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

MapFields doesnt work in the "counterFlowFlame2D" tutorial case

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

Like Tree2Likes
  • 2 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 12, 2016, 11:29
Default MapFields doesnt work in the "counterFlowFlame2D" tutorial case
  #1
New Member
 
christos panagopoulos
Join Date: Apr 2016
Posts: 7
Rep Power: 5
panachristos is on a distinguished road
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:

Code:
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 is offline   Reply With Quote

Old   April 15, 2016, 13:19
Default Please any help???
  #2
New Member
 
christos panagopoulos
Join Date: Apr 2016
Posts: 7
Rep Power: 5
panachristos is on a distinguished road
I am still facing this problem. Anybody to help?
panachristos is offline   Reply With Quote

Old   April 16, 2016, 12:28
Default
  #3
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,956
Blog Entries: 43
Rep Power: 121
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick question: Which specific OpenFOAM version are you using?
__________________
wyldckat is offline   Reply With Quote

Old   April 17, 2016, 05:15
Default
  #4
New Member
 
christos panagopoulos
Join Date: Apr 2016
Posts: 7
Rep Power: 5
panachristos is on a distinguished road
Dear Bruno,

Thank you for the reply! I am using 2.3.x version.
panachristos is offline   Reply With Quote

Old   April 17, 2016, 18:39
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,956
Blog Entries: 43
Rep Power: 121
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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:
Code:
mapFields ../counterFlowFlame2D -consistent -sourceTime 'latestTime' -mapMethod mapNearest
How I figured it out:
Code:
mapFields ../counterFlowFlame2D -consistent -sourceTime latestTime -help
Then:
Code:
mapFields ../counterFlowFlame2D -consistent -sourceTime latestTime -mapMethod a
and got this:
Code:
--> FOAM FATAL ERROR: 
a not found in table.  Valid entries: 
3
(
cellVolumeWeight
direct
mapNearest
)
Elham and panachristos like this.
wyldckat is offline   Reply With Quote

Old   April 18, 2016, 05:22
Default
  #6
New Member
 
christos panagopoulos
Join Date: Apr 2016
Posts: 7
Rep Power: 5
panachristos is on a distinguished road
Thank you Bruno!

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

With kind regards,
Christos
panachristos is offline   Reply With Quote

Old   April 18, 2016, 12:56
Default
  #7
New Member
 
christos panagopoulos
Join Date: Apr 2016
Posts: 7
Rep Power: 5
panachristos is on a distinguished road
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.
panachristos is offline   Reply With Quote

Old   June 30, 2017, 07:34
Default
  #8
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 319
Rep Power: 12
Andrea_85 is on a distinguished road
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:

Code:
Overlap volume: 0
which is not correct

If i use mapNearest it gets stuck forever at this point

Code:
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
Andrea_85 is offline   Reply With Quote

Old   November 2, 2017, 22:40
Default
  #9
Member
 
Dominic
Join Date: Jan 2017
Posts: 41
Rep Power: 5
DominicTNC is on a distinguished road
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
DominicTNC is offline   Reply With Quote

Old   August 26, 2018, 22:27
Default
  #10
Senior Member
 
Elham
Join Date: Oct 2009
Posts: 184
Rep Power: 12
Elham is on a distinguished road
Quote:
Originally Posted by DominicTNC View Post
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
Elham is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
HronTurekFsi tutorial case using icoFsiElasticNonLinULSolidFoam MarcelK OpenFOAM Running, Solving & CFD 9 February 25, 2019 03:25
Propeller case in AMI tutorial reza1980 OpenFOAM Running, Solving & CFD 68 November 28, 2017 22:37
[SOWFA] NREL SOWFA Tutorial case mohsen.boojari OpenFOAM Community Contributions 0 March 8, 2016 11:35
Cavity tutorial case shinde.gopal OpenFOAM Running, Solving & CFD 3 June 12, 2015 06:50
oscillatingInletACMI2D tutorial case for compressible flow jimteb OpenFOAM Running, Solving & CFD 0 February 6, 2015 06:17


All times are GMT -4. The time now is 12:18.