Negative value of additional variable

fkzstar · October 13, 2009, 11:19

Hi All,
I've got a question about the additional variable in CFX 11.0.

It's a transient calculation with additional variable set to simulate tracer gas. The additional variable type is 'specific' with a value of 1 at one inlet and 0 at another inlet. When doing contour plots in the post-processing, I found it has a global range of -0.09 to 1.04, which is physicallly unrealistic.

Has anyone got a clue on this?

Thanks in advance.

ghorrocks · October 13, 2009, 20:01

Sounds like a classic boundedness problem. What differencing are you using for advection and time? Is your convergence tight enough.

fkzstar · October 15, 2009, 18:50

Hi Glenn,
Thanks for your reply.

I've chosen high resolution and second order Backward Euler for advection and time scheme respectively. The RMS is 1e-4 due to the limitation of computing resources. The worst overall balance of the additional variable is around 0.05% in all domains.

Looking forward to your reply.

Cheers.

Zaktatir · August 10, 2011, 07:04

Is there no approach to bound that problem of getting negative values for additional variable? (in my case Numberdensity)

ghorrocks · August 10, 2011, 07:43

I think there are methods to impose boundedness restrictions on variables but I have never done it. And in your case, the key problem appears to be loose convergence. Unless you have converged solutions doing anything else is a waste of time.

fkzstar · August 10, 2011, 08:03

forget to mention that it's unsteady calculation, and have reached periodic solutions, so that I believe good convergence is achieved. Also, any lower convergence parameters might lead to much more computational time, but might be worth trying..

Thanks again for your reply,

ghorrocks · August 10, 2011, 18:10

Definitely try tighter convergence first before anything else.

ftab · July 9, 2012, 08:21

Hi,
I know that this is an old thread, but I am facing the same problem of negative concentration and concentration more than 1 in global range of contour, while the boundary is 1 (unboundedness problem) despite the fact that my simulation is steady and the RMS is reached 10-8 for all variables except the additional variable.

Now two questions specially from Glenn:
1- How can I force the solver to converge and lower the RMS for additional variable (mass transport in this case) now that the solution is not segregated and it is not straight forward to use under-relaxation factor?

2- Is this unboundedness, which I am facing, owing to discretization and then unavoidable? or it would still be due to high RMS (10-2) of AV?

Thanks

ghorrocks · July 9, 2012, 08:29

Boundedness problems can also come from the discretisation schemes. Second order schemes can have boundedness problems, even when fully converged. What advection and time scheme are you using? Any other special discretisation?

1 - If all variables are converged except the additional variable then this is usually caused by a massive difference in time scales between the fluid time scales and the additional variable time scales. For instance, imagine a heater in a room. The hot air plume coming off the heater will have a velocity of something like 1 m/s, so has a turn over time of 30s; but it takes the heater hours to heat the room up.

The fix here is to increase the physical time step size so you can advance through time to the converged solution faster.

2 - See above, use a bounded second order scheme like high-res. Also be careful with second order time schemes.

fkzstar · July 9, 2012, 08:44

Hi,

1. for steady calculations, it might be possible to turn off the fluid dynamics and heat transfer equations to get a better convergence of the additional variable, when you believe the other quantities are fully converged. As Glenn suggest, this time you should use bigger pseudo-physical time steps (10-1000 times bigger is possible).

2. To reply Glenn's last suggestion for myself, I tried making the RMS converge to less than 10e-5 in my unsteady calculation, but the results stayed almost the same. Therefore, now I tend to believe this is a problem related to the high resolution scheme.

Quote:

Originally Posted by ftab

Hi,
I know that this is an old thread, but I am facing the same problem of negative concentration and concentration more than 1 in global range of contour, while the boundary is 1 (unboundedness problem) despite the fact that my simulation is steady and the RMS is reached 10-8 for all variables except the additional variable.

Now two questions specially from Glenn:
1- How can I force the solver to converge and lower the RMS for additional variable (mass transport in this case) now that the solution is not segregated and it is not straight forward to use under-relaxation factor?

2- Is this unboundedness, which I am facing, owing to discretization and then unavoidable? or it would still be due to high RMS (10-2) of AV?

Thanks

ftab · July 9, 2012, 11:04

Thank you both Glenn and Joe,

Answering Glenn's question, I am using High resolution scheme, with all default values and setting as I remember that you once wrote here that playing with these setting is quite dangerous and might be trouble some.
There is no other discretization setting for mass and momentum. What do you mean with time scheme? I have used auto time scale with Time scale factor 1.

ftab · July 9, 2012, 11:20

Dear Glenn,
Is there any higher scheme other than high resolution which can lead to better result? Specified blend factor or ...?

ghorrocks · July 9, 2012, 18:49

High resolution is the only scheme which has limiters to keep boundedness. The only other option is upwinding, but you will pay a price with reduced accuracy. Also keep in mind it is the additional variable advection scheme which is the issue, not the momentum equation. Make sure you are changing the advection scheme for the additional variable equation.

