FieldConvert allows the user to manipulate the Nektar++ output binary files (.chk and .fld)
by using the flag -m (which stands for module). Specifically, FieldConvert has these additional
functionalities
C0Projection: Computes the C0 projection of a given output file;
CFL: Computes the CFL number over the solution domain for Incompressible flow
QCriterion: Computes the Q-Criterion for a given output file;
L2Criterion: Computes the Lambda 2 Criterion for a given output file;
addcompositeid: Adds the composite ID of an element as an additional field;
fieldfromstring: Modifies or adds a new field from an expression involving the
existing fields;
addFld: Sum two .fld files;
combineAvg: Combine two Nektar++ binary output (.chk or .fld) field file
containing averages of fields (and possibly also Reynolds stresses) into single file;
concatenate: Concatenate a Nektar++ binary output (.chk or .fld) field file into
single file (deprecated);
divergence: Computes the divergence of the velocity field.
dof: Count the total number of DOF;
equispacedoutput: Write data as equi-spaced output using simplices to represent
the data for connecting points;
extract: Extract a boundary field;
gradient: Computes gradient of fields;
halfmodetofourier: Convert HalfMode expansion to SingleMode for further
processing;
homplane: Extract a plane from 3DH1D expansions;
homstretch: Stretch a 3DH1D expansion by an integer factor;
innerproduct: take the inner product between one or a series of fields with another
field (or series of fields).
interpfield: Interpolates one field to another, requires fromxml, fromfld to be
defined;
interppointdatatofld: Interpolates given discrete data using a finite difference
approximation to a fld file given an xml file;
interppoints: Interpolates a field to a set of points. Requires fromfld, fromxml
to be defined, and a topts, line, plane or box of target points;
interpptstopts: Interpolates a set of points to another. Requires a topts, line,
plane or box of target points;
isocontour: Extract an isocontour of “fieldid” variable and at value “fieldvalue”.
Optionally “fieldstr” can be specified for a string definition or “smooth” for
smoothing;
jacobianenergy: Shows high frequency energy of Jacobian;
qualitymetric: Evaluate a quality metric of the underlying mesh to show mesh
quality;
mean: Evaluate the mean of variables on the domain;
meanmode: Extract mean mode (plane zero) of 3DH1D expansions;
pointdatatofld: Given discrete data at quadrature points project them onto an
expansion basis and output fld file;
printfldnorms: Print L2 and LInf norms to stdout;
removefield: Removes one or more fields from .fld files;
scalargrad: Computes scalar gradient field;
scaleinputfld: Rescale input field by a constant factor;
shear: Computes time-averaged shear stress metrics: TAWSS, OSI, transWSS,
TAAFI, TACFI, WSSG;
streamfunction: Calculates stream function of a 2D incompressible flow;
surfdistance: Computes height of a prismatic boundary layer mesh and projects
onto the surface (for e.g. y+ calculation);
vorticity: Computes the vorticity field;
wss: Computes wall shear stress field;
phifile: Computes the Φ function representing a body defined in an .stl file.
Useful for the Smoothed Profile Method solver;
wallNormalData: Interpolate values for a set of points in the wall-normal direction
(for e.g. extract boundary layer profiles);
bodyFittedVelocity: Generate a body-fitted coordinate system and then project
the velocity components from Cartesian coordinate system into the new coordinate
system;
averagefld: Compute the averaging of several field files;
powerspectrum: Compute power spectrum at given regions from a 3DH1D
expansion;
zero-homo-plane: Zero a specfied homogeneous plane in wavespace.
The module list above can be seen by running the command
FieldConvert -l
In the following we will detail the usage of each module.
To smooth the data of a given .fld file one can use the C0Projection module of FieldConvert
FieldConvert -m C0Projection test.xml test.fld test-C0Proj.fld
where the file test-C0Proj.fld can be processed in a similar way as described in section 5.2
to visualise the result either in Tecplot, Paraview or VisIt.
The option localtoglobalmap will do a global gather of the coefficients and then scatter
them back to the local elements. This will replace the coefficients shared between two elements
with the coefficients of one of the elements (most likely the one with the highest id). Although
not a formal projection it does not require any matrix inverse and so is very cheap to
perform.
The option usexmlbcs will enforce the boundary conditions specified in the input xml
file.
The option helmsmoothing=L will perform a Helmholtz smoothing projection of the
form
which can be interpreted in a Fourier sense as smoothing the original coefficients using a low pass filter of the form
and so L is the length scale below which the coefficients values are halved or more. Since this form of the Helmholtz operator is not possitive definite, currently a direct solver is necessary and so this smoother is mainly of use in two-dimensions.
This module calculates the CFL number over the domain. It currently only supports
the solution results from the Incompressible flow simulaitons, i.e. the outputs of
IncNavierStokesSolver. To Estimate the CFL number, the user can run
FieldConvert -m CFL test.xml test.fld test-cfl.fld
where the file test-cfl.fld can be processed in a similar way as described in section 5.2 to
visualise the result either in Tecplot, Paraview or VisIt.
