CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Pressure Drop

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 27, 2022, 05:41
Default Pressure Drop
  #1
New Member
 
Join Date: Jan 2020
Location: Germany
Posts: 24
Rep Power: 4
IrieConqueror is on a distinguished road
Hey guys,

I'm trying to calculate pressure drop in a pipe when air is flowing through. The pipe has four straight parts and three pipe elbows (sketch in picture). I checked my simulation results and compared them with calculations from some Online Calculators from the internet. There are huge differences especially in the pipe elbows (picture). Do you have any ideas where these differences come from?

Assumptions:
INLET
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = 375 [C]
END
MASS AND MOMENTUM:
Mass Flow Rate = 435 [kg s^-1]
Mass Flow Rate Area = As Specified
Option = Mass Flow Rate
END
OUTLET
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Opening Temperature = 375 [C]
Option = Opening Temperature
END
MASS AND MOMENTUM:
Option = Opening Pressure and Direction
Relative Pressure = 0 [Pa]
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1.9 [bar]
END
END
FLUID DEFINITION: Fluid 1
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = Thermal Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
END
TURBULENT WALL FUNCTIONS:
Option = Scalable
END

Thanks

Irie
Attached Images
File Type: jpg PressureDrop.jpg (66.0 KB, 24 views)
IrieConqueror is offline   Reply With Quote

Old   September 27, 2022, 06:44
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,637
Rep Power: 25
Gert-Jan will become famous soon enough
What is the diameter of the pipe?
Gert-Jan is offline   Reply With Quote

Old   September 27, 2022, 07:59
Default
  #3
New Member
 
Join Date: Jan 2020
Location: Germany
Posts: 24
Rep Power: 4
IrieConqueror is on a distinguished road
2250 mm and the elbow bend radius 3360 mm
IrieConqueror is offline   Reply With Quote

Old   September 27, 2022, 08:21
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,637
Rep Power: 25
Gert-Jan will become famous soon enough
According to your settings, you have a density of 1 kg/m3. This means that your inlet velocity exceeds 100m/s. Is that what you expect?
If so, then you are studying an uncommon problem. Is it North Stream I or II? Nevertheless, then I would use Total Energy since you are reaching Mach=0.3.
karachun likes this.
Gert-Jan is offline   Reply With Quote

Old   September 27, 2022, 08:37
Default
  #5
New Member
 
Join Date: Jan 2020
Location: Germany
Posts: 24
Rep Power: 4
IrieConqueror is on a distinguished road
"Is it North Stream I or II?"

No but I will try Total Energy. Velo is correct. Why do you call it uncommon problem?
IrieConqueror is offline   Reply With Quote

Old   September 27, 2022, 08:50
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,637
Rep Power: 25
Gert-Jan will become famous soon enough
- Transporting 420 kg/s of air at 1.9 bar and 375°C, is not somehting I encounter very often. Therefore I was checking.
- I don't think the online tools cover these operating conditions.
- I guess you now use uniform inlet conditions? I wonder if that is correct with 100 m/s. Don't think so. Better add additional geometrical info upstream the inlet.
- Also I wonder how the velocity looks like.
Gert-Jan is offline   Reply With Quote

Old   September 27, 2022, 09:05
Default
  #7
New Member
 
Join Date: Jan 2020
Location: Germany
Posts: 24
Rep Power: 4
IrieConqueror is on a distinguished road
"- I guess you now use uniform inlet conditions? I wonder if that is correct with 100 m/s. Don't think so. Better add additional geometrical info upstream the inlet." - Could you explain a little bit more? What do you mean by "add additional geometrical info upstream the inlet"

"- Also I wonder how the velocity looks like." - picture
Attached Images
File Type: jpg Velo.jpg (39.0 KB, 12 views)
IrieConqueror is offline   Reply With Quote

Old   September 27, 2022, 10:28
Default
  #8
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,637
Rep Power: 25
Gert-Jan will become famous soon enough
- Let me reformulate..... What is present upstream the inlet? More straight duct? Or a piece of equipment where the hot air is generated. A furnace, a DeNOx installation.....
- Did you perform a mesh sensitivity check?
- Remember, total pressure is a better indicator for pressure drop than static pressure.
Gert-Jan is offline   Reply With Quote

Old   September 27, 2022, 10:50
Default
  #9
New Member
 
Join Date: Jan 2020
Location: Germany
Posts: 24
Rep Power: 4
IrieConqueror is on a distinguished road
"- Let me reformulate..... What is present upstream the inlet? More straight duct? Or a piece of equipment where the hot air is generated. A furnace, a DeNOx installation....." - unfortunately no infos about that...
"- Did you perform a mesh sensitivity check?" - I did
"- Remember, total pressure is a better indicator for pressure drop than static pressure." - I used (areaAve(Total Pressure)@Inlet - areaAve(Total Pressure)@Outlet)

I thought that the problem should be scalable until the influence of the wall is getting bigger. Thats why I ask u of uncommon problem..
IrieConqueror is offline   Reply With Quote

Old   September 28, 2022, 16:25
Default
  #10
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,116
Rep Power: 21
evcelica is on a distinguished road
In my experience hand calcs for elbows always show much higher pressure drops than a CFD result. My theory is that in CFD you have a perfect smooth bent elbow with constant cross section. The hand formulas are likely empirical and the result of some threaded elbows with expansions and contractions, or ovaling of the tube form the bend, or with internal weld protrusion at the elbows. The difference is real world elbows vs a perfect curved tube.
evcelica is offline   Reply With Quote

Old   September 29, 2022, 05:18
Default
  #11
New Member
 
Join Date: Jan 2020
Location: Germany
Posts: 24
Rep Power: 4
IrieConqueror is on a distinguished road
Thanks for your replies.

@evcelia: That makes total sense. I didn't expect such a huge difference but maybe that is the answer.
IrieConqueror is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Fluent cyclone pressure drop mkal FLUENT 1 February 20, 2020 01:55
Periodic flow using Cyclic - comparison with Fluent nusivares OpenFOAM Running, Solving & CFD 30 December 12, 2017 06:35
Pressure drop using Fan type BC Alexis Sack OpenFOAM Running, Solving & CFD 2 September 22, 2014 10:18
How to study pressure drop of continous phase in VOF model sajeesh FLUENT 4 February 5, 2014 23:01
Pipe Flow - Pressure Drop Daniel L FLOW-3D 2 December 10, 2010 05:23


All times are GMT -4. The time now is 20:14.