CNC Pocket Cam Programmer user guide
The goal of CNC Pocket Cam Programmer is to allow any general CNC professional to learn and use it easily, with minimal training, though programming experience is helpful for some advanced features. Important: this is a mobile app, not desktop CAM software. The phone's performance and memory are limited, so very large jobs or very fine settings (e.g. a large 3D model or a very small stepover) may take longer to calculate and can even stall on weaker devices. In such cases, use coarser settings or split the job into smaller parts.
Contents
- Packs
- Using the App
- G-Code Generator
- Calculators
- 3D Import
- Sketch 3D Extrude
- Photo Relief
- DXF/SVG Import
- Sketch Editor
- Machine Transfer
- Reference Tables
- Tool Library
- General
Packs
One-time purchase
Every pack is a one-time purchase and yours forever. No subscription.
PRO
Unlocks all features with the PRO badge, unlimited export, no ads.
ULTRA
Everything in PRO, plus 3D Import (STL/OBJ/3MF), and all three packs below are included.
Photo Relief Pack
Turns a photo into a 3D relief and generates the G-code for it.
DXF/SVG Pack
Import DXF and SVG drawings for G-code, plus Photo → Engrave (image to vector drawing).
3D Extrude Pack
Turns your drawing into a raised 3D model and generates the G-code for it.
Trial
During the trial ULTRA is active: every feature and pack can be tried freely. You can buy any of them meanwhile: what you buy stays yours afterwards, and the trial keeps running until it ends.
Using the App
The app is operated with the following gestures: tap, long press, drag, scroll, swipe, open, close, zoom in, zoom out, rotate, double tap. In the previews, the simulation speed can also be adjusted by moving the sliders left or right. With a little practice it becomes second nature. Explore it, try it out!
G-Code Generator
Select an operation on the Home screen or open the Generator from the G-Code menu. Choose the operation type in the top bar, then fill in the 4 tabs. Supported post processors: Fanuc, Haas, Siemens, Okuma, Mitsubishi, Mach3, GRBL.
4 Setting Tabs
Dimensions: workpiece and machining sizes. Tool: cutter diameter, flutes, tool number (T). Can load from tool library. Technology: RPM, feed rate, depth of cut. Selecting a material auto-fills these values. 3 tool materials: HSS, carbide, insert. Options: post processor, work offset (G54–G59), climb/conventional, coolant, finishing pass, units.
3D Preview
The right panel shows an animated 3D toolpath preview. Below it: raw G-code and a workshop sheet. The program can be copied, saved (.nc), shared, converted to QR code, or sent directly to the machine.
Rectangular Pocket
Enter width, length and depth. The cutter clears the pocket in spiral or zigzag passes with automatic depth stepping. Optional finishing pass with G41/G42 compensation.
Circular Pocket
Enter diameter and depth. The cutter enters with a helical ramp and clears the pocket in concentric rings.
Contour Milling
External or internal profile milling of rectangular or circular shapes. G41/G42 cutter diameter compensation with arc lead-in/lead-out to protect the surface finish.
Face Milling
Surface facing with zigzag passes. Enter the area dimensions and depth of cut.
Slot Milling
Straight or arc slot milling. The app automatically detects single-pass, medium, or wide slot from the slot width and tool diameter, and generates the appropriate toolpath. Ramp entry.
Thread Milling
Internal or external thread milling with helical interpolation (G02/G03 + Z). Thread pitch auto-fills from the thread table (e.g. M10 → 1.5mm). For single-point or multi-flute cutters. One tool can cut multiple thread sizes.
Peck Drilling
G83 peck drilling cycle: the drill retracts at each peck depth for chip removal. Configurable peck depth (Q) and safety height. Single, linear, grid, or manual hole positions.
Tapping
G84 rigid tapping. Feed rate is calculated automatically: F = RPM × pitch. Thread pitch auto-fills from the thread table.
Chamfer
Hole edge chamfering with a countersink mill. Enter hole diameter and countersink diameter: the app calculates chamfer width and depth. The cutter follows a G02/G03 circular path.
Hole Pattern
Circular or linear hole pattern with G81 drilling cycle. Enter center, radius, number of holes and start angle for circular, or start point, spacing and count for linear.
Material Database
170+ materials in 11 categories (aluminum, steel, stainless, copper, plastic, etc.) with automatic cutting speed and feed-per-tooth calculation. 3 tool materials: HSS, carbide, insert, each with different multipliers.