To perform the Q-criterion calculation and obtain an output data containing the Q-criterion solution, the user can run
FieldConvert -m QCriterion test.xml test.fld test-QCrit.fld
where the file test-QCrit.fld can be processed in a similar way as described in section 5.2 to
visualise the result either in Tecplot, Paraview or VisIt.
To perform the λ2 vortex detection calculation and obtain an output data containing the values of the λ2 eigenvalue, the user can run
FieldConvert -m L2Criterion test.xml test.fld test-L2Crit.fld
where the file test-L2Crit.fld can be processed in a similar way as described in section 5.2
to visualise the result either in Tecplot, Paraview or VisIt.
When dealing with a geometry that has many surfaces, we need to identify the composites to
assign boundary conditions. To assist in this, FieldConvert has a addcompositeid module,
which adds the composite ID of every element as a new field. To use this we simply run
FieldConvert -m addcompositeid mesh.xml out.dat
In this case, we have produced a Tecplot file which contains the mesh and a variable that
contains the composite ID. To assist in boundary identification, the input file mesh.xml should
be a surface XML file that can be obtained through the NekMesh extract module (see section
4.5.3).
To modify or create a new field using an expression involving the existing fields, one can use
the fieldfromstring module of FieldConvert
FieldConvert -m fieldfromstring:fieldstr="x+y+u":fieldname="result" \ file1.xml file2.fld file3.fld
In this case fieldstr is a required parameter describing a function of the coordinates
and the existing variables, and fieldname is an optional parameter defining the
name of the new or modified field (the default is newfield). file3.fld is the output
containing both the original and the new fields, and can be processed in a similar way
as described in section 5.2 to visualise the result either in Tecplot, Paraview or
VisIt.
To sum two .fld files one can use the addFld module of FieldConvert
FieldConvert -m addfld:fromfld=file1.fld:scale=-1 file1.xml file2.fld \ file3.fld
In this case we use it in conjunction with the command scale which multiply the values of a
given .fld file by a constant value. file1.fld is the file multiplied by value, file1.xml is the
associated session file, file2.fld is the .fld file which is summed to file1.fld and finally
file3.fld is the output which contain the sum of the two .fld files. file3.fld can be
processed in a similar way as described in section 5.2 to visualise the result either in Tecplot,
Paraview or VisIt.
To combine two .fld files obtained through the AverageFields or ReynoldsStresses filters, use
the combineAvg module of FieldConvert
FieldConvert -m combineAvg:fromfld=file1.fld file1.xml file2.fld \ file3.fld
file3.fld can be processed in a similar way as described in section 5.2 to visualise the result
either in Tecplot, Paraview or VisIt.
To concatenate file1.fld and file2.fld into file-conc.fld one can run the following
command
FieldConvert file.xml file1.fld file2.fld file-conc.fld
where the file file-conc.fld can be processed in a similar way as described in section 5.2 to
visualise the result either in Tecplot, Paraview or VisIt. The concatenate module
previously used for this purpose is not required anymore, and will be removed in a future
release.
To count the number of DOF in a solution file, one can run the following command
FieldConvert -m dof file.xml file.fld out.stdout
This module interpolates the output data to a truly equispaced set of points (not equispaced along the collapsed coordinate system). Therefore a tetrahedron is represented by a tetrahedral number of points. This produces much smaller output files. The points are then connected together by simplices (triangles and tetrahedrons).
FieldConvert -m equispacedoutput test.xml test.fld test.dat
or
FieldConvert -m equispacedoutput test.xml test.fld test.vtu
The boundary region of a domain can be extracted from the output data using the following command line
FieldConvert -m extract:bnd=2 test.xml \ test.fld test-boundary.fld
The option bnd specifies which boundary region to extract. Note this is different to NekMesh
where the parameter surf is specified and corresponds to composites rather boundaries. If bnd
is not provided, all boundaries are extracted to different fields. The output will
be placed in test-boundary_b2.fld. If more than one boundary region is specified
the extension _b0.fld, _b1.fld etc will be outputted. To process this file you will
need an xml file of the same region. This can be generated using the command:
NekMesh -m extract:surf=5 test.xml test_b0.xml
The surface to be extracted in this command is the composite number and so needs to correspond to the boundary region of interest. Finally to process the surface file one can use
FieldConvert test_b0.xml test_b0.fld test_b0.dat
This will obviously generate a Tecplot output if a .dat file is specified as last argument. A .vtu extension will produce a Paraview or VisIt output.
To perform the divergence calculation and obtain an output field containing the divergence solution, the user can run
FieldConvert -m divergence test.xml test.fld test-div.fld
where the file test-div.fld can be processed in a similar way as described in section
5.2.
