Design guidelines

We work from STEP models (.step / .stp) and DXF drawings (.dxf), both priced instantly, up to 5 MB. A DXF must be plain ASCII (a binary DXF fails to read); if one fails, re-export it as an older ASCII DXF (R12 / 2000), drawn at 1:1, as nothing checks the drawing scale. DWG, PDF, AI and EPS files are refused with a hint to export STEP or DXF.

A part larger than 5000 mm on either side is refused outright; in practice the limit is the stock sheet and the laser bed for your material (see Laser cutting).

Export the part on its own, as one solid body of even thickness, the way your CAD app’s sheet-metal tools build it: flat faces joined by round bends. We find the thickness, unfold the bends and draw the flat pattern with its bend lines; you can turn the model over in 3-D and see the flat pattern on the card. Units are read from the file (millimetres or inches).

Bends are developed with our tooling, not the radius drawn in the model: inside radius equal to the material thickness (R = T) and K-factor 0.44 (Aluminium 0.43). The outside dimensions of your model are kept: when our radius differs from the model’s, the flat faces either side give up the difference.

Countersunk holes are recognised and priced as countersinks. A model we can’t unfold automatically (formed features such as louvers, embosses or ribs, counterbores, a rolled or conical shape, more than one body) is refused with the reason; send it through Request a quote and we price it by hand.

Set the DXF’s units ($INSUNITS) to millimetres. The unit codes we read are inches (code 1), millimetres (code 4), centimetres (code 5), metres (code 6). Any other or missing unit code is read as millimetres and you get a warning, so check the size shown on the card before you add the part.

If the declared unit would make the part absurdly large (10× or more over the 5000 mm ceiling, say a mm drawing exported as metres) we re-read it in millimetres; if that reading fits, we use it and the warning quotes both sizes. A part that is merely over the ceiling in its declared unit is refused with a hint to re-export in mm.

Upload one part and set the quantity on the card. A file holding several separate outlines is priced as one part the size of everything together, and it gets no folded 3-D preview.

LINE, ARC, CIRCLE, LWPOLYLINE / POLYLINE (with arc bulges) are read exactly; ELLIPSEs from a fine sampling. SPLINEs are read from their control points and put the drawing into review (one with only fit points can only be approximated), so convert splines to arcs or polylines before export. Blocks (INSERT) are expanded, including arrays; a missing block definition also means review, and a file with more than 5,000 block instances or 20,000 pieces is refused, so explode very large arrays. TEXT, MTEXT, dimensions, hatches, points and any other entity type are ignored and named on the card, so convert text or fills to outlines if they must be cut. Layout (paper-space) objects are skipped. Circles, arcs, ellipses, polylines and blocks drawn mirrored (extruded along −Z) are read where they appear; one tilted out of the drawing plane is skipped and puts the drawing into review. A file with no cuttable shapes at all is refused.

We cut exactly the shapes in your part preview. The laser file is written from our reading of your drawing, not copied from it, so anything skipped here is not cut, and is not charged.

Keep cut geometry on ordinary layers. A layer whose name contains BEND or FOLD (or BND, CREASE, KNICK, BIEGE, BRAKE, or the whole words HEM, SCORE, FORM) holds bend lines, not cuts; a name containing VCUT or GROOVE holds V-groove marks; a layer named exactly TRIM is dropped. Names containing UNFOLD (FreeCAD’s Unfold_Sketch) are ordinary cut layers. Entities inside a block that sit on layer 0 take the layer the block is inserted on.

Nothing on these layers is cut: a hole drawn on TRIM or a V-groove layer, or a circle on a bend layer, is left out, and the card says so (straight runs on a bend layer are read as bends). Move it to an ordinary layer if it should be cut.

Every cut path must form a closed shape. Ends within 0.2 mm of each other are joined for you; a contour that still doesn’t close, or three lines meeting at one point, is flagged and the drawing goes to review. Lines drawn twice are removed; collinear lines that overlap are flagged (at 5 or more the drawing goes to review) because the laser would cut them twice.

A very dense cut (1,500 pierces per m² or more) also goes to review. When there is anything to note, the card lists it under “How we read it” (folds, ignored objects, duplicates, several parts…), shows open, double-cut and approximated geometry as amber warnings, and marks up to 50 open ends, duplicates and overlaps on the preview.

A closed shape inside another is a hole; a shape inside a hole is kept as an island. Loose pieces that would fall out of a cut-out (the inside of an “O”) are cut as drawn, so add bridges if you need them attached.

A part must fit on one of your material’s stock sheets (the card names the sheet when a part doesn’t fit): the short side across the sheet width, the long side along its length, with no kerf or edge margin, so the listed sizes are literal maxima. Uncoated stainless (every finish) is nested that way and never turned sideways; on brushed stock that puts the grain along the longer side of your part, and you can’t ask for the grain across it. Pre-coloured stock is nested either way. Parts that fit no sheet are refused with the sheet size named.

