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

Extreme Temperature again...

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

Like Tree1Likes
  • 1 Post By matw

Reply
 
LinkBack Thread Tools Display Modes
Old   November 1, 2006, 04:36
Default Extreme Temperature again...
  #1
Tuw
Guest
 
Posts: n/a
Hi guys,

I get extreme temperature when I try to simulate 2 domain (continuum zone), fluid and solid. The solid zone is in the fluid zone. I set the solid with heat generation (total heat dissipation is 150W), and the fluid which is air, with pressure inlet and outlet and wall with constant temperature.

Thanks to Razvan, I have managed to simulate 2 different continuum zone by assigning "no boundary condition" for the connecting surfaces of the 2 zones but connecting all the 2 surfaces into 1, in gambit.

My setting for the pressure inlet is gauge total pressure : 10 Pascal, and for pressure outlet is gauge pressure 0 Pascal.

At first 20 iteration, the residual of energy goes just fine and reaches 10-6, after that, it increase exponentially to 10-2 and cannot converge.

Finally, i get unphysical range of temperature from -3500 to 14900K...

Anyone please help me. Thanks in advances!

  Reply With Quote

Old   November 1, 2006, 04:54
Default Re: Extreme Temperature again...
  #2
Andrew Garrard
Guest
 
Posts: n/a
I posted a very similar question a while ago and didn't manage to get an answer I could implment.

http://www.cfd-online.com/Forum/fluent.cgi?read=43545

I suspected the problem was due to grid quality and I am still testing that theory. How many cells are producning unphysical temperatures? What are the equiangle skew and aspect ratio stats for your grid?
  Reply With Quote

Old   November 1, 2006, 05:29
Default Re: Extreme Temperature again...
  #3
nabeel mohsin
Guest
 
Posts: n/a
hello every body luckily i am doing same case of fluid passing through heated cylinder and same case that residual goes down but did not converge. i am also trying and likely to share if get any answer nabeel

  Reply With Quote

Old   November 1, 2006, 13:47
Default Re: Extreme Temperature again...
  #4
sam
Guest
 
Posts: n/a
hello nabeel where r u . Stil in F 11/2 :P
  Reply With Quote

Old   November 1, 2006, 15:06
Default Re: Extreme Temperature again...high heat flux
  #5
matw
Guest
 
Posts: n/a
Hi all - I've been over this and I've detailed the fix for my particular problem. My problem was periodic flow in a pin fin array heated from one surface.

Firstly - Try the node based gradient option (in solver settings)

Secondly - If you're using a tetrahedral grid, try switching secondary gradients off. Do this by typing the following at the command prompt

>(rpsetvar 'temperature/secondary-gradient? #f)

making sure you include the brackets.

Thirdly, change the multigrid settings (solve>controls>multigrid) for energy. Set it to W cycle with a termination criteria of 0.01 (or smaller).

Hope this helps you gentlemen - it took a few months to sort that problem out so count yourselves lucky! Hope it works.

PS I am now having exactly the same problem with transient conjugate heat transfer - any advice would be much appreciated!
haoxin likes this.
  Reply With Quote

Old   November 2, 2006, 00:59
Default Re: Extreme Temperature again...
  #6
nabeel mohsin
Guest
 
Posts: n/a
i am not that nabeel you are thinking astonishing

  Reply With Quote

Old   November 2, 2006, 06:09
Default Re: Extreme Temperature again...high heat flux
  #7
nabeel mohsin
Guest
 
Posts: n/a
hello i am facing problem regarding heat transfer around aroung heated cylinder through coil. when i choose pressure inlet BC it does not converge but if i use velovity inlet it converge. same problem in 2d and 3d can yout tell me the problem nabeel
  Reply With Quote

Old   November 2, 2006, 06:15
Default Re: Extreme Temperature again...high heat flux
  #8
Tuw
Guest
 
Posts: n/a
Hi matw,

Thanks for your suggestion. I am currently trying to solve my problem using your way. But can i ask a question? For the second settting, you recommended to turn off the secondary-gradient (since i am using tetrahedral grid), so i input command prompt as (rpsetvar 'temperature/secondary-gradient? #f), then fluent will come out with

>(rpsetvar 'temperature/secondary-gradient? #f)

>temperature/secondary-gradient?

Is this ok? or i have to provide an answer to it?

Anyway, i just try to simulate using your setting, will let u know the result soon!