To compute the spatial gradients of fields one can run the following command
FieldConvert -m gradient:vars=u,v,p:dirs=x,y test.xml test.fld test-grad.fld
or
FieldConvert -m gradient:vars=0,1,2:dirs=0,1 test.xml test.fld test-grad.fld
where vars specifies the field numbers (starting from 0) or variable names to process and vars
specifies the spatial directions to compute derivatives. All fields will be processed if vars is not
set. All spatial directions will be used if vars is not set. The output file file-grad.fld can be
processed in a similar way as described in section 5.2 to visualise the result either in Tecplot,
Paraview or VisIt.
To obtain full Fourier expansion form a HalfMode result, use the comand:
FieldConvert -m halfmodetofourier:realmodetoimag=value1,value2 file.xml half_mode_file.fld single_mode_file.fld
In linear stability analysis with halfmode expansion, the variable w, whose variable number is
2, is a imaginary mode but it is output as a real mode in the eigenvector field file.
By setting option realmodetoimag=2, w can be transformed to a imaginary mode
correctly.
To obtain a 2D expansion containing one of the planes of a 3DH1D field file, use the command:
FieldConvert -m homplane:planeid=value file.xml file.fld file-plane.fld
If the option wavespace is used, the Fourier coefficients corresponding to planeid are
obtained. The command in this case is:
FieldConvert -m homplane:wavespace:planeid=value file.xml \ file.fld file-plane.fld
The output file file-plane.fld can be processed in a similar way as described in section 5.2
to visualise it either in Tecplot or in Paraview.
To stretch a 3DH1D expansion in the z-direction, use the command:
FieldConvert -m homstretch:factor=value file.xml file.fld file-stretch.fld
The number of modes in the resulting field can be chosen using the command-line parameter
--output-points-hom-z.
The output file file-stretch.fld can be processed in a similar way as described in section
5.2 to visualise it either in Tecplot or in Paraview.
You can take the inner product of one field with another field using the following command:
FieldConvert -m innerproduct:fromfld=file1.fld file2.xml file2.fld \ out.stdout
This command will load the file1.fld and file2.fld assuming they both are spatially
defined by files.xml and determine the inner product of these fields. The input option
fromfld must therefore be specified in this module.
Optional arguments for this module are fields which allow you to specify the fields that you
wish to use for the inner product, i.e.
FieldConvert -m innerproduct:fromfld=file1.fld:fields="0,1,2" file2.xml \ file2.fld out.stdout
will only take the inner product between the variables 0,1 and 2 in the two fields files. The default is to take the inner product between all fields provided.
Additional options include multifldids and allfromflds which allow for a series of fields to
be evaluated in the following manner:
FieldConvert -m innerproduct:fromfld=file1.fld:multifldids="0-3"\ file2.xml file2.fld out.stdout
will take the inner product between a file names field1_0.fld, field1_1.fld, field1_2.fld and field1_3.fld with respect to field2.fld.
Analogously including the options allfromflds, i.e.
FieldConvert -m innerproduct:fromfld=file1.fld:multifldids="0-3":\ allfromflds file2.xml file2.fld out.stdout
Will take the inner product of all the from fields, i.e. field1_0.fld,field1_1.fld,field1_2.fld and field1_3.fld with respect to each other. This option essentially ignores file2.fld. Only the unique inner products are evaluated so if four from fields are given only the related trianuglar number 4 × 5∕2 = 10 of inner products are evaluated.
This option can be run in parallel.
To interpolate one field to another, one can use the following command:
FieldConvert -m interpfield:fromxml=file1.xml:fromfld=file1.fld \ file2.xml file2.fld
This command will interpolate the field defined by file1.xml and file1.fld to the new
mesh defined in file2.xml and output it to file2.fld. The fromxml and fromfld must be
specified in this module. In addition there are two optional arguments clamptolowervalue
and clamptouppervalue which clamp the interpolation between these two values. Their
default values are -10,000,000 and 10,000,000.
If the fromfld is a 3DH1D field and uses HalfMode expansion, you can use
realmodetoimag=n1,n2,...,nm to transform the n1,n2,...,nmth variables from real modes to
imaginary modes. Variable index starts from 0.