Calculators
Available in the Calc menu. Each calculator is standalone: enter the known values, the app computes the rest.
Speed & Feed
Enter cutting speed (Vc) and tool diameter → RPM. Enter RPM, flutes and feed-per-tooth (fz) → feed rate (F). Results can be transferred to the Generator with one tap.
Triangle Solver
Right triangle: enter any 2 sides or 1 side + 1 angle, and the app solves the rest. Useful for angle setups and dimension calculations.
Unit Conversions
Metric ↔ imperial: length (mm↔inch), area, volume.
Milling Calculator
Material removal rate (MRR), required machine power (kW), machining time, chip thinning correction, and ball-end mill cusp height based on stepover.
Drilling Calculator
Drill RPM and feed rate from Vc, drilling time, drill point length (from point angle), tap drill size calculation (major diameter + pitch + thread percentage).
Material Weight
Select a shape (box, cylinder, tube, sphere), enter dimensions and material (11 built-in + custom density) → volume and weight.
3D Import
Access via the "3D Import" card on the Home screen. A 4-step wizard guides you: file → 3D preview → machining parameters → toolpath result.
Supported Formats
STL (binary and ASCII), OBJ (Wavefront), 3MF. For photo-based relief see the Photo Relief card on the Home screen.
Stock Dimensions (Blank Size)
The raw material block size the model is carved from. Typical case: an aluminium or wood billet you want to mill a 3D model out of. Three modes:
(1) Model bounding box: block matches the model bounding box exactly (no extra material around the model). This is the default.
(2) Bbox + offset: adds an extra layer of material around the model. EXAMPLE: model 80×80×16 mm, XY offset = 1 mm, Z top = 3 mm, Z bottom = 0 mm → block becomes 82×82×19 mm (80 + 1 left + 1 right = 82, height 16 + 3 = 19).
(3) Absolute size: directly enter block X/Y/Z in mm. The model is centered in XY.
In the generated G-code Z=0 maps to the TOP of the block, and X0/Y0 to the BLOCK CORNER (or block CENTER with the CENTER reference). You can probe the zero point on the actual block held in the vise, no need to find the model corner/top under the block.
The 3D preview shows an amber wireframe around the block. If the block is smaller than the model in any axis the Generate button is disabled (red error).
All four roughing strategies can clear the material around the model: Parallel XY (raster) and Trochoidal sweep the full area with a zig-zag pattern. Waterline traces only the perimeter. Contour Offset walks concentric rings: it now treats the model as an island and safely removes the side stock as well.
6 Machining Strategies
Waterline: horizontal slicing, ideal for steep walls. Parallel XY: zigzag raster, ideal for flat surfaces. Contour offset: concentric rings inward. Trochoidal: semicircular looping path, lower tool load for hard materials. Surface following: 3-axis ball-end mill surface tracking (X/Y/Z simultaneous), best surface quality. 4 directions: along X, along Y, spiral, scallop. Steep/Shallow: automatically uses waterline for steep areas and surface following for flat areas.
Multi-Tool Support
Chain up to 5 tools: T1 roughing → T2 finishing → T3–T5 extra passes. Each has separate tool, strategy and parameters. Automatic M06 tool change insertion.
Rest Machining
When enabled, the T2 finishing tool only cuts where the larger T1 couldn't reach (corners, narrow areas, concave surfaces). Reduces machining time.
Pencil Milling
Extra finishing pass along concave edges (fillets, inside corners) where the ball-end mill couldn't fully reach.
Plunge Type
Vertical (straight down), ramp (diagonal entry), or helical (spiral entry).
Machining Direction
6 directions: top, bottom, front, back, left, right. The app automatically rotates the model to machine from the selected direction.
Machining Boundary
Set an X/Y region: only the selected area will be machined.
Linking
Z-level transition optimization between contours. Direct: full retract to safe Z. Skim: low retract above highest Z. Ramp: simultaneous G01 X/Y/Z to next contour. Reduces non-cutting time.
Adaptive Feed
Reduces feed rate at sharp direction changes (corners) on waterline contours. Configurable minimum feed percentage. Prevents tool deflection and improves surface finish.
Arc Fitting
Detects circular arcs in waterline contours and outputs G02/G03 instead of many G01 segments. Smaller G-code, smoother machine motion. Tolerance configurable.
