# Pressure drop at various pipe locations

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 March 10, 2017, 11:20 Pressure drop at various pipe locations #1 New Member   Inderjeet Singh Join Date: Feb 2017 Posts: 8 Rep Power: 9 Hello all, I have to perform a 3-D CFD analysis of air flow in a pipe using Fluent. Experimentally the inlet is attached to blower for providing some fixed mass flow rate or velocity. The length of pipe will be say 50 inches and i have to measure pressure at 5 diff. locations say- 5, 10, 20,30,40, and outlet at 50 inches. Q 1. What will be best model for analysis ? Q 2. Which type of boundary conditions should be applied at inlet and outlet - Velocity inlet and pressure outlet ? Q 3. How can i measure pressure difference at those 5 locations. Q 4. Will "Pressure-outlet" boundary condition by default sets Outlet pressure to Atmospheric pressure ?? Q 5. Will there be difference in these 2 Cases - Case A - Modelling full 50 inches and calculating pressure difference at 5 locations from one Simulation. Case-B - Modelling 5 lengths differently and analyze them separately with Pressure-Outlet boundary condition. I would like if the answer mentions to my question number. Thanx in advance Last edited by Inderjeet Singh; March 10, 2017 at 11:26. Reason: missed some points to mention

 March 11, 2017, 06:57 #2 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,686 Rep Power: 66 1. What physics are you trying to model? Choose the model that contains those physics. 2. Never ask someone else what your boundary conditions are. You are always responsible for knowing this. If you don't, then go meditate until you do. Just like in mathematics, your problem is not specified until you have a a domain, governing equations, boundary conditions, and initial conditions. 3. Define a precise definition of pressure difference. Do you mean difference in pressure between two points, difference in average pressure between two planes? What are the planes, what are the averages? And then do so in Fluent. In Fluent it's very easy to export pressure at probe points and surfaces. And then you can calculate pressure drop on your own after. 4. The default value pressure outlet is 0 Pa. The default operating pressure is 101325 Pa. It is so easy to change these numbers though, does it really matter what the default settings are? 5. Yes there will be a difference, but arguably a small one. First, your mesh will not be the same, so you will end up with different results. Second, if you have the same velocity inlet and same atmospheric pressure at the outlet, you'll end up with different massflows. Third, even if you changed the outlet pressure for each case, at a pressure outlet boundary you are imposing a certain distribution (default uniform) for the pressure which may not match the distribution the flow would normally have. Therefore, in general, I recommend you do Case A. You can do Case B if you can't afford the computation. However, these days RAM and cpuhours are really cheap. Inderjeet Singh likes this.

March 13, 2017, 09:26
#3
New Member

Inderjeet Singh
Join Date: Feb 2017
Posts: 8
Rep Power: 9
Quote:
 Originally Posted by LuckyTran 1. What physics are you trying to model? Choose the model that contains those physics. 2. Never ask someone else what your boundary conditions are. You are always responsible for knowing this. If you don't, then go meditate until you do. Just like in mathematics, your problem is not specified until you have a a domain, governing equations, boundary conditions, and initial conditions. 3. Define a precise definition of pressure difference. Do you mean difference in pressure between two points, difference in average pressure between two planes? What are the planes, what are the averages? And then do so in Fluent. In Fluent it's very easy to export pressure at probe points and surfaces. And then you can calculate pressure drop on your own after. 4. The default value pressure outlet is 0 Pa. The default operating pressure is 101325 Pa. It is so easy to change these numbers though, does it really matter what the default settings are? 5. Yes there will be a difference, but arguably a small one. First, your mesh will not be the same, so you will end up with different results. Second, if you have the same velocity inlet and same atmospheric pressure at the outlet, you'll end up with different massflows. Third, even if you changed the outlet pressure for each case, at a pressure outlet boundary you are imposing a certain distribution (default uniform) for the pressure which may not match the distribution the flow would normally have. Therefore, in general, I recommend you do Case A. You can do Case B if you can't afford the computation. However, these days RAM and cpuhours are really cheap.

Thanx for the Reply LuckyTran..

Well Actually i am confused mainly between pressure measuring system in Fluent. Like if a want to measure pressure drop at constant mass flow rate across 50 inch long pipe, should i model 50 inch exactly with the pressure-outlet condition or some extra length (10-15 inches) to eliminate the effect of immediate exit to the atmosphere and then measure at 50inch.

In real experimental analysis, like pressure is measured few pipe diameters before the outlet to atmosphere.

March 13, 2017, 09:52
#4
Senior Member

Kushal Puri
Join Date: Nov 2013
Posts: 182
Rep Power: 12
Quote:
 Originally Posted by Inderjeet Singh Thanx for the Reply LuckyTran.. Well Actually i am confused mainly between pressure measuring system in Fluent. Like if a want to measure pressure drop at constant mass flow rate across 50 inch long pipe, should i model 50 inch exactly with the pressure-outlet condition or some extra length (10-15 inches) to eliminate the effect of immediate exit to the atmosphere and then measure at 50inch. In real experimental analysis, like pressure is measured few pipe diameters before the outlet to atmosphere.
You just extend the length of the pipe at least 3 times of diameter of piper from the orignal exit. Because even your pipe is discharging into the atmosphere the pressure at the exit is not the atmospheric pressure (it will be more then that). If you know the pressure at the exit of the pipe the use that pressure as pressure outlet. If you dont know the pressure, what i suggest is just make some big box at the end of the pipe, which will act as pressure outlet and you will get good results.

Hope you have some idea, how to proceed from here.

March 14, 2017, 22:53
#5
New Member

Inderjeet Singh
Join Date: Feb 2017
Posts: 8
Rep Power: 9
Quote:
 Originally Posted by Kushal Puri You just extend the length of the pipe at least 3 times of diameter of piper from the orignal exit. Because even your pipe is discharging into the atmosphere the pressure at the exit is not the atmospheric pressure (it will be more then that). If you know the pressure at the exit of the pipe the use that pressure as pressure outlet. If you dont know the pressure, what i suggest is just make some big box at the end of the pipe, which will act as pressure outlet and you will get good results. Hope you have some idea, how to proceed from here.
Thanx for the help Kushal..
Yes things are getting more clear now..

" Because even your pipe is discharging into the atmosphere the pressure at the exit is not the atmospheric pressure (it will be more then that)." - This makes things even more clear ..

And yes the pressure conditions at outlet are unknown so it will be not suitable to use any specific pressure value at Outlet boundary condition..

Anyways i guess Pressure outlet condition with 3-5 pipe diameters extra than the require length will do the job.

Thanks again for so much help.

 Tags cfd, pipe flow, pressure

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post n.tanabi Main CFD Forum 1 January 3, 2016 09:33 mnolan93 FLUENT 1 December 15, 2014 07:26 monty_p20 FLUENT 0 November 17, 2011 17:18 Daniel L FLOW-3D 2 December 10, 2010 04:23 lou FLUENT 0 September 21, 2005 00:58

All times are GMT -4. The time now is 07:16.

 Contact Us - CFD Online - Privacy Statement - Top