Rendered from src/settings/README.md in the repository — edit it there.

Slicing Parameters & Settings

Configuration for slicing behavior and printer control. All values stored as JSON.

Quick Reference

Slicing Parameters (params.*)

Parameter	Type	Default	Range	Effect
layer_height	mm	0.2	0.1–0.4	Distance between layers
wall_thickness	mm	1.2	0.8–2.0	Perimeter width
infill_density	0–1	0.15	0.0–1.0	0=hollow, 1=solid
print_speed	mm/s	120	10–500	Fallback speed for any role without its own
nozzle_temp	°C	210	180–250	Heat level (material-dependent)
bed_temp	°C	60	20–100	Bed heat (material-dependent)
seam_position	enum	aligned	see Seam Position	Where each closed-loop seam sits
min_infill_extrusion_mm	mm	0.4	0.0–nozzle	Drops sub-threshold solid-surface and sparse-infill segments to cut tiny travels
coasting_distance_mm	mm	0	0.0–1.0	Length of un-extruded tail at the end of each path
thumbnail_enabled	bool	true	true/false	Embed a PNG thumbnail comment block in output G-code (Thumbnail group)
thumbnail_size_px	px	320	64–1024	Square thumbnail resolution (the quality knob)
thumbnail_view	enum	isometric	isometric/front/rear/left/right/top	Fixed camera angle the UI renders the thumbnail from
thumbnail_theme	enum	transparent	light/dark/transparent	Fixed thumbnail background (independent of app/OS theme)
thumbnail_color_mode	enum	filament	generic/filament/custom	Model colour in the thumbnail: neutral / filament / chosen
thumbnail_custom_color	hex	#e0912f	#rrggbb	Model colour used when thumbnail_color_mode = custom

Infill (params.*)

Parameter	Type	Default	Effect
infill_pattern	enum	TpmsD	see below
infill_base_angle	°	45	Sparse fill direction; alternating layers add 90°
infill_anchor_percent	%	400	How far a lone infill line end runs along the wall, as a % of the bead spacing
infill_anchor_max_mm	mm	20	Longest wall stretch that may join two infill lines; 0 = no anchoring
infill_every_layers	count	1	Print sparse infill once every N layers, at N× the height (1 = off)
infill_combination_max_layer_height_mm	mm	0	Cap on the combined height; 0 = use the nozzle diameter
solid_infill_every_layers	count	0	Force a solid internal layer every N layers (0 = off)

Infill patterns: Rectilinear, AlignedRectilinear, Grid, Triangles, TriHexagon, Cubic, Honeycomb, Concentric, Gyroid, TpmsD.

Density is measured against the bead spacing (width − h·(1 − π/4)), so a requested density equals the deposited volume at any line width — and every pattern deposits the same amount. See src/infill/README.md.

Surfaces (params.*)

Parameter	Type	Default	Effect
surface_infill_angle	°	45	Solid fill direction; alternates 90° per layer
top_surface_pattern	enum	rectilinear	Fill pattern for the visible top surface
bottom_surface_pattern	enum	rectilinear	Fill pattern for the bottom surface
internal_solid_infill_pattern	enum	monotonic	Fill pattern for forced internal solid layers
ironing_enabled	bool	false	Sweep finished top surfaces with a near-dry smoothing pass
ironing_type	enum	top_surfaces	top_surfaces / topmost_only / all_solid
ironing_flow	%	10	Material deposited, as a share of a normal bead
ironing_spacing	mm	0.1	Pitch between ironing passes
ironing_speed	mm/s	20	0 = fall back to top_surface_speed
ironing_angle	°	-1	-1 = follow the layer's own fill angle

Surface patterns: rectilinear, aligned-rectilinear, monotonic, monotonic-line, concentric. "Monotonic" draws every line in the same direction, so the nozzle never travels back over a line it just laid.

Ironing carries the Ironing role (;TYPE:Ironing) and its own speed and acceleration. Its width is ironing_spacing × ironing_flow, which keeps the flow reduction out of the G-code generator's flow-ratio parameter — that deliberately reads a non-positive ratio as 1.0, so routing a "wipe only" setting through it would lay a full-width bead at 0.1 mm pitch.

Dimensional compensation (params.*)

Parameter	Type	Default	Effect
xy_size_compensation	mm	0	Grow (+) or shrink (−) every contour; also tightens holes
xy_hole_compensation	mm	0	Enlarge (+) or tighten (−) holes only, applied after
elephant_foot_compensation_mm	mm	0.2	Shrink the layers at the bed to undo the first layer's squish
elephant_foot_layers	n	1	How many layers the correction tapers over

Both are applied to the raw contours between slicing and wall generation — the only point at which the rest of the pipeline's measurements stay true. See src/core/compensation.rs.

xy_size_compensation follows the PrusaSlicer/Slic3r meaning (one number, and growing the part necessarily tightens its holes); xy_hole_compensation follows Orca/Bambu's separate hole delta. They are separate fields because collapsing them into one signed value gets imported Orca profiles wrong by 2δ on every hole.

