openfoam merge requestshttps://develop.openfoam.com/Development/openfoam/-/merge_requests2020-06-05T13:42:24Zhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/354ENH: Improve and verify atmBoundaryLayerInlet conditions2020-06-05T13:42:24ZKutalmış BerçinENH: Improve and verify atmBoundaryLayerInlet conditions### Summary
- Related to the log-law type ground-normal inflow boundary conditions for
wind velocity and turbulence quantities for homogeneous, two-dimensional,
dry-air, equilibrium and neutral atmospheric boundary layer (ABL) m...### Summary
- Related to the log-law type ground-normal inflow boundary conditions for
wind velocity and turbulence quantities for homogeneous, two-dimensional,
dry-air, equilibrium and neutral atmospheric boundary layer (ABL) modelling
- ENH: Generalises Richards-Hoxey expressions. This allows to input experimental profiles or heuristic spatial-variant profiles in a mathematically consistent way.
Yang, Y., Gu, M., Chen, S., & Jin, X. (2009).
New inflow boundary conditions for modelling the neutral equilibrium
atmospheric boundary layer in computational wind engineering.
J. of Wind Engineering and Industrial Aerodynamics, 97(2), 88-95.
DOI:10.1016/j.jweia.2008.12.001
- ENH: Adds new generalised `atmBoundaryLayerInletOmega` boundary condition by using:
Yang, Y., Gu, M., & Jin, X., (2009).
New inflow boundary conditions for modelling the
neutral equilibrium atmospheric boundary layer in SST k-ω model.
In: The Seventh Asia-Pacific Conference on Wind Engineering,
November 8-12, Taipei, Taiwan.
- ENH: Adds new verification case `tutorials/verificationAndValidation/atmosphericFlows/HargreavesWright_2007` by using:
Rectangular prism shown in FIG 1 of
Hargreaves, D. M., & Wright, N. G. (2007).
On the use of the k–ε model in commercial CFD software
to model the neutral atmospheric boundary layer.
Journal of wind engineering and
industrial aerodynamics, 95(5), 355-369.
DOI:10.1016/j.jweia.2006.08.002
Benchmark data:
HW, 2007 FIG 6
- BUG: Fixes value-entry behaviour in `atmBoundaryLayerInlet` (fixes #1578) (Thanks to @perjorgensen for the bug report).
- Without this change:
- for serial-parallel computations, if `value` entry is available in
an `atmBoundaryLayerInlet` BC, the theoretical ABL profile expressions
are not computed, and the `value` entry content is used as a profile data
- for parallel computations, if `value` entry is not available, `decomposePar`
could not be executed.
- With this change:
- assuming `value` entry is always be present, the use of `value` entry for
the ABL profile specification is determined by a flag `initABL`
- the default value of the optional flag `initABL` is `true`, but whenever
`initABL=true` is executed, `initABL` is overwritten as `false` for the
subsequent runs, so that `value` entry can be safely used.
- BUG: Ensures `atmBoundaryInlet` conditions are Galilean-invariant (fixes #1692)
- DOC: Improves `atmBoundaryLayerInlet` header documentation
### Resolved bugs (If applicable)
#1578
#1692
### Details of new models (If applicable)
##### kEpsilon-parallelHierarchical8-Gcc74DP:
![Ux_upstream](/uploads/8586589de26be6cbf33602f420b1872d/Ux_upstream.png)
![Ux_mid](/uploads/e89a57641ff4799d90e60b760bac2cb8/Ux_mid.png)
![Ux_downstream](/uploads/5227ff27d82ad807ed12b216f4d8d87e/Ux_downstream.png)
![epsilon](/uploads/75d3f250399b9ecd27ccab11f424299c/epsilon.png)
![k](/uploads/9796779be6eebebdc8ac92ec22e3335f/k.png)
##### kOmegaSST-parallelHierarchical8-Gcc74DP:
![Ux_upstream](/uploads/4a7d7c94ea8b5a3147b16d0b05013be4/Ux_upstream.png)
![Ux_mid](/uploads/be83cc10455335ae3c85f9237fc1e489/Ux_mid.png)
![Ux_downstream](/uploads/1f31d8d2ef9872f4be0ac0dba5e8234b/Ux_downstream.png)
![k](/uploads/ecbebd53a4c6614877dece10e61f2a71/k.png)
![omega](/uploads/0420c6c1d4637f756d92992b7f884568/omega.png)
### Risks
##### Regression
Bitwise regression is preserved.
