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

What went wrong?-Panick

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 26, 2002, 10:11
Default What went wrong?-Panick
  #1
Julie
Guest
 
Posts: n/a
Hi guys,

I posted my problem a while ago. WHile some do not understand my question,some agrees that my problem is because of my meshing.

To make long story short. I inputed my inlets as Velocity_inlets and keyed in the value of 0.625m/s as inlet velocity in y componenet. But after convergence, when i did a report/surface intergral/facet average/velocity/y component,the value I get is not even near 0.625m/s, in fact I got about 0.55m/s, however the mass flow rate at that inlet calculated by fluent was correct as shown in report/fuxes.

SO was the results at the outlets, which differs even more from the actual value.I wondered if it was to do with the mesh.So after refineing the mesh, from the actual 0.2intervel size at all the edges of my model to 0.1 size and even decrease the convergence criterion value. And there was improvement, but still not enough. I got 0.59m/s from the original 0.55m/s.

Was it REALLY the grid? How much is enough? I cant reduce it any further, my mesh file will be too huge. Was it Really the grid, or have i done something wrong? Anyone experienced my problem b4??
  Reply With Quote

Old   July 26, 2002, 11:42
Default Re: What went wrong?-Panick
  #2
sohail
Guest
 
Posts: n/a
Hi,

Can you tell me what convergence criterion you have taken before and know.
  Reply With Quote

Old   July 26, 2002, 23:51
Default Re: What went wrong?-Panick
  #3
Julie
Guest
 
Posts: n/a
Hi,

Well I used to take the defaults, so it will be like 10e-3 for continuity,x-velocity,y-velocity,z-velocity

In my revised model, I change the convergence criterion to continuity,x-velocity,y-velocity,z-velocity to 10e-5
  Reply With Quote

Old   July 27, 2002, 03:36
Default Re: What went wrong?-Panick
  #4
Sohail
Guest
 
Posts: n/a
I think it will be better if you try with 10e-6 and see the result I hope you will be very much close to your values Regards Sohail
  Reply With Quote

Old   July 27, 2002, 04:39
Default Re: What went wrong?-Panick
  #5
david
Guest
 
Posts: n/a
Why don't you locally refine the mesh near the inlet and outlet and let gambit mesh the rest of the domain. I am pretty sure, its the mesh.

DC
  Reply With Quote

Old   July 28, 2002, 15:37
Default Re: What went wrong?-Panick
  #6
Peter
Guest
 
Posts: n/a
Ok, you need to be sure that the case is fully converged, the residuals must be flat and decreased several orders of magnitude. What you can do to check if you reached convergence or not is to define a surface or rake inside you domain and to plot the mass flow across the surface o rake against the number of iterations. You should see oscillations at the beginning and then you should get an horizontal line when you reached convergence. I got some discrepancies when I tried to compare the output of surface integrals and the quantities you specify in the boundary condition panels. As far as I know FLUENT performs interpolation to obtain these surface integrals values and therefore errors can occur. They should become smaller as you improve the mesh density as you have noticed. I would trust however the results from Report/Fluxes, not totally the results from Report/surface integrals
  Reply With Quote

Old   July 29, 2002, 02:14
Default Re: What went wrong?-Panick
  #7
Ashu
Guest
 
Posts: n/a
I think you compute the average outlet velocity from the mass outflux. Also try refining the mesh and see if it changes. Then compute the velocity based on the mass out-flux. I hope you would match results if you keep refining the mesh. Also try using small value of residual for continuity 1e-5 etc. so that the mass is balanced.

Ashu
  Reply With Quote

Old   July 29, 2002, 09:57
Default Hey thanks all, does grid adaption help?
  #8
Julie
Guest
 
Posts: n/a
Hey

Thank you so much for all your kind response!

Firstly, I will refine the mesh using gambit, then reduce the convergence criterion in Fluent.

It's really nice of Peter to suggest the method of checking convergence, and it is DEFINITELY a relief to know that there are pple experiencing discrepancy in the results like I have. 2 of my friends are using gambit and Fluent and none of them has the same kind of problem which I face, I was really lost when it happened to me!

Recently, I was reading the manuals, and I wonder if Grid Adaption could do the trick in helping to achieve better accuracy in my case too. Anyone, any suggestion or advice regarding that?

Thanks once again!
  Reply With Quote

Old   July 30, 2002, 01:45
Default Re: What went wrong?-Panick
  #9
Julie
Guest
 
Posts: n/a
Hi again,

Sorry, if this qn is easy, but how do I plot the mass flow rate with number of iterations?

The options under "Plot" is plotting with respect to distance in the domain and also does not have mass flow rate option for the Y axis function, and the "plot residuals" do not have mass flow rate option in it..
  Reply With Quote

Old   July 30, 2002, 02:18
Default Re: What went wrong?-Panick
  #10
Ashu
Guest
 
Posts: n/a
Mass flux can be defined as velocity) * (rho)* (density), in user field function. Then use this as variable in solution monitor (surfaces).

But why you wnat to see the variation in mass flow? Once you get the converged residuals, the velocity, mass etc. are going to remain same - converged value.

Hope this helps. Ashu
  Reply With Quote

Old   July 30, 2002, 03:30
Default Re: What went wrong?-Panick
  #11
Julie
Guest
 
Posts: n/a
Hi Ashu,

I want to see the variation because, I have put in 10e-6 for the convergence criteria in residuals, and for the solution to converge, it takes a really long time.

If I could see the variation of mass flux with number of iterations, then perhaps if the mass flux does not change much with the number of iterations, I could have known when to stop iterating.

I am just afraid that having 10e-6 is really redundant when 10e-5 could have made my soultions accurate enough, then I do not need to use so much time for iteration.
  Reply With Quote

Old   July 31, 2002, 01:39
Default Re: What went wrong? Don't Panick
  #12
Ashu
Guest
 
Posts: n/a
If you can't use mass flow rate as User field function and monitor it, use velocity itself to see whether solution is converged or not. Also stop iteration and check the mass flux run again for few iterations and see if mass flux has changed, if not that is your converged result.

Hope this makes sense.

Ashu
  Reply With Quote

Old   July 31, 2002, 07:08
Default Re: What went wrong?Trying to calm down..
  #13
Julie
Guest
 
Posts: n/a
Yap I get wat you mean.

Meanwhile I also know how to plot mass flow rate aganist iterations from Atholl's response.

Guess with both ways, I would be sure of how to determine convergence.
  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
Warning: Dynamic zone with wrong CG using 6DOF Manoj Kumar FLUENT 1 August 11, 2012 04:03
MRFSimpleFoam: wrong boundary conditions on rotating walls cves OpenFOAM Bugs 3 May 3, 2010 03:38
BuoyantBoussinesqSimpleFoam and axial-symmetric results wrong mass flow Thomas Baumann OpenFOAM 6 December 21, 2009 11:31
udf error srihari FLUENT 0 February 9, 2009 10:00
Pressure contour seems wrong??? Harry Qiu FLUENT 1 June 29, 2001 05:53


All times are GMT -4. The time now is 07:45.