To interpolate discrete point data to a field, use the interppointdatatofld module:
FieldConvert -m interppointdatatofld:frompts=file1.pts file1.xml file1.fld
or alternatively for csv data:
FieldConvert -m interppointdatatofld:frompts=file1.csv file1.xml file1.fld
This command will interpolate the data from file1.pts (file1.csv) to the mesh and
expansions defined in file1.xml and output the field to file1.fld. The file file.pts must
be of the form:
1<?xml version="1.0" encoding="utf-8" ?> 2<NEKTAR> 3 <POINTS DIM="1" FIELDS="a,b,c"> 4 1.0000 -1.0000 1.0000 -0.7778 5 2.0000 -0.9798 0.9798 -0.7980 6 3.0000 -0.9596 0.9596 -0.8182 7 4.0000 -0.9394 0.9394 -0.8384 8 </POINTS> 9</NEKTAR>
where DIM="1" FIELDS="a,b,c specifies that the field is one-dimensional and contains three
variables, a, b, and c. Each line defines a point, while the first column contains its
x-coordinate, the second one contains the a-values, the third the b-values and so on. In case of
n-dimensional data, the n coordinates are specified in the first n columns accordingly. An
equivalent csv file is:
# x, a, b, c 1.0000,-1.0000,1.0000,-0.7778 2.0000,-0.9798,0.9798,-0.7980 3.0000,-0.9596,0.9596,-0.8182 4.0000,-0.9394,0.9394,-0.8384
In order to interpolate 1D data to a nD field, specify the matching coordinate in the output
field using the interpcoord argument:
FieldConvert -m interppointdatatofld:frompts=1D-file1.pts:interpcoord=1 \ 3D-file1.xml 3D-file1.fld
This will interpolate the 1D scattered point data from 1D-file1.pts to the y-coordinate of
the 3D mesh defined in 3D-file1.xml. The resulting field will have constant values along the
x and z coordinates. For 1D Interpolation, the module implements a quadratic scheme
and automatically falls back to a linear method if only two data points are given.
A modified inverse distance method is used for 2D and 3D interpolation. Linear
and quadratic interpolation require the data points in the .pts-file to be sorted by
their location in ascending order. The Inverse Distance implementation has no such
requirement.
You can interpolate one field to a series of given points using the following command:
FieldConvert -m interppoints:fromxml=file1.xml:fromfld=\ file1.fld:topts=file2.pts file2.dat
This command will interpolate the field defined by file1.xml and file1.fld to the points
defined in file2.pts and output it to file2.dat. The fromxml and fromfld must be
specified in this module. The format of the file file2.pts is of the same form as for the
interppointdatatofld module:
1<?xml version="1.0" encoding="utf-8" ?> 2<NEKTAR> 3 <POINTS DIM="2" FIELDS=""> 4 0.0 0.0 5 0.5 0.0 6 1.0 0.0 7 </POINTS> 8</NEKTAR>
Similar to the interppointdatatofld module, the .pts file can be interchanged with a .csv file
(the output can also be written to .csv):
# x, y 0.0,0.0 0.5,0.0 1.0,0.0
There are three optional arguments clamptolowervalue, clamptouppervalue and
defaultvalue the first two clamp the interpolation between these two values and the third
defines the default value to be used if the point is outside the domain. Their default values are
-10,000,000, 10,000,000 and 0.
In addition, instead of specifying the file file2.pts, a module list of the form
FieldConvert -m interppoints:fromxml=file1.xml:fromfld= \ file1.fld:line=npts,x0,y0,x1,y1 file2.dat
can be specified where npts is the number of equispaced points between (x0,y0) to (x1,y1).
This also works in 3D, by specifying (x0,y0,z0) to (x1,y1,z1).
An extraction of a plane of points can also be specified by
FieldConvert -m interppoints:fromxml=file1.xml:fromfld=file1.fld:\ plane=npts1,npts2,x0,y0,z0,x1,y1,z1,x2,y2,z2,x3,y3,z3 file2.dat
where npts1,npts2 is the number of equispaced points in each direction and (x0,y0,z0),
(x1,y1,z1), (x2,y2,z2) and (x3,y3,z3) define the plane of points specified in a clockwise or
anticlockwise direction.
In addition, an extraction of a box of points can also be specified by
FieldConvert -m interppoints:fromxml=file1.xml:fromfld=file1.fld:\ box=npts1,npts2,npts3,xmin,xmax,ymin,ymax,zmin,zmax file2.dat
where npts1,npts2,npts3 is the number of equispaced points in each direction and
(xmin,ymin,zmin) and (xmax,ymax,zmax) define the limits of the box of points.
There is also an additional optional argument cp=p0,q which adds to the interpolated fields
the value of cp = (p-p0)∕q and cp0 = (p-p0 + 0.5u2)∕q where p0 is a reference pressure and
q is the free stream dynamics pressure. If the input does not contain a field “p” or a velocity
field “u,v,w” then cp and cp0 are not evaluated accordingly.
If the fromfld is a 3DH1D field and uses HalfMode expansion, you can use
realmodetoimag=n1,n2,...,nm to transform the n1,n2,...,nmth variables from real modes to
imaginary modes. Variable index starts from 0.
You can interpolate one set of points to another using the following command:
FieldConvert file1.pts -m interpptstopts:topts=file2.pts file2.dat
This command will interpolate the data in file1.pts to a new set of points defined in
file2.pts and output it to file2.dat.