##### Changes to user input
- `zGround` is silently deprecated, and its functionality is now inherently computed.
- `d` is introduced for `displacement height`.
- ~~`Uref` and `Zref` are noisily deprecated:~~
- ~~`Uref` is renamed as `uRef` since it refers to a scalar rather than a vector `U`.~~
- ~~`Zref` is renamed as `zRef` since it was always a scalar.~~
### Future work
- These inlet conditions are limited to the surface layer portion of the atmospheric boundary layer:
- Neutral-stratified
- Dry-air
- No Ekman layer
- These inlet conditions can/should be generalised to stable/unstable stratification as well as into the Ekman layer since neutral conditions are **very rare**.
- Spatial variation in input of aerodynamic roughness length, `z0`, and displacement height, `d`.
- Further consistent boundary conditions are required to improve the verification case in terms of `nut` predictions for
- Top boundaries
- Ground boundariesv2006Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/363ENH: New atmospheric boundary layer (ABL) model suite (Part 1)2020-06-09T10:09:12ZKutalmış BerçinENH: New atmospheric boundary layer (ABL) model suite (Part 1)### Summary
This commit is the first main commit of a collaborative work between `OpenCFD Ltd.`-`ENERCON Gmbh`-`CENER`, for which there will be another comprehensive commit in the next release (may include SOWFA-6 - [see](https://gith...### Summary
This commit is the first main commit of a collaborative work between `OpenCFD Ltd.`-`ENERCON Gmbh`-`CENER`, for which there will be another comprehensive commit in the next release (may include SOWFA-6 - [see](https://github.com/NREL/SOWFA-6/issues/11) for exchange of ideas).
With this commit, OpenFOAM learns:
- How to comprehensively model (RANS) surface and Ekman atmosphere layers under (slightly/very) stable/unstable/neutral atmospheric stability conditions over spatiotemporal-variant terrain (e.g. partially forestry plain).
### Details
Please refer to the header file documentation for complete set of details.
- 8 new `fvOption`s that are usable with epsilon/omega-based RANS closure models:
- atmAmbientTurbSource
- atmBuoyancyTurbSource
- atmCoriolisUSource
- atmLengthScaleTurbSource
- atmPlantCanopyTurbSource
- atmPlantCanopyUSource
- atmPlantCanopyTSource
- atmNutSource
- 7 new `wall function`s shipped with `PatchFunction1` and `TimeFunction1` support for the input entries:
- atmAlphatkWallFunction
- atmEpsilonWallFunction
- atmNutkWallFunction
- atmNutUWallFunction
- atmNutWallFunction
- atmOmegaWallFunction
- atmTurbulentHeatFluxTemperature
- A new function object to quantify the [Obukhov length](http://glossary.ametsoc.org/wiki/Obukhov_length#:~:text=Obukhov%20length,consumption%20of%20turbulence%20kinetic%20energy.):
- ObukhovLength
- 3 new tutorials involving `buoyantBoussinesqSimpleFoam` verifications in comparison to field measurements:
- `verificationAndValidation/atmosphericFlows/atmFlatTerrain`
- verification with the `Leipzig` field experiment
- illustration of precursor/successor field mapping
- `verificationAndValidation/atmosphericFlows/atmForestStability`
- verification with the Sweden field experiment
- 2 new actuator disk modelling approaches in the existing `actuationDiskSource` wherein the incoming velocity measurements can now be held by using `topoSet`s.
### Resolved bugs (If applicable)
None.
