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

Solving Additional Variable in CFX?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 17, 2005, 08:44
Default Solving Additional Variable in CFX?
  #1
Tuks
Guest
 
Posts: n/a
Hi all, I want to solve equations for three variables(P1, P2, P3) as additional variables. The equation for the variable variation with time is,

DPi/Dt = (Nitotal-Gtotal*Piavg)/Vg for i=1,2,3 ----(a)

WHERE

Piavg = volumeAve(Pi)@Domain1 AND Vg=constant.

Nitotal = volumeInt(Ni)@Domain1 AND Ni=K*(C - Piavg)

Gtot = N1total + N2total + N3total.

Is it possible to solve above equations (a)?

Rightnow i am solving additional variable by Diffisive transport equation. with Diffisivity = 1E-10 m^2/s. and Source = RHS of eq(a).

Can we use volmeAve and volumeInt over Domain in CEL?

when i tried in CFX-10.0-Pre i got following error. "The function 'volumeAve' referenced in parameter 'Source' in object '/FLOW/DOMAINomain1/SUBDOMAIN:subreact/SOURCES/EQUATION SOURCE:SourceP2' has an invalid argument, 'N2total'. Only arguments that consist of a single variable name are supported by the solver."

What is this error?

NOTE: I am using the variable composition mixture in Domain1

Thank you in advance.

Regards Tuks

  Reply With Quote

Old   November 17, 2005, 10:34
Default Re: Solving Additional Variable in CFX?
  #2
Rui
Guest
 
Posts: n/a
Hi,

Yes, you can use volumeAve and volumeInt in CEL.

About the error, try this: create an additional variable (algebraic equation) for each Ni

Regards,

Rui
  Reply With Quote

Old   November 17, 2005, 13:09
Default Re: Solving Additional Variable in CFX?
  #3
Rui
Guest
 
Posts: n/a
Take a look at the Documentation; Reference Material; CFX Expression Language; CEL Variables, Functions and Constants; CEL Functions; Additional CFX-Solver CEL Functions; variable (page 47 in CFX-5.7.1 Documentation)
  Reply With Quote

Old   November 17, 2005, 15:15
Default Re: Solving Additional Variable in CFX?
  #4
Tuks
Guest
 
Posts: n/a
Hi Rui,

Thanks you for suggestions, it really helped a lot. I defined the each Ni as Additional Variable (algebraic equations). It works well. The documentation suggested also helped.

Now i could solve the equations. Yet to check validation with known values, but atleast solution has started quite well.

Thank you again

Regards

Tuks

  Reply With Quote

Old   November 18, 2005, 01:51
Default Re: Which one is right?
  #5
Tuks
Guest
 
Posts: n/a
Hi all,

I am solving the reactions in single phase, the fluid in Domain is VARIABLE COMPOSITION MIXTURE (userMix). If additional variables are defined and we want to use those in CEL expressions then how we write those in expressions? Example, If N1 is additional variable.

a1 = volmueAve(N1)@Domain1 OR a1 = volumeAve(userMix.N1)@Domain1.

Which one is right? Because both are NOT giving any ERROR in Pre but in Post it says 'userMix.N1' doesnot exist?

Thanks in advance

Regards

Tuks
  Reply With Quote

Old   November 18, 2005, 10:33
Default Re: Which one is right?
  #6
opaque
Guest
 
Posts: n/a
Dear Tuks,

For the ANSYS CFX solver both are correct; however, CFX-Post only understands what it is available in the results file. For your case (single phase I assume) only N1, and/or N1.Volumetric/Specific are available in the results file.

If you want to use the same set of expressions in the CFX-Solver and CFX-Post, you must stick to the common syntax. That is, phase name prefixing is not needed for single phase flows since the phase name is implied.

Good luck,

Opaque.

  Reply With Quote

Old   November 18, 2005, 12:40
Default Re: Which one is right?
  #7
Tuks
Guest
 
Posts: n/a
Hi Opaque,

Thank you for your sugesstions.

Regards Tuks
  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
transsonic nozzle with rhoSimpleFoam Unseen OpenFOAM Running, Solving & CFD 7 April 16, 2014 03:38
Forces in OF15 richard OpenFOAM Running, Solving & CFD 166 September 17, 2011 03:24
lift and drag on ship superstructures vaina74 OpenFOAM Running, Solving & CFD 3 June 8, 2010 12:30
Negative value of k causing simulation to stop velan OpenFOAM Running, Solving & CFD 1 October 17, 2008 05:36
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


All times are GMT -4. The time now is 10:49.