CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS (http://www.cfd-online.com/Forums/ansys/)
-   -   How to slove "temperature limited to 1.0000e+00001 in cells.." (http://www.cfd-online.com/Forums/ansys/67016-how-slove-temperature-limited-1-0000e-00001-cells.html)

Conan July 31, 2009 03:41

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

Chris D July 31, 2009 16:13

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.

deepak July 31, 2009 20:18

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
------------------------------------------------------------------------

Conan August 1, 2009 06:43

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 (Post 224905)
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 August 1, 2009 14:53

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 August 2, 2009 12:15

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 (Post 224963)
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 August 3, 2009 08:37

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 (Post 224993)
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.


los October 2, 2009 08:31

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

abrar October 19, 2009 15:08

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.

TomP November 19, 2009 03:32

set the limit yourself
 
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

jbrace December 4, 2009 15:32

this is a hard problem to figure out.

Kamu November 15, 2012 09:43

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!

ruturaj171 October 16, 2014 09:11

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 .....?

R4RAHUL October 24, 2014 02:25

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

sircorp June 10, 2015 08:10

Quote:

Originally Posted by Chris D (Post 224905)
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


All times are GMT -4. The time now is 20:41.