### Verifications
The model suite was verified for `neutral stability` by the `Leipzig` experiment for which all the details can be found in, and can be reproduced by `verificationAndValidation/atmosphericFlows/atmFlatTerrain`
`buoyantBoussinesqSimpleFoam-kEpsilon`:
<img src="/uploads/96349ecee9d1561d196795b266d22cdd/u-z.png" width="250" height="500">
<img src="/uploads/146d8921d130e210f27b21f1c8a902ce/v-z.png" width="250" height="500">
`buoyantBoussinesqSimpleFoam-kOmegaSST`:
<img src="/uploads/aead7fafb086e2d918302d45660e8e61/u-z.png" width="250" height="500">
<img src="/uploads/bca10f4506b06986ed47c2114e9c43ad/v-z.png" width="250" height="500">
In addition, the model suite was verified for all spectrum of stability conditions with forestry ground by the `Sweden(?)` experiment for which all the details can be found in, and can be reproduced by `verificationAndValidation/atmosphericFlows/atmForestStability`
`buoyantBoussinesqSimpleFoam-kEpsilon` (wind speed, turbulent kinetic energy, and wind veer profiles, respectively):
<img src="/uploads/370aca91fc19f2fbb719ce4655ad4618/uNorm-zNorm.png" width="600" height="500">
<img src="/uploads/e024e77ee5460299774ccaeff9e360c5/kNorm-zNorm.png" width="600" height="500">
<img src="/uploads/d292e5901e01dbb0bc517d9c76be79b2/veer-zNorm.png" width="600" height="500">
with the Obukhov lengths:
veryStable = 44.7979
stable = 300.723
slightlyStable = 859.962
neutral = undefined
slightlyUnstable = -547.088
unstable = -265.992
`buoyantBoussinesqSimpleFoam-kOmegaSST` (wind speed, turbulent kinetic energy, and wind veer profiles, respectively):
<img src="/uploads/4e19e3e02e97044e8d2dda9e718e2e32/uNorm-zNorm.png" width="600" height="500">
<img src="/uploads/8803c8bbe63de1ac2015310615521fa2/kNorm-zNorm.png" width="600" height="500">
<img src="/uploads/c938b5ae2d5fd19e5116bd00b910809a/veer-zNorm.png" width="600" height="500">
with the Obukhov lengths:
veryStable = 67.5555
stable = 396.562
slightlyStable = 1147.69
neutral = undefined
slightlyUnstable = -707.885
unstable = -319.368
Furthermore, the persistence of atmospheric boundary layer inlet profiles downstream were quantified in comparison to the profiles near the outlet, and it was found out that the overall discrepancy is within 2%:
(wind speed, turbulent kinetic energy, turbulence intensity, and temperature horizontal profiles, respectively)
<img src="/uploads/e01e5f6429cb054adda7bddc649d4348/Horizontal_MagU.png" width="600" height="500">
<img src="/uploads/78472b8205b8c79a611793a9b0a6933a/Horizontal_k.png" width="600" height="500">
<img src="/uploads/f001568734ac5b398018ba1fd5349aa2/Horizontal_TI.png" width="600" height="500">
<img src="/uploads/21eaa5b3ec305eacb8f2af11c0226985/Horizontal_T.png" width="600" height="500">
### Risks
- **User input change:** `nutkAtmRoughWallFunction` is renamed without extra support to `atmNutkWallFunction` (ensured the bitwise regression)
- Since the majority of the utilities above are new, the potential effects on the existing utilities would only be unexpected.
