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

How to simulate a diffuser in ansys fluent

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

Like Tree2Likes
  • 1 Post By Kushal Puri
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 6, 2017, 00:41
Default How to simulate a diffuser in ansys fluent
  #1
New Member
 
Saibal
Join Date: Feb 2017
Posts: 3
Rep Power: 7
Hello_Fluent is on a distinguished road
Hello friends,
I am trying to simulate a subsonic diffuser by ANSYS 14.5 _ FLUENT. My Inlet mach number is 0.9 and Inlet gas is Air. I want to increase pressure at the outlet of a diffuser. So I have added a diverging area diffuser at the end of a pipe through which the flow is taking place. But in my result instead of rise in pressure and decreasing in velocity, reverse is taking place. Pressure is decreasing and velocity is increasing. Please help me out which boundary condition and solver I have to choose to obtain the exact result.

Please give some suggestion about simulation of compressible flow in a diffuser.
Attached Images
File Type: jpg FFF-4.2_pressure.jpg (55.4 KB, 43 views)
File Type: jpg FFF-4.2_velocity.jpg (56.7 KB, 34 views)
Hello_Fluent is offline   Reply With Quote

Old   February 6, 2017, 09:24
Default
  #2
Senior Member
 
Kushal Puri
Join Date: Nov 2013
Posts: 183
Rep Power: 11
Kushal Puri is on a distinguished road
Quote:
Originally Posted by Hello_Fluent View Post
Hello friends,
I am trying to simulate a subsonic diffuser by ANSYS 14.5 _ FLUENT. My Inlet mach number is 0.9 and Inlet gas is Air. I want to increase pressure at the outlet of a diffuser. So I have added a diverging area diffuser at the end of a pipe through which the flow is taking place. But in my result instead of rise in pressure and decreasing in velocity, reverse is taking place. Pressure is decreasing and velocity is increasing. Please help me out which boundary condition and solver I have to choose to obtain the exact result.

Please give some suggestion about simulation of compressible flow in a diffuser.
What are the boundary conditions you are using?
Kushal Puri is offline   Reply With Quote

Old   February 7, 2017, 00:07
Default
  #3
New Member
 
Saibal
Join Date: Feb 2017
Posts: 3
Rep Power: 7
Hello_Fluent is on a distinguished road
Thank you for the reply.

I am completely describing my problem details:
For the case of diffuser:
Inlet Diameter-55 mm.
Outlet diameter-110 mm.
Inlet pressure- 410043 Pascal
Inlet temperature-483 K.
Inlet gas-Air
Inlet Density-2.9563 kg/m3
Inlet velocity- 397 m/s.
As the temperature at the inlet is 483K, Mach number at the inlet is 0.9, because the velocity of sound at inlet is around 440 m/s.
During problem solving through Fluent,
I have used P inlet as the inlet boundary condition.Gauge total pressure is 693400Pascal as I found it from isentropic table corresponding to M=0.9.
Initial gauge pressure is 410043Pascal and Inlet temperature is 483K.
For the outlet boundary condition, I have used P outlet as the boundary condition and the gauge pressure at outlet is 101325 Pascal.
Operating condition pressure as 0 pascal.
When I did not get the result, I changed the P outlet gauge pressure value to a higher pressure value than the Pinlet as I obtain that value from analytical calculation, but at that time also I found errors like reverse flow condition and divergence of the solution etc.
In the solution method I used Implicit+AUSM second order upwind scheme.

Please suggest me the appropriate procedure for solving a diverging diffuser.

Thank You
Hello_Fluent is offline   Reply With Quote

Old   October 30, 2018, 09:21
Default
  #4
Member
 
MWRS
Join Date: Apr 2018
Posts: 98
Rep Power: 6
waseeqsiddiqui is on a distinguished road
Please help
waseeqsiddiqui is offline   Reply With Quote

Old   November 1, 2018, 02:46
Default
  #5
Senior Member
 
Kushal Puri
Join Date: Nov 2013
Posts: 183
Rep Power: 11
Kushal Puri is on a distinguished road
Quote:
Originally Posted by waseeqsiddiqui View Post
Please help
You can use a mass flow inlet and provide the pressure value in supersonic gauge pressure and also use coupled solver. Exred the outlet domain more. And increase also the outlet pressure..
I
waseeqsiddiqui likes this.
Kushal Puri is offline   Reply With Quote

