Graphical User Interface (GUI)

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

If you download the source, make sure you follow the installation.

Versioning Note

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


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 initial 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.

The Graphical User Interface (GUI) looks like:


A somewhat messy, but more featured image:


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

  • section cuts

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

  • custom results from a CSV file

  • modern Nastran support - Patran 2005 can’t read in models that pyNastranGUI can - not an advantage for newer versions

  • reduction of required licenses

  • 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

  • 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.

Additional formats include:

  • abaqus

  • cart3d

  • panair

  • tecplot

  • AFLR

  • bsurf

  • surf

  • ugrid

  • stl

  • usm3d


Major 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.)

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


      • 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


Select the components from:
  • Magnitude (X, Y, Z)

  • X

  • Y

  • Z

Any combination of terms is allowed. Note that if no components are selected, all components will be used. If Magnitude and X are selected, Magnitude will be used.

Additionally, to determine the fringe/color values, the vector must be reduced using:

  • Magnitude : takes the L2-norm of the vector sqrt(x^2 + y^2 + z^2); positive

  • Value : returns the signed value of a component. Note that if multiple components are selected, Magnitude will be selected by default.

Note that the animation scale factor is tied to the magnitude, so if you select Z displacment and it doesn’t dominate the response, you will need to adjust the scale factor.


Other than some arrows, SPC Force and Displacement work the same way.

There are 5 nodes (N1-N4 + centroid) for each quad across two layers (top/bottom) for a total of 10 result locations per quad element. This needs to be reduced down to multiple nodes or a single centroidal value.

Centroidal stresses may be selected. Note that Nodal Combine isn’t going to do much if only Centroid is selected.

../_images/results_plate_stress_centroid.png ../_images/results_plate_stress_centroid_zoom.png

Additionally, there are likely neighboring elements too, so the Nodal Combine option defines how multiple values at a given node are handled (e.g., Mean, Max, Min). The typical way to plot solid stress/strain is with the Mean option. The other options are most useful for checking how well the model is converged.

../_images/results_plate_stress_nodal.png ../_images/results_plate_stress_nodal_zoom.png

Derivation Method

Derivation Method looks at a single given node/centroid (both layers) and “reduces” it down to a single value/layer. Min/Max are common, but “Absolute Max” provides the “worst” value by looking at the min/max of each node and taking the biggest value and then using the sign to indicate tension or compression.

The included methods are:
  • Absolute Max

  • Min

  • Max

  • Mean

  • Standard Deviation

  • Difference (Max - Min)

Nodal Combine

Nodal Combine takes the “reduced” values from “Derivation Method” and does a similar combination. Additionally, there’s a centroidal option.

The included methods are:
  • Centroid

  • Mean

  • Absolute Max

  • Min

  • Max

  • Standard Deviation

  • Difference (Max - Min)

Solid Stress / Strain

There are two options for solid stress/strain:
  • Centroid

  • Corner (Nodal)

Centroidal stresses may be selected. Note that Nodal Combine isn’t going to do much if only Centroid is selected.


The typical way to plot solid stress/strain is with the Mean option.


Nodal Combine

Nodal Combine “reduces” multiple layer results from different elements down into a single value at each node.

The supported methods are:
  • Mean

  • Absolute Max

  • Min

  • Max

  • Standard Deviation

  • Difference (Max - Min)

Composite Plate Stress / Strain


Derivation Method “reduces” multiple layer results down into a single value at each element centroid.

The supported methods are:
  • Mean

  • Absolute Max

  • Min

  • Max

  • Standard Deviation

  • Difference (Max - Min)

Shear-Moment-Torque Plot

If you included GPFORCE(PLOT) = ALL in your BDF, you can create a shear force diagram/bending moment diagram.

The goal is to define a starting (blue point) and ending point (red point) to define a vector. Along that vector a series of cutting planes (num Planes) will be defined. At the points where the planes and the vector cross, a coordinate system will be created.


Load the model and select the result from the results sidebar. Then open the Shear, Moment, Torque tool from the Tools menu:


The menu will pop up and you can define the starting/ending points. The origin of each coordinate system is automatically calculated, so two additional points/vectors are required. The CORD2R option requires two vectors and the Vector requires two vectors.

The goal here is to define the cutting plane where the section cut will be. Note that the direction of axes affects the sign of the force/moment. Note that the “x-direction” of the vector and the output coordinate system are not the same.


You can test the cutting plane by pressing Plot Plane:


Once you’re happy with the coordinate system and the plane press Apply to generate a series of plots:


Note that the i Station of the plot corresponds to the distance along the vector, so it is not what is seen in

The more standard way to present the information using the global y-axis. That requires doing a post-processing step either in Excel/separate script/Jupyter Notebook.

