Problem with stabilisation of velocity

[Joshua_Klein]

Hello,

I have a problem with FDS. I want to stabilise a velocity of 2 m/s in a tunnel, but I find no way. I have tried two ways:

1) Establishing a difference of pressure between entry and exit

2) Establishing a supply vent in the entry

What I find in both cases is a velocity field which varies throughout time and oscillates between 0 and 3 m/s. I have waited a long time and it still doesn't work.

I attach the files of both cases.

Thank you very much for your help. Best regards.

[Randy McDermott]

I could not open your zip files.  We would not need anything zipped, just a simple input file.  Attached is a simple version of specifying a velocity inlet that gives 2 m/s in a tunnel.  Are you saying you've tried this and it is not working for you?

--
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+unsubscribe@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/529b533a-5609-4472-80c8-1962fc518183%40googlegroups.com.

For more options, visit https://groups.google.com/d/optout.

[fde]

DYNAMIC_PRESSURE value is 15 Pa only. That will take a quite amount of time to level off in 900m tunnel. 

To try, set pressure to 500 Pa, you will see velocity stables within 1-2 min. The pressure you set might take 20 min simulation time. 

[dr_jfloyd]

Try tightening the VELOCITY_TOLERANCE.  I tightened to 0.01 and at 75 s I am seeing a reasonable looking velocity slice down the center of the tunnel.

On Friday, November 10, 2017 at 10:26:28 AM UTC-5, Randy McDermott wrote:

I could not open your zip files.  We would not need anything zipped, just a simple input file.  Attached is a simple version of specifying a velocity inlet that gives 2 m/s in a tunnel.  Are you saying you've tried this and it is not working for you?

On Thu, Nov 9, 2017 at 7:44 PM, Joshua_Klein <kleinj...@gmail.com> wrote:

Hello,

I have a problem with FDS. I want to stabilise a velocity of 2 m/s in a tunnel, but I find no way. I have tried two ways:

1) Establishing a difference of pressure between entry and exit

2) Establishing a supply vent in the entry

What I find in both cases is a velocity field which varies throughout time and oscillates between 0 and 3 m/s. I have waited a long time and it still doesn't work.

I attach the files of both cases.

Thank you very much for your help. Best regards.

--
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.

[Joshua_Klein]

Hello Mr Floyd,

I have tightened the velocity tolerance to 0.01 and my results don't improve.

I send attach the fds file and the pictures of the instants t=30s, t=60s, t=90s, t=120s, t=150s.

Regards.

[dr_jfloyd]

Are you running the most recent version of FDS?  Did you increase tolerance and maximum pressure iterations?  I do not see this behavior with FDS 6.6 with an increased velocity tolerance (and increased max pressure iterations to ensure the tolerance can be reached).

[dr_jfloyd]

You may also need to tighten the tolerance more.

[Joshua_Klein]

Hello Mr Floyd,

Following your suggestion, I have downloaded the latest version of FDS (6.6.0). I have simulated 180s of the time, and, unfortunatey, the results haven't changed with a tolerance of 0.01 in the velocity. I believe there is something that is not working and I have no idea what it is.

I send you the pictures of the instants t=30s, t=60s, t=90s, t=120s, t=150s, t=180s.

Could you suggest me another measure to solve this problem?

Thank you very much, cheers.

[Randy McDermott]

See if 

&PRES SOLVER='GLMAT' /

helps.  If this does not work, then the problem is not with the pressure solver.

To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+unsubscribe@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/570d6074-2018-44d5-b7e7-8317ae75dfd3%40googlegroups.com.

[Kevin]

This is a one mesh case. I do not believe this has to do with the pressure solver. Rather, I see

PLOT3D_QUANTITY='VOLUME FRACTION','U-VELOCITY','EXTINCTION COEFFICIENT','TEMPERATURE','VISIBILITY', PLOT3D_SPEC_ID(1)='CARBON MONOXIDE'/

in the input file, and then I see figures that seem to have been drawn by some other plotting package, potentially misinterpreting the conventional definitions of a Plot3D file, both NIST and NASA's. What exactly are we looking at here? I am running the case and I do not see anything unusual.

[Joshua_Klein]

What I have found unusual is that the velocity doesn't stabilise throughout time in a single value, but instead, it oscillates between 0 and -3m/s.

What I expected is the velocity stable in -2,1m/s in the whole tunnel.

Regards.

[Joshua_Klein]

By the way, the pictures that I have sent refer to the center of he tunnel (y=0). Unfortunately, I chose y=-4 fo the slice in smokeview, where the velocity varies differently, maybe this is causing some confusion.

Cheers.

[Kevin]

I am running the case called Pr_cond_vel.fds. How are you measuring the velocity? You do not have a VELOCITY slice, and you have changed the default quantities of the Plot3D file. When I view a vector slice, I see a relatively unchanging velocity field, but I cannot determine its speed because I do not see a velocity output.

[Salah Benkorichi]

Well, I'm getting to 2 just by around 50s. I've attached the case here.

On 11 November 2017 at 15:38, Joshua_Klein <kleinj...@gmail.com> wrote:

Hello,

I am measuring the velocity with the Plot3D output file, where the velocity of the full domain is provided, with the aid of the Tecplot software.

If I am not wrong, there is a group of slices in the fds file (the last one that I hace sent), I attach you a capture with the aid of Pyrosim.

Best regards.

To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+unsubscribe@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/2c92ae85-159b-4041-887e-88f3d1d9f973%40googlegroups.com.

[Joshua_Klein]

Hello,

I have put a slice in the center of the tunnel and launch a simulation again. The results in Smokeview confirm that the velocity, if you run longer than 60s, is not stable.

I send you some pictures of the velocity in the center of the tunnel (y=0) of the moments t=60s, t=90s, t=120s, t=170s, t=210s, t=270s, t=320s, t=360s and the FDS file.

I believe this maybe due to the size of the cells in the mesh. This has been calculated with FDS 6.6.0.

[Salah Benkorichi]

Your problem is your outputting U-VELOCITY, 

use the QUANTITY='VELOCITY' 

Check the file that I've attached in my earlier message. 

To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+unsubscribe@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/58d00b65-4f44-4021-a49b-c332be3fe2eb%40googlegroups.com.

[Kevin]

The word "unstable" is inappropriate in this context, for a variety of reasons. Your grid cells are 0.5 m, which is a very coarse grid. At best, you can expect to get the desired integrated volume flow through the tunnel, but that is all. FDS is a large eddy simulation code, so the algorithm is designed to model the turbulence and boundary layer. With such a coarse grid, however, there are limits to what you can expect from the calculation. We tell all users to do a grid resolution study before making any judgments about the "stability" of the simulation. What you really are saying is that the velocity varies as a function of height. Your profile exaggerates the effect of the wall friction because your grid is too coarse. What you might try to do is set FREE_SLIP=.TRUE. on the SURF line and make no attempt to consider the boundary layer.

[dr_jfloyd]

Have you run with the GLMAT solver?  

The default FFT solver will have small velocity errors at the wall. Given the length of your tunnel, even a very small average (~1 mm /s) error would add up to a substantial portion of the volume flow at the inlet; GLMAT will avoid this.