Our quoting software reads your drawing file directly — it measures cut lengths, detects bend lines, counts holes and checks part dimensions automatically. When a file is set up correctly, this takes seconds and your quote is ready immediately.
When a file isn't set up correctly, our system either flags it for manual review (which adds a day) or rejects it entirely. This guide covers every rule our software checks, along with the most common mistakes we see and exactly how to fix them.
Whether you're a seasoned CAD draughtsman or you drew your part in a free DXF editor last night, this guide applies to you.
DXF is our first-choice format. It is universally supported by every 2D CAD package (AutoCAD, LibreCAD, Fusion 360, SolidWorks, Inkscape, etc.) and is natively understood by laser cutting machines.
Export as DXF R12 or DXF R14 (AutoCAD 2000). Avoid DXF 2010+ if you're on older software — some entities like HATCH and MLEADER are not required for flat patterns and can confuse parsers.
If your part has bends and you are working in a 3D CAD package (Fusion 360, SolidWorks, CATIA, Inventor), export the flat pattern as a STEP or STP file. Our software will unfold it and read the sheet body automatically.
Do not send the folded/3D body — we need the flat pattern. Most 3D CAD tools have a "Flat Pattern" or "Unfold" command that will generate this for you.
If you designed your part in a drawing or illustration tool (Inkscape, Illustrator, CorelDRAW), export as DXF. If you modelled it in a 3D parametric CAD tool, export the flat pattern as STEP. When in doubt, DXF is the safest choice.
All dimensions in your DXF file must be in millimetres (mm). Our system assumes 1 drawing unit = 1 mm. A 200 mm × 100 mm plate must be exactly 200 × 100 units in the file.
- AutoCAD / DraftSight:
UNITScommand → set to Decimal, Millimeters - Fusion 360: Document settings → Units → mm
- SolidWorks: Tools → Options → Document Properties → Units → MMGS
- Inkscape: File → Document Properties → Display Units → mm, then export DXF at scale 1.0
Never scale your drawing before exporting. The geometry in the DXF file must match the real-world part size exactly. If your CAD tool asks for a scale factor during DXF export, leave it at 1.0.
If you received a DXF from a client that looks too small or too large in your viewer, measure a known dimension before uploading — do not just scale it to look right.
| Scenario | File unit | Result |
|---|---|---|
| Correct | 1 unit = 1 mm (millimetres) | ✓ Quotes correctly |
| Drawn in inches, not converted | 1 unit = 25.4 mm | ✗ Quoted ~25× too large |
| Exported at scale 0.001 (metres) | 1 unit = 0.001 mm | ✗ Part reads as microscopic |
| Scaled to fit on A4 in drawing | 1 unit ≠ 1 mm | ✗ Wrong dimensions, wrong price |
Place your part's outer silhouette on a layer named PROFILE (or CUT or 0). This must be a single, fully closed polyline or spline. Every corner must be connected — no gaps.
Think of the profile as the shape of the flat metal blank before any folding happens. It represents exactly where the laser will cut the outside edge.
Place any internal holes, slots, cutouts or pockets on a layer named HOLES (or CUTOUT). Each cutout must also be a fully closed contour. The laser uses this layer to cut everything inside the profile.
Do not mix holes with the profile layer — our system treats each layer independently when measuring cut length and quoting.
If your part has bends, add each fold line as an open line or polyline on a layer named BENDS (or BEND or FOLD). Bend lines must run fully across the width of the part at the fold location.
The number of lines on this layer directly determines the number of press brake operations in your quote.
Our parser accepts profile, PROFILE, Profile — all the same. It also recognises common aliases: cut, outline, outer for profiles; hole, cutout, punch for holes; bend, fold, crease for bend lines. Anything else is ignored and treated as annotation.
A profile drawn as 12 separate LINE entities that happen to touch end-to-end is not the same as a single closed LWPOLYLINE. Always join or "pedit" your segments into a single contiguous polyline before exporting.
- AutoCAD:
PEDIT→ Multiple → select all → Join → Yes - Fusion 360: Modify → Join Curves
- Inkscape: Path → Combine, then ensure the path is closed
Delete any centre lines, construction geometry, title block borders, hatching, or drawing frames before exporting. These entities add unnecessary cut length to your quote — our system measures every line on a cut layer.
A tidy approach: duplicate your drawing, delete everything that isn't a cut contour or bend line, and export that clean file.
For a circular hole in a 3.0 mm sheet, the minimum diameter is 3.0 × 1.2 = 3.6 mm. Our software will flag any hole below this threshold.
The narrowest dimension of any slot or rectangular cutout must be at least equal to the sheet thickness. A 1.6 mm sheet needs slots at least 1.6 mm wide. Tighter than this causes the kerf to close and the offcut to stick.
Cutting a hole very close to the part edge can cause the thin strip of material between them to warp or tear during cutting. Keep all holes at least 2× the sheet thickness away from any edge. Our system will warn you — but it won't automatically reject the file.
| Thickness | Min round hole ⌀ | Min slot width | Min edge distance |
|---|---|---|---|
| 0.9 mm | 1.1 mm | 0.9 mm | 1.8 mm |
| 1.2 mm | 1.5 mm | 1.2 mm | 2.4 mm |
| 1.6 mm | 1.9 mm | 1.6 mm | 3.2 mm |
| 2.0 mm | 2.4 mm | 2.0 mm | 4.0 mm |
| 3.0 mm | 3.6 mm | 3.0 mm | 6.0 mm |
| 4.0 mm | 4.8 mm | 4.0 mm | 8.0 mm |
| 5.0 mm | 6.0 mm | 5.0 mm | 10.0 mm |
Every bend line must span the full width of the part at that cross-section, from edge to edge. Short tick marks or centreline dashes are not sufficient — the machine operator needs to see where the full bend runs.
