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

Adding a user application class

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2006, 08:25
Default Thank you Niklas! It gives
  #21
newbee
Guest
 
Posts: n/a
Thank you Niklas!

It gives the same answer but now I have the correct unit.

Somehow i get a really cool section in the end of my channel (170 K). This is strange because my temperatures are defined as follows:

inlet (280 K) fixed value
internal (300 K) initial
heating wall (330 K) fixed value

I think this could have something tot do with the relaxationfactor for T but Ill look further into that.

Thanks again!
Erik
  Reply With Quote

Old   May 30, 2006, 06:00
Default Hi all, I want to add a sou
  #22
newbee
Guest
 
Posts: n/a
Hi all,

I want to add a source term to the temperature calculation for the cells that are in contact with one of the patches. So that it looks something like:

solve

(
fvm::div(phi, T)
- fvm::laplacian(alphaEff, T)
q*Aw/(rho*Cp*V)
);

where:
Aw=area of cell in contact with wall
rho=density
Cp=specific heat
V=volume of cell

for the cells that arent in contact with this patch I want to do the ordinary temperature calculation without a source i.e.:


solve
(
fvm::div(phi, T)
- fvm::laplacian(alphaEff, T)
);

Can anyone please give me an idea of how to do this?

Thank you
/Erik
  Reply With Quote

Old   May 30, 2006, 06:52
Default In other words: you want to ha
  #23
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
In other words: you want to have a patch with a constant heat flux. Like it says in the bible: "Give the emporer what belongs to the emporer and the boundary condition what belongs to the boundary condition"

What you want to do (if I remember it correctly, it can be found somewhere else on the board) is apply a fixedGradient boundary condition on that patch and leave the equation as it is (no source term).
__________________
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   May 30, 2006, 07:09
Default Thanks for your answer! I h
  #24
newbee
Guest
 
Posts: n/a
Thanks for your answer!

I have been experimenting with the fixedboundary condition for temperature and got a few results. The problem is that TempGrad=HeatFlux/heatTransfCoeff where the heat TransfCoeff is very difficult to calculate because of the high turbulance. The heat flux is on the otherhand well determend in the experiment that im trying to reconstruct.

/Erik
  Reply With Quote

Old   May 30, 2006, 07:25
Default Then there are two ways to do
  #25
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Then there are two ways to do it:

1. Program a new boundary condition (derive from fixedGradient etc). This is the recommended way, I guess

2. create at the start of the program a volScalarField qSrc that is 0 everywhere and q*Aw/(rho*Cp*V) in the cells near the patch. Then simply add the field as a source-Term to the equation. The fun part is setting that field at the start of he simulation:
a) find the patch
b) loop over the faces in the patch
c) set the value in the cell near the patch

Solution 1 is more elegant but harder if you never programmed a BC before, Solution 2 is mesier
__________________
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   May 30, 2006, 07:33
Default Thank you very much. I guess m
  #26
newbee
Guest
 
Posts: n/a
Thank you very much. I guess method 2 is for me then. Time to get craking code.
  Reply With Quote

Old   May 30, 2006, 10:07
Default are the a,b,c steps for findin
  #27
newbee
Guest
 
Posts: n/a
are the a,b,c steps for finding the cell volumes and face areas?

I have now constructed a volScalarFild containing the constant q value. I thought I could make the q*Aw/(rho*Cp*V) calculation on an other line outside the volScalarFild implementation with the a,b,c steps.

Thanks
/Erik
  Reply With Quote

Old   May 30, 2006, 10:28
Default Is the boundary field (patch)
  #28
newbee
Guest
 
Posts: n/a
Is the boundary field (patch) the outermost cell layer or is it just the surrounding of the mesh?
  Reply With Quote

Old   May 31, 2006, 07:12
Default Hi Erik! I'm having second
  #29
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Erik!

I'm having second thoughts about solution 2: you'll have to choose a boundary condition for the patch anyway (fixedValue is out of the question and with zeroGradient I see a chance that with the source-term in the "boundary cells" I see a chance that the solution blows up, but I might be wrong).

Anyway:
@find the patch:
label patchIndex=mesh.boundaryMesh().findPatchID(patchNa me);
const fvPatch &thePatchItself=mesh.boundary()[patchIndex];

@loop over the patch:
forAll(thePatchItself,faceI) {
label cellI=thePatchItself.faceCells()[faceI];

// @set the value (just an example Aw/V):
qSrc[cellI]=mesh.Sf().boundaryField()[patchIndex][faceI]/mesh.V()[cellI];
}
__________________
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   May 31, 2006, 08:32
Default Ok, thanks for your help I wil
  #30
newbee
Guest
 
Posts: n/a
Ok, thanks for your help I will try to implement this and se if it works anyway.

When calculating Aw/V as above I get the following error message:

createFields.H:54: error: cannot convert 'Foam::Vector<foam::scalar>' to 'double' in assignment

I guess that Aw is the wrong type because i can set qSrc[celli]=mesh.V()[cellI];

do you or anyone else hava a sugestion of how to make Aw the right format?

Thanks
/Erik
  Reply With Quote

Old   May 31, 2006, 08:47
Default Sorry. I forgot. Sf is a vecto
  #31
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Sorry. I forgot. Sf is a vector normal to the face whose length is the area of the surface. simply put a mag() around the vector and everything will be well.
__________________
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   May 31, 2006, 12:29
Default Thank you very much Bernhard.
  #32
newbee
Guest
 
Posts: n/a
Thank you very much Bernhard. The calculations seems to work fine. I get 60 itterations at the most for the energy calculation. Its worse with the pressure calculation which reaches 1000 iterations and causes time step continuity errors. I guess thats caused by bad intitial values.

