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

Volume Fraction, profile data problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 18, 2009, 07:34
Unhappy Volume Fraction, profile data problem
  #1
Member
 
Join Date: Aug 2009
Posts: 42
Rep Power: 8
cfxmar is on a distinguished road
Hi,
I´m simulating waves using profile data at the inlet. As I have experimental data from the height of the wave vs time, I used a profile data containing x,y,z and volume fraction as columnes.
The results aren´t correct.

x and y are fixed values (the point where the height of the wave is measured). I have put x as the time and y = 0 all time.
z is the mesured height.
Volume Fraction values are 1 or 0 depending on the value of z (positive or negative)
The expression: Filename.Volume Fraction((t*1[s^-1]*1[m]),y,z)
It doesn´t work!!!
Would kindly anyone tell me what could be wrong?
Thank you very much in advance

Cfxmar
cfxmar is offline   Reply With Quote

Old   August 18, 2009, 18:25
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,931
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I think a 1D interpolation function would be more appropriate than the 3D one you are using. Try that.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   August 19, 2009, 04:39
Default
  #3
Member
 
Join Date: Aug 2009
Posts: 42
Rep Power: 8
cfxmar is on a distinguished road
Thank you, Glenn.
I have tried that but as the problem is 3D, the profile data needs three columns for x,y,z and one for the volume fraction. CFX doesn´t let me load the profile data file with only 2 columns (one for x as the time and one for the volune fraction)
cfxmar is offline   Reply With Quote

Old   August 19, 2009, 04:47
Default
  #4
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 533
Rep Power: 11
Lance is on a distinguished road
I just did the same thing, but for a measured mass flow rate instead and a 1D profile data function worked fine for me.

Looks like:
FUNCTION: MassFlowInlet
Argument Units = [m]
Extend Max = true
Extend Min = true
File Name = massflow.csv
Option = Profile Data
Spatial Fields = X
DATA FIELD: Mass Flow Rate
Field Name = Mass Flow Rate
Result Units = [kg s^-1]
END
END

and the boundary condition:
BOUNDARY: inlet
Boundary Type = INLET
Location = F18.16
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = MassFlowInlet.Mass Flow Rate(FT)
Option = Mass Flow Rate
END
TURBULENCE:
Option = Low Intensity and Eddy Viscosity Ratio
END
END
END

where FT is defined as FT = 1[m/s]*t

Lance
Lance is offline   Reply With Quote

Old   August 19, 2009, 05:45
Default
  #5
Member
 
Join Date: Aug 2009
Posts: 42
Rep Power: 8
cfxmar is on a distinguished road
Thank you very much, Glenn and Lance.
I´m running the simulation, tomorrow I will see the results.

Cfxmar
cfxmar is offline   Reply With Quote

Old   August 19, 2009, 08:09
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,931
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
I have tried that but as the problem is 3D, the profile data needs three columns for x,y,z and one for the volume fraction. CFX doesn´t let me load the profile data file with only 2 columns (one for x as the time and one for the volune fraction)
Come on, think outside the square.... You don't need a whole variable field to store the volume fraction. It can be stored as a single number (that is the height of the surface at that time) and the volume fraction field can be evaluated for height from that using a simple CEL step or if function. Now you can use a 1D interpolation function.
ghorrocks 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
How to give volume fraction in multiphase models chhanwal FLUENT 0 August 13, 2009 00:07
On the damBreak4phaseFine cases paean OpenFOAM Running, Solving & CFD 0 November 14, 2008 22:14
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
How to apply negtive pressure to outlet bioman66 CFX 5 June 3, 2006 01:40


All times are GMT -4. The time now is 12:41.