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

How to Monitor Volume at specific value

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 15, 2014, 06:08
Default How to Monitor Volume at specific value
  #1
New Member
 
Marcin
Join Date: Apr 2014
Posts: 4
Rep Power: 3
czuapucci is on a distinguished road
I have a question regarding CFX Pre. I would like to set a monitor in a following way:

[*]Monitor volume (inside fluid domain) which is defined as Iso-volume at value (this can be done in POST - no clue if possible in PRE).[*]For instance I want to measure volume of air inside fluid domain, which has Temperature = 350K and I would like to monitor that in solver manager during simmulation


Have you ever came accross such a problem?
Any tips which way to go?
czuapucci is offline   Reply With Quote

Old   April 15, 2014, 08:16
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You cannot do isovolume in the solver.

This series of expressions will get close to it:
InTemperatureRange = if(T<351[K] && T>349[K],1,0)
AirVFInTempRange = Air.Volume Fraction * InTemperatureRange
AirVolumeInRange = volumeInt(AirVFInTempRange)@DomainName

Then assign AirVolumeInRange to a monitor point.
ghorrocks is offline   Reply With Quote

Old   April 15, 2014, 09:10
Default
  #3
New Member
 
Marcin
Join Date: Apr 2014
Posts: 4
Rep Power: 3
czuapucci is on a distinguished road
Thanks Glen!
Another question though:
Analogic to already posted - I want to monitor the Volume of methane at its Lower Explosive Limit (LEL=4.4% mol/mol)

As I understood - If I use following:

This defines cloud of CH4 at ~LEL and "rejects" volume which does not meet requirement
InLELRange = if(CH4 Ideal Gas.Molar Fraction <0.045[mol/mol] && CH4 Ideal Gas.Molar Fraction>0.043[mol/mol],1,0)

Definition of the volume meeting ~4.4% mol/mol
CH4_VF_InLELRange = CH4 Ideal Gas.Molar Fraction * InLELRange

Integration of defined CH4 volume in my Fluid Domain
CH4VolumeInLELRange = volumeInt(CH4_VF_InLELRange)@DomainName


Please Let me know if it makes sense. I will try to implement that in my model and will share if it worked.
czuapucci is offline   Reply With Quote

Old   April 15, 2014, 09:47
Default
  #4
New Member
 
Marcin
Join Date: Apr 2014
Posts: 4
Rep Power: 3
czuapucci is on a distinguished road
OK - After Introducing proposed expressions (for temperature) I am receiving an error message from PRE:

The function 'volumeInt' referenced in parameter 'Expression Value' in object '/FLOW:Flow Analysis 1/OUTPUT CONTROL/MONITOR OBJECTS/MONITOR POINT:Cloud Size' has an invalid argument, 'AirVFInTempRange'. Only arguments that consist of a single recognised variable name are supported by the solver.

Any Ideas how to fix that?
czuapucci is offline   Reply With Quote

Old   April 15, 2014, 18:39
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,809
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
First of all - I used a volume integral over the volume fraction. This gives the total volume. Your post #3 does a volume integral of the molar fraction which is a different thing, and will not give volume.

Second - The error message is clear, if cannot find the variable it is naming. Sometimes CEL gets the order of expressions mixed up as it is trying to evaluate the AirVFInTempRange expression after the volumeInt expression and this leads to an error as the volumeInt expression has undefined variables. Try putting the entire expression on one expression:

AirVolumeInRange = volumeInt(Air.Volume Fraction * if(T<351[K] && T>349[K],1,0))@DomainName
ghorrocks is offline   Reply With Quote

Reply

Tags
cfx.pre.volume.monitor

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
error message cuteapathy CFX 14 March 20, 2012 07:45
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56
Simulation of a single bubble with a VOF-method Suzzn CFX 18 October 2, 2009 04:18
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 12:02


All times are GMT -4. The time now is 13:27.