Density/Temperature problem

Maddin · May 28, 2009, 10:08

Hey guys,

I've got a problem and i have no idea what I can do.
I have a pipe, in this pipe I have a second smaller pipe.
In each pipe is a gas.
The gas in the big pipe has 300°C and the gas in the small pipe has 25°C.
When I make a run the Energy and the second gas don't converges.

When I look at the density or temperature in the geometry scene I see the problem.

3-5 cells after the inlet of the second gas the temperature raises up to 500°C and the density falls down.

What is here the problem what I have?
The mesh looks really good.
The gas is non reacting when this is important.

When I find no solution I will ask the support...

vishyaroon · May 28, 2009, 12:32

Is this a conjugate heat transfer problem? If so you may want to check the solid-fluid interface.

Maddin · May 28, 2009, 16:06

I want to see the "mixing" of the two gases.
But I think the problem is maybe the second small pipe for the second gas.
I will make a run without the second gas, maybe there is already the problem.

Maddin · May 29, 2009, 04:25

So the run is still working. Energy is still on a high level (1.55...E-01) and didn't change very much.
Mesh looks good (had made it very fine around the zone which made problems).
I will try to make a run without pipe... or change the AMG solver? What do you think?

Any ideas how I can bring the second gas into the middle of the other pipe?

SKK · June 2, 2009, 08:50

You can remove the cells where the temperature is higher than what is realistic. This will replace these 'offending' cells with symmetry boundary cells. This might get rid of your problem, but only do so if only relatively small number of cells are causing problem.

Maddin · June 2, 2009, 13:19

There were only 3-5 cells where I have the problem.
The temperature is lower now. I have made the cell size smaller in this area. Tomorrow I should know if it works.

/edit: How can I remove this "bad" cells?

xamo · June 3, 2009, 03:36

Hi,

my experience is, that AMG is better for such problems than CG. Also always use double precision.

If you do not have conjugate heat transfer in solid you can try to switch the bad cells into solid and they will be ignored during the calculation.

Regards
xamo

Maddin · June 3, 2009, 04:01

With the smaller cells the temperature peak is no problem anymore.
But the energy converged very slow, the second gas also converged very slow.

What is "CG"?

xamo · June 4, 2009, 02:03

Hi,

i´m sorry, I thought this is a STARCD problem....

In STARCD under Solution Method (for Scalar Solver Type) you can choose CG (default) and AMG. CG stands for Conjugate Gradient (algorithm).

I do not know if you can choose this in CCM+.

Regards
xamo

Maddin · June 4, 2009, 03:02

Hmm I tried to simulate a test case and there is the same problem.
Mesh is very fine, don't have any idea.
Will make a "simple" case today and then look if there is the same problem.
When I can't get a solution I will speak to the support.
Maybe one bug more...

SKK · June 4, 2009, 04:53

Both in Fluent and STAR CCM+ energy converges slowly. Also, the make note that the residuals are 'normalised' so the actual values may be very small.

In STAR CCM+ you do not have the luxury of changing AMG to CG (as far as I know).

The reason you have high temperature in those few cells is because the final qulaity of those cells either after finite volume or interface creation were compromised. This is why you can either remove these cells or remesh to create better quality cells (as you have done). To remove these high temperature cells use split by function (temperature in your case, you may have to use derived part to set the criterion you need). Then you can either delete these newly created region or set the physics to null.

Also another method to removel bad cells in general is to right click on the region and select remove invalid cells. This process will create a separate region with bad cells and set them to symmetry boundary conditions. You can either delete them or leave them.

I found in some cases I have had to use both of the above methods to get the solution to work. In some cases you have to 'initialise' the solution before removing invalid cells and then re-initialise the solution WITHOUT removing solution. This is especially the case when you are creating these bad cells during the 'interface' creation stage as you initialise the solution.

Hope this helps.

Maddin · June 4, 2009, 06:37

Thanks for you answer.
I have shown it a other guy and I think we have found a solution.
I didn't had changed the specific heat etc. in my gas components, we think because of the different density the solver tried to balance this difference with this high temperature.

May 28, 2009, 10:08	Density/Temperature problem	#1
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	Hey guys, I've got a problem and i have no idea what I can do. I have a pipe, in this pipe I have a second smaller pipe. In each pipe is a gas. The gas in the big pipe has 300°C and the gas in the small pipe has 25°C. When I make a run the Energy and the second gas don't converges. When I look at the density or temperature in the geometry scene I see the problem. 3-5 cells after the inlet of the second gas the temperature raises up to 500°C and the density falls down. What is here the problem what I have? The mesh looks really good. The gas is non reacting when this is important. When I find no solution I will ask the support...