v2006Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/364ENH: Miscellaneous enhancement/features and bug fixes2020-06-11T12:30:36ZKutalmış BerçinENH: Miscellaneous enhancement/features and bug fixesv2006Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/367AMI code enhancements2020-06-24T21:12:39ZAndrew HeatherAMI code enhancements### Summary
**Note: this is beta-level code and will receive further updates in future releases**
This change set includes:
- New option for `cyclicAMI` and `cyclicACMI` patches to perform topological updates to enforce a 1-to-1 m...### Summary
**Note: this is beta-level code and will receive further updates in future releases**
This change set includes:
- New option for `cyclicAMI` and `cyclicACMI` patches to perform topological updates to enforce a 1-to-1 match between source and target patches to ensure conservation across AMI patches and greatly reduced pressure field perturbations. Changes based on ref [1]
- Deprecated `directAMI`; replaced by `nearestFaceAMI`
- Significant code refactoring
### Resolved bugs (If applicable)
- General AMI conservation issues/noisy pressure predictions
### Details of new models (If applicable)
- Backwards compatibility [should be] maintained
- New topological changes triggered by using a special mesh motion solver: `dynamicFvMesh dynamicMotionSolverFvMeshAMI;`
- this may be absorbed into the 'standard' `dynamicMotionSolverFvMesh` model in future releases
- Test case: [mixerVesselAMI2D_with-boundary-layers.tgz](/uploads/4ca838c78e139007cb6f2f06026bdf07/mixerVesselAMI2D_with-boundary-layers.tgz)
| dynamicMotionSolverFvMesh | dynamicMotionSolverFvMeshAMI |
| ------ | ------ |
| ![plot](/uploads/37f8e095ad01c8c10dcdb9ab40ffa74c/plot.png) v2006| ![plot](/uploads/ad90049926e774bd3127256f86f0e075/plot.png) v2006|
| ![plot](/uploads/7a0930907ab64ac5941c6bcf781e17ba/plot.png) v1912| |
Note: since the AMI code triggers topological updates, to reconstruct parallel cases:
- use `reconstructParMesh` to reconstruct the mesh at each time, followed by `reconstructPar` to reconstruct the fields; or
- use `redistributePar -reconstruct` to reconstruct both mesh and fields (in parallel)
- Code refactoring has enabled greater control of the AMI; the AMIMethod can now be set in the `polyMesh/boundary` file, e.g.
```
AMI2
{
type cyclicAMI;
inGroups 1(cyclicAMI);
nFaces 96;
startFace 6336;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch AMI1;
// New optional entries
AMIMethod faceAreaWeightAMI;
restartUncoveredSourceFace 1;
}
```
### Deprecations
The `directAMI` method has been deprecated and replaced by the faster and more robust, new `nearestFaceAMI` method. The new method creates a 1-to-1 mapping based on the nearest face.
### Risks
- Significant change to AMI code
- Not only affects cyclic patches, but other areas of the code that make use of the tooling, e.g.:
- mapped patches
- mapFieldsPar
- region models (film modelling)
- mapping function objects
### Known issues/to check
When using `dynamicMotionSolverFvMeshAMI`
- restart behaviour not currently available
### Tests
Checked on the following cases:
- pimpleFoam/laminar/mixerVesselAMI2D
- pimpleFoam/RAS/oscillatingInletACMI2D
- XiDyMFoam/annularCombustorTurbine
- {customer turbo machinery}
For each, the `dynamicMotionSolverFvMesh` option recovers v1912 behaviour
### References
[1] H.J. Aguerre, S. Márquez Damián J.M. Gimenez, N.M.Nigro, *Conservative handling of arbitrary non-conformal interfaces using an efficient supermesh*, Journal of Computational Physics 335(15)21-49. 2017. https://doi.org/10.1016/j.jcp.2017.01.018
### Acknowledgements
- Many thanks to Horacio Aguerre @aguerrehoracio and Santiago Márquez @santiagomarquezd for bringing the methodology to our attention and for many useful discussions and testing throughout these developments.v2006https://develop.openfoam.com/Development/openfoam/-/merge_requests/369New Weber number cloud function object2020-06-11T14:00:37ZAndrew HeatherNew Weber number cloud function objectExample usage:
cloudFunctions
{
WeberNumber1
{
type WeberNumber;
}
}
This will calculate and write the Weber number field as a 'standard' cloud field, available for post-proces...Example usage:
cloudFunctions
{
WeberNumber1
{
type WeberNumber;
}
}
This will calculate and write the Weber number field as a 'standard' cloud field, available for post-processing alongside other lagrangian fields in the lagrangian/<cloudName> directory.
