 ## Fluids

• hugo CFD
Subscriber

Hello.

I am simulating a laminar flow, of air, in a duct of rectangular section, with heat transfer at constant temperature. The upper and lower faces transfer heat the sides are adiabatic.

After simulating with fluent function, I intend to calculate the flow of heat on the walls analytically and compare with the results of the fluent. For the analytical calculation I adopted the following method:

- defined a horizontal plane along the length of the duct, where the distance from the wall is approximately half the height of the cell immediately after the wall.

- I removed the air temperature in this plane

I used the law of fourier

However, the results between the calculated and the obtained CFD are quite different. What could be wrong with the approach?

Regards

• Karthik R

Hello,

I am trying to understand your calculation. Are you suggesting that the estimated Fluent surface heat flux is different from your method (where are you taking temperature on a clip plane and using Fourier's law)? I'd like to ask you a few more questions regarding your analysis.

• What is the parameter you are interested in? Heat Transfer Coefficient or Surface heat Flux?

• You seem to be trying to understand how Fluent is doing its calculation. Is that correct?

• What distance are you using in Fourier's law? Do you have a uniform grid? Do you know your grid size?

• If you are estimating heat transfer coefficient, you might want to take notice of your reference temperature in Fluent. You should be able to see this temperature in Fluent.

Thank you.

Best Regards,

Karthik

• hugo CFD
Subscriber

Yes. There is a difference between the flow of heat that results from fluent and my method. I apply the law of fourrier in the following points: 0,000

0.005 0.015 0.025 0.035 0.045 0.055 0.065 0.075 0.085 0.095 0.105 0.115 0.125 0.135 0.145 0.156 0.165 0.175 0.185 0.15 0.205 0.215 0.225 0.235 0.245 0.255 0.265 0.275 0.855 0.255 0.235 0.385 0.325 0.335 0.345 0.355 0.365 0.375 0.385 0.365 0.405 0.415 0.425 0.435 0.445 0.455 0.465 0.445 0.485 0.495 0.500. The length of the conduit is 0.5 m. The temperature difference used in the law is between the T constant of the surface and the temperature of the bulk at these points.

• Both

• Yes

• The distance used in the fourier law is half the height of the cell immediately following the wall. I will send an attachment of the document to observe the mesh used.

• hugo CFD
Subscriber The mesh is uniform. The dimensions of the elements are 0.250 mm. The inflation has 10 layers. the maximum thickness is 0.3 mm. The distance from the plane to the surface is 0.000005 m

• DrAmine
Ansys Employee

Can you shed some more lights on your method and what you are actually comparing. Again snapshot from Fluent and details about your method are needed.

• hugo CFD
Subscriber

I am simulating a laminar flow of air passing through a duct of rectangular section. There is heat transfer between the duct walls and the fluid. The heat transfer is characterized by the constant temperature of the duct. With the simulation I intend to know the coefficient of heat transfer by convection and the heat flux in the surfaces of constant temperature.

However, in order to validate the values that result from fluent, I have been performing analytical calculations in order to obtain values for the variables in question.

Thus, to obtain the heat flow, I used the fourier law.

To calculate the heat flux using this law, it is necessary to know the temperature difference between the wall and the fluid near the wall. To do this, I created a near wall plan and removed the temperature values for the points indicated above. The distance from this plane to the wall is half the height of the cell just after the wall.

By the difference of temperature, distance and k, the heat flux for each of these points is calculated.

Any questions?

regards

• Karthik R

Hello,

Can you please share the results (both surface heat flux and heat transfer coefficient) based on your calculation and that obtained from Fluent? What value of k are you using?

I understand that you are attempting to learn how Fluent calculates surface heat flux.

Thank you.

Best Regards,

Karthik

• hugo CFD
Subscriber

I send you the excel. I think it's simple to understand.

(Please change the file extension to .xlsx, so you can open it.)

• DrAmine
Ansys Employee

At the wall you can access the wall adjacent temperature which will be the fluid temperature of the first cell off the wall. Moreover "total surface heat flux" for each facet can be accessed as post-processing variable which you could use as conservative variable for post-processing.

• Karthik R

Hello,

Just to add to the above comment by abenhadj, you do not have to explicitly create a clip-plane. You can use the wall adjacent temperature to get the temperature of the cell adjacent to the wall. You will also need the distance of the first cell from the wall. Please be careful when using this distance, especially for a 3D case. You might not have a uniform grid along the length and the heat flux you estimate might not match with values provided by Fluent.

About the heat transfer coefficient, I urge you to have a look at the reference value being used by Fluent. This is an important value Fluent uses to compute the heat transfer coefficient.

I hope this sheds some more light.

Best Regards,

Karthik

• hugo CFD
Subscriber

How do I know the distance from the wall to the first cell? I used inflation.

• DrAmine
Ansys Employee

You have everything you require to compare with your analytical solution:

-Wall Heat Flux (W/m^2)

-Heat Flow through the walls (W)

-Heat Transfer Coefficient (as Kremella said check here the reference temperature) (W/m^2/K)

Cell Wall distance is not calculated in laminar case.  An UDF needs to be used to get it.

But why do you want to compare to the first cell? Which value would that add to your case/project/work?

• hugo CFD
Subscriber

From what I understand you have suggested using the Wall temperature given by fluent, instead of creating the plan I mentioned, right?

So, by using the fourier law, on the fluid side, for analytical calculation, I need the temperature difference between the wall and the first cell and the distance between the two surfaces. So my question is how I know this distance.

I assume there is another analytical way of calculating.

• Karthik R

Hello,

As mentioned by abenhadj, since you are running a laminar flow simulation, you have to use a UDF to get the thickness of your first layer. You need to save this thickness via a UDF on a cell by cell basis. Unfortunately, as far as I am aware, there is no other way of doing this.

I am trying to understand your primary motivation behind this study. Could you please elaborate on the purpose?

Thank you.

Best Regards,

Karthik

• hugo CFD
Subscriber

but If define the inflation through the first layer height, it is possible to consider that the distance between the wall and the first cell is half the height of the cell? since the finite volume method has the node in the center of the cell.

I have to optimize a plate heat exchanger, but first, I need to know how fluent calculates the variables, so that I can do the study better.

• DrAmine
Ansys Employee

Still do not know why you need that but here a workaround if you do not want to use UDF and solve poisson equation to have the distance.

Turn on a turbulence model like sst, run one or few iterations then export the cell wall distance variable wherever you want / need. The variable is available for each cell. It might match the half distance /sizing of your first inflation layer (Fluent cell centered FV code)

Fluent solves for the Fourier's law whenever the flow is laminar on the fluid side of a wall: q=Lamda*partial_T/partial_n. 