|
[Sponsors] |
September 23, 2005, 07:05 |
HI,
remove all Patches with
|
#1 |
Senior Member
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 17 |
HI,
remove all Patches with zero faces in it from the 'boundary' file in the polymesh directory and try. Pierre (colleague, who can't be bothered to register) |
|
September 23, 2005, 08:18 |
Hi Markus/Pierre,
I have g
|
#2 |
New Member
Max
Join Date: Mar 2009
Posts: 24
Rep Power: 17 |
Hi Markus/Pierre,
I have good & bad news: - your trick works, that means the mapFields goes to the end w/o problems; - nothing is written in the target directory! It is the same behaviour I get without -consistent flag. In my boundary files I have just a wall, inlet/outlet and wedge (two different patches) faces. Have you suggestion how I can debug further? Thanks Massimiliano |
|
September 23, 2005, 12:41 |
Right then, well it worked for
|
#3 |
Member
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 17 |
Right then, well it worked for me following these steps:
i.e if mapping from SourceCase/500/ to TargetCase/500/ - make sure the latter dir exists - In the target case, make sure that no previous internal Fields are written, specify instead for example for variable U internalField uniform (0.569 0 0); (no list size specified) - pray to the CFD god I couldn't explain why it works rather than another way, but I trust that doensn't bother you that much right now. Pierre |
|
September 23, 2005, 12:46 |
Have a look at the source code
|
#4 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
Have a look at the source code: it's all to do with how you specify which time directory from the source case you want to map and where you want to put the results. If you use things like startTime or latestTime, it's easy to get confused...
Nothing wrong with the code as far as I know. Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
September 26, 2005, 04:20 |
Hi Hrvoje,
you were right,
|
#5 |
New Member
Max
Join Date: Mar 2009
Posts: 24
Rep Power: 17 |
Hi Hrvoje,
you were right, nothing wrong with the code. It was my fault: in the targetDir the controlDict had a false startTime (0.0091 instead 0.00091). I can only say that an error message (like "restart directory not found") could help me to find the problem Anyway, this was a good reason to compile OpenFoam in debug mode and look inside it... Just a last question: each time I run blockMesh defaultFaces patch is created (with 0 faces) and this is a problem for mapFields (see the first message). How can I avoid it? Thanks Massimiliano |
|
September 26, 2005, 05:33 |
A zero sized patch defaultFace
|
#6 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
A zero sized patch defaultFaces is kept if mergePatchPairs option is used.
There used to be a reason for this but I forgot why... |
|
December 14, 2007, 15:34 |
Hi all,
I'm trying to do a
|
#7 |
Senior Member
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 |
Hi all,
I'm trying to do a mapfields from one case to another. Only the mesh has been refined, so that geometry is essentially the same. Here is the excerpt from mapFields: /*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.4.1 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : mapFields . re65 . re65new -consistent Date : Dec 10 2007 Time : 07:57:15 Host : moondance PID : 6167 Root : Case : Nprocs : 1 Source: "." "re65" Target: "." "re65new" Create databases as time Source time: 110 Target time: 110 Create meshes Source mesh size: 3653328 Target mesh size: 29226624 It has been at this state for about 4 days now. Is this normal when working with such mesh sizes? The machine running mapFields has eight 2.8 GHz opteron processors with 128GB memory. |
|
May 11, 2008, 05:53 |
Hi Srinath,
No, this is not n
|
#8 |
Senior Member
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 17 |
Hi Srinath,
No, this is not normal. Something else: I have the experience that using consistent on refined meshes is not always ok. Especially when there are curved areas near the boundaries the domain might have been changed, causing mapfields to fail on consistent. However switching it off and supplying a patch map list works perfect. Also if you interpolate to a case with different boundary conditions, the latter works. Brgds Mark |
|
November 17, 2008, 03:18 |
Hi all,
I need to use the c
|
#9 |
Senior Member
stephane sanchi
Join Date: Mar 2009
Posts: 314
Rep Power: 18 |
Hi all,
I need to use the command 'mapFields' between a coarse emsh and a medium mesh. I have used the 'rasInterFoam' solver until time t = 0.094 sec. The case with the coarse mesh has run on 10 processors. The case with the medium mesh will run on 10 processors. Could someone tell me the command to map the 'coarse' solution on the 'medium' grid. Thanks. Regards, Stephane. |
|
July 22, 2009, 08:55 |
|
#10 | |
Member
Marco Turchi
Join Date: Jul 2009
Location: Pesaro, Italy
Posts: 31
Rep Power: 17 |
First of all you have to run "blockMesh", for the new mesh.
Then, probably, the command you are looking for is: Quote:
You have to specify also the reference case directory. I hope it is useful! MT |
||
December 4, 2012, 20:12 |
|
#11 |
Senior Member
Join Date: Nov 2012
Posts: 171
Rep Power: 14 |
Hi All,
Can I ask you a question about the utility mapFields? My question is as follows: I got the simulation results with structured meshes. Now I generated the unstructured meshes (totally the same geometry but on one wall a small inlet is newly generated). I list all other boundaries except that wall in patchMap list. All other procedures are followed by the friends posted in this forum. The mapped field file is generated, but the internal flow fields are completely wrong. This is not what I want. Can I only map the internal flow field from structured to an unstructured meshes? Those boundary values are obtained through the boundary treatment as specified in the target case? Thanks. -hz |
|
December 5, 2012, 08:58 |
|
#12 |
Member
Marco Turchi
Join Date: Jul 2009
Location: Pesaro, Italy
Posts: 31
Rep Power: 17 |
Hi,
what do you mean with "the internal flow fields are completely wrong"? Have you the possibility to run the new geometry? Perhaps you can use mapField to have an initial (wrong) flow field, then run some coarse cases and then refined the mesh (untill you want or you have the capacity). I hope it is useful, otherwise ask! |
|
December 5, 2012, 09:33 |
|
#13 |
Senior Member
Join Date: Nov 2012
Posts: 171
Rep Power: 14 |
Hi Zebu83,
I am sorry, I did not express this clearly. In the source mesh, the flow field is fully developed. This is the reason why I would like to map this to my new unstructured meshes. I want to start based on this results. However, when I mapped the results to the target case, they are completely different. I tried the following several ways: 1, leave the patchMap and cuttingPatches lists blank 2, leave the cuttingPatches blank, and write some of the boundary in patchMap The mapped results are always the one I mentioned above. In fact, I would like to only the internal fields, because the boundary values can be calculated directly according to the specification in the target case (unstructured meshes). Thank you very much. hz |
|
September 22, 2014, 04:14 |
|
#14 |
New Member
sandy
Join Date: Aug 2011
Posts: 13
Rep Power: 15 |
Hi OpenFOAM users,
In regard to mapfields usage, it needs to be mentioned that the target fields files SHOULD NOT have the entry in the form of nonuniform list. If it is please make it uniform with a single value and let mapFields create the non uniform field based on source fields. Thanks Sandy |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
MapFields only on internal fields | cosimobianchini | OpenFOAM Pre-Processing | 5 | May 5, 2020 07:08 |
MapFields | Luiz Eduardo Bittencourt Sampaio (Sampaio) | OpenFOAM Pre-Processing | 18 | September 28, 2017 12:06 |
MapFields failure or incorrect mesh | jvn | OpenFOAM Pre-Processing | 19 | November 29, 2012 07:13 |
MapFields turbulent pipe flow | anita | OpenFOAM Pre-Processing | 5 | July 4, 2008 00:29 |
MapFields | cpplabs | OpenFOAM Running, Solving & CFD | 3 | February 17, 2008 06:08 |