CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User 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 Tree39Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 31, 2009, 04:41
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: 17
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, 17:13
Default
  #2
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 17
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.
teguhtf, sircorp, Mohsin and 32 others like this.
Chris D is offline   Reply With Quote

Old   July 31, 2009, 21:18
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, 07:43
Default
  #4
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 17
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, 15:53
Default
  #5
Senior Member
 
Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 17
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, 13:15
Default
  #6
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 17
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, 09:37
Default
  #7
New Member
 
gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 17
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, 09:31
Default
  #8
los
Member
 
Tiago Macarios
Join Date: Mar 2009
Posts: 35
Rep Power: 17
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
Zari likes this.
los is offline   Reply With Quote

Old   October 19, 2009, 16:08
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.
korcanates likes this.
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: 14
Rep Power: 17
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
Gaurav16420 likes this.
TomP is offline   Reply With Quote

Old   November 15, 2012, 09:43
Default
  #11
Member
 
Join Date: Sep 2011
Posts: 39
Rep Power: 15
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, 10:11
Default
  #12
New Member
 
Join Date: Jan 2014
Posts: 11
Rep Power: 12
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, 03:25
Default
  #13
New Member
 
rahul kumar
Join Date: Jun 2014
Posts: 24
Rep Power: 12
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, 09:10
Default
  #14
Member
 
Shane
Join Date: Oct 2009
Posts: 52
Rep Power: 17
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

Old   April 15, 2016, 11:13
Default
  #15
New Member
 
Gabes
Join Date: Apr 2016
Posts: 11
Rep Power: 10
Grandup is on a distinguished road
Hello ,
i'm done what you said . my case is ( absorption of solar radiation by a liquid (solar salt) between two walls .and the probleme of temperature limited to 1,0000 ..... appear in the 28 iterations when the energy residual intersect with the XYZ velocities . how can i fix this prob ?
Picture 1 the contours distribution after iterations
picture 2 after doing the iso value ... Thanks
Attached Images
File Type: png 16.PNG (15.3 KB, 283 views)
File Type: png 7.PNG (31.3 KB, 247 views)
Grandup is offline   Reply With Quote

Old   January 14, 2017, 09:55
Default Material property variation with temperature
  #16
New Member
 
Amir
Join Date: Sep 2011
Posts: 10
Rep Power: 15
amir00251 is on a distinguished road
You may want to check if the material properties such as specific heat capacity, viscosity, etc are set to change with temperature.
If you have them constant, it creates a domino effect and creates convergency issues for energy.
amir00251 is offline   Reply With Quote

Old   June 7, 2017, 04:33
Default
  #17
New Member
 
Rana
Join Date: May 2017
Posts: 10
Rep Power: 9
Rana shaharyar is on a distinguished road
can some one please tell i am doing turbulence model calculation on 3d wing i have to include heat transfer effects also so plz tell when i have to on my energy equation or i should on my flow and energy equation simultaneously.
Rana shaharyar is offline   Reply With Quote

Old   June 16, 2017, 18:47
Default
  #18
New Member
 
yardena jodeck
Join Date: May 2017
Posts: 29
Rep Power: 9
BlackHeartInertia is on a distinguished road
I what is the problem with that i have that message and it says temperature limited to 1 in 11 cells or in 10 or i 13 but my problem has more than 400000 cells

Sent from my SM-G570M using CFD Online Forum mobile app
BlackHeartInertia is offline   Reply With Quote

Old   December 2, 2017, 16:55
Default
  #19
Senior Member
 
Yuehan
Join Date: Nov 2012
Posts: 142
Rep Power: 14
wc34071209 is on a distinguished road
I am running a transient simulation with dynamic mesh. At some certain time steps, it reports the same message. However, at some other time steps, it runs okay.

I checked the two cells that have temperature less than 1 K. They don't look highly skewed or nonorthogonal. Can somebody tell me why?

Thank you!
wc34071209 is offline   Reply With Quote

Old   June 10, 2019, 10:27
Default
  #20
New Member
 
Join Date: Jun 2019
Posts: 1
Rep Power: 0
jlekuona is on a distinguished road
Quote:
Originally Posted by wc34071209 View Post
I am running a transient simulation with dynamic mesh. At some certain time steps, it reports the same message. However, at some other time steps, it runs okay.

I checked the two cells that have temperature less than 1 K. They don't look highly skewed or nonorthogonal. Can somebody tell me why?

Thank you!
Try refining your mesh in Fluent with the command:
mesh → repair-improve → improve-quality
it worked for me!
hanheihei likes this.
jlekuona is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[Netgen] Import netgen mesh to OpenFOAM hsieh OpenFOAM Meshing & Mesh Conversion 32 September 13, 2011 06:50
How to deal with "Temperature limited to 1.000000e+000... Conan FLUENT 0 April 7, 2009 02:40
reversing flow Martin Siemens 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 Siemens 2 August 3, 2005 01:32


All times are GMT -4. The time now is 12:39.