Similarly to the interppoints module, the target point distribution can also be specified
using the line, plane or box options. The optional arguments clamptolowervalue,
clamptouppervalue, defaultvalue and cp are also supported with the same meaning as in
interppoints.
One useful application for this module is with 3DH1D expansions, for which currently the interppoints module does not work. In this case, we can use for example
FieldConvert file1.xml file1.fld -m interpptstopts:\ plane=npts1,npts2,x0,y0,z0,x1,y1,z1,x2,y2,z2,x3,y3,z3 \ file2.dat
With this usage, the equispacedoutput module will be automatically called to interpolate the field to a set of equispaced points in each element. The result is then interpolated to a plane by the interpptstopts module.
Extract an isocontour from a field file. This option automatically take the field to an
equispaced distribution of points connected by linear simplicies of triangles or tetrahedrons.
The linear simplices are then inspected to extract the isocontour of interest. To specify the
field fieldid can be provided giving the id of the field of interest and fieldvalue provides
the value of the isocontour to be extracted.
FieldConvert -m isocontour:fieldid=2:fieldvalue=0.5 test.xml test.fld \ test-isocontour.dat
Alternatively fieldstr="u+v" can be specified to calculate the field u + v and extract its
isocontour. You can also specify fieldname="UplusV" to define the name of the isocontour in
the .dat file, i.e.
FieldConvert -m isocontour:fieldstr="u+v":fieldvalue=0.5:\ fieldname="UplusV" test.xml test.fld test-isocontour.dat
Optionally smooth can be specified to smooth the isocontour with default values
smoothnegdiffusion=0.495, smoothnegdiffusion=0.5 and smoothiter=100. This option
typically should be used wiht the globalcondense option which removes multiply defined
verties from the simplex definition which arise as isocontour are generated element by element.
The smooth option preivously automatically called the globalcondense option but this has
been depracated since it is now possible to read isocontour files directly and so it is useful to
have these as separate options.
In addition to the smooth or globalcondense options you can specify removesmallcontour=100
which will remove separate isocontours of less than 100 triangles.
FieldConvert -m jacobianenergy file.xml file.fld jacenergy.fld
The option topmodes can be used to specify the number of top modes to keep.
The output file jacenergy.fld can be processed in a similar way as described in section 5.2 to
visualise the result either in Tecplot, Paraview or VisIt.
The qualitymetric module assesses the quality of the mesh by calculating a per-element
quality metric and adding an additional field to any resulting output. This does not require
any field input, therefore an example usage looks like
FieldConvert -m qualitymetric mesh.xml mesh-with-quality.dat
Two quality metrics are implemented that produce scalar fields Q:
By default a metric outlined in [16] is produced, where all straight sided elements have quality Q = 1 and Q < 1 shows the deformation between the curved element and the straight-sided element. If Q = 0 then the element is invalid. Note that Q varies over the volume of the element but is not guaranteed to be continuous between elements.
Alternatively, if the scaled option is passed through to the module, then the scaled
Jacobian
(i.e. the ratio of the minimum to maximum Jacobian of each element) is calculated. Again Q = 1 denotes an ideal element, but now invalid elements are shown by Q < 0. Any elements with Q near zero are determined to be low quality.
To evaluate the mean of variables on the domain one can use the mean module of FieldConvert
FieldConvert -m mean file1.xml file2.fld out.stdout
This module does not create an output file which is reinforced by the out.stdout option. The integral and mean for each field variable are then printed to the stdout.
To obtain a 2D expansion containing the mean mode (plane zero in Fourier space) of a 3DH1D field file, use the command:
FieldConvert -m meanmode file.xml file.fld file-mean.fld
The output file file-mean.fld can be processed in a similar way as described in section 5.2 to
visualise the result either in Tecplot or in Paraview or VisIt.
To project a series of points given at the same quadrature distribution as the .xml file and write out a .fld file use the pointdatatofld module:
FieldConvert -m pointdatatofld:frompts=file.pts file.xml file.fld
This command will read in the points provided in the file.pts and assume these are
given at the same quadrature distribution as the mesh and expansions defined in
file.xml and output the field to file.fld. If the points do not match an error will be
dumped.
The file file.pts which is assumed to be given by an interpolation from another source is of
the form:
1<?xml version="1.0" encoding="utf-8" ?> 2<NEKTAR> 3 <POINTS DIM="3" FIELDS="p"> 4 1.70415 -0.4 -0.0182028 -0.106893 5 1.70415 -0.395683 -0.0182028 -0.106794 6 1.70415 -0.3875 -0.0182028 -0.106698 7 1.70415 -0.379317 -0.0182028 -0.103815 8 </POINTS> 9</NEKTAR>
where DIM="3" FIELDS="p specifies that the field is three-dimensional and contains one
variable, p. Each line defines a point, the first, second, and third columns contains the
x,y,z-coordinate and subsequent columns contain the field values, in this case the p-value So
in the general case of n-dimensional data, the n coordinates are specified in the first n columns
accordingly followed by the field data. Alternatively, the file.pts can be interchanged with a
csv file.