See example in `$FOAM_TUTORIALS/lagrangian/sprayFoam/aachenBomb/constant/sprayCloudProperties`v2006Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/379remove cyclic dependencies for phase systems2020-08-06T06:23:44ZMark OLESENremove cyclic dependencies for phase systems### centralize more libraries in src/phaseSystemModels
### avoid phaseSystem cyclic dependencies, reduce number of libraries
Previously the phaseSystems had a number of smaller libraries to
provide interface and model properties. ...### centralize more libraries in src/phaseSystemModels
### avoid phaseSystem cyclic dependencies, reduce number of libraries
Previously the phaseSystems had a number of smaller libraries to
provide interface and model properties. However, the cyclic
dependencies between phaseSystem and the models (and turbulence)
causes extreme difficultly for mingw linking. The potential
additional flexibility is not actually used anywhere.
- libincompressibleMultiphaseSystems
- removed: libmassTransferModels
- libmultiphaseSystem
- removed: libcompressibleMultiphaseEulerianInterfacialModels
- libreactingMultiphaseSystem
- removed: libreactingPhaseSystem
- removed: libreactingEulerianFvPatchFields
- removed: libreactingEulerianInterfacialCompositionModels
- removed: libreactingEulerianInterfacialModels
- removed: libmultiphaseReactingTurbulenceModels
- libreactingTwoPhaseSystem
- removed: libreactingPhaseSystem
- removed: libreactingEulerianFvPatchFields
- removed: libreactingEulerianInterfacialCompositionModels
- removed: libreactingEulerianInterfacialModels
### Avoid duplicate symbol for phaseCompressibleTurbulenceModels.
Common turbulence models are defined in libreactingMultiphaseSystem,
and libmultiphaseReactingTurbulenceModels is now redundant.
The libtwoPhaseReactingTurbulenceModels extends the common models
for reactingTwoPhaseSystem.Sergio FerrarisSergio Ferrarishttps://develop.openfoam.com/Development/openfoam/-/merge_requests/386ENH: PatchParticleHistogram: add a new cloud FO2020-11-13T09:23:26ZKutalmış BerçinENH: PatchParticleHistogram: add a new cloud FO### Summary
Computes a histogram for the distribution of particle diameters
and corresponding number of particles hitting on a given list of patches.
A minimal example by using `constant/reactingCloud1Properties.cloudFunctions`:
...### Summary
Computes a histogram for the distribution of particle diameters
and corresponding number of particles hitting on a given list of patches.
A minimal example by using `constant/reactingCloud1Properties.cloudFunctions`:
```
patchParticleHistogram1
{
// Mandatory entries (unmodifiable)
type patchParticleHistogram;
patches (<patch1> <patch2> ... <patchN>);
nBins 10;
min 0.1;
max 10.0;
maxStoredParcels 20;
}
```
### Risks
No change to user inputs / no risk to regression.
PS: approval/feedback please @mark @Sergio @Mattijs @PrashantAndrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/399ENH: outletMappedUniformInlet: add optional fraction and offset2020-12-16T18:28:32ZKutalmış BerçinENH: outletMappedUniformInlet: add optional fraction and offset### Summary
The new functionality optionally allows the patch-averaged
value to be scaled and/or offset by a pair of specified values.
Example of the boundary condition specification:
```
<patchName>
{
// Mandatory entries...### Summary
The new functionality optionally allows the patch-averaged
value to be scaled and/or offset by a pair of specified values.
Example of the boundary condition specification:
```
<patchName>
{
// Mandatory entries (unmodifiable)
type outletMappedFilterInlet;
outletPatch <outletPatchName>;
// Optional entries (unmodifiable)
fraction 0.1;
offset 10; // (1 0 0);
phi phi;
// Optional (inherited) entries
...
