Graphical User Interface (GUI)¶

Overview¶

The pyNastran GUI was originally developed to solve a data validation problem. It’s hard to validate that things like coordinate systems were correct if you can’t look at the geometry in a native format. As time went on, niche features that were needed (e.g., aero panels) that were not supported natively in Patran 2005, were added. The goal is not to replace a code like Patran or FEMAP, but instead complement it.

Since the intial development, the GUI has become significantly more capable by adding features such as displacements and forces, so the need for a code like Patran has decreased, but will not be eliminated.

Introduction¶

The Graphical User Interface (GUI) looks like:

A somewhat messy, but more featured image:

../_images/eigenvectors_groups_legend.png

The GUI also has a sidebar and transient support.

Advantages of pyNastranGUI¶

command line interface for loading models

simple scripting

nice looking models

intuitive rotation

niche features - aero panels - aero splines - aero spline points - control surfaces

custom results from a CSV file

64 bit support - Patran 2005 can’t read in models that pyNastranGUI can - not an advantage for newer versions

animated gifs

Advantages of Patran/FEMAP¶

CAD geometry support (e.g., IGES, Parasolid)

geometry creation (e.g., points, surfaces)

meshing

edit materials/properties

much better picking support

much better groups

better use of memory

grid point forces

many more…

Purpose of additional formats¶

Over time, pyNastran has also added converter and GUI support for additional formats. Nastran is not the only piece of the analysis puzzle and there is a need for niche engineering formats.

While, you could convert a Cart3d model (a simple triangulation) to another format like Nastran, you would need to map the geometry/result quantity of interest (e.g., Mach Number) to something like pressure. That’s unintuitive and also requires writing an ill-defined format converter. It’s nice to load it natively as you can also automatically create other quantities (e.g., the bounding CFD box, free edges).

Finally, adding support for alternate formats drives GUI development. The model reload functionality was added to address loading the latest time step of a Usm3d model. It was repurposed to reload the geometry for other formats. This is very useful when creating aero panels and you want to see your changes. The groups functionality benefits all formats.

Additonal formats include:

panair

cart3d

stl

tecplot

AFLR

bsurf

surf

ugrid

usm3d

Setup Note¶

Download the entire package from Github or just the GUI executable.

If you download the source, make sure you follow the installation and use setup.py develop and not setup.py install.

Python 2.7 with vtk==5.10.1 or vtk==6.3.0 with PyQt4 will give you the best looking GUI with v1.0; vtk==7 will work though.

The master requires vtk==7 or vtk==8 and works in either Python 2.7/3.5+ and PyQt4/5.

Running the GUI¶

On the command line:

>>> pyNastranGUI

To view the options:

>>> pyNastranGUI --help

  Usage:
    pyNastranGUI [-f FORMAT] INPUT [-o OUTPUT]
                 [-s SHOT] [-m MAGNIFY]
                 [-g GSCRIPT] [-p PSCRIPT]
                 [-u POINTS_FNAME...] [--user_geom GEOM_FNAME...]
                 [-q] [--groups]
    pyNastranGUI [-f FORMAT] INPUT OUTPUT [-o OUTPUT]
                 [-s SHOT] [-m MAGNIFY]
                 [-g GSCRIPT] [-p PSCRIPT]
                 [-u POINTS_FNAME...] [--user_geom GEOM_FNAME...]
                 [-q] [--groups]
    pyNastranGUI [-f FORMAT] [-i INPUT] [-o OUTPUT...]
                 [-s SHOT] [-m MAGNIFY]
                 [-g GSCRIPT] [-p PSCRIPT]
                 [-u POINTS_FNAME...] [--user_geom GEOM_FNAME...]
                 [-q] [--groups]
    pyNastranGUI -h | --help
    pyNastranGUI -v | --version

  Primary Options:
    -f FORMAT, --format FORMAT  format type (avus, cart3d, lawgs, nastran, panair,
                                             plot3d, stl, surf, tetgen, ugrid, usm3d)
    -i INPUT, --input INPUT     path to input file
    -o OUTPUT, --output OUTPUT  path to output file

  Secondary Options:
    -g GSCRIPT, --geomscript        path to geometry script file (runs before load geometry)
    -p PSCRIPT, --postscript        path to post script file (runs after load geometry)
    -s SHOT, --shots SHOT           path to screenshot (only 1 for now)
    -m MAGNIFY, --magnify           how much should the resolution on a picture be magnified [default: 5]
    --groups                        enables groups
    --user_geom GEOM_FNAME          add user specified points to an alternate grid (repeatable)
    -u POINTS_FNAME, --user_points  add user specified points to an alternate grid (repeatable)

  Info:
    -q, --quiet    prints debug messages (default=True)
    -h, --help     show this help message and exit
    -v, --version  show program's version number and exit

The standard way to run the code is simply by launching the exe. Alternatively, you can call it from the command line, which can directly load a model:

>>> pyNastranGUI -f nastran -i model.bdf -o model1.op2 -o model2.op2

The solid_bending.bdf and solid_bending.op2 files have been included as examples that work in the GUI. They are inside the “models” folder (at the same level as setup.py).