The default argument is to use the equispaced (but potentially collapsed) coordinates which can be obtained from the command.
FieldConvert file.xml file.dat
In this case the pointdatatofld module should be used without the –no-equispaced
option. However this can lead to problems when peforming an elemental forward
projection/transform since the mass matrix in a deformed element can be singular
as the equispaced points do not have a sufficiently accurate quadrature rule that
spans the polynomial space. Therefore it is advisable to use the set of points given
by
FieldConvert --no-equispaced file.xml file.dat
which produces a set of points at the gaussian collapsed coordinates.
Finally the option setnantovalue=0 can also be used which sets any nan values in the
interpolation to zero or any specified value in this option.
FieldConvert -m printfldnorms test.xml test.fld out.stdout
This module does not create an output file which is reinforced by the out.stdout option. The L2 and LInf norms for each field variable are then printed to the stdout.
This module allows to remove one or more fields from a .fld file:
FieldConvert -m removefield:fieldname="u,v,p" test.xml test.fld test-removed.fld
where the file test-removed.fld can be processed in a similar way as described in section 5.2
to visualise the result either in Tecplot, Paraview or VisIt. The lighter resulting file speeds up
the postprocessing of large files when not all fields are required.
The scalar gradient of a field is computed by running:
FieldConvert -m scalargrad:bnd=0 test.xml test.fld test-scalgrad.fld
The option bnd specifies which boundary region to extract. Note this is different to NekMesh
where the parameter surf is specified and corresponds to composites rather boundaries. If bnd
is not provided, all boundaries are extracted to different fields. To process this file you will
need an xml file of the same region.
To scale a .fld file by a given scalar quantity, the user can run:
FieldConvert -m scaleinputfld:scale=value test.xml test.fld test-scal.fld
The argument scale=value rescales of a factor value test.fld by the factor value. The
output file file-scal.fld can be processed in a similar way as described in section 5.2 to
visualise the result either in Tecplot, Paraview or VisIt.
Time-dependent wall shear stress derived metrics relevant to cardiovascular fluid dynamics research can be computed using this module. They are
TAWSS: time-averaged wall shear stress;
OSI: oscillatory shear index;
transWSS: transverse wall shear stress;
TACFI: time-averaged cross-flow index;
TAAFI: time-averaged aneurysm formation index;
|WSSG|: wall shear stress gradient.
To compute these, the user can run:
FieldConvert -m shear:N=value:fromfld=test_id_b0.fld \ test.xml test-multishear.fld
The argument N and fromfld are compulsory arguments that respectively define the number
of fld files corresponding to the number of discrete equispaced time-steps, and the first fld
file which should have the form of test_id_b0.fld where the first underscore in the name
marks the starting time-step file ID.
The input .fld files are the outputs of the wss module. If they do not contain the surface
normals (an optional output of the wss modle), then the shear module will not compute the
last metric, |WSSG|.
The streamfunction module calculates the stream function of a 2D incompressible flow, by solving the Poisson equation
where ω is the vorticity. Note that this module applies the same boundary conditions specified
for the y-direction velocity component v to the stream function, what may not be the most
appropriate choice.
To use this module, the user can run
FieldConvert -m streamfunction test.xml test.fld test-streamfunc.fld
where the file test-streamfunc.fld can be processed in a similar way as described in section
5.2.
The surface distance module computes the height of a boundary layer formed by quadrilaterals
(in 2D) or prisms and hexahedrons (in 3D) and projects this value onto the surface of the
boundary, in a similar fashion to the extract module. In conjunction with a mesh of the
surface, which can be obtained with NekMesh, and a value of the average wall shear stress, one
potential application of this module is to determine the distribution of y+ grid spacings for
turbulence calculations.
To compute the height of the prismatic layer connected to boundary region 3, the user can issue the command:
FieldConvert -m surfdistance:bnd=3 input.xml output.fld
Note that no .fld file is required, since the mesh is the only input required in order to
calculate the element height. This produces a file output_b3.fld, which can be visualised
with the appropriate surface mesh from NekMesh.
To perform the vorticity calculation and obtain an output data containing the vorticity solution, the user can run
FieldConvert -m vorticity test.xml test.fld test-vort.fld
where the file test-vort.fld can be processed in a similar way as described in section
5.2.
To obtain the wall shear stres vector and magnitude, the user can run:
FieldConvert -m wss:bnd=0:addnormals=1 test.xml test.fld test-wss.fld
The option bnd specifies which boundary region to extract. Note this is different to NekMesh
where the parameter surf is specified and corresponds to composites rather boundaries. If bnd
is not provided, all boundaries are extracted to different fields. The addnormals is an optional
command argument which, when turned on, outputs the normal vector of the extracted
boundary region as well as the shear stress vector and magnitude. This option is
off by default. To process the output file(s) you will need an xml file of the same
region.