}
```
### Details of new models
**The tutorial `airRecirculationRoom` and related visualisations are exclusively prepared by _Alseny Diallo_**.
![Screenshot_from_2020-12-10_17-22-44](/uploads/0ca11fb914f02e7f7563d0df3e800b07/Screenshot_from_2020-12-10_17-22-44.png)
![Screenshot_from_2020-12-10_18-31-08](/uploads/10d4056dd7bdaed45d29b6e0aaddadc5/Screenshot_from_2020-12-10_18-31-08.png)
![Screenshot_from_2020-12-10_18-17-30](/uploads/83048e2a11c6ace6f8ac13cdf266fd5d/Screenshot_from_2020-12-10_18-17-30.png)
![Screenshot_from_2020-12-10_17-24-11](/uploads/cb9d2e00f334ee41f3ec8e7ff07d6902/Screenshot_from_2020-12-10_17-24-11.png)
![Screenshot_from_2020-12-10_17-24-20](/uploads/38cb29fa995ff837ed520b05c9ab37a6/Screenshot_from_2020-12-10_17-24-20.png)
![Screenshot_from_2020-12-10_17-23-19](/uploads/64a9c92d494ff19cd90e8df1a5b02bc7/Screenshot_from_2020-12-10_17-23-19.png)
![Screenshot_from_2020-12-10_18-09-54](/uploads/40806bc5b100b397998d6e5db55c3e4f/Screenshot_from_2020-12-10_18-09-54.png)
### Risks
- The bug fix may further need to be tested.
- No change to user input.Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/406ENH: MPPIC dynamic mesh2020-12-17T21:18:00ZSergio FerrarisENH: MPPIC dynamic meshMajor changes:
- `MPPICCloud` and `MPPIC` parcel are not longer used. The `MPPIC` sub-models were added to the kinematic cloud. (files were not yet deleted)
- `MPPICDyMFoam` and `DPMDyMFoam` are updated to use the kinematic cloud.
- Aff...Major changes:
- `MPPICCloud` and `MPPIC` parcel are not longer used. The `MPPIC` sub-models were added to the kinematic cloud. (files were not yet deleted)
- `MPPICDyMFoam` and `DPMDyMFoam` are updated to use the kinematic cloud.
- Affecting tracking and general functionality :
dc4deb024b4c21bf13d7d79fb85153f9dc9cf89a (org)
c68e10378b1efc6a82cf9bf845e43aef49bb7665 (org)
2045de687433674739b8fc399bdb34d4975a3b38 (org)
9b57bc1855f073cedd47e407692a0e9beefe35dd : affects tgtPointFace srcPointFace member functions
- The rest are specific for `MPPIC`-submodels into kinematic cloud, wall interaction and AMI.v2012Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/407Feature iso distance surface2020-12-11T16:45:34ZMark OLESENFeature iso distance surface- Adds improved handling of distance surface edges (#1950)
- freshened some of the iso-surface and sampling surface infrastructure to eliminate duplicate code, support cellZones for all iso-surface types.
- support multiple offsets for c...- Adds improved handling of distance surface edges (#1950)
- freshened some of the iso-surface and sampling surface infrastructure to eliminate duplicate code, support cellZones for all iso-surface types.
- support multiple offsets for cutting planes and multiple iso-valuesAndrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/408ENH: noise models - added A, B, C, and D weightings to SPL2020-12-11T20:22:09ZAndrew HeatherENH: noise models - added A, B, C, and D weightings to SPL### Summary
Added A, B, C and D weightings to the SPL predictions and code refactoring
### Resolved bugs (If applicable)
none
### Details of new models (If applicable)
Gains:
![noiseModelWeights](/uploads/cbc1c76a7f5e3e6c9ccbbd64...### Summary
Added A, B, C and D weightings to the SPL predictions and code refactoring
### Resolved bugs (If applicable)
none
### Details of new models (If applicable)
Gains:
![noiseModelWeights](/uploads/cbc1c76a7f5e3e6c9ccbbd646e20dc53/noiseModelWeights.png)
### Risks
(Possible regressions?)
code refactoring - point and surface noise functionality needs to be confirmed
(Changes to user inputs?)
nonev2012Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/410ENH: Function objects - added new 'multiply' function object2020-12-14T16:08:55ZAndrew HeatherENH: Function objects - added new 'multiply' function objectMultiplies a given list of (at least two or more) fields and outputs the result into a new field.
fieldResult = field1 * field2 * ... * fieldN
Minimal example by using `system/controlDict` functions:
multiply1
{
//...Multiplies a given list of (at least two or more) fields and outputs the result into a new field.
fieldResult = field1 * field2 * ... * fieldN
Minimal example by using `system/controlDict` functions:
multiply1
{
// Mandatory entries (unmodifiable)
type multiply;
libs (fieldFunctionObjects);
// Mandatory (inherited) entry (runtime modifiable)
fields (<field1> <field2> ... <fieldN>);
// Optional (inherited) entries
...