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
UDF compiling problem	Wouter	Fluent UDF and Scheme Programming	6	June 6, 2012 04:43
Incoherent problem table in hollow-fiber spinning	Gianni	FLUENT	0	April 5, 2008 10:33
natural convection problem for a CHT problem	Se-Hee	CFX	2	June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem)	ParodDav	CFX	5	April 29, 2007 19:13
Is this problem well posed?	Thomas P. Abraham	Main CFD Forum	5	September 8, 1999 14:52

May 28, 2009, 12:32		#2
vishyaroon Senior Member Aroon Join Date: Apr 2009 Location: Racine WI Posts: 148 Rep Power: 17	Is this a conjugate heat transfer problem? If so you may want to check the solid-fluid interface.

May 28, 2009, 16:06		#3
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	I want to see the "mixing" of the two gases. But I think the problem is maybe the second small pipe for the second gas. I will make a run without the second gas, maybe there is already the problem.

May 29, 2009, 04:25		#4
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	So the run is still working. Energy is still on a high level (1.55...E-01) and didn't change very much. Mesh looks good (had made it very fine around the zone which made problems). I will try to make a run without pipe... or change the AMG solver? What do you think? Any ideas how I can bring the second gas into the middle of the other pipe?

June 2, 2009, 08:50		#5
SKK Member Join Date: Mar 2009 Posts: 55 Rep Power: 17	You can remove the cells where the temperature is higher than what is realistic. This will replace these 'offending' cells with symmetry boundary cells. This might get rid of your problem, but only do so if only relatively small number of cells are causing problem.

June 2, 2009, 13:19		#6
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	There were only 3-5 cells where I have the problem. The temperature is lower now. I have made the cell size smaller in this area. Tomorrow I should know if it works. /edit: How can I remove this "bad" cells?

June 3, 2009, 03:36		#7
xamo New Member Join Date: Mar 2009 Posts: 20 Rep Power: 17	Hi, my experience is, that AMG is better for such problems than CG. Also always use double precision. If you do not have conjugate heat transfer in solid you can try to switch the bad cells into solid and they will be ignored during the calculation. Regards xamo

June 3, 2009, 04:01		#8
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	With the smaller cells the temperature peak is no problem anymore. But the energy converged very slow, the second gas also converged very slow. What is "CG"?

June 4, 2009, 02:03		#9
xamo New Member Join Date: Mar 2009 Posts: 20 Rep Power: 17	Hi, i´m sorry, I thought this is a STARCD problem.... In STARCD under Solution Method (for Scalar Solver Type) you can choose CG (default) and AMG. CG stands for Conjugate Gradient (algorithm). I do not know if you can choose this in CCM+. Regards xamo

June 4, 2009, 03:02		#10
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	Hmm I tried to simulate a test case and there is the same problem. Mesh is very fine, don't have any idea. Will make a "simple" case today and then look if there is the same problem. When I can't get a solution I will speak to the support. Maybe one bug more...

June 4, 2009, 04:53		#11
SKK Member Join Date: Mar 2009 Posts: 55 Rep Power: 17	Both in Fluent and STAR CCM+ energy converges slowly. Also, the make note that the residuals are 'normalised' so the actual values may be very small. In STAR CCM+ you do not have the luxury of changing AMG to CG (as far as I know). The reason you have high temperature in those few cells is because the final qulaity of those cells either after finite volume or interface creation were compromised. This is why you can either remove these cells or remesh to create better quality cells (as you have done). To remove these high temperature cells use split by function (temperature in your case, you may have to use derived part to set the criterion you need). Then you can either delete these newly created region or set the physics to null. Also another method to removel bad cells in general is to right click on the region and select remove invalid cells. This process will create a separate region with bad cells and set them to symmetry boundary conditions. You can either delete them or leave them. I found in some cases I have had to use both of the above methods to get the solution to work. In some cases you have to 'initialise' the solution before removing invalid cells and then re-initialise the solution WITHOUT removing solution. This is especially the case when you are creating these bad cells during the 'interface' creation stage as you initialise the solution. Hope this helps.

June 4, 2009, 06:37		#12
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	Thanks for you answer. I have shown it a other guy and I think we have found a solution. I didn't had changed the specific heat etc. in my gas components, we think because of the different density the solver tried to balance this difference with this high temperature.