CFDTOOLS

Introduction

The CFDTOOLS is a collections of python interface to set, run and post-process commercial softwares. Currently two major parts is involved: the Metacomp CFD++ and Tecplot.

CFD++

CFD++ is a wide-used compuational fluid dynamic software suite. All functions provided in the software suite can be directly run through the command line of Windows/Linux system. Here, Python interfaces are implmented to operate CFD++ through cmd/powershell.

The implmentation are based on CFD++ 14.1.

Tecplot

A collections of tools to let python export/import data in tecplot format. The tools only require you to install numpy and python3. There is no need to install pytecplot, which requires TecPLUS(TM) maintenance service.

The interfaces are modified from Luo Han. The structure of the code is reorganized, and the usable range is broadened. The main two functions are:

• py2tec: export data in tecplot format
• tec2py: import data in tecplot format

Disclaimer

CFD++ is a software suite that is available for use on all computer systems developed by Metacomp Technologies, which is a leading provider of software tools for major aerospace, defense, and automobile manufacturers. Tecplot is the name of a family of visualization & analysis software tools developed by Tecplot, Inc., which is headquartered in Bellevue, Washington. Any illegal use of the brand name and related products is beyond the expectation of the author of cfdtools. The author of cfdtools doesn't take any responsibility for the conditions.

The cfdtools is licensed with GPL 3.0 or later. You are welcome to distribute the codes and you are not required to cite anything. But if you make any modifications, you are required to open source.

Manual (CFD++)

start

To use the interface to CFD++, one should first create a object of class cfdpp with the code below:

op = cfdpp(op_dir='D:\\cfdppfolder')

The absolute path is recommanded. The op_dir can also be set later by

op.set_path(op_dir='D:\\cfdppfolder')

Several additional options need to be assigned when creating the object:

• core_number: core number to conduct cfd (should be assigned when you want to run cfd++ with cfdtools)
• ave_window: the number of calculation step of average window.
  • When reading cfd++ outputs, sometimes (often in unsteady flowfield simulations) we need to average on last several calculation steps to obtain a averaged flowfield or coefficients. The average window (how long you want the average invovle) can be set here.
  • ave_window = 0 means no average.
• verbose: how to display infomation during the run
  • verbose = All: display all infomation
  • verbose = Warning: only display warnings
  • verbose = None: display nothing

set running parameters

The parameters of cfd++ can be quarry and set with two groups of commands:

• For ordinary settings:

  Most of settings in CFD++'s .inp file is in the format of key value. For example, ntstep 500 in line 56 means the calculation takes 500 steps.

  If you don't know the setting that you want to change corresponds to which key, you may change it in gui and compare the later and former `.inp` file to find out.

  cfdtools offer you the interface to acquire and set those parameters. For acquisition, use:

  op.read_para(key='somekey')

  For assignment, use:

  op.set_para(key='somekey', value='somevalue')

• For output variables settings:

  The npfopts.inp file determine which variables to be output (by neutral plotter and tecplot). If you want to output a variable, use:

  op.set_para(key='P', value='yes', file='node')

• For infomation set:

  • edit info set

    The operations with infoset is a bit complicated.

    When you want to change the value in a infoset, i.e., to set the outlet pressure in info set No.8 to 101325, use:

    op.set_infset(inf_num=8, values=[101325]):

    note that the infoset for outlet bc only contain 1 parameters, so the length of the list given to values is 1.

    if you want to set a inlet conditions (pressure, temperature, k, eps) in info set No.8, use:

    op.set_infset(inf_num=8, values=[ptub, ttub, 1.2e5, 8.0e-4])

    the order is the same with in gui.

    For more complex usage, if you want to just set the pressure and temperature without modify the turbulance infomation k and eps, you can use the keyword for filter filte like:

    op.set_infset(inf_num=8, values=[ptub, ttub, 0, 0], filte=[2, 3])

    It means the value in values at index no. 2 and 3 will be neglected, and the original value in .inp on that place will be keep.

    Be carefull that the infoset number is not the boundary condition number!

  • add infoset

    If you want to add a new info set, use:

    new_idx = op.new_infset(typ='backpressure', values=[101325])

    the new index of the infoset will be returned (as a int).

    Currently, the bc types below are listed:

    type	number of values needed	code number in CFD++
    sym	0	6
    wall	0	7
    charactistic	7	16
    backpressure	1	35
    totalpt	4	82
    mfr	4	98

  • change the infoset for a boundary

    Then you may want to assign this new infoset to a boundary condition, use:

    op.change_infset(bc_num=12, typ='backpressure', infset_num=new_idx)

run CFD

It is very easy to run CFD++! If the the computation domain has not be divided into parts for mpi (there should be mcfd_metis.graph and mcpusin.bin.## in the folder is the division is done), use the following command to divide:

op.metis()

the core number is decided when creating the object op.

Then:

op.run_cfd(restart=False, step=1500)

a new console window will automaticly open and the calculation is done in that thread, the main thread will wait until calculation down.

If you want to assign some running parameters before running cfd, you can give the parameters by a keyword dict, like:

op.run_cfd(restart=False, step=1500, cfllbg=0.1)

means the cfl number at beginning is set to 0.1. Remind that the .inp is changed pertually.

read output data

• read area

  the geometry area(s) or length(for 2D) of given boundary condition(s) can be read by:

  area = op.read_area(typ, bc_series)

  • The typ can be x, y, or z, indicating the projection area along that direction respectively.
  • The bc_series is a list containing the boundary number(s). The returned result is the algebra summation of the area of all the boundary(s) in the list.

• read flux

  read flux is alike read area. The energy flux, mass flux, momentum flux (on three directions) and moment (along the axis of three directions) can be read by:

  flux = op.read_flux(typ, bc_series)

  • The typ can be: energy, mass, fx, fy, fz, mx, my, mz
  • The bc_series is defined same as read_area
  • The result will be averaged by the setting when create the op. If you want to override that setting, you can assign it by ave_window=100 in the parameter.
  • The 3D reference point for moment calculation is defined in gui (default (0,0,0)), if you want to output moment according to other pivot (x1, y1, z1), add move_axis=(x1, y1, z1) in parameter

• extract values on bc

  read the values on a given boundary.

  bcdata = op.extract_bc(bc_series, forcenew, remove=True, is_sort=None)

  • A tecplot file of each boundary in the list bc_series will appear contain the data on that boundary (the variables are the same as in flowfield)
  • if boundary is 1D, the data is read via cfdtools.tecplot and returned.
  • if is_sort is assigned to a variable, i.e, is_sort='Y', the retured data will be sorted by Y.

• extract straight line

  linedata = extract_line(st, ed, forcenew, remove=True, var='P T U V W R M')

  • A line from st (a Tuple with three components) to ed (a Tuple with three components) will be create. And everywhere the created line intersect with grid line, a datapoint is interpolated and returned.
  • The returned data is in cfdtools.tecplot format