CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Nusselt Number calculation in Ansys CFX (http://www.cfd-online.com/Forums/cfx/84138-nusselt-number-calculation-ansys-cfx.html)

 azurespirit January 20, 2011 21:25

Nusselt Number calculation in Ansys CFX

Hi,

I am running 2D jet impingement problem on my CFX. To get ahead with the theoretical aspects etc, I need to calculate the Nusselt Number and Nu distribution across the wall, so I can compare it against an experimental case.

The problem is I am unsure of how to calculate the Nu from the data in CFX post processing. I know that heat fluxes are to be calculated first, but can someone please direct me as to how I could go about finding a solution. Help please.

Thanks.:)

 pavitran January 21, 2011 10:25

Hi

Nu= HL/k

H=wall heat transfer coefficient, (This variable is available in CFX post, take area average)
L= reference length
k= Thermal conductivity of working fluid.

Heat transfer coefficient in cfx is calculated as

H= q/(Thot-Tcold)

where q=wall heat flux in W/m2
Thot= Temperature of the heated surface
Tcold= Temperature at the near wall node.

By default cfx considers Tcold as near wall node temperature(This makes your Nusselt number taking very high values).

To be consistent with literature, you can replace the Tcold temperature with the ambient/far field temperature. You can do this by going into expert parameters and find "tbulk for htc", and change the temperature(in kevlin).

 azurespirit January 21, 2011 10:43

Hi,

I did realise the math eventually. The problem is with the post processing software as I don't really know it well enough. How do I extract the heat flux values for my wall? Do I need to alter any boundary conditions for the wall, to include heat flux terms?

Also, I suppose the values for heat flux will be local from that how can I extract Nu number distribution over the entire span on wall?

 azurespirit January 21, 2011 16:04

I tried the method that you have mentioned, and it works fine. But this way the problem is I can't extract heat coefficient values at various points along my wall, instead what I get is a area average. But for my Nusselt number distributions, I need heat coefficient values at discrete points. Can you please help me by telling how to extract these from cfx-post.

I am able to create a contour plot of heat coefficient values on wall, but I am not able to extract these values in a table. Is this possible in cfx-post? Once I get these values I can calculate the Nu number, as I already have values for k (air at 25 deg c being the working medium).

 pavitran January 21, 2011 22:02

Hi

1. Create a line/polyline in cfxpost.
2. Write an expression for Nusselt number.
3. Use chart option & plot Nu no. on the created line/polyline.
You can find these operations in some tutorials, just check them in help file.:)

 ghorrocks January 22, 2011 06:06

You should be able to get HTC evaluated at all points, not just a surface average. You probably have to set up a CFD-Post variable to get it if the default HTC is wrong (which it will be if you have not set "tbulk for htc").

 azurespirit January 22, 2011 14:57

I tried both methods:

First with specifying the 'tbulk for htc' in expert parameters. I specified the value as 298 Kelvin since the farfield temperature on the part 'OUTLET' in contour plot that I had created earlier reported 299 K, which is quite close. Also, the reason being my inlet fluid is air at 25 deg C, which is 298 K.

The problem with this method was that the value for area avg Wall heat transfer coefficient showed up as ZERO. I might have gone wrong with specifying the value in 'tbulk for htc'. Please let me know if you understand.

When I ran the simulation without specifying the 'tbulk for htc' the post processor gave an average value for htc as 273 W m^-2 K^-1. Again, I have no way to verify this value. But this method at least returns a value.

As for calculating the Nu number distribution, as pavitran suggested, I created an expression for Nu number using a variable for wall htc, and expressions for characteristic length and thermal conductivity (0.026 for air at 25 deg C. The expression evaluates perfectly. Again I encountered problem after this, I created a line, but firstly it doesn't show in the 3-d viewer and I'm not sure what I did wrong. I created the line using TWO POINT method, and specified the two points as the geometric coordinates of my wall (since it is a 2d simulation). And I chose the SAMPLE type. But it doesn't show.

Moreover, I continued by trying to plot the chart anyway by choosing the LINE as reference. The chart is also empty. I am currently hung about in this situation, please suggest any advise that might be of help.

 azurespirit January 27, 2011 13:10

Hi,

 samanpnh February 8, 2013 16:51

2 Attachment(s)
I wrote a code that gives average nusselt number in steady state as a scalar number for a cylinder in cross flow with Induced Vibrations
local nusselt
nuL= (Wall Heat Flux *shoa*2[m])/(75 [K]*Thermal Conductivity )
that 75 is Temperature difference
average nusselt number
nuave=areaAve(nuL)@Pipe1

but I need a way that plot average nusselt number as a function of time like the follow picture

 marcoac14 February 11, 2013 00:49

2 Attachment(s)
Hello guys,

I'm also trying to calculate Nusselt number in a internal flow.