Old   November 3, 2018, 10:04
Default
  #6
Member
 
MWRS
Join Date: Apr 2018
Posts: 98
Rep Power: 6
waseeqsiddiqui is on a distinguished road
Quote:
Originally Posted by Kushal Puri View Post
You can use a mass flow inlet and provide the pressure value in supersonic gauge pressure and also use coupled solver. Exred the outlet domain more. And increase also the outlet pressure..
I
Could you tell me what the Guage pressure, initial supersonic Guage pressure in pressure inlet and outlet mean?
In terms of static pressure total pressure etc.
waseeqsiddiqui is offline   Reply With Quote

Old   February 26, 2019, 12:21
Default
  #7
Member
 
MWRS
Join Date: Apr 2018
Posts: 98
Rep Power: 6
waseeqsiddiqui is on a distinguished road
Quote:
Originally Posted by Kushal Puri View Post
You can use a mass flow inlet and provide the pressure value in supersonic gauge pressure and also use coupled solver. Exred the outlet domain more. And increase also the outlet pressure..
I
So I specify the theoretically evaluated static pressure at outlet or any certain value that is higher than inlet?
waseeqsiddiqui is offline   Reply With Quote

Old   February 26, 2019, 14:43
Default
  #8
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,057
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
At outlets: you need to specify the static pressure



Quote:
Originally Posted by waseeqsiddiqui View Post
Could you tell me what the Guage pressure, initial supersonic Guage pressure in pressure inlet and outlet mean? In terms of static pressure total pressure etc.
At inlets: you specify the total pressure if you use the pressure inlet BC or the mass-flow rate if you use the mass flow rate BC. So you take your value for the total pressure and put it into the box labeled
Code:
Gauge Total Pressure (pascal)
If your inlet is subsonic you are done. If the inlet is supersonic, then you need to specify (in addition to the total pressure or mass flow rate) the static pressure. You take your static pressure and put it into the box labeled:
Code:
Supersonic/initial Gauge Pressure (pascal)
If your inlet is subsonic, this input has no effect and is ignored. You can put in any value and it won't matter if your inlet is subsonic. This box has another purpose during initialization and that's why it is labeled supersonic/initial. It actually has two purposes.

Almost all pressures in Fluent are gauge pressures, so that the letters Gauge appear everywhere for redundancy.
waseeqsiddiqui likes this.
LuckyTran is offline   Reply With Quote

Old   February 26, 2019, 21:47
Default
  #9
Member
 
MWRS
Join Date: Apr 2018
Posts: 98
Rep Power: 6
waseeqsiddiqui is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
At outlets: you need to specify the static pressure





At inlets: you specify the total pressure if you use the pressure inlet BC or the mass-flow rate if you use the mass flow rate BC. So you take your value for the total pressure and put it into the box labeled
Code:
Gauge Total Pressure (pascal)
If your inlet is subsonic you are done. If the inlet is supersonic, then you need to specify (in addition to the total pressure or mass flow rate) the static pressure. You take your static pressure and put it into the box labeled:
Code:
Supersonic/initial Gauge Pressure (pascal)
If your inlet is subsonic, this input has no effect and is ignored. You can put in any value and it won't matter if your inlet is subsonic. This box has another purpose during initialization and that's why it is labeled supersonic/initial. It actually has two purposes.

Almost all pressures in Fluent are gauge pressures, so that the letters Gauge appear everywhere for redundancy.
Always a pleasure to hear it from you.
waseeqsiddiqui is offline   Reply With Quote

Reply

Tags
ansys 14.5 fluent, compressible flow, subsonic flow in diffuser

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
drag coefficient in ansys fluent 12.0 krishna FLUENT 19 April 12, 2018 01:49
Can you help me with a problem in ansys static structural solver? sourabh.porwal Structural Mechanics 0 March 27, 2016 18:07
simulate the melting of Phase Change Material in ansys fluent WanAsyraf FLUENT 2 March 9, 2016 11:19
Ansys structural and fluent for FSI assafwei FLUENT 1 June 20, 2014 11:56
Help to simulate evaporation in ANSYS Fluent german.gd20 Fluent Multiphase 2 April 8, 2014 14:35


All times are GMT -4. The time now is 17:42.