Our laser bed is 1524 × 4000 mm. A part bigger than the bed but on a stocked sheet is sent for review rather than refused. Checked automatically · sent for the fabricator’s review

Uploaded drawings: the smallest hole must be at least max(3 mm, 1 × thickness) across, e.g. 3 mm in 1.2 mm, 4 mm in 4 mm. Smaller goes to review. We measure holes (inner contours); narrow necks or tabs in the outer outline are not measured automatically, so keep them at least as wide as the material thickness.

Cut-to-size sheet and drawn cutouts: any cutout smaller than max(3 mm, 1 × thickness) across (including a round hole below 0.5 × thickness) goes to review. Metal bridges narrower than 1 × thickness (between two cutouts, or a cutout and the edge) can warp or burn through and go to review.

Sides from 5 mm up to the largest stock sheet for the material. Up to 20 cutouts per part, each at least 3 mm across (round holes from Ø3 mm; the editor offers up to Ø150 mm), at least 3 mm inside every edge and not overlapping each other. Open edge notches aren’t possible on a cut-to-size sheet (draw the outline in a DXF instead). Drawn shapes must be right-angled loops. In the profile builder, holes are Ø3–Ø150 mm, up to 100 per piece, with 3 mm of metal around each.

Countersinking is for flat-head screws: pick the screw for the hole, and we cut the hole for it and a 90° cone for its head to sit flush. It needs at least 2 mm of sheet, as thinner stock can’t seat the cone. It is charged per hole. In an uploaded drawing, draw the through-hole size.

Customer-supplied drawings are fabricated as we read them: every cut contour in your file is the cut path (see “How we read it” on the card); nothing is added, offset or resized. Check every dimension before ordering; manufacturing tolerances are in the order terms below.

One straight LINE per bend, at the bend centre-line, on a layer whose name contains BEND or FOLD (also read: BND, CREASE, KNICK, BIEGE, BRAKE, and the whole words HEM, SCORE, FORM / FORMING / FORMED). Names containing UNFOLD are cut layers. Cut geometry can be on any other layer except one named TRIM (dropped) or one containing VCUT / GROOVE (read as V-groove marks, not cuts).

Put the direction and angle in the layer name: BEND_UP / BEND_DOWN, and the angle as the number next to UP / DOWN / BEND / FOLD, e.g. BEND_UP_45 or FOLD-DN-135 (a number elsewhere in the name is used only if there is no other; anything outside 1–180° reads as 90°). With no number a bend is read as 90°. In our own shop files BEND_UP means the flange rises toward the good (finished) face; use the same convention and mark both directions consistently. A suffix like _R2 (radius) or _T1.5 (thickness) is not an angle.

Ignored on purpose: bend annotation layers, meaning a bend word plus extent, label, tangent, text or note (Fusion 360’s BEND_EXTENT, FreeCAD’s Unfold_Sketch_Bend_Labels, BEND_NOTES), curved lines on a bend layer (bends must be straight), and bend lines drawn outside the metal. Each bend line is clipped to the material, and collinear pieces of one bend are merged, but two parallel lines a few millimetres apart are two bends.

Bends are priced from the merged bend lines: a rate per metre of bend length plus a set-up charge per fold. The card’s 3-D fold view folds your drawing at the angles in the layer names; if a tray’s layers name no angle and its corner mitres only close at another angle, the preview folds at that angle and says so. Sizes in the preview are the developed flat’s, with no bend allowance. The angles and directions in your file are read for the preview and the fold count. The shop folds from your drawing and notes, so state anything unusual there.

Longest bend line up to 4000 mm. Sheet up to 5 mm thick can be folded; thicker gauges are laser-cut flat only. Folded profiles are at least 50 mm long and have at most 61 faces.

A flange must be long enough for the brake to grip. The first and last faces of a profile need at least the edge minimum, faces between two folds the internal minimum (hard limits in the profile builder). Box walls and returns whose flat length (height or width minus the outside setback) is below the practical minimum go to review. Keep drawn cutouts the listed distance from a bend line in the profile builder, or the fold distorts them (review; holes entered by count aren’t position-checked).

Uploaded drawings with bend lines are not measured against this table automatically, so design to it: the shop folds from your drawing and there is no automatic hold for a short flange. The inside radius shown is the default for that gauge; a material can carry its own. Not checked automatically

Our fabrication drawings (not the price) are developed with an inside bend radius equal to the material thickness (R = T) and a K-factor of 0.44 (Aluminium 0.43), per material where one is set. Bend allowance = θ·π/180 · (R + K·T); outside setback = tan(min(θ, 90°)/2) · (R + T); all builder widths are outside dimensions.

