G-code Generation¶

This example demonstrates exporting toolpaths to G-code for desktop FDM 3D printers like Prusa, Ender, or Ultimaker.

What You'll Learn¶

Configuring printer parameters with GcodeConfig
Positioning mesh for delta vs cartesian printers
Generating G-code from printpoints
Understanding the G-code structure (header, purge, toolpath, footer)

G-code Basics¶

G-code is the standard language for CNC machines and 3D printers. Each line is a command:

G1 X100 Y50 Z0.2 E1.5 F3600  ; Move to X=100, Y=50, Z=0.2 while extruding 1.5mm at 3600mm/min

Common commands:

Command	Description
`G0` / `G1`	Linear move (G0 = rapid, G1 = controlled)
`G28`	Home axes
`G90` / `G91`	Absolute / relative positioning
`M104` / `M109`	Set extruder temp (no wait / wait)
`M140` / `M190`	Set bed temp (no wait / wait)
`M106` / `M107`	Fan on / off

The Pipeline¶

flowchart LR
    A[Slice Mesh] --> B[Create PrintPoints]
    B --> C[Configure GcodeConfig]
    C --> D[Generate G-code]
    D --> E[Save .gcode File]

Step-by-Step Walkthrough¶

1. Setup and Configuration¶

from pathlib import Path
from compas.datastructures import Mesh
from compas.geometry import Point
from compas_slicer.config import GcodeConfig
from compas_slicer.pre_processing import move_mesh_to_point

mesh = Mesh.from_obj(DATA_PATH / 'simple_vase_open_low_res.obj')

# Create G-code configuration
gcode_config = GcodeConfig()

2. Position Mesh for Printer Type¶

if gcode_config.delta:
    # Delta printers: origin at center
    move_mesh_to_point(mesh, Point(0, 0, 0))
else:
    # Cartesian printers: center in build volume
    move_mesh_to_point(mesh, Point(
        gcode_config.print_volume_x / 2,
        gcode_config.print_volume_y / 2,
        0
    ))

Delta vs Cartesian

Delta printers: Circular build plate, origin at center (0, 0, 0)
Cartesian printers: Rectangular build plate, origin at corner (0, 0, 0)

3. Slice and Process¶

from compas_slicer.slicers import PlanarSlicer
from compas_slicer.post_processing import generate_brim, simplify_paths_rdp, seams_smooth

slicer = PlanarSlicer(mesh, layer_height=4.5)
slicer.slice_model()

generate_brim(slicer, layer_width=3.0, number_of_brim_offsets=4)
simplify_paths_rdp(slicer, threshold=0.6)
seams_smooth(slicer, smooth_distance=10)

4. Create PrintPoints¶

from compas_slicer.print_organization import PlanarPrintOrganizer, set_extruder_toggle

print_organizer = PlanarPrintOrganizer(slicer)
print_organizer.create_printpoints()
set_extruder_toggle(print_organizer, slicer)

5. Generate and Save G-code¶

from compas_slicer.utilities import save_to_text_file

gcode_text = print_organizer.output_gcode(gcode_config)
save_to_text_file(gcode_text, OUTPUT_PATH, 'my_gcode.gcode')

GcodeConfig Parameters¶

The GcodeConfig dataclass controls all printer parameters:

Hardware Settings¶

Parameter	Default	Description
`nozzle_diameter`	0.4 mm	Nozzle diameter
`filament_diameter`	1.75 mm	Filament diameter (1.75 or 2.85)
`delta`	False	Delta printer flag
`print_volume`	(300, 300, 600)	Build volume (x, y, z) in mm

Temperature & Fan¶

Parameter	Default	Description
`extruder_temperature`	200°C	Hotend temperature
`bed_temperature`	60°C	Heated bed temperature
`fan_speed`	255	Part cooling fan (0-255)
`fan_start_z`	0.0 mm	Height to enable fan

Extrusion¶

Parameter	Default	Description
`layer_width`	0.6 mm	Extrusion width
`flowrate`	1.0	Flow multiplier
`flow_over`	1.0	Overextrusion factor near bed
`min_over_z`	0.0 mm	Height for overextrusion

Motion¶

Parameter	Default	Description
`feedrate`	3600 mm/min	Print speed (60 mm/s)
`feedrate_travel`	4800 mm/min	Travel speed (80 mm/s)
`feedrate_low`	1800 mm/min	First layer speed (30 mm/s)
`feedrate_retraction`	2400 mm/min	Retraction speed
`acceleration`	0	Acceleration (0 = default)
`jerk`	0	Jerk (0 = default)

Retraction¶

Parameter	Default	Description
`z_hop`	0.5 mm	Z lift during travel
`retraction_length`	1.0 mm	Filament retraction distance
`retraction_min_travel`	6.0 mm	Minimum travel to trigger retraction

Custom Configuration¶

Override defaults when creating the config:

gcode_config = GcodeConfig(
    extruder_temperature=210,
    bed_temperature=65,
    feedrate=2400,  # 40 mm/s
    layer_width=0.45,
    retraction_length=0.8,
)

Or load from a TOML file using PrintConfig:

from compas_slicer.config import PrintConfig

config = PrintConfig.from_toml("my_printer.toml")
gcode_config = config.gcode

G-code Structure¶

The generated G-code has four sections:

1. Header¶

;G-code generated by compas_slicer
T0                             ;select tool 0
G21                            ;metric units
G90                            ;absolute positioning
M140 S60                       ;set bed temp (no wait)
M104 S200                      ;set extruder temp (no wait)
M109 S200                      ;wait for extruder temp
M190 S60                       ;wait for bed temp
G28 X0 Y0                      ;home X and Y
G28 Z0                         ;home Z

2. Purge Line¶

;Purge line
G1 Z0.2                        ;move to purge height
G1 X5 Y5                       ;move to purge start
G1 Y150 E3.5                   ;purge line 1
G1 X5.6                        ;step over
G1 Y5 E3.5                     ;purge line 2
G92 E0                         ;reset extruder position

3. Toolpath¶

;Begin toolpath
G1 F1800                       ;slow feedrate for adhesion
G1 X50.000 Y30.000 Z0.200
G1 X51.234 Y30.567 E0.125
...

;End of print
G1 E-1.0                       ;final retract
G1 Z10.000                     ;lift nozzle
G1 X0 Y0                       ;move to home
M104 S0                        ;extruder heater off
M140 S0                        ;bed heater off
M84                            ;motors off

Volumetric Extrusion¶

The G-code generator calculates extrusion using volumetric math:

\[E = \frac{d \cdot h \cdot w}{\pi (D/2)^2} \cdot f\]

Where:

\(E\) = extrusion length (mm)
\(d\) = travel distance (mm)
\(h\) = layer height (mm)
\(w\) = path width (mm)
\(D\) = filament diameter (mm)
\(f\) = flow rate multiplier

This ensures correct material deposition regardless of layer height or path width.

Complete Code¶

--8<-- "examples/4_gcode_generation/example_4_gcode.py"

Running the Example¶

cd examples/4_gcode_generation
python example_4_gcode.py

With visualization:

python example_4_gcode.py --visualize

Output: examples/4_gcode_generation/data/output/my_gcode.gcode

Key Takeaways¶

Configure for your printer: Set temperatures, speeds, and retraction for your specific machine
Position mesh correctly: Delta vs cartesian printers have different origins
Volumetric extrusion: Automatically calculates correct E values
Modular structure: Header/purge/toolpath/footer makes debugging easier

Next Steps¶

Scalar Field Slicing - Custom slicing patterns
Print Organization - More fabrication parameters