Replies: 20 comments 26 replies
|
"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. |
|
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. |
|
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. |
|
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. |
|
You also need to measure pressure outside the region where the flow contracts and expands. |
|
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'/ &MESH ID='MESH-01', IJK=44,44,33, XB=-2.375,3.125,-2.875,2.625,0.0,4.125, MPI_PROCESS=0/ &DEVC ID='GAS', QUANTITY='PRESSURE', XYZ=-1.25,0.0,2.875/ &SURF ID='Surface01', &OBST ID='Obstruction', XB=-1.125,-0.875,-1.5,1.0,5.0,6.25/ &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/ &SLCF QUANTITY='PRESSURE', ID='Pressure', PBY=0.0/ &TAIL / |
|
I ran the case. A few comments:
|
|
I wanted to check if there’s something I might be missing in the setup or interpretation. |
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.
|
|
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. |
|
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. |
|
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 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. |
|
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. |
|
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. |
|
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. |
|
A new test bundle has been posted. |
|
Can I check whether any of the newer versions of (FDS) now account for rectangular openings using a discharge coefficient of 0.68 by default? Also, if I want to model an orifice in [CONTAM] which requires inputs such as area, flow exponent, discharge coefficient, and Reynolds number, how can I align or match those inputs so that they are consistent with an FDS model |
|
Try the nightly build of FDS. Note that FDS and CONTAM are completely different models. CONTAM takes a discharge coefficient as input. FDS computes a flow field from which the discharge coefficient can be calculated. |
|
Can I check which version is the night build? |
Following up for completeness - the no slip treatment does have a big impact on the smoke movement in tunnels, especially with arched ceilings. There is more to it in relation to grids as well (need ~0.3 m (max) to 0.2 m (better)) to properly predict backlayering. I am working on a more detailed paper to summarize findings but just wanted to flag that this does have an impact of significance for the tunnel smoke movement. The no-slip treatment gets better agreement with experiment with the free slip predicts more backlayering. |
|
I am attempting to model two staircases with a supply fan, each connecting to a lobby that in turn connects to a corridor with an opening. All doors and openings are modelled as holes. I have attempted this with both the new test version and the old version, and the pressure varies as expected. However, I noticed that the pressure drop across the door results in a Cd that drops below 0.5. Generally, a door or rectangular opening has a discharge coefficient in the range of 0.65 and should not vary significantly with flow rate or configuration. Does this mean the flow is not properly resolved, even though I am using a dense mesh with a few grid cells across the door? |
|
If by a "few grid cells" you mean you just have 3 or 4 cells across the door, then you may not have enough resolution to capture the pressure drop. |
|
I have 8 cells across the door. I have tried with 4 cells and 8 cells and results are quite close |
|
0.65 is representative for a hole on a wall which is sufficiently far from nearby obstructions. Whereas a door is a hole which is closeby to surrounding obstructions. It is flush to ground (there is no contraction from that side), close to ceiling and walls (less contraction). Even moving door location horizontally will affect the wake flow and will change the pressure drop (and Cd) effectively. So, 0.65 is not an accurate fixed number that fits to all rectangular openings. It is recommended to be used if you do not have any other information about the pressure drop over the opening. |
|
Noted however, in my case cd varied from 0.7 to 0.5 while varying flow rate. And based on handbooks and experimental data cd should not change much with flow rate and also for an opening with a same shape (rectangular) pressure drop is governed by orrifice equation |
|
Cd is dependant on Reynolds number, and therefore the velocity. So it can vary. |
|
It is difficult to comment on this without a simple example. The exact geometry may matter. Can you create a simplified version of your case that demonstrates that the orifice coefficient differs from what you expect. Keep in mind that even with 8 cells spanning the opening, that may not be sufficient to capture the details of the flow through the orifice. FDS does not have any sort of empirical orifice flow model. It simply computes the flow and wall friction, which should be close to, but probably not exactly like the real flow. |
|
I want to provide a working link to the paper pdf: https://media.thunderheadeng.net/femtc/2014_d2-11-takacs-paper.pdf. The original Files.Thunderheadeng.com site is no longer in use. |
|
A relevant code change for this Discussion thread is found here |
|
(Seeking a bit more information about how this impacts modeling airflow with the newly released version FDS-6.11.0.) I think the change appears in the FDS 6.11.0 release notes as "New treatment of corner boundary condition," and in the new version of the Technical Reference Guide, section: 4.4.2 Corners, in addition to this code change^ Is the development team planning to document any differences in the V&V guides for 6.11.0? Generally, please share ways to learn more about this subject, if available. Thank you! |
|
A user identified a discrepancy in the results of a simulation. We identified the cause, implemented a fix, documented that fix, created a test case to ensure that the fix stays fixed, and reran all the validation cases in preparation of a minor release. That's about it. We make these kinds of changes routinely, where we see that there is a slightly better way to do something. This forum, the Issue Tracker, and our V&V cases are the primary way we document things. It would be very difficult to write extensive discussions in the manuals about these things, and we don't have time to write journal articles about them, even if those articles were to be accepted. |
|
@mcgratta , since we mention about changes, I would like to ask a tip/recommendation. What is the easiest way to list the changes on the user guide? E.t.c. is there a Github fuction that we can see headings in which a change happened between versions? I usually go through/skim complete user guide page by page but I imagine there might be a more efficient way. Thanks. |
|
There are a few things you can do:
|
|
Thank you for all tips! |
|
For some simulations of Memorial Tunnel fires at 50 MW… FDS 6.7.6 – no backlayering at 2.56 m/s (free stream) Release notes state this for FDS 6.7.8: The treatment stress and vorticity at external "corner edges" has changed. This change was made to fix issues with specified tangential velocity components applied at vents. This change may result is noticeable differences in the flow field near vent outlets for coarse calculations. FDS 6.9 – backlayering at 2.56 m/s Release notes stat this for FDS 6.11: New treatment of corner boundary condition. The corner treatment referred to in this discussion has proven significant for the tunnel backlayering problem. However, I was surprised by the results with earlier versions. I also note that in FDS 6.7.5 I had some models that had more backlayering, however, these models were simulated with much simpler inlet obstructions, and in effect the flow coming towards the fire/ceiling plume had not become fully turbulent. I have since run additional analysis that shows the impact of inlet obstructions (on 6.11) and getting a fluctuating velocity field onto the fire is important and if fluctuations are not present, then the backlayering increases. The change to 6.7.8 was surprising as I thought from this discussion here that this change occurred a long time ago. But it seems that this small change was critical. Any thoughts on the details here of what changed between versions and how it might have affected things? |
|
Looking at the release notes This change in the treatment of corners was done several years before that treatment changed again. Corner boundary conditions are tricky because one could argue for or against a particular treatment because there is no obvious right or wrong. These are approximations made on grids that are fairly coarse. |
|
Is this change (below, for FDS 6.7.8) different to the one implemented in relation to this thread (and now implemented in FDS 6.11), or similar? Release notes state this for FDS 6.7.8: The treatment stress and vorticity at external "corner edges" has changed. This change was made to fix issues with specified tangential velocity components applied at vents. This change may result is noticeable differences in the flow field near vent outlets for coarse calculations. |
|
I'm fairly sure that the change involved similar issues. I'd have to dig into the logs to find out exactly. |
Uh oh!
There was an error while loading. Please reload this page.
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?
All reactions