CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Nusselt Number calculation in Ansys CFX

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 20, 2011, 21:25
Default Nusselt Number calculation in Ansys CFX
  #1
New Member
 
Shashank
Join Date: Jul 2010
Posts: 18
Rep Power: 7
azurespirit is on a distinguished road
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.
azurespirit is offline   Reply With Quote

Old   January 21, 2011, 10:25
Default Hi
  #2
Member
 
Dynampally Pavitran
Join Date: Mar 2010
Location: India
Posts: 73
Rep Power: 7
pavitran is on a distinguished road
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).
amin_gls likes this.
pavitran is offline   Reply With Quote

Old   January 21, 2011, 10:43
Default
  #3
New Member
 
Shashank
Join Date: Jul 2010
Posts: 18
Rep Power: 7
azurespirit is on a distinguished road
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 is offline   Reply With Quote

Old   January 21, 2011, 16:04
Default
  #4
New Member
 
Shashank
Join Date: Jul 2010
Posts: 18
Rep Power: 7
azurespirit is on a distinguished road
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).
azurespirit is offline   Reply With Quote

Old   January 21, 2011, 22:02
Default Hi
  #5
Member
 
Dynampally Pavitran
Join Date: Mar 2010
Location: India
Posts: 73
Rep Power: 7
pavitran is on a distinguished road
  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.
amin_gls likes this.
pavitran is offline   Reply With Quote

Old   January 22, 2011, 06:06
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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").
ghorrocks is offline   Reply With Quote

Old   January 22, 2011, 14:57
Default
  #7
New Member
 
Shashank
Join Date: Jul 2010
Posts: 18
Rep Power: 7
azurespirit is on a distinguished road
Thanks for the advise.

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 is offline   Reply With Quote

Old   January 27, 2011, 13:10
Default
  #8
New Member
 
Shashank
Join Date: Jul 2010
Posts: 18
Rep Power: 7
azurespirit is on a distinguished road
Hi,

I am awaiting for any replies with some help. Anybody got suggestions? Please help.
azurespirit is offline   Reply With Quote

Old   February 8, 2013, 16:51
Default
  #9
New Member
 
saman
Join Date: Jan 2013
Posts: 9
Rep Power: 4
samanpnh is on a distinguished road
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
of course I Send the variable nuave to a monitor point, but it gives this error in follow picture. please help me
Attached Images
File Type: jpg 1.jpg (34.8 KB, 106 views)
File Type: jpg 2.jpg (52.6 KB, 102 views)
samanpnh is offline   Reply With Quote

Old   February 11, 2013, 00:49
Default
  #10
New Member
 
Marco Correa
Join Date: Jan 2013
Posts: 8
Rep Power: 4
marcoac14 is on a distinguished road
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
Attached Images
File Type: jpg meanTemperature_Incropera_1.jpg (83.9 KB, 113 views)
File Type: jpg meanTemperature_Incropera_2.jpg (59.0 KB, 72 views)
marcoac14 is offline   Reply With Quote

Old   February 11, 2013, 00:59
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   February 11, 2013, 01:11
Default
  #12
New Member
 
Marco Correa
Join Date: Jan 2013
Posts: 8
Rep Power: 4
marcoac14 is on a distinguished road
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 is offline   Reply With Quote

Old   February 11, 2013, 01:44
Default
  #13
New Member
 
Marco Correa
Join Date: Jan 2013
Posts: 8
Rep Power: 4
marcoac14 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
marcoac14 is offline   Reply With Quote

Old   February 11, 2013, 05:53
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   February 11, 2013, 08:19
Default
  #15
New Member
 
Marco Correa
Join Date: Jan 2013
Posts: 8
Rep Power: 4
marcoac14 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
marcoac14 is offline   Reply With Quote

Old   February 11, 2013, 18:07
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   February 11, 2013, 18:53
Default
  #17
New Member
 
Marco Correa
Join Date: Jan 2013
Posts: 8
Rep Power: 4
marcoac14 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
marcoac14 is offline   Reply With Quote

Old   February 12, 2013, 07:05
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
My post #11 had a suggestion which does not require sweeping a plane over a length. Try that.
marcoac14 likes this.
ghorrocks is offline   Reply With Quote

Old   February 15, 2013, 00:30
Default
  #19
New Member
 
Marco Correa
Join Date: Jan 2013
Posts: 8
Rep Power: 4
marcoac14 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
My post #11 had a suggestion which does not require sweeping a plane over a length. Try that.
Thanks for helping!
marcoac14 is offline   Reply With Quote

Old   April 24, 2013, 17:35
Default
  #20
New Member
 
siavash azadi
Join Date: Apr 2013
Posts: 1
Rep Power: 0
siavash_y is on a distinguished road
Quote:
Originally Posted by marcoac14 View Post
Thanks for helping!
I have the same problem, did u find a solution marcoac?
siavash_y is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Specify number of cores that CFX should use. Lance CFX 14 April 1, 2014 10:43
DecomposePar unequal number of shared faces maka OpenFOAM Pre-Processing 6 August 12, 2010 09:01
CFX doesn't continue calculation... mactech001 CFX 6 November 15, 2009 22:25
Unaligned accesses on IA64 andre OpenFOAM 5 June 23, 2008 10:37
Nusselt Number of the order of 35000 chinmay FLUENT 4 May 31, 2001 03:06


All times are GMT -4. The time now is 15:38.