Thank you again
/Erik
  Reply With Quote

Old   June 2, 2006, 02:12
Default aha,.. the pressure with 10
  #33
newbee
Guest
 
Posts: n/a
aha,..

the pressure with 1000 iterations is calculated with OpenFOAMs BCs taken from simpleFoam. My temperature calculations are done with 5 -50 iterations which may still be too much.

Anyway I need to do something about the pressure.

Thanks for your help so far anyway! It gave me better understanding.

/Erik
  Reply With Quote

Old   June 6, 2006, 05:11
Default Hi, I'm not getting reasonabl
  #34
newbee
Guest
 
Posts: n/a
Hi,
I'm not getting reasonable results from my source term mentioned above which is implemented in the following way:


//find the patch:
label patchIndex=mesh.boundaryMesh().findPatchID("hole") ;
const fvPatch &thePatchItself=mesh.boundary()[patchIndex];

//loop over the patch:
forAll(thePatchItself,faceI) {
label cellI=thePatchItself.faceCells()[faceI];

//set the value (just an example Aw/V):
Aw[cellI]=mag(mesh.Sf().boundaryField()[patchIndex][faceI]);
V[cellI]=mesh.V()[cellI];
S[cellI]=Aw[cellI]/V[cellI];
}

//With the energy equation as the following:

solve
(
fvm::div(phi, T)
- fvm::laplacian(alphaEff, T)
- S*q/(rho*Cp)
);


(Aw=cell area faceing heated wall; are the seme for all heated cells)
(V=volume of cell; gets biger along heated patch)

The problem is that I need a large cell structure in order to gett more heat to the smaler cell volumes as the code above implies. When I want to make the cell structure smaller to improve the resolution It switches so that more heat is transfered to the larger cell volumes instead of the smaler ones which is expected.

Do you Bernhard or maybe someone else know what I can do to always get most heat to the smaler cellvolumes.

I would like to attach describing graphes from paraFoam but I dont know how.

Thanks
/Erik
  Reply With Quote

Old   June 7, 2006, 07:32
Default does a finer mesh always lead
  #35
newbee
Guest
 
Posts: n/a
does a finer mesh always lead to greater reselotion or could it cause computational errors as my problem stated above. Because I really expect the source to give a higher temperature in a more narrow channel.

Thanks
/Erik
  Reply With Quote

Old   June 7, 2006, 09:56
Default Hi Erik! Problems like that
  #36
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Erik!

Problems like that is why a boundary condition should be implemented with a boundary condition (and not a source-term).

Instead of a solution I have some questions:
- are the V and Aw fields necessary? (I think temporary scalars inside the loop are sufficient)
- with higher resolution you mean: a) the faces on the patch have a higher resolution b) the third dimension pointing away from the patch has a higher resolution c) both?

Pictures would be helpful. See in the tab on the left of the Window under Documentation->Formatting how to append these
__________________
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   June 7, 2006, 10:48
Default test http://www.cfd-online.co
  #37
newbee
Guest
 
Posts: n/a
test

  Reply With Quote

Old   June 7, 2006, 11:06
Default Hi again Bernhard Thanks ag
  #38
newbee
Guest
 
Posts: n/a
Hi again Bernhard

Thanks again for helping me. I choose the source term method just because it should be easier and its probably still too advanced for me to implement my own BC. Anyhow here are three pictures of my channel. the three strait patches are symmetry sides and the curved one should be a heat source. The pictures show that the temperature is higher in the more narrow part of the channel for the rough grading and vice versa for the finer grading. According to experimental data the rough grading describes the temperature most correctly.

10x10x30

15x15x30

30x30x30


kind regards
/Erik
  Reply With Quote

Old   June 7, 2006, 11:23
Default I have made Aw and V temporary
  #39
newbee
Guest
 
Posts: n/a
I have made Aw and V temporary scalars once again like you sugested. I just tried makeing volscalarfields of them to se if it resolved any computational errors if there where any but I got the exact same result.

With resolution I ment a) i.e. more measuring points and better physical representation caused by better correspondance with continuity.

Thanks
/Erik
  Reply With Quote

Old   June 7, 2006, 11:44
Default Hi Erik! The last number of
  #40
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Erik!

The last number of subdivisions (30) which is fixed is in the direction pointing "away" from the viewer? (With resolution I meant "grid"-reolution, so I guess of the three choices given above it is c.) )

Questions about the pictures:
- in the second picture I see a discontinuity of the temperature on the curved surface. Where is that from?
- funny thing is that I can believe that the pictures with the coarsest and the finest grid (first and third) were calculated with the same conditions, but not for the second. Have you checked that?
- were all simulations done to the same level of convergence?
__________________
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
Tmp class maka OpenFOAM Bugs 2 August 20, 2008 14:53
Class Project Tiger Main CFD Forum 5 March 13, 2006 16:58
OpenFoam 12 Adding a user application class vvqf OpenFOAM Pre-Processing 3 October 27, 2005 13:18
Adding new class in version 12 billy OpenFOAM Pre-Processing 1 October 10, 2005 04:47
Expanding a class fabianpk OpenFOAM 0 October 3, 2005 04:26


All times are GMT -4. The time now is 18:57.