[panachristos]

Hello Foamers,

I am a new member in this community and this is my first post/thread.

To begin, i ran the case 'counterFlowFlame2D' from the tutorials and it is okay.

Then, i want to refine the mesh so i did the followings:

1)create a directory called 'counterFlowFlame2DFine'
2)copy into it 'constant' and 'system' from the original case
3)in blockMeshDict i refined the mesh from (100 40 1) to (200 80 1)

Then i ran the case by typing:
a)blockMesh
b)mapFields ../counterFlowFlame2D -consistent -sourceTime 'latestTime'

And i am getting the following message:

Create databases as time
Case   : ../counterFlowFlame2D
nProcs : 1

Source time: 0.2
Target time: 0

Create meshes

Source mesh size: 4000  Target mesh size: 16000


Consistently creating and mapping fields for time 0.2

Creating mesh-to-mesh addressing for region0 and region0 regions using cellVolumeWeight
    Overlap volume: 0
Creating AMI between source patch fuel and target patch fuel using faceAreaWeightAMI
    AMI: Creating addressing and weights between 40 source faces and 80 target faces
    AMI: Patch source sum(weights) min/max/average = 1, 1, 1
    AMI: Patch target sum(weights) min/max/average = 1, 1, 1
Creating AMI between source patch air and target patch air using faceAreaWeightAMI
    AMI: Creating addressing and weights between 40 source faces and 80 target faces
    AMI: Patch source sum(weights) min/max/average = 1, 1, 1
    AMI: Patch target sum(weights) min/max/average = 1, 1, 1
Creating AMI between source patch outlet and target patch outlet using faceAreaWeightAMI
    AMI: Creating addressing and weights between 200 source faces and 400 target faces
    AMI: Patch source sum(weights) min/max/average = 1, 1, 1
    AMI: Patch target sum(weights) min/max/average = 1, 1, 1
    interpolating thermo:psi
    interpolating N2
    interpolating O2
    interpolating dQ
    interpolating CO2
    interpolating p
    interpolating CH4
    interpolating T
    interpolating H2O
    interpolating thermo:alpha
    interpolating U

End

The problem as you can see is the Overlap volume: 0

So, from original case only the boundary fields have been patched to the new case and not the internal fields. Then, do you have any idea what to do ?

Best regards,

Christos

[panachristos]

I am still facing this problem. Anybody to help?

[wyldckat]

Quick question: Which specific OpenFOAM version are you using?

[panachristos]

Dear Bruno,

Thank you for the reply! I am using 2.3.x version.

[wyldckat]

Quick answer: I believe this was a bug in OpenFOAM 2.3.x that was fixed in 2.4.x or 3.0.x.

Anyway, this worked for me:

mapFields ../counterFlowFlame2D -consistent -sourceTime 'latestTime' -mapMethod mapNearest

How I figured it out:

mapFields ../counterFlowFlame2D -consistent -sourceTime latestTime -help

Then:

mapFields ../counterFlowFlame2D -consistent -sourceTime latestTime -mapMethod a

and got this:

--> FOAM FATAL ERROR: 
a not found in table.  Valid entries: 
3
(
cellVolumeWeight
direct
mapNearest
)

[panachristos]

Thank you Bruno!

This is a nice way to overcome the bug caused by cellVolumeWeight !!!
It works now.

With kind regards,
Christos

[panachristos]

Actually I just found that mapNearest method does not patch ALL fields correctly!

For example, for this counterflowflame2D case it does not patch correctly the fields of p,alpha and psi !

Since, 2.3.x version looks to have many bugs regarding mapFields, i recommend to use another version for mapping e.g. 2.2.2, as already Philipp has mentioned in an older threat:

http://www.cfd-online.com/Forums/ope...-question.html

Thus, i followed his advice and the mapping was correctly done.

[Andrea_85]

Hi,

i know it is an old thread but i am having problems in using mapFields under openfoam 2.3.1. I want to map (only) the internal fields between two inconsistent geometries that overlap in a specific region, therefore i left the mapFieldsDict empty. Both cellVolumeWeight and direct method do not interpolate anything since they both return:

Overlap volume: 0

which is not correct

If i use mapNearest it gets stuck forever at this point

Creating mesh-to-mesh addressing for region0 and region0 regions using mapNearest

.

I tried to compile mapField 2.4.x under my version of openfoam but it does the same. mapfields 3.0.x or 2.2.2 do not complie under 2.3.1.

any idea about having a working mapFields under openfoam 2.3.1?
How did you compile mapFields 2.2.2 under 2.3.x?


Best,
Andrea

[DominicTNC]

Hi,

I am facing the same problem as mentioned by Andrea. Using OF2.4.0, Overlap volume gives 0 if direct map method is used. If mapNearest is used, the program stuck forever at the same point.

P.S. My mapFieldsDict is empty also.

Any comments are appreciated. Thank you.



Dominic

[Elham]

Originally Posted by DominicTNC

Hi,

I am facing the same problem as mentioned by Andrea. Using OF2.4.0, Overlap volume gives 0 if direct map method is used. If mapNearest is used, the program stuck forever at the same point.

P.S. My mapFieldsDict is empty also.

Any comments are appreciated. Thank you.



Dominic

Dear Dominic,


Do you remember how you could fix the problem? I am facing the same issue.


Cheers,


Elham