
[Sponsors] 
August 18, 2009, 07:34 
Volume Fraction, profile data problem

#1 
Member
Join Date: Aug 2009
Posts: 42
Rep Power: 9 
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 

August 18, 2009, 18:25 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,059
Rep Power: 101 
I think a 1D interpolation function would be more appropriate than the 3D one you are using. Try that.
Glenn Horrocks 

August 19, 2009, 04:39 

#3 
Member
Join Date: Aug 2009
Posts: 42
Rep Power: 9 
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) 

August 19, 2009, 04:47 

#4 
Senior Member
Lance
Join Date: Mar 2009
Posts: 606
Rep Power: 13 
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 

August 19, 2009, 05:45 

#5 
Member
Join Date: Aug 2009
Posts: 42
Rep Power: 9 
Thank you very much, Glenn and Lance.
I´m running the simulation, tomorrow I will see the results. Cfxmar 

August 19, 2009, 08:09 

#6  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,059
Rep Power: 101 
Quote:


Thread Tools  
Display Modes  


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 