The output fields are the wall shear stress in the streamwise direction (Shear_x), the vertical
direction (Shear_y) and its magnitude (Shear_mag) for 2D simulations. For 3D simulations,
wall shear stress in the spanwise direction (Shear_z) is also included in the output
fileds.
.stl files, errors may occur if triangles are placed exactly at
90∘.This FieldConvert module converts a binary .stl CAD file into .fld or .vtu/.dat files
that can be used as inputs for the Smoothed Profile Method solver. Running the
command:
FieldConvert -m phifile:file=geom.stl:scale=value session.xml geom.fld
will generate an output file geom.fld with all the information required to define a shape
function Φ representing the geometry specified in geom.stl. The option scale sets the value
of ξ as it is described in the Synopsis chapter of the Incompressible N-S solver. If the output
file gets the extension .vtu or .dat, the module will produce a graphical representation of the
shape function; however, the recommended way to proceed is to generate an .fld file and
then, use FieldConvert to obtain the .vtu or .dat files if needed for visualisation purposes:
FieldConvert -m phifile:file=geom.stl:scale=value session.xml geom.fld FieldConvert session.xml geom.fld geom.vtu
This module can also be used to produce a .fld and .vtu / .dat file of shapes defined
directly in the session file through an analytical expression. In this case, the commands
simplify to:
FieldConvert -m phifile session.xml geom.fld FieldConvert session.xml geom.fld geom.vtu
The algorithm computes an octree for the triangles that define the 3D object in the .stl file,
and then loops over all the nodes of the computational mesh looking for the shortest distance
to the 3D object. Since this module is currently in experimental phase, it only runs in serial
and therefore its performance in computing the shape function from the .stl file is limited,
especially in 3D cases. In addition to this, it is recommended to make sure that the angles
between triangles are not strictly equal to 90∘, since the algorithm will probably fail to find
the real Φ function.
To obtain the values of an array of points in the wall-normal direction, such as boundary layer profiles, the user can run:
FieldConvert -m wallNormalData:bnd=0:xorig="0.5,0,0":projDir="0,1,0":maxDist=0.1:\ distH=0.1:nptsH=0.01:d=0.2 test.xml test.fld test.pts
The option bnd specifies the target boundary region, to which the input point specified by
xorig will be projected as the first point in the interpolation points array. The projection
direction is specified by projDir, which does not have to be a unit vector but will be
automatically normalized. The input point and projetion direction must be set carefully to
make sure a projected point can be found on the target boundary. In cases with curved
boundaries on which multiple projected points might exist, the user can use maxDist to
limit the maximum projection distance between the input point to the projected
point.
After the projected point is found, this module will compute the wall-normal direction at the
point, and an array of points will be set in this direction. The number of points is
specified by nptsH, and the parameter d controls the distribution of the points as
follows
![({ tanh[(1 - ξ)atanh (√1---δ)])}
h(ξ) = H 1 - ----------√---------------
( 1 - δ )](user-guide46x.svg)
where ξ is equally-spaced parametric parameter varying from 0 to 1; H is the distance between
the first point (on the booundary) and the last point, which is specified distH; δ is given by d.
This distribution is employed for 0 < δ ≤ 0.95 while δ > 0.95 for evenly-spaced
distribution.
Finally, this module will interpolate the values at the points from test.fld, and save the result in test.pts.
In practice, it is convenient to use this module interactively to find/visualize/adjust profile distributions. This can be achieved by using the NekPy interface. A sample Pyhton script is provieded in the following
1import sys 2from NekPy.FieldUtils import * 3 4field = Field(sys.argv, forceoutput=True, error=True) 5InputModule.Create("xml", field, "mesh.xml","session.xml").Run() 6InputModule.Create("fld", field, "field.fld").Run() # e.g. x,y,u,v,p 7ProcessModule.Create("wallNormalData", field, 8 bnd=str(bnd), xorig=str(xorig), projDir=str(projDir), 9 maxDist=str(maxDist), distH=str(distH), nptsH=str(nptsH), 10 d=str(d)).Run() 11 12# Get data arrays from interpolation 13y = field.GetPts(1) 14u = field.GetPts(2)
To obtain the velocity components in the body-fitted coordinate system, the user can run:
FieldConvert -m bodyFittedVelocity:bnd=0:assistDir="0,0,1":checkAngle=1:\ distTol=1.0e-12:bfcOut=1 mesh.xml session.xml field.fld bfvFile.fld
The option bnd specifies the reference boundary composite to set up the body-fitted
coordinate system with the help of vector specified by assistDir. For any point inside the
domain, the the body-fitted coordinate system has three directions, i.e. main tangantial
direction (0), normal direction (1) from the nearest point on the wall to the point , and minor
tangential direction (2) specified by assistDir. Since the directions 1 and 2 are
known, the main tangantial direction (0) can be computed by the cross product of
them.