First layer (params.*)

Parameter	Type	Default	Effect
first_layer_height	mm	0	Thickness of the bottom layer; 0 = use layer_height

Affects both geometry and flow: the slicer gives layer 0 its own Z span, and the generator charges it at that height via path_heights. Suppressed when a raft is present, since the raft then owns bed contact.

Bridge & overhang (params.*)

Parameter	Type	Default	Effect
bridge_speed	mm/s	10	Print speed for bridge / overhang-perimeter extrusions (slow = smooth)
enable_overhang_speed	bool	true	Grade perimeters by unsupported fraction instead of one flat bridge_speed
overhang_1_4_speed	RelativeSpeed	no override	Deg1 (0–25% unsupported, to ~27° from vertical); % of perimeter_speed
overhang_2_4_speed	RelativeSpeed	no override; "50%"/"35%" on the high-speed/maximum presets	Deg2 (25–50%, ~27–45°); % of perimeter_speed
overhang_3_4_speed	RelativeSpeed	no override	Deg3 (50–75% unsupported, ~45–56°); % of bridge_speed
overhang_4_4_speed	RelativeSpeed	"80%"	Deg4 (75–100% unsupported, ~56–63°); % of bridge_speed

Each value may also be a literal mm/s. The angles are for 0.2 mm layers on a 0.4 mm nozzle — a degree is layer_height × tan(lean) / nozzle_diameter, so thinner layers push every band steeper. Past 100% the bead has left the layer below altogether and the segment is retagged OverhangPerimeter; below that it stays a wall, graded by degree.

RelativeSpeed (src/settings/relative_speed.rs) is a bare number (absolute mm/s) or a "NN%" string (a fraction of the field named by that property's x-relative-to schema extension) — "no override" means the literal legacy 0 sentinel, which still resolves to the source field's own speed (bridge_speed for Deg3/Deg4, by degree rather than by role). | bridge_flow_ratio | 0–1.5| 1.5 | Flow multiplier for bridge lines (>1 fuses strands into a smooth floor) | | bridge_anchor_mm | mm | 0.4 | Inflate the bridge region outward to anchor strands into solid material | | bridge_min_area_mm2 | mm² | 0.5 | Drop bridge candidates smaller than this; reclassified as BottomSurface | | bridge_noise_filter_mm | mm | 0.05 | Morphological-open radius to wipe sub-pixel slivers before bridge detection | | bridge_fan_speed | 0–1 | 1.0 | Part-cooling duty while printing Bridge segments (per-segment override) | | bridge_angle | ° | 0 | Force one bridging direction; 0 = auto-detect, 180 = horizontal |

Cooling & chamber (params.*)

The filament owns the material policy, the printer owns the hardware capability; fan_configs stays the printer-side adaptive layer-time table. Full precedence rules in gcode/README.md.

Parameter	Type	Default	Effect
fan_speed	0–1	1.0	Ceiling the adaptive fan_configs curve is clamped to (the high-temp material gate)
first_layer_fan_speed	0–1	0.0	Part-cooling duty while pinned by disable_fan_first_layers
disable_fan_first_layers	n	1	Bottom layers where part cooling is pinned; bridge/overhang overrides are suppressed there
min_layer_time_s	s	4	Shortest a layer may take; below it the layer is slowed, then dwelled. Filament profiles set their own
min_print_speed	mm/s	10	Floor the slowdown will not go below
overhang_fan_speed	0–1	1.0	Part-cooling duty on overhang segments (needs enable_overhang_speed)
overhang_fan_threshold	0–1	0.5	Unsupported fraction above which overhang_fan_speed engages
heated_chamber	bool	false	Printer capability — without it no M141/M191 is ever emitted
chamber_temp	°C	0	Chamber target; bed armed + M141/M191 soak run before the start G-code
chamber_temp_first_layer	°C	0	First-layer soak target (0 = use chamber_temp); restored at layer 2

Retraction (params.*)

Parameter	Type	Default	Effect
retract_mm	mm	1.0	Filament pulled back on a retracting travel
retract_speed_mm_min	mm/min	2400	Retract / un-retract feedrate
z_hop_mm	mm	0.2	Nozzle lift during a retracting travel
retract_before_travel_mm	mm	1.0	Minimum travel distance before a retraction is triggered
retract_restart_extra_mm	mm	0.0	Extra prime length added on un-retract to compensate for travel ooze
retract_on_layer_change	bool	false	Retract before every layer-change Z move
use_firmware_retraction	bool	false	Emit G10/G11 and sync the firmware (M207/M208 or SET_RETRACTION)
use_relative_e_distances	bool	false	Emit M83 + incremental E (G1 … E<delta>) instead of M82 absolute positions
wipe	bool	true	Retrace the just-printed path while retracting to smear ooze onto printed material
wipe_distance_mm	mm	1.0	How far to wipe (capped at the previous path's length) when wipe is enabled
retract_before_wipe_percent	0–1	0.0	Fraction of the retraction performed before the wipe (the rest is distributed along it)

