
[Sponsors] 
July 6, 2019, 22:56 
Pressure drop across a converging nozzle

#1 
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Hi guys,
I'm currently doing an analysis at work for the pressure drop across a converging nozzle. Nozzle is used for supply air ventilation into a train tunnel. Due to probity and confidentiality I am unable to post any pictures, but here is a brief description of the geometry and flow conditions The nozzle has the inlet, with air flowing horizontally (i.e left to right) and then has a 30degree transition downwards and makes it way to the outlet. The overall length of the nozzle is about 4m. Nozzle Inlet Area: 8m2 Nozzle Outlet Area: 2m2 Nozzle Inlet Volume Flow: 65m3/s Trying to understand: The pressure drop across the nozzle. The boundary conditions i applied in CFX: Inlet: Volume Flow Rate Outlet: Averaged Static Pressure Walls: No slip wall Result: I was getting a whopping 700Pa loss across the nozzle. Comparing this to previous project example, they were getting maximum 60Pa loss across their nozzles of a similar shaped geometry and similar flow rates. Either they were fudging their numbers (i only have a report to read off for their results) or I am doing something wrong. Question: Am I applying the correct boundary conditions for this sort of case in CFX? Is a 700Pa loss across this nozzle really possible? Thanks guys! (First post here ) 

July 7, 2019, 06:42 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,476
Rep Power: 140 
FAQ on accuracy: https://www.cfdonline.com/Wiki/Ansy..._inaccurate.3F
Is it possible to loose 700Pa over a nozzle? Yes, certainly is. You can loose far more than that if you design it that way. Just a wild stab in the dark  are you sure you are accounting for pressure loss due to Bernoulli correctly? That is, the total pressure of the flow? If the previous project reported total pressure and you are reporting static pressure from a region of high flow velocity that could create a huge (and misleading) pressure drop.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

July 7, 2019, 07:35 

#3  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
For my current project, I followed what the previous project report input, which was; Mass flow Inlet, Averaged static pressure outlet. Honestly I am not sure what pressure they were reporting, because it literally just had a table with the pressure loss values. They didn't have any pressure contour plots in the report, which is making me question whether the numbers are correct. I am taking the total pressure from the Inlet minus the Outlet to calc the pressure drop (700Pa). Is this the correct way to determine the PD? And are my boundary conditions correct? (I searched around for internal flow examples and it was mainly Mass Flow Inlet (65m3/s) and Average Static Pressure outlet of (zero)). Cheers. 

July 7, 2019, 19:16 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,476
Rep Power: 140 
Your boundary conditions have to match what you are modelling and I don't know the details of what you are modelling so cannot comment on whether your boundary conditions are correct.
But to reiterate my previous point  You have your outlet as a static pressure boundary at zero pressure. What is the average velocity at this boundary? Does the stagnation pressure of this velocity account for your discrepancy in pressures?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

July 8, 2019, 20:10 

#5  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
1) Inlet = Mass Flow Rate, Outlet = Avg Static Pressure (0Pa Relative Pressure) 2) Inlet = Mass Flow Rate, Outlet = Avg Static Pressure (1atm Relative Pressure) 3) Inlet = Mass Flow Rate, Outlet = Static Pressure (0Pa Relative Pressure) 4) Inlet = Mass Flow Rate, Outlet = Static Pressure (1atm Relative Pressure) I've set monitor points at the inlet and outlet and plotted graphs for "Pressure", "Total Pressure" and "Absolute Pressure". All four cases for Pressure and Absolute Pressure resulted in a 623630Pa drop. Total Pressure didn't give me any values. I also monitored the velocity at inlet and outlet and they were "correct" (compared to basic hand calcs). I guess my final question is, am I using the correct pressure variable for my results. I am getting confused as to what "Pressure", "Total Pressure" and "Absolute Pressure" mean in CFX. I've read up on other posts and can't really grasp what I should be using. Is there anyway to plot on a graph the pressure against the stream flow? Cheers. 