}
Serves as a precursor to a more general function object based on the `fieldExpression` toolchainv2012Mark OLESENMark OLESENhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/414Feature function1 limit range2020-12-16T17:13:16ZAndrew HeatherFeature function1 limit rangeFunction1 wrapper that limits the input range of another Function1
Example usage for limiting a polynomial:
limitedPolyTest limitRange;
limitedPolyTestCoeffs
{
min 0.4;
max 1.4...Function1 wrapper that limits the input range of another Function1
Example usage for limiting a polynomial:
limitedPolyTest limitRange;
limitedPolyTestCoeffs
{
min 0.4;
max 1.4;
value polynomial
(
(5 1)
(-2 2)
(-2 3)
(1 4)
);
}
Here the return value will be:
- poly(0.4) for x <= 0.4;
- poly(1.4) for x >= 1.4; and
- poly(x) for 0.4 < x < 1.4.v2012Mattijs Janssens4-Mattijs@users.noreply.develop.openfoam.comMattijs Janssens4-Mattijs@users.noreply.develop.openfoam.comhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/417ENH: Added new filmFlux function object2020-12-21T18:06:59ZAndrew HeatherENH: Added new filmFlux function objectCalculates the mass flux for surface film models.
Example usage:
filmFlux
{
type filmFlux;
writeControl writeTime;
result myPhi; // optional
}Calculates the mass flux for surface film models.
Example usage:
filmFlux
{
type filmFlux;
writeControl writeTime;
result myPhi; // optional
}v2012Kutalmış BerçinKutalmış Berçinhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/425ENH: new solvers: overPhaseChangeInterFoam and overCompressibleInterDyMFoam2021-03-24T13:15:23ZSergio FerrarisENH: new solvers: overPhaseChangeInterFoam and overCompressibleInterDyMFoamKutalmış BerçinKutalmış Berçinhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/431ENH: solarLoad: new load model, timeDependent2021-03-31T10:13:54ZKutalmış BerçinENH: solarLoad: new load model, timeDependent### Summary
- `TimeFunction1` input for direct solar irradiation (w/m2)
- `TimeFunction1` input for diffuse solar irradiation (w/m2)
- `TimeFunction1` input for `spectralDistribution`
### Details of new models (If applicable)
The foll...### Summary
- `TimeFunction1` input for direct solar irradiation (w/m2)
- `TimeFunction1` input for diffuse solar irradiation (w/m2)
- `TimeFunction1` input for `spectralDistribution`
### Details of new models (If applicable)
The following entry set in the `simpleCarSolarPanel` tutorial produces the attached animation:
```
sunLoadModel timeDependent;
directSolarRad table
(
(0 500)
(5 500)
(10 0)
);
diffuseSolarRad 0;
spectralDistribution table
(
(0 (2.0 1.2))
(1 (1.1 1.3))
);
```
[animation-Qprimary-fps1.avi](/uploads/da0024e0ed222190543e189e7691247c/animation-Qprimary-fps1.avi) (animation is prepared by Alseny Diallo).
### Risks
No changes in user input or simulation output.
There seems to be a previous bug in `solarLoad` model, where `wallCoupled` entry was undefined in one of the constructors. We have fixed this bug; however, the fix is not backward compatible since we cannot define an undefined behaviour. For this reason, you may need to add `wallCoupled` keyword to the `radiationProperties` dictionary to keep all output the same from one version to the next, otherwise `qr` field content may end up being always zero for some cases.