Machine (params.*)

Parameter	Type	Default	Effect
z_offset_mm	mm	0.0	Added to every Z coordinate in the output G-code to compensate a mis-zeroed Z endstop (negative lowers the nozzle). Emitted coordinates and layer markers only — the model, statistics and your start/end G-code are untouched. See gcode/README.md.

Global Settings (top-level)

Field	Type	Default	Description
gcode_flavor	string	"marlin"	Firmware dialect ("marlin" or "klipper")
start_print_gcode	string | null	null	Custom start G-code block or file path
end_print_gcode	string | null	null	Custom end G-code block or file path
lifecycle_markers	object	{}	Per-flavor layer lifecycle marker config (see below)

Config Priority

Settings are resolved in this order (highest priority first):

1. CLI arguments          (--layer-height, --gcode-flavor, --start-print-gcode, …)
2. slicer.json            (project config in CWD, or --config FILE)
3. ~/.config/slicer-engine/settings.json  (user config)
4. Built-in defaults

Each layer overrides only the keys it specifies; unset keys fall through to the next layer.

Project Config (slicer.json)

Place a slicer.json file in your project directory to set per-project defaults that override the user config without touching it. Only the keys you include are overridden.

{
  "params": {
    "layer_height": 0.15,
    "nozzle_temp": 215
  },
  "gcode_flavor": "klipper"
}

The file is auto-discovered when you run any slice command from the same directory. You can also point to it explicitly:

slicer-engine slice --input model.stl --config ./path/to/slicer.json

User Config (settings.json)

The persistent user-level config lives at:

Platform	Path
Linux	~/.config/slicer-engine/settings.json
macOS	~/Library/Application Support/slicer-engine/settings.json
Windows	%APPDATA%\slicer-engine\settings.json

Managed via the settings set / settings get subcommands (see below).

JSON Structure

Global settings file (settings.json or slicer.json)

{
  "params": {
    "layer_height": 0.2,
    "wall_thickness": 1.2,
    "infill_density": 0.15,
    "print_speed": 120.0,
    "nozzle_temp": 210.0,
    "bed_temp": 60.0
  },
  "gcode_flavor": "marlin",
  "lifecycle_markers": {
    "klipper": {
      "enabled": true,
      "layer_change": ";LAYER_CHANGE",
      "z_marker": ";Z:{z}",
      "height_marker": ";HEIGHT:{height}",
      "before_layer_change": ";BEFORE_LAYER_CHANGE",
      "after_layer_change": ";AFTER_LAYER_CHANGE",
      "type_annotation": ";TYPE:{type}",
      "width_annotation": ";WIDTH:{width}mm"
    }
  }
}

start_print_gcode and end_print_gcode are omitted from the file when null. lifecycle_markers is omitted entirely when the map is empty (i.e. all defaults are in effect).

Lifecycle Markers

Layer lifecycle markers are comments that slicer-aware firmware and post-processing scripts use to track progress, drive LED effects, pause at layers, etc.

How it works

Each firmware flavor can have its own LifecycleMarkerConfig entry in the lifecycle_markers map. Flavors not present in the map use the built-in defaults (enabled, standard OrcaSlicer/PrusaSlicer comment format).

When enabled: false, the generator emits a minimal ; layer z=… comment instead of the full lifecycle block.

Per-flavor configuration (LifecycleMarkerConfig)

Field	Default emitted comment	Supported placeholders
enabled	true	—
layer_change	;LAYER_CHANGE	{z}, {height}
z_marker	;Z:{z}	{z}
height_marker	;HEIGHT:{height}	{height}
before_layer_change	;BEFORE_LAYER_CHANGE	{z}
after_layer_change	;AFTER_LAYER_CHANGE	{z}
type_annotation	;TYPE:{type}	{type}
width_annotation	;WIDTH:{width}mm	{width}

All string fields are optional — omit them to keep the built-in default for that marker.

