Coefficient of Discharge

[MAHLY361]

I am attempting to replicate the test using the paper https://files.thunderheadeng.com/femtc/2014_d2-11-takacs-paper.pdf, which validates the test in accordance with EN 12101-2, Annex B, using FDS/PyroSim. However, the pressure values I am outputting are slightly lower than those in the paper, resulting in a higher discharge coefficient (Cd).

Should the pressure be obtained using the pressure gas-phase device as shown below, or do I need to incorporate an additional value?

[drjfloyd]

"slightly different" could have a number of meanings. A couple of comments:

-There is a range of c_d values for an orifce that depends on the geometric details of the contraction and expansion area. Any obstructions inside the vent will also impact the c_d. Your geometry does not appear to be indentical to the paper. Some of this could be your geometry has an expected c_d that differs from the paper

-The paper states:

"The chamber pressure was calculated from integrating the time and space average of the values of the manometer placed near to the four walls. To be noted, these manometers did not indicate any considerable difference in space. The pressure values in time showed some fluctuations. For time integration, the average value was taken into account in a simulation time of 20-25 s. "

You appear to be doing something different. The paper doesn't have the input file or a very detailed description of the pressure measurements. You could try contacting the authors for details on exactly what they did.

[Er9y714]

I had reproduce a few cases from this paper and I remember mesh size, compartment size, measurement points, inlet/outlet VENT locations and flow direction were very important and can change the results. I agree with the comments above. I recommend to model the setup by closely following the information.

[MAHLY361]

Thanks, @drjfloyd and @Er9y714, for your responses. However, this example relates to the coefficient of discharge for rectangular openings, which is typically tested to be around 0.7.
In this paper, although I didn’t fully replicate the position of the pressure points, I did replicate essential data such as the opening dimensions and flow speed and conducted a mesh sensitivity study. I have consistently observed a Cd of 0.78 in this case and others, which is significantly higher than the expected average of 0.7.
I was wondering if I might be missing something, such as adding an adjustment value. My approach involves subtracting the pressure after the orifice from the ambient pressure (0 Pa).

[rmcdermo]

I cannot tell what your grid resolution is here relative to your geometry, but this has a big impact on whether you capture discharge coefficients correctly. You have to resolve (10-20 cells in the recirc zone) the recirculation region that causes the vena contracta.

If you cannot afford to resolve the vena, then FDS provides an HVAC model where you can specify the loss coefficient exactly.

[drjfloyd]

You also need to measure pressure outside the region where the flow contracts and expands.

[MAHLY361]

The text below is my FDS code. I’ve tried measuring further away, but the issue persists.

I note that for many rectangular AOVs, the coefficient of discharge (Cd) typically falls within the range of 0.65–0.7, which aligns with the results published in the referenced paper. However, regardless of parameter changes, I consistently obtain a Cd of approximately 0.78.

Could you provide any input on how to achieve a more accurate pressure drop that matches the expected Cd range (~0.7), in line with the paper’s findings?

Additionally, I’d like to clarify whether the HVAC loss option is applicable in this case. Would enabling it introduce additional losses, or is it redundant if the discharge coefficient for a rectangular opening is already being accounted for in the model?

&HEAD CHID='Louvre_en_test'/
&TIME T_END=30.0/
&DUMP DT_RESTART=300.0, DT_SL3D=0.25/

&MESH ID='MESH-01', IJK=44,44,33, XB=-2.375,3.125,-2.875,2.625,0.0,4.125, MPI_PROCESS=0/
&MESH ID='MESH-02', IJK=44,44,34, XB=-2.375,3.125,-2.875,2.625,4.125,8.375, MPI_PROCESS=1/
&MESH ID='MESH-03', IJK=44,44,33, XB=-2.375,3.125,-2.875,2.625,8.375,12.5, MPI_PROCESS=2/

