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

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 July 31, 2009, 03:41 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 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.

 July 31, 2009, 16:13 #2 Senior Member   Chris Join Date: Jul 2009 Location: Ohio, USA Posts: 169 Rep Power: 16 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 31 others like this.

 July 31, 2009, 20:18 #3 New Member   Deepak Thirumurthy Join Date: Jul 2009 Posts: 1 Rep Power: 0 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 ------------------------------------------------------------------------

August 1, 2009, 06:43
#4
New Member

gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 17
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 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.

 August 1, 2009, 14:53 #5 Senior Member   Chris Join Date: Jul 2009 Location: Ohio, USA Posts: 169 Rep Power: 16 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?

August 2, 2009, 12:15
#6
New Member

gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 17
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 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?

August 3, 2009, 08:37
#7
New Member

gnxie
Join Date: Mar 2009
Location: Sweden
Posts: 16
Rep Power: 17
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 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.

 October 2, 2009, 08:31 #8 Member   Tiago Macarios Join Date: Mar 2009 Posts: 35 Rep Power: 17 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.

 October 19, 2009, 15:08 #9 New Member   Join Date: Oct 2009 Posts: 2 Rep Power: 0 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.

 November 19, 2009, 02:32 set the limit yourself #10 New Member   Tom Potters Join Date: Jul 2009 Posts: 14 Rep Power: 16 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.

 November 15, 2012, 08:43 #11 Member   Join Date: Sep 2011 Posts: 39 Rep Power: 14 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!

 October 16, 2014, 09:11 #12 New Member   Join Date: Jan 2014 Posts: 11 Rep Power: 12 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 .....?

 October 24, 2014, 02:25 #13 New Member   rahul kumar Join Date: Jun 2014 Posts: 24 Rep Power: 11 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

June 10, 2015, 08:10
#14
Member

Shane
Join Date: Oct 2009
Posts: 52
Rep Power: 16
Quote:
 Originally Posted by Chris D 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

April 15, 2016, 10:13
#15
New Member

Gabes
Join Date: Apr 2016
Posts: 11
Rep Power: 10
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
 16.PNG (15.3 KB, 271 views) 7.PNG (31.3 KB, 240 views)

 January 14, 2017, 08:55 Material property variation with temperature #16 New Member   Amir Join Date: Sep 2011 Posts: 10 Rep Power: 14 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.

 June 7, 2017, 03:33 #17 New Member   Rana Join Date: May 2017 Posts: 10 Rep Power: 9 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.

 June 16, 2017, 17:47 #18 New Member   yardena jodeck Join Date: May 2017 Posts: 29 Rep Power: 9 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

 December 2, 2017, 15:55 #19 Senior Member   Yuehan Join Date: Nov 2012 Posts: 142 Rep Power: 13 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!

June 10, 2019, 09:27
#20
New Member

Join Date: Jun 2019
Posts: 1
Rep Power: 0
Quote:
 Originally Posted by wc34071209 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!

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post [Netgen] Import netgen mesh to OpenFOAM hsieh OpenFOAM Meshing & Mesh Conversion 32 September 13, 2011 05:50 Conan FLUENT 0 April 7, 2009 01:40 Martin Siemens 14 March 18, 2009 08:07 srinivas FLUENT 19 February 14, 2006 01:12 kris Siemens 2 August 3, 2005 00:32

All times are GMT -4. The time now is 04:16.

 Contact Us - CFD Online - Privacy Statement - Top