MESH Interface

[Chris]

Hi,

Are Mesh-to-Mesh Interfaces better resolved in FDS6 than in FDS5? And are coarse-to-fine-Mesh Interfaces better resolved in FDS6?

Thanks!

Best regards

Chris

[Randy McDermott]

Yes. Much. But read the users guide regarding the PRES line which may be needed in some cases.

--
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/0391eb25-d9a4-4c1b-96e0-18b854c889a8%40googlegroups.com.
For more options, visit https://groups.google.com/groups/opt_out.

[Erik Carlsson]

Hi Randy,

I'm just trying to get my head around what the PRES namelist group actually does. I have read the section about the pressure solver, but am still a little bit unsure about the implications. Can it potentially be a fix for some numerical instabilities? For example, I ran a few different cases with multiple meshes the other day, and they all returned numerical instabilities at the time step when I closed "doors" to half their width.  Looking at the smokeview Plot3D files, it seems like there are massive differences (in the order of 10^6 m/s) in velocity at some mesh boundaries. Could this potentially be solved by experimenting with the PRES group? By disabling the baroclinic torque, the simulations appear to run smoothly (which I also every now and then experienced with FDS 5.5.3). I realise that you may not be able to comment on it without looking into the Plot3D files and the input-files, but perhaps you can... :)

[Randy McDermott]

Eric,

Yes, PRES can help with instabilities. BAROCLINIC is a red herring.

For lack of a better scheme, the default velocity tolerance at a mesh interface is set to some small multiple of the mesh spacing.  This is something we are trying to get a better handle on---I mean, the units are not even consistent.  But the tolerance is problem dependent and tried to choose something that struck a balance between accuracy and speed.

When I am having stability issues, I will typically add a line like:

&PRES VELOCITY_TOLERANCE=0.001, MAX_PRESSURE_ITERATIONS=100/

This says iterate the pressure solver until you have a velocity error (mesh interfaces and solid boundaries) of max .001 m/s (obviously, with a max of 100 iterations).  This can slow things down, but usually you take more of a hit on the front end until the flow field gets well established and then the iteration could becomes reasonable.  It is certainly not as slow as having velocities of 10^6 m/s.

I'll mention that Susan Kilian's efforts in developing a global solver are still in the works.  The pressure iteration scheme is here to hold us over until the global solver is operational and robust.

I also sometimes add a boundary file of velocity error:

&BNDF QUANTITY='VELOCITY ERROR'/

This is helpful if the error is occurring at solid boundaries (usually thin obstructions).

Cheers,

Randy

On Mon, Dec 9, 2013 at 5:30 PM, Erik Carlsson <eco.ca...@gmail.com> wrote:

Hi Randy,

I'm just trying to get my head around what the PRES namelist group actually does. I have read the section about the pressure solver, but am still a little bit unsure about the implications. Can it potentially be a fix for some numerical instabilities? For example, I ran a few different cases with multiple meshes the other day, and they all returned numerical instabilities at the time step when I closed "doors" to half their width.  Looking at the smokeview Plot3D files, it seems like there are massive differences (in the order of 10^6 m/s) in velocity at some mesh boundaries. Could this potentially be solved by experimenting with the PRES group? By disabling the baroclinic torque, the simulations appear to run smoothly (which I also every now and then experienced with FDS 5.5.3). I realise that you may not be able to comment on it without looking into the Plot3D files and the input-files, but perhaps you can... :)

--

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/c16212ce-0070-465b-b447-6646aa05b626%40googlegroups.com.

[Chris]

&PRES VELOCITY_TOLERANCE=0.001, MAX_PRESSURE_ITERATIONS=100/

 

Is this kind of Default-Value to get a reasonable result or how do I get these PRES-Quantities right without doing a sensitivity-analysis?

[Randy McDermott]

I wish I had an easy answer.  As a user you need to decide how tight you want to make the mesh-to-mesh velocity tolerance and the impermeability condition (zero normal velocity) at solid boundaries (obstructions).  If you want this tolerance to be 10^-10, you will have a very slow code.  At the moment the best I can do is point you to the validation guide where you will see that our default tolerance seems to work for a wide variety of problems.  Pick a problem that most closely relates to yours and see how we handled it.  I would also suggest playing with the problem:

FDS-SMV/Verification/Pressure_Solver/duct_flow.fds

to see the effect of changing the parameters (this case is shown in Sec. 6.6 of the user guide).

In general, you will find that for external flows (plumes) the default tolerance does not need modification.  But for internal flows (ducts) you usually need a tighter tolerance so that what you push into a duct is the same volume as what comes out of it.  Of course, this is especially important if the duct flow is the ventilation source for a fire.

--

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/f0c99d88-9584-42e9-a284-062c1904e307%40googlegroups.com.

[Chris]

Thanks!

Am Sonntag, 8. Dezember 2013 17:23:42 UTC+1 schrieb Chris:

[Erik Carlsson]

Thanks Randy, that explains it really well! And in fact, the numerical instability doesn't occur now that I've re-enabled the baroclinical torgue and added the line

&PRES VELOCITY_TOLERANCE=0.001, MAX_PRESSURE_ITERATIONS=100/ 

Does anyone have any indicative numbers on the time added as a result of lower velocity error tolerance and increased pressure iterations?  I know it probably won't be directly translatable to my model, but may give an indication...  The above works for me with 0.2 m and 0.4 m cell sizes, whereas if I don't specify it, the velocity tolerance would be 0.1 m/s and 0.2 m/s, being 100 and 200 times bigger than my manually specified tolerance, plus 10 times more iterations.  It seems like that could be quite computationally costly...  (and yet I don't know if using more tolerance and less iterations will in fact result in numerical instability)

[Randy McDermott]

I have watched the development of linear solvers for the Poisson equation for 15 years now.  It is still very problem dependent and system dependent.  This is why solver libraries like hypre http://acts.nersc.gov/hypre/ give so many options.  I recommend first doing a simple analysis to see what kind of tolerance you can bear.  For example, you might say that a 1% error in your volume flow is acceptable (what's the uncertainty in your model to begin with? probably more than 1%).  What velocity error does this correspond to? (divide by a characteristic area).  Play with max pressure iterations to make sure you achieve this error within reason most of the time.  I find that 100 is a reasonable number.  Because our brute force iteration scheme to smooth the mesh boundary error converges slowly, using 1000 or so for max press it can be brutally slow and may not buy you much.  But again, I think you have to start with being honest about the error you are willing to accept in the volume flow.

--

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/61f48a12-7b88-47e8-979c-7602097725e0%40googlegroups.com.