If you upload your own flat pattern it is cut exactly as drawn, so develop it with these values, or tell us the radius and K-factor you used in the note so the fabricator can check the fold positions.

We fold your drawing (a 2-D cross-section for a simple bracket or channel, full 3-D for trays and boxes) and test the faces against each other. Metal that would pass through other metal once folded (walls wider than the corner they meet at, a flange folding into its neighbour, lips landing on each other) is shown in red in the 3-D view (a red warning for a bracket or channel), and the drawing goes to review instead of straight to payment. Fix: shorten or mitre the flaps so they meet at the corner and add a corner relief, or, if the bends aren’t 90°, put the real angle in the bend layer name.

Not checked when the folded preview can’t be built: more than 60 bends, a bend line that isn’t horizontal or vertical in the drawing, several parts in one file, or single-axis tab bends that don’t run across the part. Those go straight to the price with no automatic hold, so check them yourself and mention anything unusual in the note. Not checked automatically

A bend that stops short of the part’s edge needs a relief cut at its ends so the corner doesn’t tear. Our automatic check doesn’t look for reliefs and nothing holds the order for one. As a rule of thumb (general sheet-metal practice, not a measured limit of ours) make it at least as wide as the material thickness and as deep as the thickness plus the bend radius.

A shape that folds back through itself is refused outright (that one blocks the quote). The web between two same-direction bends must be at least 1 × the shorter adjacent side so the tooling fits, and a section that turns 270° or more must leave at least 20 mm open so it can come off the machine; tighter goes to review.

Box walls can lean 30–130° (90° = straight), with up to 20 returns per wall in three corner styles; the corner relief hole is Ø max(3 mm, 2 × thickness) and the optional corner gap is 0.5 mm. Geometry that can’t be developed (bends that overlap on the base, corner seams that collide, a rim that vanishes) is refused with the reason. Frames are rectangular only, 150–4000 mm a side, and are supplied as four loose mitred pieces, not welded.

V-grooving before folding gives a sharp inner corner. A reverse groove (grooved on the outside so the fold opens it) leaves a thin web in tension and an open notch on the outside of every corner. It is priced normally but always goes to review.

PVD (Gold, Black, Rose Gold, Champagne Gold, Bronze, Nickel Silver, Red Wine, Blue, Latte, Cocoa, Black Titanium) is available on Stainless Steel 304 and Stainless Steel 316 (the uncoated materials marked PVD-eligible in our catalogue), with a choice of coverage (one side up to both sides plus edges). It adds up to 7 working days to the order (Blue: 14 instead); a single-side PVD part supplied from pre-coloured sheet stock adds none. PVD applied after cutting (post-fab) is confirmed by our shop before payment: the quote goes for review and you pay once it’s approved. Checked automatically · sent for the fabricator’s review Powdercoat (White, Black, Grey, Blue, Red, Yellow) is available on raw materials, always as the complete finish, adding up to 5 working days. Stock that already comes colour-finished (Stainless Steel 304 PVD, Stainless Steel 316 PVD, Mild Steel Powdercoated, Aluminium Powdercoated) cannot be coated on top; order a raw material for a post-applied colour. Only the longest coating lead on an order counts, on top of the lead-time tier; colour, coverage and part size change the coating price, shown when you pick it. Deburring for smoothed edges is an option on uploaded drawings, cut-to-size sheets and folded profiles (priced per metre of cut edge); boxes and frames are not deburred.

Hard limits (a part that fits no sheet, a bend line longer than the folder, a gauge too thick to fold, a countersink in sheet that’s too thin, a coating the material can’t take, a box or profile whose geometry can’t be developed) show in red with what to change. The part can’t be added to the cart, and one such part blocks the whole checkout; fix the drawing (or the settings) and re-upload.

Things a machine can’t judge alone (a hole at the edge of what cuts cleanly, an open contour or many overlapping lines, approximated splines, faces that pass through each other when folded, a very tight channel, a box wall or return below the practical bending minimum) show in amber. The price is a real quote (indicative for estimated geometry) and the part goes in the cart, but the checkout button reads Submit for review instead of pay; the quote page then asks for your email and an optional note. We email you when the fabricator has looked at it, and payment unlocks if it can be made. If the fabricator adjusts the price you see that on the quote before you pay. The review is free. If it can’t be made as drawn you’re told, with the fabricator’s note when they leave one, and the quote page lets you reopen the part in the configurator to adjust it. There is no charge for a declined review.

Prefer to fix it yourself? The amber message says what tripped and how to fix it. Re-upload the corrected DXF and the price updates on the spot.

Most drawings do. Glance at the size and any “How we read it” notes under the preview, then pay. Once an order is paid it can’t be reopened or edited (see the order terms), so this is the moment to be sure.