You can also run it like:

>>> pyNastranGUI model.bdf model1.op2

Here the code will guess based on your file extension what your file format is. If you want to load a second OP2, you must use -o model2.op2.

Features¶

fringe plot support

elemental/nodal results

custom CSV results

deflection results

force results

command line interface

scripting capability

high resolution screenshot

show/hide elements

can edit properties (e.g. color/opacity/size) using Edit Geometry Properties... on the View menu

legend menu

animation menu

save/load view menu

Minor Features¶

snap to axis

clipping customization menu

edges flippable from menu

change label color/size menu

change background color

attach simplistic custom geometry with the Load CSV User Geometry or the -user_geom option

additional points may be added with the Load CSV User Points or the --user_points option

Nastran Specific Features¶

attach multiple OP2 files

supports SPOINTs

displacement/eigenvectors/nodal force results

scale/phase editable from legend menu

rotated into global frame

Edit Geometry Properties

SPC/MPC/RBE constraints

CAERO panel, subpanels

AEFACT control surfaces

SPLINE panels/points

bar/beam orientation vectors

CONM2

BDF Requirements¶

Entire model can be cross-referenced

Same requirements as BDF (include an executive/case control deck, define all cross-referenced cards, etc.)

Versioning Note¶

The GUI download is typically newer than the latest release version.

Additional Formats¶

Some of the results include:

Nastran ASCII input (*.bdf, *.nas, *.dat, *.pch, *.ecd); binary output (*.op2)

geometry

node ID

element ID

property ID

material ID

thickness

normal

shell offset

PBAR/PBEAM/PBARL/PBEAML type

element quality (min/max interior angle, skew angle, taper ratio, area ratio)

real results

stress, strain

displacement, eigenvector, temperature, SPC forces, MPC forces, load vector

complex results

displacement, eigenvector

Cart3d ASCII/binary input (*.tri); ASCII output (*.triq)

Node ID

Element ID

Region

Cp, p, U, V, W, E, rho, rhoU, rhoV, rhoW, rhoE, Mach

Normal

LaWGS input (*.wgs)

Panair input (*.inp); output (agps, *.out)

Patch ID

Normal X/Y/Z

Centroid X/Y/Z

Area

Node X/Y/Z

Cp

STL ASCII/binary input (*.stl)

Normal X/Y/Z

Tetgen input (*.smesh)

Usm3d surface input (*.front, *.cogsg); volume input (*.cogsg); volume output (*.flo)

Boundary Condition Region

Node ID

Cp, Mach, T, U, V, W, p, rhoU

Features Overview¶

Edit Geometry Properties¶

The View -> “Edit Geometry Properties” menu brings up:

This menu allows you to edit the opacity, line width, point size, show/hide various things associated with the model. The geometry auto-updates when changes are made.

Modify Legend¶

The View -> “Modify Legend” menu brings up:

This menu allows you to edit the max/min values of the legend as well as the orientation, number format (e.g. float precision) and deflection scale. Defaults are stored, so they may always be gone back to. The geometry will update when Apply/OK is clicked. OK/Cancel will close the window.

Animation Menu¶

The animation menu is a sub-menu found on the legend menu. Hover over the cells for more information.

Animation of Displacment/Mode Shapes (Animate Scale)¶

You must load the animation menu when a displacement-like result is active. You may then change to a scalar result to show during the animation. For the following SOL 101 static deflection result, Animate Scale is used to scale the current result (Displacement). The iCase value corresponds to case that is currently active (Displacement) and is automatically populated when you click the Create Animation button from the Legend menu.

If you would like to plot a separate result (e.g., Node ID), switch to that result. The iCase value will not change. When you click Run All, the iCase value is pulled and the deflection shape is calculated. Make sure you actually have a deflected geometry.

In your output folder, you will find:

If the file is too big, shrink the size of the window. Make the max deflection of the image fill the screen. Leave minimal whitespace.

Note

If unlickling Repeat? doesn’t disable gif looping, upgrade imageio.

Animation of Complex Mode Shapes (Animate Phase)¶

Complex Mode Shapes are simple and similar to the Animate Scale option. Here, the phase angle sweeps from 0 to 360 degrees. Note that this option only shows up when you have a complex result for iCase.

Animation of Time/Frequency/Load Step Results (Animate Time)¶

This option is recommended only for constant time/frequency/load step results. It is now necessary to learn how to set iCase. In the Application log, you’ll see:

COMMAND: fname=gui_qt_common.pyc lineNo=316 cycle_results(case=10)

Check your first (assume 10), second (assume 11), and final time step (assume 40) for their iCase values.

For deflection results loaded from an OP2, the iCase Delta will be 1, but depending on the frame rate and total time you want, you can skip steps.

Note that there is currently no way to plot a transient result other than the deflection unless you want to use scripting.

Picking Results¶

Click on the Probe button to activate probing. Now click on a node/element. A label will appear . This label will appear at the centroid of an elemental result or the closest node to the selected location. The value for the current result quantity will appear on the model. You can also press the p button.

