CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   When to stop the iteration? (http://www.cfd-online.com/Forums/fluent/117649-when-stop-iteration.html)

oldisbest May 13, 2013 03:22

When to stop the iteration?
 
1 Attachment(s)
Hello,
I have one similified model for micro-channel heat exchanger. Please find the attachment of detailed discription.

only about 0.8 million meshes but quality is bad (several sharp angles near tangency area). Although I'm proficient in Gambit and know the skills to improve the volume mesh quality, I consider my problem as a common case and can be calculated without diverging issue.

So for saving time, I gave up to improve my meshes in all 6 options(1 baseline and 5 modified).

I choose SST-KW with low-RE correlation, and reduce relaxing factors. and what's important, I deactive energy equation for first-round iteration, and all 6 option got perfact results for flow and turbulence equations, converged at about 500 steps.
Then in second-round iteration, I deactive flow and turbulence while active energy equation. As usual, I reduce the convergence residual of energy equation to 1e-8, and add a monitor for mass-averaged temperature at outlet.

The monitored temperature seems change quickly in first 5-10 steps while became almost flat when residual is about 2e-7, then, every 5-6 step, the temperature will still increased by 0.01 degree C.

So I try to resuming the iteration, the residual curve of energy start rising. and then, temperature is out of limitation, that's a signal of divergence.

I found this problem happened in all the 6 options, since the final difference of monitored temperature of each option is smaller then 0.3-0.5 degree C. So in my simulation the results will influenced by whole iteration steps, I am afraid it can't reflect the actual phenomenon.

blackmask May 13, 2013 03:49

There is no option other than improving your mesh. What's the temperate difference between the inlet and outlet? What is the Reynolds number based on channel width? What are the discretization schemes? You should try structured mesh for simple geometry.

oldisbest May 13, 2013 04:08

Re
 
Reynolds number is about 250.
Temperature of air inlet is 35 deg C.
Temperature of heating wall is 50 deg C.

Air outlet temperature based on current CFD results is about 47 deg C.

SIMPLE method and second-order up-stream discretization is adopted except pressure (Standard)

Quote:

Originally Posted by blackmask (Post 427097)
There is no option other than improving your mesh. What's the temperate difference between the inlet and outlet? What is the Reynolds number based on channel width? What are the discretization schemes? You should try structured mesh for simple geometry.


blackmask May 13, 2013 05:17

The flow should be laminar. I did not compute but a 0.3-0.5K temperate different at the different results in large log mean temperature difference, right? The pressure difference is a much more useful indicator for mesh independence. Please find the pressure difference for all six cases.

oj.bulmer May 13, 2013 07:35

You have a conjugate heat transfer, along with not-so-simple flow passage- why do you say you know the simulation is a simple case? Shouldn't the mesh independence study, along with the quality improvement, be on the top of your to-do list?

OJ

oldisbest May 20, 2013 00:25

Quote:

Originally Posted by blackmask (Post 427121)
The flow should be laminar. I did not compute but a 0.3-0.5K temperate different at the different results in large log mean temperature difference, right? The pressure difference is a much more useful indicator for mesh independence. Please find the pressure difference for all six cases.

I saw some persons were using standard k-e model in similar phisical model. and they got the results with 10-15% error (compared with test).

Yes, to adopt laminate flow model with viscous heating, the calculation can be easily converged, and I found the results of flow field is very close to the one with previous sst-kw model.

anyway, I will use laminate flow model later in this kind of problem since its calculation effiency.

To stop the calculation when considering heat transfer I now set the energy residue to default 1e-6.

oldisbest May 20, 2013 00:34

Quote:

Originally Posted by oj.bulmer (Post 427157)
You have a conjugate heat transfer, along with not-so-simple flow passage- why do you say you know the simulation is a simple case? Shouldn't the mesh independence study, along with the quality improvement, be on the top of your to-do list?

OJ

It's a regular case with less than 1 million meshes, incompressible fluid, constant material properties, only conductive and convetive heat transfer involved. In my work, it's really a simple case.

Mesh sensitivity and quality is really important for a new simulation, thanks for your suggestion.

oldisbest May 20, 2013 00:50

My second-round iteration will do some modifications on the model.
I will consider the tube-inside refrigerant flow which is two-phase.
So their will be two kinds of fluid, one is air, the other is two-phase refrigerant(FREON).

Do you know how to do the definition in FLUENT?
I found if two-phase model is activated, the material option in fluid cell boundary condition would be missing. That means the outside air can not be defined.

Can I define it as three-phase flow with air, liquid refrigerant, gas refrigerant.

Quote:

Originally Posted by oldisbest (Post 427087)
Hello,
I have one similified model for micro-channel heat exchanger. Please find the attachment of detailed discription.

only about 0.8 million meshes but quality is bad (several sharp angles near tangency area). Although I'm proficient in Gambit and know the skills to improve the volume mesh quality, I consider my problem as a common case and can be calculated without diverging issue.

So for saving time, I gave up to improve my meshes in all 6 options(1 baseline and 5 modified).

I choose SST-KW with low-RE correlation, and reduce relaxing factors. and what's important, I deactive energy equation for first-round iteration, and all 6 option got perfact results for flow and turbulence equations, converged at about 500 steps.
Then in second-round iteration, I deactive flow and turbulence while active energy equation. As usual, I reduce the convergence residual of energy equation to 1e-8, and add a monitor for mass-averaged temperature at outlet.

The monitored temperature seems change quickly in first 5-10 steps while became almost flat when residual is about 2e-7, then, every 5-6 step, the temperature will still increased by 0.01 degree C.

So I try to resuming the iteration, the residual curve of energy start rising. and then, temperature is out of limitation, that's a signal of divergence.

I found this problem happened in all the 6 options, since the final difference of monitored temperature of each option is smaller then 0.3-0.5 degree C. So in my simulation the results will influenced by whole iteration steps, I am afraid it can't reflect the actual phenomenon.



All times are GMT -4. The time now is 09:48.