&DEVC ID='GAS', QUANTITY='PRESSURE', XYZ=-1.25,0.0,2.875/
&DEVC ID='GAS01', QUANTITY='PRESSURE', XYZ=-1.25,0.0,3.875/
&DEVC ID='GAS02', QUANTITY='PRESSURE', XYZ=-1.25,0.0,1.0/
&DEVC ID='GAS03', QUANTITY='PRESSURE', XYZ=-1.25,0.0,2.0/
&DEVC ID='GAS04', QUANTITY='PRESSURE', XYZ=2.25,0.0,2.875/
&DEVC ID='GAS05', QUANTITY='PRESSURE', XYZ=2.25,0.0,3.875/
&DEVC ID='GAS06', QUANTITY='PRESSURE', XYZ=2.25,0.0,1.0/
&DEVC ID='GAS07', QUANTITY='PRESSURE', XYZ=2.25,0.0,2.0/

&SURF ID='Surface01',
RGB=26,204,26,
HEAT_TRANSFER_COEFFICIENT=0.0,
VEL=-0.2/

&OBST ID='Obstruction', XB=-1.125,-0.875,-1.5,1.0,5.0,6.25/
&OBST ID='Obstruction', XB=-2.375,-0.875,-1.5,-1.25,5.0,5.25/
&OBST ID='Obstruction', XB=-2.375,-0.875,0.75,1.0,5.0,5.25/
&OBST ID='Obstruction', XB=-2.375,1.625,-1.25,0.75,5.0,5.25/
&OBST ID='Obstruction', XB=-2.375,3.125,-2.875,-1.5,5.0,5.25/
&OBST ID='Obstruction', XB=-2.375,3.125,1.0,2.625,5.0,5.25/
&OBST ID='Obstruction', XB=-0.875,1.875,-1.5,-1.25,5.0,6.25/
&OBST ID='Obstruction', XB=-0.875,1.875,0.75,1.0,5.0,6.25/
&OBST ID='Obstruction', XB=1.625,1.875,-1.25,0.75,5.0,6.25/
&OBST ID='Obstruction', XB=1.875,3.125,-1.5,1.0,5.0,5.25/

&HOLE ID='Hole', XB=-0.875,1.625,-1.25,0.75,5.0,5.25/

&VENT ID='Mesh Vent: MESH-02 [XMAX]', SURF_ID='OPEN', XB=3.125,3.125,-2.875,2.625,5.2,8.375/
&VENT ID='Mesh Vent: MESH-02 [XMIN]', SURF_ID='OPEN', XB=-2.375,-2.375,-2.875,2.625,5.2,8.375/
&VENT ID='Mesh Vent: MESH-02 [YMAX]', SURF_ID='OPEN', XB=-2.375,3.125,2.625,2.625,5.2,8.375/
&VENT ID='Mesh Vent: MESH-02 [YMIN]', SURF_ID='OPEN', XB=-2.375,3.125,-2.875,-2.875,5.2,8.375/
&VENT ID='Mesh Vent: MESH-03 [XMAX]', SURF_ID='OPEN', XB=3.125,3.125,-2.875,2.625,8.375,12.5/
&VENT ID='Mesh Vent: MESH-03 [XMIN]', SURF_ID='OPEN', XB=-2.375,-2.375,-2.875,2.625,8.375,12.5/
&VENT ID='Mesh Vent: MESH-03 [YMAX]', SURF_ID='OPEN', XB=-2.375,3.125,2.625,2.625,8.375,12.5/
&VENT ID='Mesh Vent: MESH-03 [YMIN]', SURF_ID='OPEN', XB=-2.375,3.125,-2.875,-2.875,8.375,12.5/
&VENT ID='Mesh Vent: MESH-03 [ZMAX]', SURF_ID='OPEN', XB=-2.375,3.125,-2.875,2.625,12.5,12.5/
&VENT ID='Vent', SURF_ID='Surface01', XB=-2.375,3.125,-2.875,2.625,0.0,0.0/

&SLCF QUANTITY='PRESSURE', ID='Pressure', PBY=0.0/
&SLCF QUANTITY='VELOCITY', ID='Pressure01', PBY=0.0/

&TAIL /

[mcgratta]

I ran the case. A few comments:

1. I do not know if this simulation is resolved enough to capture the boundary layer effects, orifice sharpness, etc.
2. I suggest that you repeat the calculation where the flow is in the x direction rather than z. I would just want to eliminate any possibility that there is a background pressure gradient which would confuse the issue.
3. Do you have experimental data for a configuration exactly as you have it? I ask because there are subtle effects like Reynolds number, edge sharpness, etc, that might complicate the result. Usually, these nominal discharge coefficients are for sharp edges, and in FDS you would need a very fine grid to capture these edge effects.

