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

francis turbin difference between experiment values and CFD

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 23, 2009, 23:02
Default francis turbin difference between experiment values and CFD
  #1
New Member
 
snoopy
Join Date: Dec 2009
Posts: 8
Rep Power: 7
snoopy is on a distinguished road
Hello.
I have something to solve urgently. Please please help me.
I have flow rate 1.37 m^3/s at outlet from an experiment.
I imposed initial conditions as 4.16ATM pressure at inlet but after CFX 11 runned I got a result 2 m^3/s at outlet.
As I told you, I have to have result as 1.37 m^3/s at outlet.
What should I do?
I already checked modeling, scale and fluid properties and so on.
Thank you in advance.
Have a nice day.
snoopy is offline   Reply With Quote

Old   December 25, 2009, 03:20
Default
  #2
Member
 
Join Date: Nov 2009
Posts: 49
Rep Power: 7
Abou ali is on a distinguished road
Hi,
It may be that you have a problem with boundary conditions, you should take a look on this section from the CFX Help: ANSYS CFX Reference Guide | ANSYS CFX Best Practices Guide for Turbomachinery | Liquid Pumps and Turbines | and if the problem persists you should give us more details about the boundary conditions.
Abou ali is offline   Reply With Quote

Old   December 28, 2009, 00:21
Default Hi Ali
  #3
New Member
 
snoopy
Join Date: Dec 2009
Posts: 8
Rep Power: 7
snoopy is on a distinguished road
Hi Mr. Ali. Thank you for your kind response.
I read turbomachinery boundary condition and set boundary conditions as it is said.
I set inlet BC as 547.76 ATM of total pressure and outlet BC as 1370 kg/s of flow rate.
But I can't find any difference between pressure of inlet and outlet.
How can I fix it?
Thank you in advance.
snoopy is offline   Reply With Quote

Old   December 28, 2009, 00:43
Default
  #4
Member
 
SanS
Join Date: Mar 2009
Posts: 42
Rep Power: 8
sans is on a distinguished road
Hi, Simple question, has your simulation fully converged? because there is no point in discussing results of an unconverged simulation.
Also where is this mass flow being measured? Is it at the outlet of the domain?
sans is offline   Reply With Quote

Old   December 28, 2009, 01:38
Default Re
  #5
New Member
 
snoopy
Join Date: Dec 2009
Posts: 8
Rep Power: 7
snoopy is on a distinguished road
Hi. My result are fully converged.
And I got results of inlet condition and outlet conditon from the experiment. I measured mass flow rate at outlet.
Do you have any idea?
snoopy is offline   Reply With Quote

Old   December 28, 2009, 02:07
Default
  #6
Member
 
SanS
Join Date: Mar 2009
Posts: 42
Rep Power: 8
sans is on a distinguished road
Can you post an .out file here?
sans is offline   Reply With Quote

Old   December 28, 2009, 02:14
Default hi
  #7
New Member
 
snoopy
Join Date: Dec 2009
Posts: 8
Rep Power: 7
snoopy is on a distinguished road
Hi

Do you know how to send file to you here?
or please give me your e-mail address?
snoopy is offline   Reply With Quote

Old   December 28, 2009, 03:05
Default hi
  #8
New Member
 
snoopy
Join Date: Dec 2009
Posts: 8
Rep Power: 7
snoopy is on a distinguished road
Hi
I attached out file. please read it and give me a great idea.
have a nice day
snoopy is offline   Reply With Quote

Old   December 28, 2009, 03:12
Default
  #9
Member
 
Join Date: Nov 2009
Posts: 49
Rep Power: 7
Abou ali is on a distinguished road
Hello all,
The used BC at inlet is unrealistic, a total pressure of 547.76 ATM is very high and you can't find a correct solution.
It's a good idea to attach your output file here.
Go to the bottom of the Reply to Thread page, in the Additional Options you can find Attach Files .

Abou ali is offline   Reply With Quote

Old   December 28, 2009, 03:12
Default hi
  #10
New Member
 
snoopy
Join Date: Dec 2009
Posts: 8
Rep Power: 7
snoopy is on a distinguished road
Hi
I attached out file. please read it and give me a great idea.
have a nice day

PS : inlet condition is 45m of head at inlet.
and according to my calculation, the total pressure is 4.5 ATM + 0.5 * density * velocity^2 is 547.76 ATM
am I wrong?
Attached Files
File Type: txt outfile.txt (26.7 KB, 11 views)
snoopy is offline   Reply With Quote

Old   December 28, 2009, 03:58
Default
  #11
Member
 
Join Date: Nov 2009
Posts: 49
Rep Power: 7
Abou ali is on a distinguished road
Hi,
After reading your output file, I find this tow mistacs:

1- MASS AND MOMENTUM:
Option = Total Pressure
Relative Pressure = 547.76 [atm]
END

As I sad previously the total pressure is not correct????!!!!!

2- BOUNDARY: SH02
Boundary Type = WALL
Frame Type = Rotating
Location = SHROUD1 2
BOUNDARY CONDITIONS:
WALL INFLUENCE ON FLOW:
Option = No Slip
END
END
END

This Boundary is defined as rotating Boundary, but in reality it isn't. To define it as stationary, go to the Boundary Details and activate Wall Velocity then select Counter Rotating Wall in the option Box.
You have to do that for all stationary boundaries in the rotating domain.
Abou ali is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
validation of CFD and windtunnel experiment M.Arun prasad FLUENT 4 March 13, 2008 03:12
CFD VALUES AT EXPERIMENTAL POINT J FLUENT 1 September 25, 2005 16:55


All times are GMT -4. The time now is 12:04.