July 8, 2019, 21:09 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,476
Rep Power: 140 
GertJan's post at the end of this is a quick summary of the various pressures: Invalid Exponentiation
I am recommending you check the total pressure drop (not the static pressure drop, which is what "pressure" and "absolute pressure" will give you). The total pressure is the pressure when the flow is brought to a stop with no losses. So for flow with a velocity there will be a dynamic pressure caused by stopping the flow which will increase the pressure. The dynamic pressure is added to the static pressure to give the total pressure. While this may sound confusing, and I am probably not explaining it very clearly  but it is basic and fundamental fluid mechanics so make sure you understand it before proceeding. Any fluid mechanics textbook will have a chapter on this stuff.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

July 9, 2019, 03:46 

#7  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
I do understand that Total Pressure = Static Pressure + Dynamic Pressure (0.5 x density x velocity square). And yes, I am trying to find the Total Pressure Loss across the nozzle. This is what I would be looking for if I was doing hand calcs for the pressure drop across a duct fitting (transition duct, duct bend) for example. I have been measuring Total Pressure from a point at the Inlet and subtracting the Total Pressure from a point at the outlet, and my result is zero. As for Static Pressure, I get a result of 630Pa. Not sure why. I think I am starting to understand what I am modelling. The model is taking the flow into the nozzle, and then supplying it into an open space (0Pa, or 1atm). As the flow exits the nozzle at 32.5m/s (65m3/s divide 2m2 area), there is a big exit loss. If I do a hand calculation for a sudden expansion with a K factor of 1; 0.5*1.213*(32.5)square = 641Pa. Very similar to what CFX is giving me. Is my understanding correct? What I am trying to understand is the pressure loss across the nozzle itself ONLY, not including the exit loss. Is there anyway to model this or post process this number? Thanks. 

July 9, 2019, 19:27 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,476
Rep Power: 140 
If you want the nozzle only then put a surface at the nozzle exit plane and get the area average total pressure. Compare that to the inlet total pressure and you have the total pressure loss.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

July 9, 2019, 20:05 

#9  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
Would you mind letting me know how I can do that? I am assuming I still have to treat the nozzle exit as an "Outlet". And am I trying to put a plane right before the exit and measuring the are avg total pressure there? Or are you talking about something else completely different? I'm not too sure how to put a surface at the nozzle exit plane Cheers 

July 10, 2019, 11:26 

#10 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
So it sounds like you are only modeling the nozzle? And have nothing after the exit modeled?
In that is the case, then exit should already be a plane, so just use the expression: areaAve(Total Pressure)@Inlet  areaAve(Total Pressure)@Outlet. Pictures would help us understand exactly what you are doing. But the way you are doing this (using boundary values to calculate pressure drop) may not be entirely accurate, if you use the total pressure value at your inlet, and are not including anything after nozzle exit. See the discussion here: Calculating Loss Coefficient in 4way Junctions This of course depends on the accuracy you require. 

July 10, 2019, 19:54 

#11  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
However, to be honest, I'm still confused as to what the difference between Total Pressure and Pressure within Ansys CFX. areaAve(Total Pressure)@Inlet  areaAve(Total Pressure)@Outlet: gave me 37Pa areaAve(Pressure)@Inlet  areaAve(Pressure)@Outlet gave me: 650Pa What is the definition and meaning of "Pressure" in CFX? I'm having trouble understanding the User Guide and its definition @.@.... 

July 11, 2019, 02:10 

#12 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,476
Rep Power: 140 
Total Pressure = static pressure +0.5*density*velocity^2.
Pressure = static pressure Looks like my guess that Bernoulli effects are causing your problems was correct Make sure you understand the Bernoulli equation and what it means  there are lots of tutorials on it around, like http://hyperphysics.phyastr.gsu.edu/hbase/pber.html
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. 

July 15, 2019, 04:09 

#13  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
I understand that Total Pressure = "Pressure" + Dynamic Pressure But my results are saying (using the areaAve expression) Total Pressure = 38Pa "Pressure" = 650Pa Can you please try to explain: 1. Why is Static Pressure higher than Total Pressure. 2. Are you able to plot the both pressures against the nozzle "distance" with these numbers? (Starting from Inlet and making your way to the Outlet). I'm struggling to do this Am I getting all the concepts wrong? Thanks so much for you time. 