Lead-in / Lead-out
Tangential semicircular entry/exit on waterline contour passes: perpendicular offset from the first segment. Prevents witness marks on the workpiece surface.
Undercut Warning
After loading the model, a dialog warns if the geometry contains undercuts (downward-facing surfaces unreachable from above). Suggests machining from multiple directions if needed.
Stock Simulation
3D material removal visualization: green (finished), yellow (partial), red (untouched). The cutter moves smoothly along the toolpath (lerp interpolation between keyframes). The M button overlays the model wireframe on the toolpath for comparison. The 3D button in the top-right corner of the preview switches between 2D and 3D view.
Save Project
On the Result screen, tap the Save icon (top right). Enter a name: the project is saved to the Home screen under "Saved Projects". All parameters and the imported file are stored. Loading a saved project restores everything so you can edit and regenerate.
Sketch 3D Extrude
Open it via the "Sketch 3D Extrude" card on the Home screen. You draw a 2D design, the app raises every shape and text from a base plate into a 3D model and hands it to the 3D machining flow. Typical uses: name plates, door signs, badges and simple raised parts. The simulation quality does not reflect the real quality; it is like this only because of the mobile-optimized operation.
Workpiece and zero point
On opening, enter the plate width and depth. Choose the zero point: Corner puts X0 Y0 at the bottom left corner, Center puts it in the middle of the plate. The last used size is filled in automatically. Tap the size chip at the top to change the workpiece or the zero point later, the drawing keeps its position on the plate.
Drawing
Pick a tool from the palette (rectangle, circle, text, hole patterns) and the element is placed at the canvas center. Tap an element to select it, edit its exact values in the bottom panel, or drag it to move it. The "+ 4 corner holes" button adds mounting holes in one tap. Undo and Redo live in the top bar, the grid button toggles snapping. After placing and adjusting each element, it is best to save with the small orange save icon on the panel.
Handling the view and elements
On the canvas, pinch with two fingers to zoom in and out, and drag with two fingers to pan the view. A single tap selects an element; tapping an empty spot clears the selection. You can drag a selected element into place with one finger, and the X and Y coordinates show next to your finger while you drag. The exact sizes and values of the selected element are set in the panel that opens at the bottom, where you can also duplicate or delete it. When you change the workpiece size, the view fits to the plate automatically.
Base plate and height
Base plate is the solid bottom thickness; Height is how far the shapes rise above it; the finished part is the sum of the two. Hole depth is measured from Z0, the top of the part. 0 cuts a through hole; a value larger than the total thickness over-drills past the bottom so the hole breaks out cleanly.
3D Extrude and machining
Tap "3D Extrude" to build the model (Cancel stops it). It opens in a slim machining screen where you set the roughing tool, speeds and an optional finishing tool. The background is cleared and the drawn shapes and text stay raised. Holes are made by a SEPARATE step after the surface: a simple straight peck drill at each hole, so mount a drill bit the size of the hole. Hole depth is measured from Z0 (the top of the part); 0 means a through hole.
Suggested starting settings
By default the app sets up a two-tool scheme for raised 2.5D text and shapes, a good starting point for most jobs. T1 is the rougher: a FLAT end mill with the Parallel (raster) strategy, it clears the background and cuts the flat floor to its final depth, leaving only a thin collar of stock on the letter walls. T2 is the finisher: a FLAT end mill with the wall-profile (Island Profile) strategy, it traces every letter wall top to bottom for a clean, sharp result, walls only, since T1 already finished the floor. Both are flat end mills (not ball nose), because the letters have flat tops and straight vertical walls. The roughing only goes as deep as the relief (how far the shapes rise above the base plate), so the base plate always stays intact, and the tool may overhang the outer plate edge by a tool radius so the edge comes out clean. The finishing tool is the biggest factor in wall quality: it must be small enough to fit between the letter strokes, or those walls (and the floor in very tight gaps) stay rough. A smaller tool (a V-bit for fine or script fonts) gives smoother, sharper walls. The demo starts with a 4 mm rougher and a 1 mm finisher; for a first try just generate with the presets, then adjust everything to your machine and material.
Saving
On the machining screen the Save action stores the whole project and also saves the drawing as an editable template under the same name. Two cards appear in the Saved Projects list: the project reopens into the machining view with model, parameters and G-code, the drawing reopens into this editor so the design can be changed later. The bookmark icon in the top bar saves the drawing alone, and leaving with unsaved changes also offers saving.
