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

groovyBC for defining heat influx at the boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 25, 2014, 01:06
Default groovyBC for defining heat influx at the boundary
  #1
New Member
 
Delstat
Join Date: Apr 2013
Posts: 15
Rep Power: 5
pradeepramesh is on a distinguished road
Hi ,

I am using laplacianfoam for a heat-block case. I have gone thru the discussion - "Mixed BC - heat transfer - laplacianFoam"
http://www.cfd-online.com/Forums/ope...acianfoam.html.

From the forum discussions - "externalWallHeatFluxTemperature" and "groovyBC" were pointed out.

I am interested to apply heat influx at the boundary wall.Please find the attached snapshot for more info.

How to apply "groovyBC" for defining heat influx at the boundary in a heat-block?

Thank you,
Pradeep
Attached Images
File Type: jpg GroovyBC influx.JPG (65.7 KB, 17 views)
pradeepramesh is offline   Reply With Quote

Old   August 25, 2014, 17:38
Default
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,972
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by pradeepramesh View Post
Hi ,

I am using laplacianfoam for a heat-block case. I have gone thru the discussion - "Mixed BC - heat transfer - laplacianFoam"
http://www.cfd-online.com/Forums/ope...acianfoam.html.

From the forum discussions - "externalWallHeatFluxTemperature" and "groovyBC" were pointed out.

I am interested to apply heat influx at the boundary wall.Please find the attached snapshot for more info.

How to apply "groovyBC" for defining heat influx at the boundary in a heat-block?

Thank you,
Pradeep
With "fractionExpression '0'" you're on the right track. What gradientExpression is supposed to to be depends on your physics (which heat-flux you want to prescribe). Rewrite it so that you get an expression "dT/dx = ....". Then you'll just have to take what is on the right hand side of that expression and write it down as a groovyBC-expression (Note: x in this case is not the x in the cartesian coordinates but normal to the wall)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   August 25, 2014, 22:33
Default
  #3
New Member
 
Delstat
Join Date: Apr 2013
Posts: 15
Rep Power: 5
pradeepramesh is on a distinguished road
Thank you very much Bernhard
pradeepramesh is offline   Reply With Quote

Old   August 26, 2014, 00:02
Default
  #4
New Member
 
Delstat
Join Date: Apr 2013
Posts: 15
Rep Power: 5
pradeepramesh is on a distinguished road
Dear Bernhard,

For a case, flux is ------------>>>> q = -(k) * (dT/dx)

(dT/dx) = - q /k

We have :

"q" is the heat flux : q = 10 (W/m2),

"k" is the thermal Conductivity of the material : k = 200 (W/mK)


HTML Code:
Outwall
{
        type                          groovyBC;
        value                         uniform 293;
        gradientExpression 	 (-q)/k";
        fractionExpression 	 "0";
        variables 			 q=10;k=200";
}
I would like request your feedback on the above mentioned BC.

Thank you!
pradeepramesh is offline   Reply With Quote

Old   August 26, 2014, 08:12
Default
  #5
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,972
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by pradeepramesh View Post
Dear Bernhard,

For a case, flux is ------------>>>> q = -(k) * (dT/dx)

(dT/dx) = - q /k

We have :

"q" is the heat flux : q = 10 (W/m2),

"k" is the thermal Conductivity of the material : k = 200 (W/mK)


HTML Code:
Outwall
{
        type                          groovyBC;
        value                         uniform 293;
        gradientExpression 	 (-q)/k";
        fractionExpression 	 "0";
        variables 			 q=10;k=200";
}
I would like request your feedback on the above mentioned BC.

Thank you!
That should work. Sign depends on your definition of the flux.

I usually limit myself to answers about the technical aspects of swak4Foam. Physics is your own responsibility
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   August 26, 2014, 19:54
Default
  #6
New Member
 
Delstat
Join Date: Apr 2013
Posts: 15
Rep Power: 5
pradeepramesh is on a distinguished road
Thank you very much. It worked!
pradeepramesh is offline   Reply With Quote

Old   November 13, 2014, 23:34
Default
  #7
New Member
 
Chris Ostrom
Join Date: Jul 2014
Posts: 4
Rep Power: 4
costrom is on a distinguished road
would it be possible to use a 'q' file that is the output from a different solver instead of defining one constant value for q on the boundary?
costrom is offline   Reply With Quote

Old   November 14, 2014, 06:01
Default
  #8
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,972
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by costrom View Post
would it be possible to use a 'q' file that is the output from a different solver instead of defining one constant value for q on the boundary?
Currently no. Unless the data is a 1D-function q(s). Then you can use a lookup

I've explained it a number of times in different places: it is not THAT easy to do it in a general way (fileformats, different discretizations, error handling, parallel etc)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   November 14, 2014, 06:52
Default
  #9
New Member
 
Chris Ostrom
Join Date: Jul 2014
Posts: 4
Rep Power: 4
costrom is on a distinguished road
I apologize for asking a question that has been answered elsewhere, but...

I have a qMean file resulting from a dsmcFoam run, and I would like to use the heat fluxes from that as a boundary condition for a laplacianFoam runcase. is this currently possible in openFOAM 2.3.x without editing the *.h, *.c files?
costrom is offline   Reply With Quote

Old   November 14, 2014, 08:16
Default
  #10
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,972
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by costrom View Post
I apologize for asking a question that has been answered elsewhere, but...

I have a qMean file resulting from a dsmcFoam run, and I would like to use the heat fluxes from that as a boundary condition for a laplacianFoam runcase. is this currently possible in openFOAM 2.3.x without editing the *.h, *.c files?
I'm not familiar with that solver. qMean is average in time or average in space as a function of time or space?

Depending on that timeVaryingMappedFixedValue might be able to help you
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider 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
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
CFX doesn't continue calculation... mactech001 CFX 6 November 15, 2009 22:25
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Water vapour condensation in CFX-5.7.1 hdj CFX 1 November 27, 2005 08:15
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 04:26.