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

Some help simulating Magnus Force using Fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 27, 2002, 05:43
Default Some help simulating Magnus Force using Fluent
  #1
Michele Spinolo
Guest
 
Posts: n/a
Hi netters,

I'm tring to study Magnus Force on infinite (2D) cylinder using Fluent, but results I obtain doesn't match sperimental datas: in particoular I can't see Negative Magnus force that I should have during the transition from laminar-tourbulent to fully developed toubulent motus, the results Fluent gives to me for both Cd and Cl coefficient (note that I inserted in Fluent correct reference values for my problem) are too far from experimental results, even with no spin for the cylinder (Cl goes rightly to 0 but Cd doesn't give me good results (it should change with Reynolds number during the transition written before, but it's very far from the range it should belong: sperimentally from ~1.3 to 0~0.35, with Fluent always near 0.15-0.25)

I setted Fluent with uncompressible fluids (air max speed is near 20m/s), RSM model with standard coefficients, standard wall function for near wall treatment, double precision solver.

Mesh is very well done with Gambit, near cylinder I used Map scheme and first lenght is 1*10^-5, I can see very well velocity profiles changeing and stall point, I'm quite sure it's not a mesh problem.

I read in some old posts that to simulate more accurately magnus force you should change a coefficent in k-e model, but i don't know which and the correct value, maybe it's the same for RSM model (it solves k-e equations too....).

So at the end of this: can someone help me? did someone already studied Magnus force with Fluent (I can use both 5.4.8 and 6.0.12) and had good results and could help me?

If you need more details please ask.

Thank you very much Michele Spinolo
  Reply With Quote

Old   June 27, 2002, 05:51
Default Re: Some help simulating Magnus Force using Fluent
  #2
Jonas Larsson
Guest
 
Posts: n/a
Fluent can not predict transition - if you turn on a turbulence model you will most likely get fully turbulent bouyndary-layers from the start. If you are trying to simulate a regime where boundary layer transition is important you will most likely run into trouble.

Btw, have you made sure that you have the first grid cell at y+ between something like 30 and 200 (a must if you use wall-functions)?

  Reply With Quote

Old   June 27, 2002, 06:14
Default Re: Some help simulating Magnus Force using Fluent
  #3
Michele Spinolo
Guest
 
Posts: n/a
Y+ is "wall Yplus" I can find in display/contours/turboulence? If it's this I have a value under 5 near the 2D cylinder, the dominium I created is 60x20 and the cylinder has diameter 1.4.

I tried to simulate transition from laminar to tourbulent becouse I have this kind of experimental datas (from Re=~0 to Re=5*10^5), and i can't validate other simulation.

Could someone give me more Cd (and if someone have Cl too) for a spinning or at least non spinning cylinder in a fully developed tourbolent flow? (giving Re number too?)
  Reply With Quote

Old   June 27, 2002, 06:28
Default Re: Some help simulating Magnus Force using Fluent
  #4
Jonas Larsson
Guest
 
Posts: n/a
Yep, that is the right Yplus - if it is below 5 in the cells next to the cylinder surface your wall-functions will not work very well. You need to have y+ above 20 (and below something like 200 - varies depending on the Re number) for wall functions. You can either refine your mesh so that y+ is below 1 everywhere and use the Low-Re Wolfstein two-layer model or you can coarsen your grid next to the walls to get y+ bigger than 20 so that you can use wall-functions. Fluent 6 has a new wall-treatment which they claim can swith seamlessly between these models to work on any grid. I haven't checked how it performs in the difficult case when you have y+=5 though (anyone?).

If you are looking for other good test-cases you can take a look at the links in the reference section.
  Reply With Quote

Old   June 27, 2002, 08:00
Default Re: Some help simulating Magnus Force using Fluent
  #5
Michele Spinolo
Guest
 
Posts: n/a
I have Y+ under 1 near the cylinder, but it's higher than 1 (from 1 to 3000) near wall domains, now i'm tring to use 2 layer zonal model as wall treatment, do you think I should have Y+ under 1 also in the zone near domain's wall (it's very far from cylinder)?

Thanks
  Reply With Quote

Old   June 27, 2002, 10:24
Default Re: Some help simulating Magnus Force using Fluent
  #6
Jonas Larsson
Guest
 
Posts: n/a
If it is a wall you should, but it will probably not affect your results close to the cylinder. Perhaps it is better to set it to a symmetry boundary - then you don't have to worry about y+.
  Reply With Quote

Old   June 27, 2002, 12:57
Default Re: Some help simulating Magnus Force using Fluent
  #7
Michele Spinolo
Guest
 
Posts: n/a
Jonas, thank you very much! great idea to set as a symmetry boundary condition!

near the cylinder I have Y+=0, i did some run with 2 layer zonal model (more than 4000 iterations) but i get Cd=0.16 instead of Cd=0.4 (experimentally), the cylinder is not spinning. I don't really know why...or better maybe I know why: with 2 layer zonal model i don't have the negative pressure in the rear of the cylinder (opposite part of flow inlet) that i have with standard wall treatment...

Another question (you are very patient) how can i obtain a higerh value of Y+ near the cylinder (with a more larger mesh?) so I can use standard wall treatment?

Thankx Michele
  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
UDF in Fluent Andrew Fluent UDF and Scheme Programming 4 March 16, 2012 04:35
Abaqus - Fluent Coupling WITHOUT MPCCI s.mishra FLUENT 0 May 1, 2011 09:45
Circulator Simulating with Fluent Software arya FLUENT 0 March 14, 2009 03:56
Simulating a static mixer in Fluent Novice FLUENT 1 January 26, 2009 14:09
Force calculation in Fluent Jason FLUENT 0 February 15, 2005 17:15


All times are GMT -4. The time now is 07:56.