Photo Relief
Access via the "Photo Relief" card on the Home screen. Pick a photo (JPG/PNG/BMP/WebP) and the app converts it into a grayscale heightmap relief mesh, then generates the toolpath. Best for portraits, logos and decorative panels.
Supported Images
JPG, PNG, BMP, WebP. Grayscale conversion is automatic: lighter pixels become higher relief (or inverted on demand). High-contrast photos with clean backgrounds give the best result.
Relief Parameters
Width: physical X size on the stock (mm/inch). Depth: total relief height (Z). Base: flat material layer left below the relief. Resolution: grid sampling density (higher = sharper detail, longer machining). Invert: flip so darker pixels become higher.
Recommended Strategy
Surface Following with a ball-end mill gives the smoothest result. Steep/Shallow is a good automatic choice for mixed terrain. Multi-tool: T1 roughing → T2 finishing ball-end usually halves machining time without losing detail.
Preview & Simulation
Use the 3D preview to verify the relief direction and depth before generation. After generation the toolpath simulation shows the rapid + cutting moves, with the same stock-collision checks as the 3D Import flow.
Save Result
Tap the Save icon (top right) on the Preview screen. Enter a name: the project is saved to the Home screen under Saved Projects. Loading it restores the image, parameters and G-code.
DXF/SVG Import
Access via the "DXF Import" card on the Home screen. 4-step wizard: file → preview → parameters → result. Opening a DXF/SVG file from the phone's file manager also launches the app.
Engrave
The cutter follows the drawing lines at a fixed depth. For text, logos, and decorations.
External Profile
Milling the outside of closed contours with G41/G42 compensation.
Internal Profile
Milling the inside of closed contours.
Hold-down tabs
Available in the profile modes, below the lead in and lead out settings. The app leaves small bridges at the bottom of the cut so the finished piece stays attached and cannot break loose or fly off before the program ends. Set the tab count, height and length, the tabs are spaced evenly along the contour, also on arc segments. After machining, snap the tabs off with a knife or chisel and sand the spots smooth.
Text Engraving
Type text and engrave it using 10 single-line CNC fonts (Hershey). Supports accented characters (á, ö, ű, ß, ñ, etc.).
Supported DXF Elements
Line, circle, arc, polyline (with arc segments), point, spline, ellipse, block reference (INSERT with scaling and rotation).
Supported SVG Elements
Line, circle, ellipse, rectangle (with rounded corners), polygon, polyline, path (Bézier curves, arcs), groups with nested transforms.
Save Project
On the Result screen, tap the Save icon (top right). Enter a name: the project is saved to the Home screen under "Saved Projects". All parameters and the imported file are stored. Loading a saved project restores everything so you can edit and regenerate.
Photo → Engrave
Vectorize a photo or scan into engrave-ready contours. Pick from gallery or shoot directly with the camera; the engine runs Potrace-quality tracing on-device: no upload. Supports JPG / PNG / WebP up to 2048 px (HEIC on Android 9+).
Presets & sliders
Four one-tap presets: Logo / Handwriting / Drawing / Silhouette. For finer control: threshold (Otsu / manual / adaptive), denoise, min spot size (turdsize), smoothness (alphaMax). Invert + 90°/180°/270° rotation buttons.
Tips for best results
Use high-contrast black-and-white sources for cleanest output. If a low-contrast warning appears, try adaptive threshold. If too many tiny paths appear, raise Min spot size. Tap Save as DXF or Open in DXF Import to continue to G-code.
What to use it for
Signs, name plates, logos, silhouettes, a child's drawing or a handwritten signature carved into wood, MDF, acrylic, plastic or aluminium with a CNC router. In DXF Import you then pick engrave (along the line) or a profile cut (outside / inside the outline).
Output mode switch at the top of the panel:
• Outline: traces the shape's contour. For thin strokes BOTH edges are drawn, so a V-bit gives the classic tapered sign look. Best for logos, signs and silhouettes.
• Centerline: traces the shape's medial axis (one stroke = one path). Best for handwritten signatures, thin-line drawings and single-line fonts with a V-bit, so the engraved line follows the centre of the stroke instead of doubling each edge.