July 16, 2019, 04:08 

#14  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
My total pressure difference between the Inlet and Outlet is 37.6Pa My pressure (static im assuming) between the Inlet and Outlet is 657Pa. I'm having difficulty relating the total pressure and "pressure" to each other. Inlet Boundary Condition = Mass flow = 78.85kg/s Outlet Boundary Condition = Avg Static Pressure = 0Pa Relative Pressure 

July 16, 2019, 11:17 

#15 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
You have to understand the difference between static and total pressure. It was explained several times, while at the same time, being basic fluid mechanics principals. Total pressure includes the dynamic head.
After you get that, then what I said in the other thread about the 4 way junction applies. The boundaries you are using are not what they will really be. Your inlet has uniform flow velocity coming in. That won't be the case. I would include up and downstream geometry in your simulation, then subtract out their pressure drop contributions. Or put planes at your points of interest. Does the outlet go to a smaller duct, or an exit into a room? Read this thread again: Calculating Loss Coefficient in 4way Junctions 

July 16, 2019, 19:53 

#16  
New Member
Michael
Join Date: May 2014
Posts: 28
Rep Power: 11 
Quote:
I also understand that the current uniform velocity profile entering the nozzle will not be the actual case (hence will be adding safety factor on top of the results, as we always do in engineering). The outlet will be discharging into a large tunnel, so essentially an abrubt expansion right after exiting the nozzle. The "exit loss" with K = 1 for abrupt expansion will be: (0.5*1.213*1)*(32.5)^2 = ~641Pa Ultimately, I want to add the total pressure drop across the nozzle into a total system pressure loss calculation before this "exit loss". So in this nozzle case, as it goes from an opening to a smaller opening, there is a static pressure differential causing the fluid to flow from the inlet to the outlet. As the cross sectional area changes throughout the nozzle, there is a static pressure loss and a dynamic pressure gain (as the fluid velocity is increasing). However, ultimately there will be a total pressure loss across the nozzle (essentially a fitting loss like a bend/transition in the a duct). When I mentioned that I was having difficult relating the static and total pressure, I meant the resulting numbers that I had received. Total pressure: 37.6Pa Pressure: 657Pa Is total pressure not supposed to be larger than static pressure at all times? Unless these values are negative values. So if plotted on a pressure vs distance (as you pass through the nozzle), then 37.6Pa will be plotted higher than 657Pa and both make its way to the 0 value, where the difference between the two lines will be the dynamic pressure value. Reading your 4 way junction post, are you trying to say that the "Static Pressure" that CFX is outputting is including the exit loss? So in my case 657Pa static loss includes the exit loss? So my nozzle static loss would be 657Pa  ~641Pa = 16Pa. So 37.6Pa = 16Pa + Pd, Pd = 21.6Pa? I understand that I should be also modelling upstream and downstream geometry for the nozzle as well, but due to time restraints and limited resources at work, we were hoping to get atleast a total pressure loss value somewhere close to being in the ball park. But I seem to have delved into my own personal brain confusion and am trying to understand what the total and static pressure loss values really mean from CFX. 

July 17, 2019, 13:22 

#17 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
Yes, total pressure is always >= static pressure at any one location, but you are comparing these two pressure values between two different locations. Static pressure loss, vs total pressure loss. Static pressure loss will be greater when transitioning from a larger to smaller cross section as the velocity increases.
Exit loss is not a real thing. It is an acceleration loss from the beginning, where the fluid accelerated from zero velocity to some positive velocity and converted some static pressure into dynamic pressure ((rho/2)*Vel^2). notice this is exactly the pressure drop for K=1 for an exit. We normally do not add it at the beginning as we would have to keep track of the changes the whole time as cross section changed, so it is just added at the end as an "exit loss" So CFX's static pressure difference you show does not specifically include the "exit loss". But it does show what would essentially be the exit loss (exit dynamic pressure) minus the dynamic head at your inlet. See my calcs, this should explain everything: 

Tags 
cfx, nozzle 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how can make normal shock in the nozzle at inlet B.C : Pressure Far field  SonicGhoul  FLUENT  2  May 8, 2016 05:16 
Pressure drop using Fan type BC  Alexis Sack  OpenFOAM Running, Solving & CFD  2  September 22, 2014 09:18 
Mass flow rate prediction of Purge control valve using set pressure drop  enr_venkat  CFX  11  February 27, 2014 11:30 
How to study pressure drop of continous phase in VOF model  sajeesh  FLUENT  4  February 5, 2014 22:01 
compressible flow in a counterflow nozzle  d.vamsidhar  FLUENT  0  November 24, 2005 01:45 