Nestpact Documentation

Nestpact is a DXF nesting optimization tool for CNC cutting. It takes your part outlines and material sheets, computes the most efficient layout, and gives you a ready-to-cut DXF or G-code file. It also accepts STL, OBJ, PLY, and 3MF files, extracting the 2D silhouette automatically before nesting.

Building an integration? See the Developer API for the REST endpoints, authentication, and code examples.

Workflow

Every job follows four stages.

File Support

DXF, DWG & SVG parts and sheets

DXF files are parsed using ezdxf. Supported entities include LINE, LWPOLYLINE, POLYLINE, CIRCLE, ARC, SPLINE, ELLIPSE, and INSERT (block references). The parser runs in two modes:

• Material mode (merge_holes=True): all geometry on the sheet is merged into a single boundary polygon.
• Parts mode (merge_holes=False): holes (interior rings) are preserved so the nesting engine can perform hole-filling.

DWG and SVG files are accepted too: they are converted to DXF on upload (SVG via svgelements, with every transform flattened so files from Illustrator, Inkscape and Figma come in clean) and then follow the same parsing path.

3D files: STL, OBJ, PLY, 3MF

3D files go through a silhouette extraction pipeline before reaching the nesting engine:

1. The mesh is loaded with trimesh.
2. The largest planar facet group is found using a graph-based facet detection algorithm (requires networkx). If the graph engine is unavailable, the oriented bounding box shortest axis is used as a fallback.
3. That face is reoriented to face +Z, and every triangle is projected onto the XY plane.
4. The projected triangles are unioned with Shapely to produce a single silhouette polygon.
5. The silhouette is handed to the nesting engine exactly like any DXF part.

Libraries & Presets

Signed-in users get reusable libraries, so a sheet, a part, or a set of settings only has to be prepared once. Using a library item never consumes the original: it is copied into the job, so the saved version stays intact for the next time you need it.

Sheet library

Save any material sheet (an uploaded DXF outline or a manual size) as a named plate you can reload from the sheet picker. Banked offcuts appear in the same picker, so remnants and full sheets live side by side.

Offcuts

After a nest, save the unused area of the sheet as an offcut. It becomes an irregular reusable sheet in your library, so a later job can be nested onto the remnant instead of a fresh plate. This closes the loop on material waste.

Part library

Save frequently cut parts (each with a cached thumbnail) and drop them into any job from the part picker. Every use copies the part into the job, so quantities and edits never touch the saved original.

BOM import

Import a bill of materials to add many parts at once with their quantities, instead of adding each part by hand.

Nesting presets

Save a full set of nesting settings (gap, rotation, optimization level, G-code options, and so on) as a named preset, then apply it to future jobs in one click. Presets are stored per account and follow you across devices.

Nesting Engine

The nesting engine combines multiple placement and optimization algorithms with true-shape collision detection. The settings below are exposed in the Configure step of the wizard.

Optimization level

Controls how hard the engine searches for a better layout. Higher levels try more sorting strategies and rotation angles, which improves material utilization but takes longer to run. For most production jobs, Thorough is a good starting point. For concave or interlocking parts, Interlock and Extreme use true No-Fit-Polygon nesting (NFP) to fit parts against each other's real outlines and pack them noticeably tighter.

Rotation mode

Determines which orientations the engine is allowed to try for each part. Allowing more rotations gives the engine more placement candidates, which often improves utilization, but increases run time proportionally. If your parts are grain-sensitive (wood, fabric, rolled metal) you may want to restrict this to none or 90.

Gap (minimum stock between parts)

When the Tool diameter setting is 0 (laser, plasma, waterjet), Gap is the raw outline-to-outline distance the engine maintains between adjacent parts. Set it to at least your kerf width so parts do not end up undersized after the beam or saw eats into the gap.

When Tool diameter is set (CNC router), Gap becomes the minimum material web that physically remains between two finished parts after cutting. The engine places outlines at Gap + Tool diameter apart so that the two cutter paths — each removing material out to half the bit's diameter — leave exactly Gap mm of untouched stock between them. Set Gap to 0 if you only need the bits to not overlap, or raise it for a wider land.

