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

What is the significance of the input vectors (e1, e2, d, f) in porousSimpleFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 21, 2011, 13:28
Question What is the significance of the input vectors (e1, e2, d, f) in porousSimpleFoam
  #1
Member
 
Alex
Join Date: Jun 2010
Location: Planet Earth
Posts: 43
Rep Power: 7
bigbang is on a distinguished road
I'm solving a flow through a radiator using porousSimpleFoam. I understand Darcy's law to the extent of what I read in wikipedia, but what is the coordinate system for and why does d and f have vectors associated with them?
bigbang is offline   Reply With Quote

Old   July 22, 2011, 04:28
Default
  #2
New Member
 
Dima Risch
Join Date: Jun 2011
Location: Cologne
Posts: 22
Rep Power: 6
dima is on a distinguished road
The d f coefficients are relative to the porousZone and the resistance is described in each direction

so it is better to set the porousZone parallel to the e1 e2 plane to ease the entry for d and f

that is what i have understood
dima is offline   Reply With Quote

Old   July 22, 2011, 06:54
Default
  #3
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by bigbang View Post
I'm solving a flow through a radiator using porousSimpleFoam. I understand Darcy's law to the extent of what I read in wikipedia, but what is the coordinate system for and why does d and f have vectors associated with them?
Any two of e1, e2, e3 can be used to define a local coordinate system (1,2,3 are the local x,y,z directions).
The d is darcy law and f is the Forchheimer coeff.

If you have an isotropic porosity you can take any arbitrary local coordinate system (eg, take the global system) and use the same d/f coefficients for each direction. For convenience, you can set one coffecient direction and use a negative coefficient (eg, -1) as a multiplier for the other two directions.

We often have porosities that only allow flow in one-direction. Our convention is to specify the coordinate system so that this is the local 'z' flow direction.
olesen is offline   Reply With Quote

Old   July 22, 2011, 11:18
Default
  #4
Member
 
Alex
Join Date: Jun 2010
Location: Planet Earth
Posts: 43
Rep Power: 7
bigbang is on a distinguished road
Quote:
Originally Posted by olesen View Post
Any two of e1, e2, e3 can be used to define a local coordinate system (1,2,3 are the local x,y,z directions).
The d is darcy law and f is the Forchheimer coeff.
I'm not clear on how to specify the value of e1 and e2. Shouldn't there just be a single vector to define the flow direction? My goal is to model the flow through a vehicle's radiator. So the flow is going along the x direction. How would I define that with e1 and e2 in porousZones file

Here is the code taken from angleDuct tutorials in $FOAM_RUN/tutorials/incompressible/porousSimpleFoam

Code:
1
(
	radiator
	{
        	coordinateSystem
        	{
			e1  (0.70710678 0.70710678 0);
			e2  (1 0 0);
        	}
		Darcy
		{
			d   d [0 -2 0 0 0 0 0] (5e7 -1000 -1000);
			f   f [0 -1 0 0 0 0 0] (0 0 0);
		}
	}
)
bigbang is offline   Reply With Quote

Old   July 22, 2011, 11:31
Default
  #5
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by bigbang View Post
I'm not clear on how to specify the value of e1 and e2. Shouldn't there just be a single vector to define the flow direction?
But in the general case a porosity is not rotationally symmetrical, thus you need to define an extra vector to specify the orientation of the coordinate system. If you dig into the coordinateRotation documentation, you'll see that any moderate non-orthogonality is absorbed into the second vector.

You might then want to have 'e3' (ie, local z-direction) being the defined flow direction and add 'e1' (ie, local x-direction) to orient about this axis.
olesen 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
cannot input CATIA *.model into gambit soilinkin FLUENT 10 January 12, 2011 01:47
Integration Points and normal area vectors Bloshchitsyn Vladimir CFX 0 November 26, 2007 08:35
2 velocity vectors ashish CFX 3 June 19, 2007 18:32
Velocity vectors SA Main CFD Forum 1 March 8, 2007 03:04
ANSYS ICEM CFD: lsdyna input file creation problem Evan CFX 0 June 15, 2006 13:12


All times are GMT -4. The time now is 03:13.