaluating any of the quantities.

Hope the above helps

Thank you for your feedback.

I had been computed some parameters and I did obtain some results.

1. Imbalance of H-energy was about 0.05%. After decreasing of residual to 10^-7 I have got imbalance of H-energy about 0.02% and this was minimum asimptotic value.

2. I have been computed energy balance equation in CFD Post how your are recommended earlier. I have got imbalance about 1.6% for the both 10^-6 and 10^-7 residuals. Components that were based on enegry balance equation were about 6286 W for Wall Heat Flux component and 6386 W for water heating component.

3. Tbulk(x) graph was linear.

Later I had changed boundary conditions at sidewall to adiabatic and added constant heat source with the value 100000 W/m2 as pkladisios recommended. Result was the same.

I have read FAQ about accuracy. From list of possible errors the most accurate in my case is grid sensitivity. Earlier I have computed other cases with y+~1 and result of Heat Transfer Coefficient for Water domain was much more accurate in CFX. At this moment I can't tell you exact value of Heat Transfer Coefficient for this case but error was less then 100%.

I have done a lot of computations of Heat Transfer Coefficient in CFX for Gases (Pr~0.25), Liquid Metals (Pr~0.025) and Water (Pr~6). Average error of Heat Transfer Coefficient in case of Liquid Metal or Gas simulation was about 30-65% for meshes with y+~10-15 and about 15-30% for meshes with y+~1 at wide range of Reynolds numbers.
In those conditions error of Fluent simulation was about 10-35%.

But in case of Water simulation in CFX I have reached error higher than 300%.

Do you get accurate answers when you run a Re which results in a laminar flow?

Re=1000;
Nu=4.40 (theoritical one is 4.36 for circular pipe with uniform heating and constant heat flux boundary conditions);
Hydraulic Resistance Coefficient ksi = 0.065 (theoretical one is ksi=64/(Re^0.25)=0.064).

I wonder how you calculate Qwall, Twall and Tliquid in CFX and Fluent? I mean what variables you use?

The laminar flow result is quite accurate so it looks like the issue is associated with the turbulence model.

There are some options in the turbulence models, especially the SST model. Have you tried some of those options?

I have tried to vary turbulent Pr for Gas and Liquid metal simulations, especially at low Re. And there I was able to reduce error to 15-25% in cases when Prt~1.3-1.5. In other words increasing of Prt 1.5 times leads to reducing of error from 35-65% to 15-25%.
For water simulation with Pr~5 empirical Prt~0.85-0.9 by this reason I didn't try to change it.

Earlier I've used CFX 15.0.7 and there was only one available parameter for k-omega SST model - Prt. In current version (16.2) more available parameters, but I didn't try to change them yet.

Moreover hydraulic resistance coefficient and velocity profile in the pipe are pretty accurate. And main problem with heat transfer. As I now in k-omega SST turbulent model only Prt adjust heat transfer.

I suppose that main problem may be connected with Automatic near wall function for Heat Transfer (Kader model).
1. I was used near wall function in both CFX (Automatic Near-Wall function) and Fluent (Standart Near-Wall function).
2. When I've computed Yplus for both simulations with exactly the same meshes I have obtained different results in CFD-Post. For Fluent YPlus=5, for CFX YPlus=10. This is because of YPlus in CFX is based on node center, but in Fluent YPlus is based on cell center.
3. May be there error in CFX that connected with the determination of YPlus.
4. I didn't try to use User-defined near-wall function in CFX yet.

Qwall = lengthAve(Wall Heat Flux)@Polyline 1
Twall = lengthAve(Temperature)@Polyline 1 (here Polyline 1 is external line in the pipe cross-section Plane 1)
Tliquid = massFlowAve(Temperature)@Plane 1 (Plane 1 located at x/d~150).

Keep in mind that in CFX by default:
Wall Heat Flux = hc * (Twall - Tref) where
Tref is Wall Adjacent Temperature that is average T in control volume next to wall and hc is also based on this temperature. So it might be different with your Tliquid and when you divide Qwall by (Twall - Tliquid) you get wrong result.
To base Wall Heat Flux on some far-field value instead of the Wall Adjacent
Temperature, use the Expert Parameter “tbulk for htc”.

May be that is the reason.

If your polyline is not exactly on the wall (including mesh effects on the curved outer wall) then Twall could be off and that would put the Nusselt number calculation out.

Polyline was created by crossing of sidewall and flat Plane 1. I suppose this polyline is pretty accurate.
Anyway in the same CFD post state that I was created for CFX I have obtained very accurate heat transfer coefficient bases on ANSYS Fluent results.

I suppose that there it is no doudbt about the way how wall heat flux applied on boundary. Enegry balance was pretty good. I also have tried to make adiabatic conditions at the sidewall and apply heat source with the same Heat Flux. The result was the same.

Ghorrocks could you compute heat transfer coefficient for turbulent flow of water with Re=100000 in CFX on your PC? Preferable turbulence model is k-omega SST, mesh must to be with y+=10 (for d=0.01 [m] first control volume must to be equal to y=0.00002 [m]). Circular pipe must to be about 100 gauges to obtain stabilized turbulence mode of the flow.

alpha=Qwall/(Twall-Tbulk);
Nu=alpha*diameter/lambda;

Sorry, I don't have time to do your model.

Maybe I can suggest you do a heat transfer on a flat plate? That simplifies things greatly and might allow you to work out what is causing the problem.

Better share your project.

Done. http://rghost.ru/64KNFYGHC

Well. Heat Fluxes is obviously equal. Next
1. Fluent: Twall = 303.7, Tliquid = 301.1, dT = 2.6
2. CFX: Twall = 301.8, Tliquid = 301.1, dT = 0.7

So, I think problem is that T is almost constant in the domain. IMO difference between Twall about 0.6% is normal. But it affects Nu considerably. Maybe Nu is not best criterion here. Or maybe you should try to use double precision solver.

Look, in Celsius difference between 2.6 C and 0.7 C in % with average liquid temperature about 28C is very high. In other word it isn't correct to present temperature in %.

I'd used double presision solver in computations and the same result for temperature was obtained.

In my case Qwall isn't high enough. By this reason dT is low. That's why I shouldn't consider natural convection and inconsistency of properties in a liquid that may affect on the heat transfer coefficient.
But low dT isn't the reason of the fault in heat transfer coefficient that may observed due to numerical errors. That's because of accuracy of the numerical simulation (double) is much higher than observed error.