Differing results in modeling a square diffuser using HVAC vent surface on FDS

[elangsz]

Hello im trying to model a 400 mm x 400 mm square diffuser using FDS with a flowrate of 500 cfm (0.24 m3/s), here are the flow parameters and dimensions (free area is the gap on the diffuser)

So the important parameter to take from the calculation above is to make a boundary vent that delivers 500 cfm of air, with a resultant velocity of 4.92 m/s thats directed 15 - 30 degree from ceiling level (based on actual diffuser specs), heres the fds diffuser model parameters

so to model the diffuser i created four separate HVAC supply vents, each with the size of 300 mm x 150 mm that have a flowrate of 125 cfm (500 cfm divided by 4, due to 4 separate vents), connected to the return HVAC vent via ducts and nodes, in which the supply vents are positioned at the ceiling level which is Z = 3 and the return vent on the floor which is Z = 0. Based on my calculation i shared with you on the above, the normal velocity (W velocity) is 1.31 m/s with the tangential velocity (U or V velocity, depending on which vent) is 4.738 m/s in order to get a resultant velocity of 4.92 m/s thats directed 15 - 30 degree from ceiling level

ok now to verify whether my input is already correct or not, i put up some devices. First is the surface integral to measure flowrate at each of the HVAC supply vents (in which its already showing 125 CFM per vent as expected), then i also put a device to measure the normal velocity of the HVAC supply diffuser (already showing a normal velocity of about 1.31 m/s for every supply vent as expected). After that i also wanted to make sure that the tangential velocity (U or V velocity) on the HVAC supply vent shows a value of about 4.7381 m/s so i put up a gas phase device to measure either the U or V velocity at the diffuser level (3 m, and the result is zero) and a level below it (2.85 m), however the results from these gas phase device are far from 4.7381 m/s. The tangential velocity of vent 1 (about 2.4 m/s) is different to whats shown for vent 2-4 (about 0.9 m/s). I also put some slices to measure the U/V velocity and velocity (resultant velocity, as i understand it) on the X and Y plane and it is shown that the maximum value of the U/V velocity is about 4.7381 m/s whereas the velocity is only about 2.556, why is it different? just wanted to make sure before i use this small model to on a larger scale simulation

ok now to sum up my questions

1. How can i make sure that my diffuser model is working as intended? so far the parameter that i made sure is only the normal velocity of the HVAC supply (via solid phase and gas phase device at the vent boundary) and the flowrate (via spatial integration of normal velocity at the vent boundary)
2. How can i make sure that my HVAC vent louver direction (as per user guide section 10.2.7) is correct? based on the normal velocity of 1.31 m/s and tangential velocity of 4.7381 m/s i input the UVW = 0,3.614,-1 (vent 1)
3. Why does the U velocity and V velocity slice at Y = 4 shows different value compared to velocity at Y = 4

Since there hasn’t been much discussion on implementing HVAC vents with louvers on this page, I hope this post can shed some light on how to effectively model an HVAC diffuser in FDS. Ive also attach the FDS file and device file if anyone wants to check on it. many thanks!

device results file
device results.csv

FDS file
square diffuser test.txt

diffuser parameter excel file
diffuser flow parameter.xlsx

[drjfloyd]

Going to convert this to a discussion.

[drjfloyd]

The only way to introduce mass into the domain via a VENT is the normal flow. Tangential flow cannot add masss. You should set the HVAC VOLUME_FLOW to the flow into the domain you want.

In terms of the tangential flow your vents are 2 cells x 1 cell in size. With only a couple of grid cells across the vent, you are not well resolved, and there is only so much you should expect in terms of getting the flow angle you input. You may want to make simple test case where you just have a vent on the ceiling in an otherwise open domain with a 2:1 aspect ratio and look to see how the resulting flow changes as you vary the resolution.

[elangsz]

Noted, thank you for the clarification.

Regarding the flowrate of the supply vent, the solid surface measurement device has confirmed that each vent delivers 125 CFM (total: 500 CFM). I’ve also entered this value using the HVAC VOLUME_FLOW parameter as youve mentioned earlier, so I consider this matter resolved.

As for the resolution variation, I’ll give it a try and will update here once I have the results. Another question—if refining the resolution shows that it’s working as intended, does that confirm my input is already correct? And if I use that same diffuser model for a simulation of a large mall lobby, where the main focus is thermal comfort near ground level, but keep the mesh around the diffuser coarse (since it’s not the main focus), would the results still be acceptable?

[drjfloyd]

I cannot judge acceptability of results for you. The tolerable error for an analysis is something that you the model user plus any stakeholders need to determine. I recommend doing a grid study to assess how coarse you can make your grid. Assuming you have a large open area with multiple supply vents that are equally spaced, you try something like model a single vent with symmetry conditions on the sides to limit the domain size and use that as a surrogate geometry for the grid study.

[elangsz]

Awesome, that really clears up how I should approach this—specifically regarding the mesh sensitivity study. I’ll make sure to do that, thank you.
Now, one more thing: regarding my earlier question on the velocity slice versus the U or V velocity slice—why do the values differ so much? I’ve shared the slice images as well. Based on my calculations (Excel file), the resultant velocity near the diffuser should be at least around 4.92 m/s, with the tangential velocity at 4.74 m/s. The U velocity slice shows 4.74 m/s as the maximum value (as expected), but the velocity slice only shows 2.556 m/s. Why is that?

[drjfloyd]

The default slice file format shows an interpolated value to enable drawing smooth contours. A CELL_CENTERED slice shows the actual cell value.

The slice is showing the velocity in the gas which is going to be the result of how the boundary condition at the wall interacts with the bulk flow in the domain. You only have two cells for the vent and cannot expect to be well resolved for the flowfield adjacent to vent.