[EP#1484](https://exchange.openfoam.com/node/1484)v2106Andrew HeatherAndrew Heatherhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/457support parallel creation of finiteArea meshes with on-the-fly decomposition ...2021-05-28T18:14:55ZMark OLESENsupport parallel creation of finiteArea meshes with on-the-fly decomposition of fields #2084v2106Sergio FerrarisSergio Ferrarishttps://develop.openfoam.com/Development/openfoam/-/merge_requests/468AMI improvements2021-06-18T10:32:20ZAndrew HeatherAMI improvements- Added new faceAreaWeightAMI2D AMIMethod:
- performs intersection using a new 2D triangle class;
- candidate face matches set using an AABBTree method (vs advancing front for
faceAreaWeightAMI).
- Use by setting the AMIMethod...- Added new faceAreaWeightAMI2D AMIMethod:
- performs intersection using a new 2D triangle class;
- candidate face matches set using an AABBTree method (vs advancing front for
faceAreaWeightAMI).
- Use by setting the AMIMethod entry when specifying the AMI in the
constant/polyMesh/boundary file, e.g.
AMI
{
type cyclicACMI;
AMIMethod faceAreaWeightAMI2D; // new method
Cbb 0.1; // optional coefficient
nFaces 1000;
startFace 100000;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch AMI1;
nonOverlapPatch AMI1_non_overlap;
}
- The optional Cbb coeffcient controls the size of the bounding box used when
looking for candidate pairs; the value of 0.1 is the default and worked well
for a large range of test cases. For badly matched AMI patches this may need
to be increased.
- Deprecated the partialFaceAreaWeightAMI class - primarily used by ACMI:
- functionality now offered by the AMI variants.
- ~~NOTE: both AABBTree and octree variants included for review; ***ONLY 1 METHOD TO BE ADDED***~~
EDIT: octree method remoedv2106Mattijs Janssens4-Mattijs@users.noreply.develop.openfoam.comMattijs Janssens4-Mattijs@users.noreply.develop.openfoam.comhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/470ENH: Added new multiRegion function object2021-06-16T11:48:22ZAndrew HeatherENH: Added new multiRegion function objectWrapper that clones the supplied object for each region.
Simplifies setting up identical post-processing requirements for multi-
region cases. Applies the supplied function to all regions by default.
Example of function object specific...Wrapper that clones the supplied object for each region.
Simplifies setting up identical post-processing requirements for multi-
region cases. Applies the supplied function to all regions by default.
Example of function object specification:
multiRegion
{
type multiRegion;
libs (utilityFunctionObjects);
...
function
{
// Actual object specification
type fieldMinMax;
libs (fieldFunctionObjects);
fields (<field1> .. <fieldN>);
}
// Optional entries
regions (region1 region2);
}
Where the entries comprise:
Property | Description | Required | Default value
type | Type name: multiRegion | yes |
function | Function object sub-dictionary | yes |
regions | List of region names | no | allv2106Mark OLESENMark OLESENhttps://develop.openfoam.com/Development/openfoam/-/merge_requests/471ENH: Adding new permeable boundary conditions and a tutorial2021-06-17T21:01:28ZSergio FerrarisENH: Adding new permeable boundary conditions and a tutorial- 4d2e6e63f9b99d97dc83d2ee7b41d0fc47030d88: ENH: Adding new permeable boundary conditions
- `prghPermeableAlphaTotalPressure` for `p_rgh`
- `pressurePermeableAlphaInletOutletVelocity` for `U`
- new helper class for pressure-r...- 4d2e6e63f9b99d97dc83d2ee7b41d0fc47030d88: ENH: Adding new permeable boundary conditions
- `prghPermeableAlphaTotalPressure` for `p_rgh`
- `pressurePermeableAlphaInletOutletVelocity` for `U`
- new helper class for pressure-related BCs: `updateableSnGrad`
- 2a3b41e523cba5490a7cbd408e92a5c964e970a2: TUT: new multiphase tutorial: `damBreakPermeable`v2106Andrew HeatherAndrew Heather