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

Heat Transfer from a cylinder in cross-flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 1, 2007, 10:23
Default Heat Transfer from a cylinder in cross-flow
  #1
Mat W
Guest
 
Posts: n/a
I'm modelling a cylinder in cross-flow using 3d double precision unsteady solver with the geometry that can be found in a paper published by Eckert and Soehngen (1952) [cylinder in a channel]. The Reynolds numbers range from 120 to 600, i.e. laminar and energy equations are being solved. This simple test case gives a 14% Nusselt number error at the front stagnation point and 100% error at the rear of the pin, although the general trends appear reasonable - maximum Nusselt number at the stagnation point reducing to a minimum near the point of separation then recovering in the wake. Grid independence has been proven and the solution is converged. Strouhal numbers are correct.

My question is this - there are no viscous turbulence models being used, the grid is fine enough to resolve the boundary layer so why is difference between experiment and CFD so great? Any views would be much appreciated, Thanks, Mat
  Reply With Quote

Old   October 2, 2007, 05:39
Default Re: Heat Transfer from a cylinder in cross-flow
  #2
Haroon Junaidi
Guest
 
Posts: n/a
Well, Are you sure is you are using bousinesq density model, than you have input the right density and the thermal expansion coefficient.

This greatly changes the result. Also for natural convection problems, your BL mesh size should be generally less than 1 mm. Adapt the grid if it isnt.

Regards

Haroon
  Reply With Quote

Old   October 2, 2007, 07:21
Default Re: Heat Transfer from a cylinder in cross-flow
  #3
Mat W
Guest
 
Posts: n/a
Haroon,

Thanks for the reply but I'm not sure the Boussinesq density model is appropriate here where Re=600. This is forced convection, the Grashof number is less than 1 (around 0.12). Bouyancy is negligible.

Any other ideas where the difference may come from?

Mat
  Reply With Quote

Old   October 2, 2007, 10:21
Default Re: Heat Transfer from a cylinder in cross-flow
  #4
Haroon Junaidi
Guest
 
Posts: n/a
One more thing, how big is your computational domain. It should be five hydraulic diameters all around the cylinder. In the wake region it should be 8 hydraulic diameters. Please check this.

Please check if you have scaled the Grid accurately in Fluent. Very important!

Use QUICK scheme. It works well with low Re flows particularly when the quad grid is used.

I had a fluctuating wake when I solved a cylinder problem. This was due to vortex shedding. Try modelling only half the cylinder using symmetry. This solved my problem.

Hope this helps
  Reply With Quote

Old   October 2, 2007, 11:53
Default Re: Heat Transfer from a cylinder in cross-flow
  #5
Mat W
Guest
 
Posts: n/a
Thank-you for your sensible suggestions. The cylinder diameter under examination is 12.7mm with a cylinder length of 228mm. The channel is 1000mm long so it meets the entrance/exit length criteria you state.

The grid has been scaled correctly.

The QUICK scheme has been used on the momentum and energy discretisation.

As for the fluctuating wake- this is the only way to physically model this problem correctly so I would prefer not to impose a symmetry condition on the centreline. I'm quite sure that the model is correct but I hoped that someone might be able to suggest reasons for the differences between experiment and CFD other than the usual (iterative convergence error, discretisation error, roundoff).

For example, the flow looks like it is separating too early from the cylinder in the CFD- why might this be? The laminar equations should predict separation from a cylinder accurately shouldn't they?

Any answers would be welcome.
  Reply With Quote

Old   October 3, 2007, 04:23
Default Re: Heat Transfer from a cylinder in cross-flow
  #6
Haroon Junaidi
Guest
 
Posts: n/a
Dont take this as an answer, these are just guesses.

May be the reason of early separation is no slip condition in your CFD model where as in the reported data there might be some slip.

I have solved convection problems but I have always achieved strikingly close results. One case in particular was the flow over flat plate but had high Re number.

If there is a fluctuating wake than try modelling the problem as un-steady. You will see quicker convergence and try to plot the variation of Nu with time. You would probably have a sinosodial curve. Integrating that would give you the final Nu.

Thats all I can think of.

regards

Haroon

  Reply With Quote

Old   October 3, 2007, 05:00
Default Re: Heat Transfer from a cylinder in cross-flow
  #7
Mat W
Guest
 
Posts: n/a
Thanks Haroon,

The model is unsteady and the circumferential Nu distribution around the cylinder is time averaged.

I will have a think about the no-slip condition you mentioned, but the scale of the experiment should mean these effects are negligible.

Thanks again, Mat
  Reply With Quote

Old   October 4, 2007, 05:43
Default Re: Heat Transfer from a cylinder in cross-flow
  #8
Faik Hamad
Guest
 
Posts: n/a
I am just starting to use FLUENT. can any one help to start generating the geometery for a heat transfer from a cylinder in cross flow in a pipe.

Thank you
  Reply With Quote

Old   October 4, 2007, 17:19
Default Re: Heat Transfer from a cylinder in cross-flow
  #9
Brian M. Holley
Guest
 
Posts: n/a
Regarding the leading edge stagnation region, you might check the cylinder midspan surface static pressure as a function of circumferential arc length. The satic pressure profile should be parabolic in the stagnation region. Hiemenz flow (see Schlichting) is an exact analytical solution for flow impinging on a plate, and based on your pressure field you can determine the displacement thickness of the stagnation boundary layer, which is constant in Hiemenz flow. In order to resolve the heat transfer in that region, you should have five or so grid cells within that displacement thickness. If you have one or fewer, that may be the problem. For more details, check a paper from IGTI in Montreal 2007, GT2007-28120.
  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
Two-sided Wall Heat Transfer BC - No Separate Solid Mesh and No Heat Transfer Coeff swahono OpenFOAM Running, Solving & CFD 8 February 26, 2015 05:30
Heat Transfer from a Rough Cylinder in Tunnel RE=2.2E5 M=0.07 aerothermal OpenFOAM Running, Solving & CFD 9 May 23, 2013 04:12
Multiphase flow and conjugate heat transfer simulation awacs OpenFOAM Running, Solving & CFD 8 March 1, 2013 06:25
heat transfer in two-phase flow Leonid Fromzel CFX 0 April 8, 2008 05:57
Heat transfer Inviscid pipe flow Dave CFX 4 March 6, 2008 11:33


All times are GMT -4. The time now is 19:12.