To Andrew Garrard,

Ya, i have seen your post previously and i do posted you a reply anyway. However, it seems not effective to your problem.

Actually, i meshed my model using gambit that comes with fluent 6.2, and not using others like TGrid or something. When meshing, I checked that the display window shows that the mesh was generated successfully without any skewed mesh. My some sort of understanding about (highly) skewed mesh, is the mesh's element feature which exceed the boundary of the actual surface of the model. So far, i manage to eliminate any skewed meshes. Can i know what you mean by equiangle skew and aspect ratio of grid?

Since my simulation cant be converged, i believe all my cells producing unphysical temperature. If i change the temperature range manually to an expected temperature range, say from 308k to 500k, some of the plane display 308k, which means same as the original temperature. Anyway, if the simulation cant converged, the result is just worthless.

Tuw
  Reply With Quote

Old   November 2, 2006, 06:25
Default Re: Extreme Temperature again...high heat flux
  #9
matw
Guest
 
Posts: n/a
Tuw,

Yes, this is correct. You are telling the software that you want it off (hence the #f). If you want to turn it back on replace the #f with a #t (as in true or false)

Good luck

  Reply With Quote

Old   November 2, 2006, 07:10
Default Re: Extreme Temperature again...high heat flux
  #10
Andrew Garrard
Guest
 
Posts: n/a
Hellow Tuw and thanks for reply. The reason that my simulations were not converging was nothing to do with the physics of the system. When I get extream temperatures I am convinced that they are due to bad mesh elements. I have some what of a complex geometry to mesh and so I was ending up with bad elements when trying to produce a quick HEX grid. Equiangle skew and aspect ratio are quality parameters that you can look at in gambit in the EXAMINE MESH tool.

In my case, when I do a contour plot of temperature, I am getting my extreme value in cells that have a very high aspect ratio, i.e., the ration of the length to width to height of teh cell is 1 x 1 x 10. I am unsure how to resolve theis problem as the volume I am trying to mesh is also high aspect ratio, e.g. 100 mm x 50 mm x 0.25 mm.
  Reply With Quote

Old   November 4, 2006, 23:27
Default Re: Extreme Temperature again...
  #11
Killian
Guest
 
Posts: n/a
hi tuw, correct me if i'm wrong, but i think that the increment of energy residual to 10-2 is due to the build up of energy within the room. The residuals for my solutions also seem to flacuate about a certain level and will not go down. I'm trying to use the unsteady solver now; maybe you can try it out too.
  Reply With Quote

Old   November 7, 2006, 03:29
Default Re: Extreme Temperature again...
  #12
Tuw
Guest
 
Posts: n/a
Hi all,

I am continuously exploring this problem. One of my friend which is having a similar problem using CFX have managed to produce a converged result. Previously he has done many trial and errors and found out that the "Y-plus" at the wall boundary obtained from his defected result is zero! meaning the node of his meshes didnt attach to the boundary.

If i m not mistaken, the normal value of y-plus is from 20 to 200. I am still studying Y-plus at the moment and not sure about this.

A possible solution from him is to make the mesh of the model smaller. I ask his mesh element volume and he say something around 3million meshes... I am not suggest that you all should use mesh volume until that high. I think the best explanation is when the mesh is smooth enough, the result obtain will be more precise. And make sure the meshes are in good condition(no skewness).

Thanks for your advice, Killian. Maybe i should try using unsteady state condition too..if time permits..hehe..

Tuw
  Reply With Quote

Old   November 12, 2006, 23:12
Default Solved half way!
  #13
Tuw
Guest
 
Posts: n/a
Hi all,

Finally i can get my simulation converged! But still half way to the final goal.

My way is to use size function to avoid high cell jump. Check your size function at gambit---tool. U can go through the gambit tutorial regarding the sedan car!

Make sure the boundary layer is small for the fluid domain near to the solid wall.

Good luck

Tuw
  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
Problem with zeroGradient wall BC for temperature - Total temperature loss cboss OpenFOAM 10 March 5, 2015 07:57
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
monitoring point of total temperature rogbrito FLUENT 0 June 21, 2009 17:31
High temperature methane+air Peter FLUENT 5 January 26, 2009 19:04
chemical reaction - decompostition La S. Hyuck CFX 1 May 23, 2001 00:07


All times are GMT -4. The time now is 06:17.