Custom Results

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 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 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 first column corresponds to the NodeID or ElementID and missing values are allowed. 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 with (%i) and (%f). Formatting works as well, so (%.3f) is valid.

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

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.

# displacement
1.0     2     3.0
2.0     5     6.0

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.

Edit Geometry Properties Menu

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 Menu

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.

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.


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

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.


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: lineNo=316 self.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.

Preferences Menu

The preferences menu allows you to change various settings. These will be remembered when you load model again. The menu looks like:


Hover over the cells for more information.

Windows preferences are stored in:
  • C:\Users\<me>\pyNastranGUI.json

Or Linux/Mac:
  • ~/pyNastranGUI.json

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 selected 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.

Center of Rotation

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

# elements 100 to the end

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

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.

You can also define groups in your BDF:

$ group: name='RLongeron MainFuseStruct Gridpoint'; nodes=167:205
$ group: name='Skin MainFuseStruc'; elements=6001:15017
$ group: name="ULFuseCanardAtch MainFuseStruct Fixed point constraints, 123"; spcs=3

$ group: name="ULFuseCanardAtch MainFuseStruct Fixed point constraints; 123"; spcs=3    (semicolon in name)

Unioned Groups (spcs becomes [1,2,3] internally):
$ group: name="spcs"; spcs=1
$ group: name="ULFuseCanardAtch MainFuseStruct Fixed point constraints, all"; spcs=1
SPC1           1  123456      13
$ group: name="spcs"; spcs=2
$ group: name="ULFuseCanardAtch MainFuseStruct Fixed point constraints, 123456"; spcs=2
SPC1           2  123456      13
$ group: name="spcs"; spcs=3
$ group: name="ULFuseCanardAtch MainFuseStruct Fixed point constraints, 123"; spcs=3
SPC1           3  123         13

Node groups will show up in the EditGeometryProperties menu, while element groups will show up in the Groups menu. Other group types are not supported in the gui.

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.



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

The scripting menu allows for custom code and experimentation to be written without loading a script from a file. All valid Python is accepted. Scripting commands should start with self.. Local variables do not need this.

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)
>>> pyNastranGUI solid_bending.bdf solid_bending.op2 --postscript

On the command line:

>>> pyNastranGUI

To view the options:

>>> pyNastranGUI --help

    pyNastranGUI [-f FORMAT] INPUT [-o OUTPUT]
                 [-s SHOT] [-m MAGNIFY]
                 [-g GSCRIPT] [-p PSCRIPT]
                 [-u POINTS_FNAME...] [--user_geom GEOM_FNAME...]
                 [-q] [--groups]
                 [-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)

    -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

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.

Option #1

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

Option #2

After the screenshot from Option 1 was created, the following code was printed out to the log. Copy and paste it into the Python Console.

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

The legend font is way to big!

The legend is tricky cause of the wide range in the number of title characters preferences.

It’s defined in terms of a percentage of screen size and the font size is defined in terms of the title character (or number size), so it’s tricky to to get a robust system. However, you do have some control:

  • legend title: - resize the window to be shorter - use the legend (View -> Modify Legend; Control+L) and add whitespace around the etitle

  • legend values: - resize the window to be narrower - use the legend (View -> Modify Legend; Control+L) and change the number format

The coordinate system/origin font is waaaay too big!

The coordinate system is dependent on zoom level and model size. You can customize:
  • coordinate system size

  • coordinate system text size

in the Preferences menu (Control+P).

I could not visualize the mesh edges within the results

Mesh edges press e for edges and b if you want to make them black. There are also pull downs on the view menu and the e option is on the toolbar (the black wireframe)

How do I clear a result?

Right click on the Case/Results tree and go to Clear Results.

It’s not easy to change between results (such as Sxx, Syy, Mises, etc.) using only the arrows

You can use K and L (lowercase) to “cycle” to different results.

How do I make the gif more responsive/smaller?

The GIF will be the same size as your screen (the part with the grey background), so make your window smaller. In general, 30 frame/second is going to look nice, but you can even get away with 10 FPS if the picture is small.

The GUI crashes when I have a model loaded and load a different one

Yeah…it does that. It’s not really designed around loading differet models. There are some objects that aren’t deleted and it’s tricky to do it right. If you mess one up, it crashes.

If you’re just modifying a deck, you can use the “Reload Model” option. It’ll reload the geometry and be quite a bit faster than going through menus. That fails sometimes as well, but is more robust.

The GUI crashes when loading an OP2?

The code is trying to match the IDs in the geometry to the IDs in the results and they don’t always match. There is some handling of this, but it’s not great.

Also, make sure you load the correct model too :)