In Centerline mode the Min spot size (turdsize) and Smoothness (alphaMax) sliders are hidden: they're Outline-specific. The Output mode is preserved when you switch presets.
**Target size (mm)**: final physical size of the cut on the CNC. The image scales proportionally. Default 200 mm. Two editable fields below the slider (Width, Height): type either one directly, decimals accepted. The lock icon keeps the aspect ratio; open it to edit W and H independently and stretch the image (e.g. to fit a 100×50 mm blank). The slider always drives the field you last tapped.
Sketch Editor
Parametric drawing editor for quick programming of simple parts: draw rectangles, circles, slots, holes, text, and the app automatically generates G-code for all elements combined. No DXF or CAD drawing needed, directly on your phone. 3-step workflow: drawing → parameters → result.
Controls
Select an element type from the left toolbar: it is placed at the canvas center on tap. Enter exact dimensions in the right panel. Tap to select, drag to move elements. Pinch to zoom and pan the canvas. Each element has its own machining mode (pocket, profile, engrave, drill) and depth setting. While editing, it is recommended to save after each operation using the Save icon. On exit, the app offers to save your drawing: saved sketches appear on the Home screen and can be reloaded and edited anytime.
8 Element Types
Rectangle: pocket, profile or engrave. Width, height, corner radius. Circle: pocket, profile or engrave. Center and radius. Slot: straight slot. Length, width, angle. Line: engrave or profile. Start and end point. Arc: engrave or profile. Center, radius, start/end angle. Circular hole pattern: evenly spaced holes on a circle. Linear hole pattern: evenly spaced holes on a line. Text: engrave with 10 fonts. Each element has its own depth and machining mode.
Drawing Functions
Workpiece: set workpiece size and origin (corner/center), shown as dashed white rectangle. Copy: duplicate selected element with +10mm offset. Grid snap: 10mm (metric) or 0.5" (imperial). Templates: save and reload drawings from the database. Undo/Redo for editing steps.
SmartCAM
Automatically optimizes machining order (drilling last, shallow to deep), warns about tool changes, and alerts when tool radius is too large for a corner.
Island Machining
When you place an element inside a pocket (e.g. a circle inside a rectangular pocket), the app treats it as an island: the material around the island is left intact during pocket clearing.
Result
3D toolpath preview with all elements combined. Selected element shown in orange, others colored by machining mode (pocket=green, external profile=cyan, internal profile=purple, engrave=yellow, drill=red).
Machine Transfer
Open it with the "Transfer" card on the Home screen, or with the Send to Machine button next to a finished G-code. 4 connection modes, each on a separate tab.
Keep the app open while sending
The program goes to the machine continuously while sending (on GRBL machines until the job ends). If you close the app, lock the phone or switch to another app, sending and the job can stop. The display stays on while sending, and Back asks before stopping.
RS-232 (USB)
Connect a USB-to-serial adapter to your phone. Select baud rate, parity, and flow control (none / XON-XOFF / RTS-CTS). Character-by-character transmission (GRBL machines: line by line). 7 preset profiles (Fanuc, Haas, etc.) with common settings. Any USB-serial adapter that uses an FTDI, CP210x, CH340/CH341, PL2303 or CDC/ACM chip works; the phone must support USB-OTG. Search term: "USB to RS232 DB9 FTDI/CH340 adapter" — any such or similar cable with one of these chips works. Available from a few euros.
USB tips
Turn on OTG in the phone settings – some phones turn it off by themselves after a few minutes. Use a data cable (a charge-only cable carries no data), and make sure the machine is switched on.
Bluetooth
Pair the machine in phone Bluetooth settings, then select it in the app. The app uses classic Bluetooth SPP. If your machine has no Bluetooth: on a machine with a serial/RS232 port, an SPP Bluetooth-serial adapter (search term: "RS232 Bluetooth SPP adapter DB9"); on a hobby GRBL controller (TTL serial pins), a few-euro HC-05/HC-06 module makes the transfer wireless. Any such or similar device that supports SPP works.
WiFi TCP
Enter the machine's IP address and port. Direct socket connection to network-enabled controllers.
WiFi tips
You find the IP address on the machine display, in the controller WiFi settings or in the router device list. The port is usually 23 (MKS DLC32: 8080). The phone and the machine must be on the same network – a guest network does not work, it isolates devices. If the connection drops while mobile data is on, turn off mobile data. Give the machine a fixed IP in the router so it does not change. On some brands the WiFi works only with their own app – use USB then.
