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

How to slove "temperature limited to 1.0000e+00001 in cells.."

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

Like Tree8Likes
  • 8 Post By Chris D

Reply
 
LinkBack Thread Tools Display Modes
Old   July 31, 2009, 03:41
Default How to slove "temperature limited to 1.0000e+00001 in cells.."
  #1
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 8
Conan is on a distinguished road
Send a message via MSN to Conan
I generated grid in GAMBIT, no error and no warning, no "highly skewness>0.97". But during iteration in FLUENT, there happened "temperature limited to 1.000e+00001 in 1 cells...". Clearly, the temperature value is not possible in my model. So, how to solve it? I have to de-select "energy" in solution panel.

So please tell me your experiences, thank you.
Conan is offline   Reply With Quote

Old   July 31, 2009, 16:13
Default
  #2
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 8
Chris D is on a distinguished road
This might happen early in your solution, but it should go away as you iterate. What happens is that FLUENT calculates some value that is below 10 K, which is (probably) unreasonable. To keep the simulation from diverging, it discards the value it calculated and uses 10 K insead.

If the warning does not go away as you iterate, try to find where the offeding cell is. You can do this by going to the adapt by iso-value menu and selecting adapt by temperature. Pick a range of temperatures (something like 5 K to 20 K), click "mark", then "manage". A menu will pop up. Now, click "display" and you should be able to see where the cell is that is giving you a problem.

You might find that the cell is near a sharp edge. Since a sharp edge is a discontinuity, FLUENT might have trouble resolving the flow in that region. To fix this, you could add grid in the region of the sharp edge or regenerate your model and round off the edge.

Finally, it might not really matter that much. If it is only one cell out of millions, and it isn't in region in which you are particularly interested, you might be able to just ignore it.
Chris D is offline   Reply With Quote

Old   July 31, 2009, 20:18
Default
  #3
New Member
 
Deepak Thirumurthy
Join Date: Jul 2009
Posts: 1
Rep Power: 0
deepak is on a distinguished road
Chris is right.
It usually occurs to me when my mesh is not good at some sharp corners. I usually refine mesh or simply ignore it as it doesn't affect my global solution.

Deepak
------------------------------------------------------------------------
deepak is offline   Reply With Quote

Old   August 1, 2009, 06:43
Default
  #4
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 8
Conan is on a distinguished road
Send a message via MSN to Conan
thanks. but when generating grids, no any errors and warnings, which means no highly skewness>0.97. In geometry, no sharp edge, but with some circular edges. My model is heated, the inlet air temperature is 300K, so all the temperature is expected more than 300K. Although the total number of cells is about 2.4M, the messege is happened only one cells. Even if I ignore it, I find the final temperatre distribution is unreasonable, and hence the heat tansfer is not correct.

I have to calculate flow first, and then open the energy solution when the flow interation is converged.






Quote:
Originally Posted by Chris D View Post
This might happen early in your solution, but it should go away as you iterate. What happens is that FLUENT calculates some value that is below 10 K, which is (probably) unreasonable. To keep the simulation from diverging, it discards the value it calculated and uses 10 K insead.

If the warning does not go away as you iterate, try to find where the offeding cell is. You can do this by going to the adapt by iso-value menu and selecting adapt by temperature. Pick a range of temperatures (something like 5 K to 20 K), click "mark", then "manage". A menu will pop up. Now, click "display" and you should be able to see where the cell is that is giving you a problem.

You might find that the cell is near a sharp edge. Since a sharp edge is a discontinuity, FLUENT might have trouble resolving the flow in that region. To fix this, you could add grid in the region of the sharp edge or regenerate your model and round off the edge.

Finally, it might not really matter that much. If it is only one cell out of millions, and it isn't in region in which you are particularly interested, you might be able to just ignore it.
Conan is offline   Reply With Quote

Old   August 1, 2009, 14:53
Default
  #5
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 8
Chris D is on a distinguished road
Does iterating until the flow is converged and then enabling the energy equation solve your problem? Do you get the warning when you turn the energy equation on?
Chris D is offline   Reply With Quote

Old   August 2, 2009, 12:15
Default
  #6
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 8
Conan is on a distinguished road
Send a message via MSN to Conan
YES. Because the model looks somewhat complex, I first enable flow solution untill the error is less than 1.E-4. Then I only open the energy solution untill the error is less than 1.E-9. During the temperature iteration, no warning is happened. In this case, Such temperature calculation is only about 50 iteration. But in my previous models, when flow and energy are computing at the same time (no warning), the iterations for temperature is about 1000. Is it becasue the flow is not converged so than the tempeature needs larger iterations? ?


What is difference between enabling flow-and-energy solution and first-flow-then-energy solution? ? If the case is steady, incompressible, constant property.



Quote:
Originally Posted by Chris D View Post
Does iterating until the flow is converged and then enabling the energy equation solve your problem? Do you get the warning when you turn the energy equation on?
Conan is offline   Reply With Quote

Old   August 3, 2009, 08:37
Default
  #7
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 8
Conan is on a distinguished road
Send a message via MSN to Conan
Problem is still happeded when I decrease the temperature iteration crietia to 1.E-10. After 200 iterations, the warning is appeared as like those cases where flow and energy are computing at the same time.

What can I do?