Tool diameter (CNC router)

The diameter of the router bit. Leave at 0 for laser, plasma, and waterjet machines — those use the Gap setting directly. When set, the nesting engine automatically adds this value to Gap when calculating how far apart to space part outlines, so Gap retains its physical meaning (stock remaining between parts) regardless of bit size. Example: a 6 mm end mill with Gap = 3 mm causes outlines to be placed 9 mm apart; after cutting, 3 mm of material is left between the two parts.

Edge offset

The minimum distance between any part and the edge of the sheet. Useful when your material has a clamping zone or a burned border that you do not want to cut into. Setting this to 0 allows parts to be placed flush against the sheet boundary.

Sorting strategy

Controls the order in which the engine places parts. The chosen strategy is one of the variables the optimization level iterates over — at higher levels all strategies are tried and the best result wins.

Hole-filling

When enabled, the engine attempts to nest smaller parts inside the holes of larger parts (for example, placing a small disc inside the circular cutout of a larger bracket). This recovers material that would otherwise be scrapped. Disable it if you need the holes to remain empty for downstream assembly reasons, or if the extra computation time is not worth it on simple flat parts with no holes.

Multi-sheet overflow

If not all parts fit on the first sheet, the engine automatically starts a second sheet and continues placing until every part in the job has been accommodated. Each sheet is downloaded as a separate DXF layer or file. You cannot disable this — if you want a single-sheet result, reduce the quantity or choose a larger sheet size.

Fill-remaining

After all unique parts have been placed once (satisfying the requested quantities), any leftover sheet area is filled with additional copies of the parts in round-robin order. This is useful when you want to cut as many parts as possible from a single sheet without specifying an exact quantity up front. Disable it if you want an exact count and do not want extras.

Post-placement compaction

After the initial placement pass, the engine runs a second sweep that nudges each placed part toward the bottom-left origin, closing any gaps that appeared because earlier placements blocked the ideal position. Compaction does not change which parts are placed — only tightens their final positions. It is always on and cannot be disabled from the UI.

Manual Editing

The layout the optimizer produces is a starting point, not a lock. Every placement can be adjusted by hand on the canvas before you export.

Moving parts

Drag any placed part to reposition it, rotate it, or duplicate it. Collision feedback warns you in real time if a move would overlap another part or run off the sheet, so a hand-tuned layout stays cuttable.

No-cut zones

Mark damaged or unusable areas so the engine avoids them. Draw a rectangle, circle, or polygon, or use the freehand scribble tool to trace an irregular defect. No-cut zones are subtracted from the usable sheet area before nesting, exactly like a hole in the material.

Measure tool

A ruler mode on the canvas toolbar measures any distance in your active unit (mm or inches), handy for checking a clearance or a specific dimension against the drawing.

Mobile photo background (QR pairing)

To trace real defects, pair your phone by scanning a QR code, photograph the actual sheet, and the picture drops onto the PC canvas as a background layer. Calibrate the scale by entering one known width, then draw no-cut zones directly over the flaws visible in the photo. The overlay opacity and visibility are adjustable.

Keyboard shortcuts

• Space and drag to pan; scroll to zoom (anchored to the cursor).
• Ctrl + Z and Ctrl + Y to undo and redo.
• Delete to remove the selected part or no-cut zone.

G-code Generation

After a nesting job completes, the placement coordinates are fed to the G-code generator. The output is a Fanuc-flavoured dialect (G21/G20, G90, G17, G94) accepted by most Fanuc-compatible controllers (LinuxCNC, GRBL, Mach3, Fanuc). Dedicated post-processor profiles are also available for Heidenhain and WoodWOP.

Output structure

Every generated program follows this structure:

1. Header comments (job ID, units, part count, bounding box, tool number).
2. Setup codes: unit system, absolute positioning, XY plane, feed-per-minute.
3. Work offset declaration (G54–G59 or G92).
4. Tool select and change (T# M06), optional tool length offset (G43 H#).
5. For each part: rapid to entry point, spindle/beam on (M03), cut the profile, spindle/beam off (M05).
6. Footer: cancel canned cycles (G80), return to origin, M30 program end and rewind.