WiFi FTP
Enter the machine's IP address, username, password and target folder. The app uploads the program as an .nc file via FTP.
GRBL machines
The app recognises GRBL controllers (hobby CNCs, e.g. 3018) when the profile has "GRBL" in its name, or (USB only) is set to 115200 or 57600 baud without flow control. It then sends line by line: after each line it waits for the machine to answer. If the machine goes into ALARM (e.g. limit switch), sending stops – check the machine, then tap Unlock ($X). If the app goes to the background while a program is sent from the Transfer screen (a call, the Home button, screen lock, another app), the machine is paused at once. When you come back, Resume continues the job from the same place, Abort stops it.
Auto-Detect
The app attempts to identify the controller type (11 types: Fanuc, Haas, Siemens, GRBL, Mach3, Okuma, Mitsubishi, LinuxCNC, Marlin, Smoothieware, FluidNC) and automatically suggests settings.
Machine Profiles
Save connection settings per machine for quick reconnection. On the Home screen, the "Last Transfer" card repeats the last successful transfer with one tap.
Reference Tables
Available in the Ref menu. All tables are searchable with the search field.
G-Code Table
49 G-codes in 6 categories: motion (G00–G03, G28), mode (G17–G21, G90/G91), coordinate (G54–G59), compensation (G40–G43), canned cycles (G73–G89), other. Each code has description and example.
M-Code Table
17 M-codes: spindle (M03–M05), coolant (M07–M09), tool change (M06), program (M00, M01, M02, M30, M98, M99).
Drill Table
Metric and imperial standard drill sizes with matching tap drill pairing.
Thread Table
4 standards: Metric coarse (M2–M48, 33 sizes), UNC (27 sizes), UNF (27 sizes), NPT (10 sizes). Each thread: designation, pitch, major/minor diameter, tap drill size.
ISO Tolerance Table
Shaft (f7, g6, h6, js6, k6, m6, n6, p6, s7) and hole (H6, H7, H8, H9, H11) tolerances for 1–400mm range. Fit calculator: enter nominal diameter and fit → min/max diameter and tolerance band.
ISO 2768 General Tolerances
Free-size tolerances (for dimensions without individual tolerance). Linear (f/m/c/v classes), chamfer, angular (deg+min), plus ISO 2768-2 geometric (H/K/L: flatness, perpendicularity, symmetry, run-out). Quick lookup by size.
Bolt Head Sizes
DIN 912 (socket head), DIN 7991 (countersunk), DIN 933 (hex head) screws M3–M20: head diameter, height, hex/wrench size, recommended hole and counterbore diameters. Quick lookup by size.
GD&T Symbols
14 ISO 1101 geometric tolerance symbols (straightness, flatness, perpendicularity, position, runout, etc.) grouped into 5 categories: form, profile, orientation, location, runout. Each row shows the drawing symbol and a short definition.
Material Database
170+ materials in 11 categories with cutting speed (Vc) and feed-per-tooth (fz). Searchable by name and category. Selecting a material applies it directly in the Generator.
Tool Library
Save Tool
In the Generator, DXF Import, 3D Import or Sketch Editor, tap the save icon to store the current tool with a name.
Load Tool
Tap the load icon to choose from saved tools. Diameter, flutes, type and tool number load automatically. If a material was selected, RPM/feed recalculates.
Stored Data
Name, type (end mill, ball end, drill, tap, V-bit, thread mill, chamfer mill), diameter, flutes, tool number (T).
General
Unit System
Switch between mm and inch in the Set menu. The entire app (generators, calculators, imports) works in the current unit. G-code automatically gets a G21 (mm) or G20 (inch) header.
Warning: previously entered values are not auto-converted when you switch units. After switching to inch, re-check every numeric field.
Program Save
Any generated G-code can be saved to the app database. On the Home screen, the "Recent Programs" section shows recent programs: tap to load, delete or share.
Export Options
Copy to clipboard, save .nc file, share with other apps, generate QR code, PDF workshop sheet, DXF export.
Save size limit
On phone, saved programs are limited to about 2 MB. Very complex 3D parts may exceed this. In such cases the app warns and skips the save. You can still send the G-code directly to the machine (without saving).
Related: FAQ, supported controllers.