As Pavitran said, by default CFX considers Tcold as near wall node temperature and Nusselt number is very high. We need to be consistent with literature in order to compare results. His solution is to define a known Tbulk (far field temperature) but as it's a internal flow and there's no far field temperature.

Incropera et al (Fundamentals of Heat and Mass Transfer) defines a mean temperature (see attached file) that is to be used in place of Tbulk. Since Tm is varies along the pipe and the expert parameter htc does not allow to use an expression I'm not able to calculate Nusselt number.

Am I doing anything wrong?

Regards,
Marco

 ghorrocks February 11, 2013 00:59

You can divide your pipe up into shorter lengths, and do areaAve() on each segment.

Alternately you could use the idea of what Incropera says by integrating enthalpy over a flow cross section, then working that back to an average temperature and use that. You can then evaluate that exactly at a point, providing you put a surface you can integrate over at that point.

 marcoac14 February 11, 2013 01:11

I'm not sure if I got what you said. Let me know if I'm wrong.

If I were to divide the pipe into shorter lengths, I'd need to do areaAve to calculate heat flux (q) and temperature (Ts) over the interface (fluid/solid), do areaAve to calculate Tm over a cross section, then calculate h = q / (Ts - Tm).

Isn't it too complicated? Isn't there an easier way to calculate htc?
I'd be easier if it were possible to set an expression for Tbulk.

Thanks

 marcoac14 February 11, 2013 01:44

Quote:
 Originally Posted by ghorrocks (Post 407044) You can divide your pipe up into shorter lengths, and do areaAve() on each segment. Alternately you could use the idea of what Incropera says by integrating enthalpy over a flow cross section, then working that back to an average temperature and use that. You can then evaluate that exactly at a point, providing you put a surface you can integrate over at that point.
Since Tm varies along the pipe (z axis), I'm trying to create a variable to plot Tm(z).

Tm defines as follows:
areaInt(Temperature*Velocity w)@Plane 0/(areaAve(Velocity w)@Plane 0*area()@Plane 0)

The problem is that in order to calculate Tm I need a plane to integrate over, but Plane 0 is static and I need to make it move along z. Is it possible?

Regards

 ghorrocks February 11, 2013 05:53

You can sweep it over z in CFD-Post using a session file.

If you want to do it in the solver you need to define the cross sections somehow (make them interfaces or similar) and send it to a monitor point.

 marcoac14 February 11, 2013 08:19

Quote:
 Originally Posted by ghorrocks (Post 407077) You can sweep it over z in CFD-Post using a session file. If you want to do it in the solver you need to define the cross sections somehow (make them interfaces or similar) and send it to a monitor point.
Thanks for helping.

I'm sorry for asking you so many questions, but I'm not an expert user. Actually I've been using the software for a month.

What's a session file and a monitor point? Is it difficult to implement any of these ideas? I need to create an expression for the htc and Nusselt and set them as an output parameter because I'm gonna use Goal Driven Optimization. The idea is to vary wall thicknes, channel width and height and mass flow to maximize Nusselt and minimize Pump power.

Meanwhile, I'm gonna search the web for it.

Regards,
Marco

 ghorrocks February 11, 2013 18:07

If you are going to do an optimisation exercise then I recommend you go to the ANSYS customer web page (from www.ansys.com) and download the tutorials on optimisation and parametric design. This will show you how to set them up.

 marcoac14 February 11, 2013 18:53

Quote:
 Originally Posted by ghorrocks (Post 407251) If you are going to do an optimisation exercise then I recommend you go to the ANSYS customer web page (from www.ansys.com) and download the tutorials on optimisation and parametric design. This will show you how to set them up.
Thanks for your suggestion but I've already done. There's an optimization chapter in CFX Tutorial. The problem is not the optimization itself, but how to get the htc in terms of the mean temperature on the cross section.

I cannot figure out how to calculate Tm along the channel automatically because it's necessary to do an areaAve over every cross section along the channel. It would be easier if it were possible to set a plane location in terms of a variable, which in my case is Z.

Thanks for spending your valuable time trying to help me.

Regards

Regards

 ghorrocks February 12, 2013 07:05

My post #11 had a suggestion which does not require sweeping a plane over a length. Try that.

 marcoac14 February 15, 2013 00:30

Quote:
 Originally Posted by ghorrocks (Post 407361) My post #11 had a suggestion which does not require sweeping a plane over a length. Try that.
Thanks for helping!

 siavash_y April 24, 2013 17:35

Quote:
 Originally Posted by marcoac14 (Post 407937) Thanks for helping!
I have the same problem, did u find a solution marcoac?

All times are GMT -4. The time now is 04:03.