Each line = one press brake operation. If you need four bends, draw four lines. Each line adds one bending charge to your quote.
A DXF is a flat drawing — it cannot communicate whether a flange bends up or down. Use the order notes field in checkout to describe your bend directions. "Bend A: 90° up, Bend B: 90° down" is sufficient. A photo of a similar part helps even more.
For complex parts with many bends, we recommend attaching a simple hand sketch or a 3D screenshot alongside the DXF.
Our press brake uses standard tooling. The default inside bend radius is approximately 1× the material thickness. You do not need to specify a bend radius in your drawing — it is fixed by the machine and tooling.
If you require a non-standard radius (tighter or looser), mention it in the order notes and we will advise on feasibility.
TEXT, MTEXT, ATTRIB, ATTDEF and LEADER entities on the PROFILE or HOLES layer are interpreted as cut geometry. This inflates your quoted cut length, slows parsing, and may cause your file to be rejected.
Move all annotations, part numbers, title blocks and dimensions to a separate layer named ANNOTATION, NOTES, or similar. Our parser will ignore anything not on a recognised cut or bend layer.
A DIMENSION entity drawn over the top of your profile adds dozens of small line segments. HATCH patterns add hundreds. Both will massively inflate your quoted cut length and may confuse the nesting software.
Move dimensions to ANNOTATION layer. Delete all hatching from the export file entirely — it serves no purpose in a cut file.
This most often happens when a drawing is copied and pasted without awareness, or when a profile is imported on top of an existing one. Two identical line segments sitting exactly on top of each other look like one — but our system counts them separately.
Use your CAD tool's "purge duplicates" or "overkill" function before exporting. In AutoCAD, the command is OVERKILL. In Fusion 360, Modify → Remove Duplicates.
Two cutout shapes that share a common edge create an ambiguous region — the laser has nowhere valid to cut. All contours must be fully independent with a small clearance (at least 2× thickness) between them. Never let one hole's boundary touch another's.
Even a gap of 0.001 mm is enough to break a profile. This often happens when lines don't quite meet at corners, especially after importing or tracing a sketch.
In AutoCAD, zoom in to every corner and verify they snap. Use PEDIT with a close tolerance to automatically bridge near-misses. Most CAD software has a "check closed" function — use it before every export.
Our parser will tell you the approximate location of any gap it finds, so you can go back and fix it quickly.
An arc that was drawn independently rather than as part of a joined polyline will be treated as a free-floating open path. Standalone arcs and splines that are not part of a closed loop are rejected. Always incorporate all arcs and curves into your LWPOLYLINE before exporting.
If your DXF contains two outer profiles (two separate closed shapes on the PROFILE layer), our parser will detect this and warn you. Only one outer boundary per file is valid.
If you have 5 different part types to order, upload 5 separate files. You can add as many files as you like to a single order in our upload tool, and set independent quantities, materials and finishes for each one.
We do the nesting on our side to maximise sheet utilisation (which keeps prices down). If you send a file with 10 copies of your part arranged on a virtual sheet, our system reads all 10 as separate profiles and will not interpret them as a quantity.
Instead: upload your single-part file and set Quantity = 10 in the order form.
AutoCAD BLOCK, INSERT and XREF entities are not raw geometry — they are references. Some DXF readers can resolve them; ours cannot guarantee it. Use the EXPLODE command on all blocks and inserts, then check the resulting geometry is clean and on the correct layers.
If your DXF was derived from a 3D model without flattening, the geometry may contain Z-coordinates (elevation). Our parser expects a flat 2D file — all Z values must be 0. Use your CAD tool's "Flatten" command or export option to strip the Z axis before sending the file.
| Parameter | Minimum | Maximum | Notes |
|---|---|---|---|
| Part width | 10 mm | 1500 mm | Sheet width limit |
| Part length | 10 mm | 3000 mm | Sheet length limit |
| Material thickness | 0.9 mm | 5.0 mm | See materials page for per-material limits |
| Bend length | — | 3200 mm | Press brake bed width |
| Bend angle | 10° | 135° | Acute bends require special tooling — request in notes |
| Part weight | — | ~50 kg | Heavier parts flagged for manual review |
| Cutting tolerance | ±0.1 mm | Fibre laser | |
| Bending tolerance | ±0.5° | CNC press brake | |
| Min hole diameter | 1.2× thickness | See table above | |
- File format: saved as .DXF or .STEP / .STP
- Units: drawing units set to millimetres
- Scale: exported at 1:1 (no scale factor applied)
- Layers: PROFILE, HOLES and BENDS layers present and named correctly
- One profile: only one closed outer boundary on the PROFILE layer
- All contours closed: no gaps in any profile or hole outline
- Segments joined: all line segments merged into continuous polylines
- No duplicates: OVERKILL or equivalent run to remove stacked lines
- No text on cut layers: all dimensions and labels moved to ANNOTATION layer
- No hatching on cut layers: all hatch objects deleted from export
- Blocks exploded: no INSERT, BLOCK or XREF entities remaining
- 2D only: all Z-values are 0 (flat geometry)
- Hole sizes: all holes ≥ 1.2× material thickness
- Edge clearance: all holes ≥ 2× thickness from nearest edge
- Part size: within 1500 × 3000 mm
- Bend directions: described in the order notes field
If you're unsure whether your drawing will pass, email it to orders@quickcut.co.za before placing your order. We'll review it within one business day and tell you exactly what (if anything) needs fixing — for free, no strings attached.