Cut operations per DXF layer

Each DXF layer in the part file can be assigned a different operation:

Arc fitting (G02 / G03)

The DXF parser converts all curves (circles, arcs, splines, ellipses) into polygon approximations because Shapely needs polygons for collision detection. The G-code generator recovers the original arcs by fitting consecutive co-circular points back into G02 (clockwise) and G03 (counter-clockwise) arc commands with IJK centre offsets.

This matters for cut quality: a controller running constant feed through a G02/G03 arc produces a smoother edge than decelerating at every chord vertex of a polygon approximation. Arc fitting can be disabled for controllers that only understand G01.

Router mode (Z axis)

By default the generator produces 2D output with no Z column, suitable for laser, plasma, and waterjet machines. Router mode is activated when a cut depth is supplied.

Lead-in / lead-out

A lead-in is a short approach move that brings the beam onto the profile away from the finished edge, so the pierce mark (which is rougher than the cut itself) lands in scrap rather than on the part. A lead-out does the same on exit. Both can be a straight line or a tangent arc, with a configurable length, and are applied only to profile rings (never to drilled or centerline operations).

Bridge tabs

Tabs are small uncut bridges that keep parts from dropping out of the sheet mid-cut. They are only applied to the outer profile cut of each part (never to holes or extra features). On the final stepdown pass the generator lifts to Safe Z across each tab location, rapids over it, then plunges back to Cut Z to continue the profile.

Tab placement follows three rules:

• Even spacing: tabs are distributed evenly around the perimeter at (i + 0.5) × perimeter / n so the first tab does not land on the pierce point.
• Corner avoidance: if an ideal position straddles a sharp corner, the tab is nudged to the nearest long segment where material exists on both sides.
• Hole proximity avoidance: tabs are kept at least 2× tab width away from interior hole edges to prevent thin slivers that snap during part removal.

Multi-tool jobs

When different DXF layers are assigned to different tool numbers, the generator emits a tool change sequence (M05 → T# M06 → optional G43 H#) automatically between rings that require different tools. The work offset is re-asserted after each change so the controller's modal state does not drift.

Work offsets

Spindle RPM

When a spindle RPM is supplied, every M03 command is augmented to M03 S#### so the controller starts the spindle at a defined speed. Without an S word, some controllers leave the spindle at its last-used speed, which can be zero. Leave this blank for laser, plasma, and waterjet machines.

Cycle time estimate

The generator returns metadata alongside the G-code text, including a rough cycle time estimate computed from total cut distance, total rapid distance, cut feed rate, and rapid feed rate. It also reports pierce count, arc count, bounding box utilization, and shortest/longest individual cut loop.

Results & Sharing

Shareable links

Turn any finished layout into a public, read-only link to send to a colleague or customer. The link shows the layout geometry only (no downloadable DXF or G-code bytes), and a watermark and expiry are applied based on your plan at the time the link is created.

Costing & quotes

Optional and off by default. When enabled in Settings, the results panel breaks down material, scrap, machine, and markup costs, plus a landed cost per part. It is a purely informational overlay: the nesting itself never depends on it.

Printable report

Generate a clean shop-floor report (print, or save as PDF) with a map of the nested sheet, numbered parts, and the key job stats. When costing is enabled, the cost breakdown is included.

Savings dashboard

Your history view summarizes how many sheets and parts you have nested and at what average utilization, for the current month and all-time, with an estimate of the material saved against a baseline. When costing prices are set, the dollar figure is shown alongside.

Re-run and email

Re-run any past job with the same or tweaked settings in one click (the parts and sheet are rebuilt from the stored job, with no re-upload needed), or email a finished result to yourself.

DXF Health Checker

The Health Checker analyzes a DXF file before nesting and reports issues that would cause a bad nest or a bad cut. It can also apply automatic fixes.

What it checks

• Unclosed polylines (open contours that do not form a valid polygon).
• Duplicate or near-duplicate geometry.
• Zero-length segments.
• Self-intersecting contours.
• Entities on layers that the nesting engine may not handle as expected.

Auto-fix

The fix endpoint attempts to close open polylines, remove duplicate entities, and simplify near-collinear points. The repaired DXF is returned as a downloadable file.