In general, when the surface is smooth, checkAngle and distTol is not needed to set up the
body-fitted coordinate system since they are specially designed for geometries with
surfarce irregularities, such a step or gap. As shown in the following sketch, the
presence of a gap in 2D geometry introduces fours singular points at the cornors, where
the body-fited velocity components will experience significant change, leading to
jump in the final fields. Considering the surfaces irregularities are typically small
in size, the user can choose to exclude the side wall(s) as reference to set up the
body-fitted coordinate system by setting boundary id=0,2,4 into one composite
while id=1,3 into another. Then only the first composte id is specified through bnd.
In this way the finaly results will be comparable with the results using the clean
geometry.
Finally, bfcOut is a bool parameter controls whether the fields for body-fitted coordinate
system will be output. This file can be read by the BodyFittedVelocity filter to process data.
See 3.5.27.
In cases the users would like to visualize the fluctuations in a 3DH1D flow field, the mean mode is expected to be removed (in the Fourier space). This can be achieved by running the current module:
FieldConvert -m zero-homo-plane:planeid=0 mesh.xml session.xml field.fld \ field-zeroMean.fld
In general, planeid can be any meaningful plane id, which is 0 by default.
FieldConvert has support for two modules that can be used in conjunction with the linear elastic solver, as shown in chapter 12. To do this, FieldConvert has an XML output module, in addition to the Tecplot and VTK formats.
The deform module, which takes no options, takes a displacement field and applies it to the
geometry, producing a deformed mesh:
FieldConvert -m deform input.xml input.fld deformed.xml
The displacement module is designed to create a boundary condition field file.
Its intended use is for mesh generation purposes. It can be used to calculate the
displacement between the linear mesh and a high-order surface, and then produce a fld file,
prescribing the displacement at the boundary, that can be used in the linear elasticity
solver.
Presently the process is somewhat convoluted and must be used in conjunction with NekMesh
to create the surface file. However the bash input below describes the procedure. Assume the
high-order mesh is in a file called mesh.xml, the linear mesh is mesh-linear.xml that can be
generated by removing the CURVED section from mesh.xml, and that we are interested in the
surface with ID 123.
# Extract high order surface NekMesh -m extract:surf=123 mesh.xml mesh-surf-curved.xml # Use FieldConvert to calculate displacement between two surfaces FieldConvert -m displacement:id=123:to=mesh-surf-curved.xml \ mesh-linear.xml mesh-deformation.fld # mesh-deformation.fld is used as a boundary condition inside the # solver to prescribe the deformation conditions.xml contains # appropriate Nektar++ parameters (mu, E, other BCs, ...) LinearElasticSolver mesh-linear.xml conditions.xml # This produces the final field mesh-linear.fld which is the # displacement field, use FieldConvert to apply it: FieldConvert-g -m deform mesh-linear.xml mesh-linear.fld mesh-deformed.xml
To obtain the averaged field of several field files, the user can run:
FieldConvert -m averagefld:inputfld=chan3DH1D_%d.chk:range=0,1,4 chan3DH1D.xml phaseavg.fld
The option inputfld specifies the format of field file name. The option range=start,skip,end
specifies the range of %d in the input file name.
To obtain the spanwise power spectrum of a 3DH1D field in a specific domain, the user can run:
FieldConvert -m powerspectrum:vars=u,v,w:box=0,0.5,0,0.5 chan3DH1D.xml chan3DH1D_0.chk chan3DH1D.plt
The option vars=u,v,w specifies the variables used to calculate the power spectrum. Both the
number and variable name can be used. The option box=xmin,xmax,ymin,ymax specifies the
domain where the power spectrum is computed.
To obtain the vortex-induced velocity, the user can run:
FieldConvert -m vortexinducedvelocity:vortex=vortexfilament.dat Helmholtz.xml Helmholtz.plt
The Lamb-Oseen vortex model is used to avoid the singularity at the vortex center. In the cylindrical coordinate, the vorticity and velocity are
![[ ( 2 )]
vr(r) = -Γ-- 1- exp - -r--
2πr 2σ2](user-guide48x.svg)
The option vortex specifies the filename that defines the vortex filaments. The format of one
vortex segment is: xstart, ystart, zstart, is half infinity (true is 1); xend, yend, zend, is
half infinity; σ, Γ. The format to define a uniform flow is: u, v, w. One example of
vortexfilament.dat that defines two-counter rotating Lamb-Oseen vortices with a uniform
background flow is
10 0.159154943091895 0 2-0.5 0 -1 1; -0.5 0 1 1; 0.1 -1 30.5 0 -1 1; 0.5 0 1 1; 0.1 1
