[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.

[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.

[deepak]

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]

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.

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.

[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?

[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.

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?

[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?

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.

[los]

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]

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]

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

[Kamu]

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]

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]

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]

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

[Grandup]

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

[amir00251]

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.

[Rana shaharyar]

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.

[BlackHeartInertia]

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

[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!

[jlekuona]

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!