Numerical Instability Error

[Timea Marton]

Hello,

 

I am currently running a simulation on FDS6.1.0, of a model with about 38 million cells. The domain is divided in 4 meshes, with cubic cell size dimensions of 20 cm over the entire domain.

The simulation is a car park setup, where the fire starts inside one car. The burner inside the car follows a prescribed design curve and should spread to the tires where an ignition temperature is set. And then supposedly to the other cars. However the simulations stops due to a Numerical Instability error at around 455 second. I have tried to find the reason by the guidelines given in the User Guide, however as it is the first time encountering such an error, this is new to me. 

• First I have looked at the Plot3D files. At time 455 the temperature distribution looks abnormal to me, as it is not uniformly distributed, and i also don't understand why the values are this low. It is  Is it possible that the instability is caused by this. If yes any hints on why this happens?

• The aspect ratio of the mesh size is no larger than 2, as all mesh cells are 20 cm, so this can not be the cause of the error.

• I would not say that the flow through the car openings represents a high speed flow through a small opening. The pressure change after the windows breaking at time 151 (which are partly open in the first car) occurs long before the instability.

• There is no sudden change in the HRR occurring at this time. In fact the HRR should be constant from 240seconds until 960s.

• The velocity files seem to show a smooth passing of the information from one mesh to another.

Can the material properties have anything to do with the error?  Could you please  give some hints on how else i can find the problem, or if i am interpreting something poorly? Any help would be kindly appreciated.

I have attached the .fds and smokeview file. The .fds file contains a lot of information about the car geometry, which i can take out if it makes it easier to read. Please let me know if there is anything i should upload, 

Thank you for your time.

Best regards,

Timi

 

[Randy McDermott]

Timi,

Once things go unstable, all bets are off with maintaining temperature bounds.  So temps below 20 C are not surprising in your plot.

It is, of course, nearly impossible to say what is causing the problem without taking on the case as an issue.  But, you might consider adding a PRES line to tighten the velocity tolerance.  Also, you can add CHECK_VN=T to MISC.  These are the first things I do if I get an instability.

&MISC CHECK_VN = .TRUE. /

&PRES VELOCITY_TOLERANCE=0.01, MAX_PRESSURE_ITERATIONS=100 /

The velocity tolerance is a guess.  Look at your .out file.  What kind of tolerance is the case holding?  How many pressure iterations is it taking?  You might need VEL_TOL=0.001.

I don't know if you jumped straight to this big a case.  But I always recommend starting with a small (coarse), single mesh case to shake down the setup.  If the above does not help, then that is the route we would have to take to start debugging.

R

--
You received this message because you are subscribed to the Google Groups "FDS and Smokeview Discussions" group.
To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+u...@googlegroups.com.
To post to this group, send email to fds...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/3059f675-adf3-442e-a713-eda958fbdf16%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

[Timea Marton]

Thank you for your quick reply.

I will first try as you suggested. I have looked at the output file and the maximum velocity error varies between numbers of the order 0.2E-02 to 0.9E-01, the latter being valid for the time closer to the instability. However at the time of the instability this number changes to an order of E+01 and E+02. I am not sure what this means.I have set the VEL_TOl to 0.001.

As for the pressure iterations , this varies from 1-10.  I have set it as suggested to 100.

I have not jumped into this big case. In my first simulations i have used simple rectangular burners, like boxes and have run the simulations with one mesh. However i did not run the more complex geometry with one mesh. I shall try that as well.

If this does no work out should i post here, or should i post on the issue tracker?

Thank you for you help,

Timi

[Brad Casterline]

I just want to mention something I have experienced but have no explanation for; a car park using small impulse fans to direct the flow toward large exhaust shafts. The entry and exit were large and always open, and the HRR was prescribed and reached steady state at about 400 sec. 1800 sec sim taking 3 weeks to complete. I had already had successful runs with the fire located in other areas. I had set RESTART to 200 sec. After 2 weeks of running it, just short of 1200 sec sim, I got a numerical instability. I checked for sudden changes, but found none. I simply restarted it, and it went from 1000 to 1800 without an instability, and with similar results to the previous runs!!!

[Randy McDermott]

Instabilities happen for a couple of reasons:

1. There may be a bug in the code.  Obviously, we try to avoid these.  But they exist.  We track down every one of them that we can reasonably get our hands on.  We have hundreds upon hundreds of test cases that we run.  If a single case goes unstable, we fix it before releasing the code.  That said, there are thousands of users with thousands of problems.  We ask your patience in helping us track down bugs.

2. You hit a Courant or Von Neumann instability.  The solutions to these problems are: (a) reduce the time step or (b) ignore the physics.  There are no proofs for stability constraints for the Navier-Stokes equations in 3D.  We base our time step restrictions on simplified linear analysis.  To be safe, you could cut the time step in half... then the code takes at least twice as long to run: 6 weeks instead of your 3.  Or, you could add so much dissipation that you need 4 times the resolution to get anything like an accurate result (see the move_slug.fds case in the verification suite).  4 times the resolution takes 256 times as long to run.

The reason a restart might not go unstable is that, if you are on the edge of an instability, minor changes can put you back in line.  If you don't believe how sensitive numerical results can be to the time step restriction, you should solve the heat equation with a first order explicit scheme with VN of 0.49999999 and 0.500000001.  The former is stable and accurate, the latter is garbage.

On Sun, Jul 20, 2014 at 2:03 PM, Brad Casterline <bcast...@fsc-inc.com> wrote:

I just want to mention something I have experienced but have no explanation for; a car park using small impulse fans to direct the flow toward large exhaust shafts. The entry and exit were large and always open, and the HRR was prescribed and reached steady state at about 400 sec. 1800 sec sim taking 3 weeks to complete. I had already had successful runs with the fire located in other areas. I had set RESTART to 200 sec. After 2 weeks of running it, just short of 1200 sec sim, I got a numerical instability. I checked for sudden changes, but found none. I simply restarted it, and it went from 1000 to 1800 without an instability, and with similar results to the previous runs!!!

--
You received this message because you are subscribed to the Google Groups "FDS and Smokeview Discussions" group.
To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+u...@googlegroups.com.
To post to this group, send email to fds...@googlegroups.com.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/9c532c65-8e58-422d-a1b6-0126cb2c00d8%40googlegroups.com.

[Brad Casterline]

Thank you Dr. McDermott, you ALL certainly have my patience, and great gratitude for what you are doing!