CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Combustion: species mass fraction's boundary conditions

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

Like Tree1Likes
  • 1 Post By ARTem

Reply
 
LinkBack Thread Tools Display Modes
Old   November 20, 2014, 04:36
Default Combustion: species mass fraction's boundary conditions
  #1
Senior Member
 
Wen Xu
Join Date: May 2014
Posts: 115
Rep Power: 3
wenxu is on a distinguished road
Hello,everyone.
Now i'm confused with the bc's settings.
Yes, I did get some idea with the pressure,velocity boundary conditions' setting. But now i simulate the coal combustion using coalChemistryFoam, and i have 5 species----CH4,CO2,O2,H2O,N2.So i should give the initial boundary conditions about all of the five species! Yes, the mass fraction of CH4, N2,O2 we already know and the max mass fraction of the products(CO2,H2O) we can also calculate. But how can we set the initial bc for the products(CO2,H2O) in the 0 folder of the boundaryField?

PS:my idea:
  • FIRST:we can calculate the products,they are both zero. And the mass fraction on the wall we should set zeroGradient.
  • SECOND:we should set all of the mass fractions of the products to zeroGradient.(coalChemistryFOAM's case set so)But i get the wrong results(the mass fractions may be even more than one!!! ) see attachment.(the read zone is wall)
PPS:This is the log of the second idea(all zeroGradient):
fieldMinMax minmaxdomain output:
Quote:
fieldMinMax minmaxdomain output:
min(p) = 99993.59018 at position (0.1423067276 -0.001535889177 0.03909566513) on processor 44
max(p) = 100057.9441 at position (-0.02876601796 -0.002455007867 -0.001637763298) on processor 0
min(U) = (0.06182562838 -0.1727735702 -0.1362042887) at position (0.0001134475403 0.003433916957 0.002707307613) on processor 1
max(U) = (10.3040291 0.1706661933 0.180937736) at position (0.01405634631 0.001614694091 0.001754794808) on processor 11
min(CO2) = 9.581539903e-05 at position (0.00743049293 -0.0001740311583 0.001975430551) on processor 7
max(CO2) = 0.5842633195 at position (0.0001132140144 -0.0001908260622 -0.004868588846) on processor 1
min(H2O) = 9.657048485e-05 at position (0.00743049293 -0.0001740311583 0.001975430551) on processor 7
max(H2O) = 0.4783360027 at position (0.0001132140144 -0.0001908260622 -0.004868588846) on processor 1
min(N2) = 0 at position (0.0005711025294 -0.0002650978475 -0.006771420691) on processor 1
max(N2) = 0.76 at position (-0.03 -0.002963781571 -0.0001174455029) on processor 0
we can see that the total max fraction of H2O and CO2 has been more than 1. They locate at the same place both at the wall.-------so...what should we do ?
Attached Images
File Type: jpg CO2CFDONLINE.jpg (17.8 KB, 10 views)
wenxu is offline   Reply With Quote

Old   November 20, 2014, 06:01
Default
  #2
Member
 
Artem Shaklein
Join Date: Feb 2010
Location: Russia, Izhevsk
Posts: 43
Rep Power: 7
ARTem is on a distinguished road
Hello, wenxu.

You should set mass fractions of products in the following way (according to OpenFOAM syntax):
initialValue uniform 0;
inlet: fixedValue uniform 0;
walls: zeroGradient;
outlet: you can go with zeroGradient, but I prefer in a case with reverse flow
type inletOutlet;
inletValue uniform 0;
value uniform 0;
its mathematical description is:
\frac{\partial Y_i}{\partial n} = 0 if outflow
Y_i = 0 if inflow
All this is according to physics: products can be generated inside a computational domain by chemistry (the source term in the transport equation), but not by flowing through boundaries (the convection and diffusion terms in the transport equation).
wenxu likes this.
ARTem is offline   Reply With Quote

Old   November 20, 2014, 07:55
Default
  #3
Senior Member
 
Wen Xu
Join Date: May 2014
Posts: 115
Rep Power: 3
wenxu is on a distinguished road
Thank you,Artem. Your answer is so clearly and powerful.I got that.regards,
wen
wenxu 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
Difficulty in calculating angular velocity of Savonius turbine simulation alfaruk CFX 8 December 3, 2013 17:51
error message cuteapathy CFX 14 March 20, 2012 07:45
mesh file for flow over a circular cylinder Ardalan Main CFD Forum 6 April 17, 2010 23:40
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
New topic on same subject - Flow around race car Tudor Miron CFX 15 April 2, 2004 06:18


All times are GMT -4. The time now is 20:31.