|
[Sponsors] |
How to map surface of one case to boundary of other cases? |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
Member
Jun
Join Date: Nov 2015
Posts: 57
Rep Power: 10 ![]() |
Dear all,
Currently, I am trying to solve a case which requires fully developed inlet velocity profile. The inlet has square cross section. In addition, the fluid is non-Newtonian so there is no exact solution for the inlet velocity profile. I have two options; putting straight channel longer than entrance length or calculating the straight channel separately and mapping the fully developed velocity profile to inlet of the original case. I know there is "mapFields" utility but that utility maps fields not surface and both cases have overlapped section. What I want is that mapping the cutting plane (not outlet patch) inside the first case to the inlet of the second case. How can I do this? Any advice would be helpful. Thanks. Jun |
|
![]() |
![]() |
![]() |
![]() |
#2 | |
Senior Member
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 237
Rep Power: 18 ![]() |
Quote:
For this problem I normally sample a plane in the source case, using foamCase as output format. Then I take the output of sample, place it in constant/boundaryData and apply it to the inlet of the second case, positioned in the same place as the cutting plane, using timeVaryingMappedFixedValue BC. I am not sure if the sampled data is ready as it is or the files need some little manipulation, but the general process is what is described above. Hope this helps, Francesco |
||
![]() |
![]() |
![]() |
![]() |
#3 |
Member
Jun
Join Date: Nov 2015
Posts: 57
Rep Power: 10 ![]() |
Dear Francesco,
Thank you for the reply. Actually, it seems that you gave me the correct solution. I thought timeVaryngMappedFixedValue BC might be the solution but I doubt whether it is or not. Anyway, I could start to check with your advice though it needs some more as you already said. The sequence is as below. 1. Sample the surface using sampleDict. Export the sampled data in the format "foamFile". 2. Make directory at constant/boundaryData/inlet/0. 3. Among the sampled data, copy "points" to constant/boundaryData/inlet. 4. Among the sampled data, copy field data to constant/boundaryData/inlet/0. in my case, I only need velocity field U so I coppied U from sampled data. 5. Header should be added for "points" and field files. As in pitzDailyExptInlet tutorial, add headers for each files. 6. Set the boundary type to timeVaryingMAppedFixedValue and add "offset (0 0 0); setAverage off;" for vector field or "offset 0; setAverage off;" for scalar field. 7. Run the simulation. I only checked it for simple 2D channel flow. I will apply this to my case and let you know the result. Again, thank you so much. Best regards, Jun Last edited by mykkujinu2201; May 23, 2019 at 04:14. |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Member
Jun
Join Date: Nov 2015
Posts: 57
Rep Power: 10 ![]() |
Dear Francesco,
I tested for my case which is about 3D problem. It works pefectly. Thank you again. Best regards, Jun |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Senior Member
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 237
Rep Power: 18 ![]() |
Great!
Have fun, Francesco |
|
![]() |
![]() |
![]() |
![]() |
#6 | |
New Member
Fab
Join Date: Apr 2019
Posts: 27
Rep Power: 7 ![]() |
I tried the following with the 2106 version.
Quote:
Well, I have no clue about what is happening, openFoam complains and says this : --> FOAM FATAL ERROR: (openfoam-2106) Only 0 provided. Need at least three non-colinear points to be able to interpolate. From Foam::coordSystem::cartesian Foam: ![]() in file triSurface/triSurfaceTools/pointToPointPlanarInterpolation.C at line 57. FOAM exiting Has anyone any idea ? I just want to use a boundaryField that I sampled from another case as a fixedValue BC, it shoudn't be that hard... Meshes are different but topologically, the patch is strictly the same... |
||
![]() |
![]() |
![]() |
![]() |
#7 | |
New Member
shiyu
Join Date: Mar 2018
Location: london
Posts: 7
Rep Power: 8 ![]() |
Hi Rotidpor, I have just encountered the same problem with version 2206. I am wondering if you have fixed this kind of error.
Thanks. Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#8 |
New Member
Fab
Join Date: Apr 2019
Posts: 27
Rep Power: 7 ![]() |
Well, it might not be the most elegant way to solve this but anyways...
I solved the issue in my case by using the file faceCenters instead of points. I just follow the procedure written here but I replace "points" by "faceCenters" (also generated by sampleDict) and rename it points. I don't know what is going on, don't know how it works but it does, at least in my case. |
|
![]() |
![]() |
![]() |
Tags |
mapfields, sampledict |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Cluster ID's not contiguous in compute-nodes domain. ??? | Shogan | FLUENT | 1 | May 28, 2014 15:03 |
Question about heat transfer coefficient setting for CFX | Anna Tian | CFX | 1 | June 16, 2013 06:28 |
domain imbalance for enrgy equation | happy | CFX | 14 | September 6, 2012 01:54 |
Axysimmetric cases compare to planar case with symmetry boundary condition | hafiidz | FLUENT | 5 | June 14, 2011 06:29 |
CFX4.3 -build analysis form | Chie Min | CFX | 5 | July 12, 2001 23:19 |