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

Quick UDS question

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 23, 2011, 13:14
Default Quick UDS question
  #1
New Member
 
Luke Holsen
Join Date: Jun 2011
Posts: 12
Rep Power: 6
lholsen08 is on a distinguished road
If I impose a constant value for a UDS at the inlet then the units are kM/m^3 ?

The UDS diffusivity is the diffusion coefficient* density of the material? Do I input the calculated value?

Thanks for the help!
lholsen08 is offline   Reply With Quote

Old   September 23, 2011, 15:18
Default
  #2
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by lholsen08 View Post
If I impose a constant value for a UDS at the inlet then the units are kM/m^3 ?

The UDS diffusivity is the diffusion coefficient* density of the material? Do I input the calculated value?

Thanks for the help!
UDS is just a scalar, you can consider it as a non-dimension variable (normalizes parameter).
UDS diffusivity is equal to (fluid density*diffusion coefficient of scalar in that fluid); this parameter should be set in FLUENT.
__________________
Amir
Amir is offline   Reply With Quote

Old   September 25, 2011, 17:18
Default
  #3
New Member
 
Luke Holsen
Join Date: Jun 2011
Posts: 12
Rep Power: 6
lholsen08 is on a distinguished road
Thank you for your response. I am still slightly confused. When I go to the materials section and open the create/edit materials window. The option says UDS DIffusivity ( kg/m-s). When you click edit it says coefficient, which would be m^2/s correct? There are no units listed on that input window.
lholsen08 is offline   Reply With Quote

Old   September 26, 2011, 03:06
Default
  #4
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by lholsen08 View Post
Thank you for your response. I am still slightly confused. When I go to the materials section and open the create/edit materials window. The option says UDS DIffusivity ( kg/m-s). When you click edit it says coefficient, which would be m^2/s correct? There are no units listed on that input window.
No, you have to set a parameter which its dimension is kg/m.s there. As I said before, this parameter is : (fluid density*diffusion coefficient of scalar in that fluid), which its dimension is kg/m.s !

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   September 26, 2011, 08:16
Default
  #5
New Member
 
Luke Holsen
Join Date: Jun 2011
Posts: 12
Rep Power: 6
lholsen08 is on a distinguished road
OK, So then the scalar would be in kg/m^3 to maintain consistent units?
lholsen08 is offline   Reply With Quote

Old   September 26, 2011, 08:28
Default
  #6
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by lholsen08 View Post
OK, So then the scalar would be in kg/m^3 to maintain consistent units?
No!!!
\frac{\partial}{\partial t} (\rho C) + \nabla . (\rho U C) = \nabla . (\rho D \nabla C)
c can have any dimension. (you have to set \rho D)

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   September 26, 2011, 08:31
Default
  #7
New Member
 
Luke Holsen
Join Date: Jun 2011
Posts: 12
Rep Power: 6
lholsen08 is on a distinguished road
OK, thank you for the quick response and all the help!
lholsen08 is offline   Reply With Quote

Old   September 26, 2011, 10:18
Default
  #8
New Member
 
Luke Holsen
Join Date: Jun 2011
Posts: 12
Rep Power: 6
lholsen08 is on a distinguished road
Thank you Amir for all your help. You are actually the one who helped me last suggesting the interpolate function and seem to be the one who knows the most about UDS.

I am trying to replicate this equation as my source term: Conc NO = (Rnomax* Conc.Oxygen)/(Conc. Oxygen + KmeNOS)

I am getting numbers with my source code but they do not match up with some previous models.

Does this look correct to you?
#include "udf.h"
/************************************************** ****************************************
This UDF calculates Source Terms for the Lumen, Endothelium, Vascular Wall, and Tissue Layer
************************************************** ******************************************/
/*** Species numbers ***/
#define Oxygen 0
#define NO 1
/************************************************** ****************************************
Endothelium
Source Terms: NO Generation and O2 Consumption
************************************************** ******************************************/
/*** Define Variables for Calculation ***/
#define RNOmax 0.000054; /*Maximum eNOS Production Rate (54 uM/s )->(M/s)*/
#define KmeNOS 4.7; /*Michaelis-Menten reaction kinetics term (4.7 Torr)*/
DEFINE_SOURCE( Endothelium_NOGen, c, t, dS, eqn)
{
real con, concNO;
concNO=((RNOmax*C_UDSI(c,t,Oxygen))/(C_UDSI(c,t,Oxygen)+(KmeNOS)));
return concNO;
}
lholsen08 is offline   Reply With Quote

Old   September 26, 2011, 13:20
Default
  #9
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by lholsen08 View Post
Conc NO = (Rnomax* Conc.Oxygen)/(Conc. Oxygen + KmeNOS)
Dear Luke,

I think there is a problem in your formula! The dimensions are not compatible; e.g., you've added Conc. Oxygen and KmeNOS which have different dimensions and also the whole dimension doesn't reduce to concentration! Maybe there are some unit multiplication factors which have dimension! (Conc. Oxygen + KmeNOS*1); check that.

Bests,
__________________
Amir
Amir is offline   Reply With Quote

Old   September 26, 2011, 14:10
Default
  #10
New Member
 
Luke Holsen
Join Date: Jun 2011
Posts: 12
Rep Power: 6
lholsen08 is on a distinguished road
Well it is a partial pressure, Henry's Law, using a Michaelis-Meneten reaction source term. So the "concentration" is really a pressure in Torr. I noted it wrong in the code and never fixed it. I really just wanted to know if the coding was correct because and would replicate the equation. I am new to C and this is my first code. Matlab is where the extent of my coding ability lies. Thank you very much for all your help! I truly appreciate it!
lholsen08 is offline   Reply With Quote

Old   September 26, 2011, 16:21
Default
  #11
Senior Member
 
Amir's Avatar
 
Amir
Join Date: May 2009
Location: Shiraz, Iran
Posts: 739
Blog Entries: 1
Rep Power: 14
Amir is on a distinguished road
Quote:
Originally Posted by lholsen08 View Post
Well it is a partial pressure, Henry's Law, using a Michaelis-Meneten reaction source term. So the "concentration" is really a pressure in Torr. I noted it wrong in the code and never fixed it. I really just wanted to know if the coding was correct because and would replicate the equation. I am new to C and this is my first code. Matlab is where the extent of my coding ability lies. Thank you very much for all your help! I truly appreciate it!
Your UDF is correct but you will need something more than this justification! if the dimension of concentrations are Torr, the dimension of "Rnomax" should be Torr too!!! However, such convection-diffusion equation is not valid for pressure!

Bests,
__________________
Amir
Amir 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
Please help student, quick question, CFD prices?? quiksilver Main CFD Forum 2 April 30, 2010 19:09
UDS question Z FLUENT 5 April 2, 2005 14:45
A good question about UDS Z FLUENT 1 March 31, 2005 15:14
UDS question Z FLUENT 1 March 31, 2005 15:08
UDS Question Z FLUENT 0 March 25, 2005 07:20


All times are GMT -4. The time now is 19:09.