The comment about time discretisation is for transient flows. If your flow is steady then ignore that comment.

October 13, 2009, 11:19	Negative value of additional variable	#1
fkzstar New Member Joe Join Date: Mar 2009 Posts: 7 Rep Power: 17	Hi All, I've got a question about the additional variable in CFX 11.0. It's a transient calculation with additional variable set to simulate tracer gas. The additional variable type is 'specific' with a value of 1 at one inlet and 0 at another inlet. When doing contour plots in the post-processing, I found it has a global range of -0.09 to 1.04, which is physicallly unrealistic. Has anyone got a clue on this? Thanks in advance.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[blockMesh] BlockMesh FOAM warning	gaottino	OpenFOAM Meshing & Mesh Conversion	7	July 19, 2010 14:11
Problems with additional variable	Krishna Premi	CFX	1	October 29, 2007 08:19
[blockMesh] Axisymmetrical mesh	Rasmus Gjesing (Gjesing)	OpenFOAM Meshing & Mesh Conversion	10	April 2, 2007 14:00
Multi_component Vs Additional Variable	Anurag	CFX	2	February 4, 2005 16:45
Replace periodic by inlet-outlet pair	lego	CFX	3	November 5, 2002 20:09

October 13, 2009, 20:01		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	Sounds like a classic boundedness problem. What differencing are you using for advection and time? Is your convergence tight enough.

October 15, 2009, 18:50		#3
fkzstar New Member Joe Join Date: Mar 2009 Posts: 7 Rep Power: 17	Hi Glenn, Thanks for your reply. I've chosen high resolution and second order Backward Euler for advection and time scheme respectively. The RMS is 1e-4 due to the limitation of computing resources. The worst overall balance of the additional variable is around 0.05% in all domains. Looking forward to your reply. Cheers.

August 10, 2011, 07:04		#4
Zaktatir Senior Member Join Date: Jan 2010 Location: Germany Posts: 268 Rep Power: 17	Is there no approach to bound that problem of getting negative values for additional variable? (in my case Numberdensity)

August 10, 2011, 07:43		#5
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	I think there are methods to impose boundedness restrictions on variables but I have never done it. And in your case, the key problem appears to be loose convergence. Unless you have converged solutions doing anything else is a waste of time.

August 10, 2011, 08:03		#6
fkzstar New Member Joe Join Date: Mar 2009 Posts: 7 Rep Power: 17	forget to mention that it's unsteady calculation, and have reached periodic solutions, so that I believe good convergence is achieved. Also, any lower convergence parameters might lead to much more computational time, but might be worth trying.. Thanks again for your reply,

August 10, 2011, 18:10		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	Definitely try tighter convergence first before anything else.

July 9, 2012, 08:21		#8
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	Hi, I know that this is an old thread, but I am facing the same problem of negative concentration and concentration more than 1 in global range of contour, while the boundary is 1 (unboundedness problem) despite the fact that my simulation is steady and the RMS is reached 10-8 for all variables except the additional variable. Now two questions specially from Glenn: 1- How can I force the solver to converge and lower the RMS for additional variable (mass transport in this case) now that the solution is not segregated and it is not straight forward to use under-relaxation factor? 2- Is this unboundedness, which I am facing, owing to discretization and then unavoidable? or it would still be due to high RMS (10-2) of AV? Thanks

July 9, 2012, 08:29		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	Boundedness problems can also come from the discretisation schemes. Second order schemes can have boundedness problems, even when fully converged. What advection and time scheme are you using? Any other special discretisation? 1 - If all variables are converged except the additional variable then this is usually caused by a massive difference in time scales between the fluid time scales and the additional variable time scales. For instance, imagine a heater in a room. The hot air plume coming off the heater will have a velocity of something like 1 m/s, so has a turn over time of 30s; but it takes the heater hours to heat the room up. The fix here is to increase the physical time step size so you can advance through time to the converged solution faster. 2 - See above, use a bounded second order scheme like high-res. Also be careful with second order time schemes.

July 9, 2012, 11:04		#11
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	Thank you both Glenn and Joe, Answering Glenn's question, I am using High resolution scheme, with all default values and setting as I remember that you once wrote here that playing with these setting is quite dangerous and might be trouble some. There is no other discretization setting for mass and momentum. What do you mean with time scheme? I have used auto time scale with Time scale factor 1.

July 9, 2012, 11:20		#12
ftab Member Ftab Join Date: Sep 2011 Posts: 87 Rep Power: 14	Dear Glenn, Is there any higher scheme other than high resolution which can lead to better result? Specified blend factor or ...?

July 9, 2012, 18:49		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	High resolution is the only scheme which has limiters to keep boundedness. The only other option is upwinding, but you will pay a price with reduced accuracy. Also keep in mind it is the additional variable advection scheme which is the issue, not the momentum equation. Make sure you are changing the advection scheme for the additional variable equation. The comment about time discretisation is for transient flows. If your flow is steady then ignore that comment.