Quote:
Originally Posted by Conan View Post
YES. Because the model looks somewhat complex, I first enable flow solution untill the error is less than 1.E-4. Then I only open the energy solution untill the error is less than 1.E-9. During the temperature iteration, no warning is happened. In this case, Such temperature calculation is only about 50 iteration. But in my previous models, when flow and energy are computing at the same time (no warning), the iterations for temperature is about 1000. Is it becasue the flow is not converged so than the tempeature needs larger iterations? ?


What is difference between enabling flow-and-energy solution and first-flow-then-energy solution? ? If the case is steady, incompressible, constant property.
Conan is offline   Reply With Quote

Old   October 2, 2009, 08:31
Default
  #8
los
Member
 
Tiago Macarios
Join Date: Mar 2009
Posts: 35
Rep Power: 8
los is on a distinguished road
as deepak said, I too sometimes get this errors with bad mesh...
what I used to do and worked was to turn the secondary gradient of temperature off, i think the code was something like this:

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

hope it helps
los is offline   Reply With Quote

Old   October 19, 2009, 15:08
Default
  #9
New Member
 
Join Date: Oct 2009
Posts: 2
Rep Power: 0
abrar is on a distinguished road
reduce your under-relaxation factors during the initial part of your simulation. You may relax them once the solution is behaving stable or as expected.
abrar is offline   Reply With Quote

Old   November 19, 2009, 03:32
Default set the limit yourself
  #10
New Member
 
Tom Potters
Join Date: Jul 2009
Posts: 10
Rep Power: 8
TomP is on a distinguished road
If the extremely low temperatures are causing divergence problems you could set this limit to a higher more reasonable value. That way it will correct the temperature when it falls below e.g. 290K instead of 10K
TomP is offline   Reply With Quote

Old   December 4, 2009, 15:32
Default
  #11
New Member
 
Join Date: Dec 2009
Posts: 1
Rep Power: 0
jbrace is on a distinguished road
this is a hard problem to figure out.
__________________
Jason
jbrace is offline   Reply With Quote

Old   November 15, 2012, 09:43
Default
  #12
Member
 
Join Date: Sep 2011
Posts: 38
Rep Power: 5
Kamu is on a distinguished road
You might also need to check your models! For example if you are modelling turbulence, you might get better convergence with a different type of wall treatment!
Kamu is offline   Reply With Quote

Old   October 16, 2014, 09:11
Default
  #13
New Member
 
Join Date: Jan 2014
Posts: 11
Rep Power: 3
ruturaj171 is on a distinguished road
Hi chris
I am getting temperature between 1K to 20K for 366 cells out of 4,00,000 cells so can I neglect Temperature limited to 1K in .....?
ruturaj171 is offline   Reply With Quote

Old   October 24, 2014, 02:25
Default
  #14
New Member
 
rahul kumar
Join Date: Jun 2014
Posts: 23
Rep Power: 3
R4RAHUL is on a distinguished road
it will not create problem if your temp. is limited 400 cells it will create if it goes upto 40,000.
your meshing has a problem your skewness must be less than 0.8
R4RAHUL is offline   Reply With Quote

Old   June 10, 2015, 08:10
Default
  #15
Member
 
Shane
Join Date: Oct 2009
Posts: 52
Rep Power: 7
sircorp is on a distinguished road
Quote:
Originally Posted by Chris D View Post
This might happen early in your solution, but it should go away as you iterate. What happens is that FLUENT calculates some value that is below 10 K, which is (probably) unreasonable. To keep the simulation from diverging, it discards the value it calculated and uses 10 K insead.

If the warning does not go away as you iterate, try to find where the offeding cell is. You can do this by going to the adapt by iso-value menu and selecting adapt by temperature. Pick a range of temperatures (something like 5 K to 20 K), click "mark", then "manage". A menu will pop up. Now, click "display" and you should be able to see where the cell is that is giving you a problem.

You might find that the cell is near a sharp edge. Since a sharp edge is a discontinuity, FLUENT might have trouble resolving the flow in that region. To fix this, you could add grid in the region of the sharp edge or regenerate your model and round off the edge.

Finally, it might not really matter that much. If it is only one cell out of millions, and it isn't in region in which you are particularly interested, you might be able to just ignore it.
Thanks Chris. I have several hundred orifices which connects two plates. This assembly is inserted in a pipe. When running fluent in pressure based energy solver, I do get same message "temperature limited to 1.00000e+00.

If I give a radius at the plate and orifice corner (at the fluid entry side), will it help to ? Or do I need to give radius on both entry and exit side or it will make no difference what so ever. The flow rate through each orifice is pretty high(more than 50 m/sec).

Currently, test fluid is air. However I wish to use a liquid fluid.

With Regards

SHANE
sircorp 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
Import netgen mesh to OpenFOAM hsieh Open Source Meshers: Gmsh, Netgen, CGNS, ... 32 September 13, 2011 05:50
How to deal with "Temperature limited to 1.000000e+000... Conan FLUENT 0 April 7, 2009 01:40
reversing flow Martin CD-adapco 14 March 18, 2009 09:07
Temparature is limited to 1.00000 in 19879 cells.. srinivas FLUENT 19 February 14, 2006 02:12
physical boundary error!! kris CD-adapco 2 August 3, 2005 00:32


All times are GMT -4. The time now is 19:38.