[MAHLY361]

I tried following the example where, as shown, any value of velocity should yield a Cd of approximately 0.68. However, despite changing the velocity in my model, I still consistently obtain a Cd of around 0.78.

I wanted to check if there’s something I might be missing in the setup or interpretation.

[MAHLY361]

I have followed the exact values of this model, yet my output pressure is 1.44Pa, compared to 1.88Pa in the paper, which results in a different CV value.

[mcgratta]

Did you ask the authors of the 2014 paper if they still have the input files? There are several parameters that might be different between your simulation and theirs. There is also the possibility that changes in FDS over the past 10 years have resulted in this difference.

[MAHLY361]

They do not seem available for contact. I have tried different mesh sizes and supply volumes, but I still get the same cv. The pressure I measure is lower than the pressure reported in the paper, which results in a higher cv. I wanted to check if anyone has measured Cv for a typical rectangular opening, in case I am missing something in the output.

[mcgratta]

I ran the case you posted above with the latest version of the FDS source and version 6.0.1 from 2013, the version used in the paper that you cite above. For the old case, the pressure rise in the compartment is 1.59 Pa; for the new it is 1.47 Pa. Assuming that the discharge coefficient is defined $C=(\dot{V}/A) \sqrt{\rho/(2 \Delta p)}$, I get, if I have done the math correctly, a discharge coefficient of 0.74 for the old case and 0.77 for the new. This doesn't completely solve the riddle, but it does imply that there probably has been some subtle change to the wall model or edge condition in FDS over the past 12 years.

This being said, we would want to simulate an actual experiment as faithfully as possible because empirical coefficients typically are not exact values but rather ranges. We would also have to run at finer resolution, etc, as is discussed above.

[mcgratta]

We have looked at cases like yours and compared against correlations reported in the Handbook of Hydraulic Resistance by Idelchik. We are experimenting with a slightly different velocity boundary condition at corners. When I test the new scheme on your case, the discharge coefficient becomes 0.66. I have not checked the Handbook to see what the correlations would say about your specific configuration. Often these correlations refer to so-called "sharp-edged" orifices, as opposed to the "thick-edged" orifice that you have. So it is not clear what one would expect in your case, but I can say that very subtle changes in the way corners are treated can lead to significant changes in discharge coefficient. Stay tuned.

[ShehabGamrah]

Thanks and 0.66 seems like the correct value as per the paper and standard manufacturers data sheet. Can you please share how you achieved the 0.66 value.

[mcgratta]

FDS uses a "wall model" to set the tangential flow velocity at a solid surface. We cannot just assume that the velocity is zero at the boundary, as it is in reality, because the grid it usually too coarse to resolve the rapidly changing tangential velocity just a few mm away from the wall. Instead, the wall model provides a grid-dependent fictitious tangential component of velocity at the wall. This velocity is less than the computed velocity in the first grid cell next to the wall, such that the difference between the two provides the proper stress and vorticity that one would expect. That is the point of a wall model. We have to assume some amount of friction and vorticity induced by the wall that we cannot predict directly unless our grid cells are sub-millimeter in size. Such a simulation would be a DNS.

Anyway, this is all well and good at flat surfaces, but corners are trickier. The techniques for determining what happens at a 90 degree turn are less well known, and over the years we have made subtle changes to how FDS deals with a corner. Sometime between 2013 and now, we made an assumption about the "slip condition", that is, the degree to which we allow the fictitious wall velocity at the corner to be the same as the surrounding flow (free-slip) or zero (no-slip). We assumed the slip condition to be half-way between free-slip and no-slip. This produced reasonable results for some validation cases where we compared velocity profiles. However, we had not considered discharge coefficients. I ran some simple test cases and compared with empirical results of Idelchik. We found that assuming no-slip at corners worked better than the half-slip assumption.

This new version should be out next week as a nightly build, once we pass our verification tests.