Placeholder reference

Placeholder	Replaced with	Example
{z}	Layer Z coordinate (3 d.p.)	0.200
{height}	Layer height from params (3 d.p.)	0.200
{type}	Extrusion role type name	WALL-OUTER, FILL
{width}	Extrusion role default width (2 d.p.)	0.40

Example: disable markers for Marlin, keep them for Klipper

{
  "lifecycle_markers": {
    "marlin": { "enabled": false },
    "klipper": { "enabled": true }
  }
}

Example: custom marker strings for a Bambu-style slicer

{
  "lifecycle_markers": {
    "marlin": {
      "enabled": true,
      "layer_change": ";BAMBULABS_LAYER_CHANGE",
      "z_marker": ";Z_HEIGHT:{z}"
    }
  }
}

CLI overrides

The --lifecycle-markers and --no-lifecycle-markers flags on the slice command override the enabled field from settings for the current invocation only:

# Force-enable markers regardless of settings
slicer-engine slice --input model.stl --lifecycle-markers

# Force-disable markers regardless of settings
slicer-engine slice --input model.stl --no-lifecycle-markers

Object settings (per-object override)

{
  "object_name": "detail_part",
  "overrides": {
    "layer_height": 0.1,
    "print_speed": 40.0
  }
}

When overrides is null, the object inherits all global settings.

CLI Commands

Get/Set Individual Values

Both flat aliases and full dot-separated paths are accepted:

# These are equivalent
slicer-engine settings get layer_height
slicer-engine settings get params.layer_height

# Set via flat alias
slicer-engine settings set layer_height 0.15

# Set via full path
slicer-engine settings set params.nozzle_temp 215

# Set top-level fields
slicer-engine settings set gcode_flavor klipper
slicer-engine settings set start_print_gcode "START_PRINT BED_TEMP=60 EXTRUDER_TEMP=210"
slicer-engine settings set end_print_gcode "END_PRINT"

# Clear an optional field
slicer-engine settings set start_print_gcode null

# JSON output
slicer-engine settings get layer_height --output-format json

Show All

slicer-engine settings show
slicer-engine settings show --output-format json

Validate

slicer-engine settings validate \
  --global global.json --object object.json

Checks constraints and ranges. Output: ✓ valid or error messages.

Diff

slicer-engine settings diff \
  --global global.json --object object.json

Shows which parameters are overridden:

layer_height    0.2 → 0.1    ✓ Override
print_speed     60  → 40     ✓ Override
nozzle_temp     210 → 210    (no change)

Validation Rules

Parameter	Constraint	Notes
layer_height	> 0	Typically ≤ nozzle diameter (0.4 mm)
wall_thickness	≥ 0.4 mm	At least one nozzle width
infill_density	0.0 ≤ x ≤ 1.0	Strict bounds
print_speed	> 0	Higher = faster but lower quality
nozzle_temp	180–250°C	Material-dependent (PLA≈210, PETG≈230)
bed_temp	20–120°C	Material-dependent (PLA≈60, PETG≈100)
gcode_flavor	"marlin" | "klipper"	Must be a known firmware dialect

Common Profiles

PLA

{
  "params": { "layer_height": 0.2, "nozzle_temp": 210, "bed_temp": 60 },
  "gcode_flavor": "marlin"
}

PETG

{
  "params": { "layer_height": 0.2, "nozzle_temp": 230, "bed_temp": 85 }
}

High-detail (Klipper)

{
  "params": { "layer_height": 0.1, "print_speed": 30, "wall_thickness": 1.6 },
  "gcode_flavor": "klipper",
  "start_print_gcode": "START_PRINT BED_TEMP=60 EXTRUDER_TEMP=210",
  "lifecycle_markers": {
    "klipper": { "enabled": true }
  }
}

Seam Position

params.seam_position controls where each closed perimeter loop begins and ends — the spot where the printer pauses, retracts, and lifts. That spot leaves a small visible blob ("the seam") on the outer wall.

Value	Vertex chosen per loop	Visual result	Best for
nearest	Closest vertex to the previous path's end	Scattered seams; minimum travel & print time	Prototypes, infill-heavy parts
rear	Vertex with the largest Y	Single seam line at the back of the model	Display pieces (Benchy-style)
aligned (default)	Vertex with the largest projection onto a fixed direction (+Y)	Consistent vertical seam line across all layers	Parts whose loops shift between layers
sharpest_corner	Vertex with the largest convex turn angle (falls back to nearest)	Seam hidden in geometry corners	Mechanical parts with hard edges
random	Hash of the loop's first-vertex bits (deterministic per loop)	Seam blobs spread evenly; no visible line	Cylinders, organic shapes

Override per-invocation from the CLI:

slicer-engine slice --input model.stl --seam-position rear

Set persistently in slicer.json / settings.json:

{ "params": { "seam_position": "sharpest_corner" } }

Hyphens and underscores are both accepted (sharpest-corner ≡ sharpest_corner). See core/README.md for the implementation details and the role-grouped path-ordering pass that consumes this setting.

Integration

See Also

• CLI Commands – Full command reference
• Slicing – How layer_height affects slicing
• Core pipeline – Path ordering & seam placement
• G-code generation – Smart-retract policy & travel sequence
• Root – Overview