For “NodeID”, the xyz of the selcted point and the node in global XYZ space will be shown. Labels may be cleared from the View menu. Text color may also be changed from the View -> Preferences menu.

Note that for line elements, you need to be very accurate with your picking. Zooming in does not help with picking like it does for shells.

Focal Point¶

Click the following button and click on the rotation center point of the model. The model will now rotate around that point.

Alternatively, hover over the point and press the f key.

Model Clipping¶

Clipping let’s you see “into” the model.

Zoom in and hover over an element and press the f key. The model will pan and now rotate around that point. Continue to hold f while the model recenters. Eventually, the frame will clip. Reset the view by clicking the Undo-looking arrow at the top.

Note that clipping currently doesn’t work…

Modify Groups¶

The View -> “Modify Groups” menu brings up:

Had you first clicked View -> “Create Groups by Property ID”, you’d get:

Add/Remove use the “Patran-style” syntax:

# elements 1 to 10 inclusive
1:10

# elements 100 to the end
100:#

# every other element 1 to 11 - 1, 3, 5, 7, 9, 11
1:11:2

The name of the group may also be changed, but duplicate names are not allowed. The “main” group is the entire geometry.

The bolded/italicized text indicates the group that will be displayed to the screen. The defaults will be updated when you click Set As Main. This will also update the bolded/italicided group.

Camera Views¶

The eyeball icon brings up a camera view. You can set and save multiple camera views. Additionally, views are written out for scripting. You can script an external optimization process and take pictures every so many steps.

User Points¶

User points allow you to load a CSV of xyz points. These may be loaded from within the GUI or from the command line.

# x, y, z
1.0, 2.0, 3.0
4.0, 5.0, 6.0

These will show up as points in the GUI with your requested filename.

User Geometry¶

User geometry is an attempt at creating a simple file format for defining geometry. This may be loaded from the command line. The structure will probably change.

The geometry may be modified from the Edit Geometry Properties menu.

# all supported cards
#  - GRID
#  - BAR
#  - TRI
#  - QUAD
#
# doesn't support:
#  - solid elements
#  - element properties
#  - custom colors
#  - coordinate systems
#  - materials
#  - loads
#  - results

#    id  x    y    z
GRID, 1, 0.2, 0.3, 0.3
GRID, 2, 1.2, 0.3, 0.3
GRID, 3, 2.2, 0.3, 0.3
GRID, 4, 5.2, 0.3, 0.3
grid, 5, 5.2, 1.3, 2.3  # case insensitive

#    ID, nodes
BAR,  1, 1, 2
TRI,  2, 1, 2, 3
# this is a comment

QUAD, 3, 1, 5, 3, 4
QUAD, 4, 1, 2, 3, 4  # this is after a blank line

Custom Scalar Results¶

Custom Elemental/Nodal CSV/TXT file results may be loaded. The order and length is important. Results must be in nodal/elemental sorted order. The following example has 3 scalar values with 2 locations. The corresponding model must have ONLY two nodes. By default, all results must be floatable (e.g., no NaN values).

# element_id, x,   y, z
1,            1.0, 2, 3.0
2,            4.0, 5, 6.0

# element_id  x    y  z
1             1.0  2  3.0
2             4.0  5  6.0

You may also assign result types.

# element_id(%i), x(%f), y(%i), z(%f)
1,                1.0,     2,     3.0
2,                4.0,     5,     6.0

Custom Deflection Results¶

Custom Elemental/Nodal CSV/TXT file results may be loaded. The order and length is important. Results must be in nodal/elemental sorted order. The following example has 3 scalar values with 2 locations. The model must have only two nodes.

# result_name
1.0     2     3.0
2.0     5     6.0

Custom Results Specific Buttons¶

Nastran Static/Dynamic Aero solutions require custom cards that create difficult to view, difficult to validate geometry. The pyNastranGUI aides in creating models. The CAERO panels are seen when a model is loaded:

Additionally, by clicking the Toggle CAERO Subpanels button, the subpanels may be seen:

Additionally, flaps are shown from within the GUI. SPLINE surfaces are also generated and may be seen on the View -> Edit Geometry Properties menu.

Scripting¶

GUI commands are logged to the window with their call signature. Scripting may be used to call any function in the GUI class. Most of these commands are written to the COMMAND output.

For example, you can:

load geometry

load results

plot unsupported result types

custom animations of mode shapes

high resolution screenshots

model introspection

create custom annotations

Command line scripting¶

geomscript runs after the load_geometry method, while postscript runs after load_results has been performed

import sys
self.on_take_screenshot('solid_bending.png', magnify=5)
sys.exit()

>>> pyNastranGUI solid_bending.bdf solid_bending.op2 --postscript take_picture.py

High Resolution Screenshots¶

Option #1¶

self.on_take_screenshot('solid_bending.png', magnify=5)

Option #2¶

On the View -> Preferences menu, change Screenshot Magnify and click Apply. Now take a screenshot.