How to model your part so the calculator and the shop read it the same way

What the calculator reads from your model

• Sheet thickness, from the two main faces. The part must have the same thickness everywhere — pockets, thinning or chamfered edges spoil it.
• A hole as a cylinder. Its diameter decides how we make it: a catalogue size by punching, anything else by laser.
• A thread only from the hole diameter — a cosmetic thread in CAD does not survive the STEP export. A certain thread is a hole at the ISO minor diameter D1 (that is how SolidWorks, Inventor and Solid Edge export a tapped hole) or a collar whose bore is the core diameter of a forming tool. A core or tap-drill diameter in flat sheet is only a “possible thread” — tick it yourself in the Holes and threads table.
• A countersink as a 90° (or 120°) cone. Every such cone is a countersink to the calculator — even a small chamfer on a hole edge.
• A collar (extrusion) as coaxial cylinders standing out of the sheet plane. The calculator checks whether the sheet has enough material for it.
• When it is unsure, it neither charges nor drops a thread silently: it prices the hole as a plain hole, flags it for review and links here.

Thread in an extruded collar

Thin sheet has too little material to carry a thread. So we first draw a collar out of the sheet — an extrusion — and form the thread into it (roll-formed, no chips). The collar is made from the material around the hole; nothing is added, so its height is set by the sheet thickness, not by the designer. We have tools for M4 (sheet up to 2.55 mm), M6 and M8 (up to 3.05 mm); recommended thicknesses are in the table.

What to model

• The collar bore is safest at the ISO minor diameter D1 (3.242 / 4.917 / 6.647) — that is what the CAD hole wizard draws for a tapped hole, and the calculator always recognises it. The core diameter of the forming tool (M4 Ø 3.7 · M6 Ø 5.55 · M8 Ø 7.4) is recognised too, as long as the collar stands out of the sheet by more than 0.3 t (✓ in the table); with a lower collar it is only a “possible thread”.
• The collar as one body with the sheet — outer diameter and height from the table. Model the same height or less; a taller collar cannot be drawn out of the sheet.
• The collar points to the die side, i.e. downwards, away from the punch. Put every collar on a part on the same side.
• You may keep the cosmetic thread in the model — we just don't read it. The thread size must follow from the hole diameter.

Guide values from volume conservation: the collar wall thins to about 0.65 t as it is drawn, and the pre-hole is about half the collar's mean diameter. The tool gives the exact shape. The calculator accepts a collar within these limits; a collar the sheet has no material for is flagged as not formable. Sheet below 1 mm (M8 below 1.5 mm) only after review.

Common mistakes

• A collar taller than the sheet allows. A real case: M8 in 3 mm sheet with a collar 7 mm below the sheet. There is not enough material for that — in reality it comes out at about 1.3 mm (total thread length ≈ 4.3 mm).
• A collar modelled as a stuck-on tube: full sheet thickness wall, flat end, no radii. That is a turned insert or a press-in nut, not an extrusion.
• A thread on the drawing only. A cosmetic thread or an “M6” callout in the PDF never reaches the geometry — the model keeps a plain hole.

Thread directly in the sheet (no collar)

In thicker sheet it is enough to punch or laser-cut a core hole and form the thread straight into the wall. Strength comes from the number of turns, i.e. thickness ÷ pitch. The calculator accepts a thread from 1.5 turns; for full strength we recommend TRUMPF's thicknesses — M4 from 1.5 mm, M6 and M8 from 3 mm. In thinner sheet, model a collar.

What to model

• A through hole at the core diameter (3.7 / 5.55 / 7.4) or at ISO D1 (3.242 / 4.917 / 6.647). D1 is a certain thread to the calculator; a core diameter in flat sheet is only a “possible thread” because plain holes often have the same size — then choose “thread” in the Holes and threads table.
• Hole edge at least one nominal thread diameter from the part edge. Forming pushes material sideways and a thin web bulges.
• Other sizes: the machine forms M2.5–M10; we have tools for M4, M6 and M8. Other sizes by arrangement.

Formed thread or rivet nut?

The classic way to put a thread into thin sheet is a rivet nut: a hole goes into the part, the nuts are ordered, received and booked, and then every one is set by hand. We form the thread on the machine in the same set-up that makes the part — the part arrives with its threads done.

• No extra part. The thread is made from the sheet itself: nothing to order, stock or fit, and nothing that can spin or work loose in the hole.
• Carries load in both directions. A note from practice: a rivet nut loaded against the direction it was set in can be pulled out of the sheet. A formed thread is part of the sheet itself, so it carries load in both directions.
• No grip range to match. A rivet nut is chosen by sheet thickness — an M8, for example, is sold separately for 1.0–3.5 mm and 3.5–6.0 mm sheet. We pick the forming tool from the thickness we read straight from your model.
• Nothing stands proud of the face. The flat head of a rivet nut sits on top of the sheet; a thread formed in the sheet adds nothing, and a collar points only to the die side.
• When a rivet nut is the better choice: you need a longer thread than the sheet or collar gives (tables above), a size outside M4–M8, or a thread in a different material than the sheet. Say so in the note to your enquiry.

Countersinks for flat-head screws

We stamp countersinks with a 90° cone for ISO 10642 countersunk socket screws — M6 and M8, sheet 2–3 mm. Stamping can push the cone at most 75 % into the sheet; the rest of the thickness must carry the load. So in 2–3 mm sheet neither an M6 nor an M8 head sinks in completely — it stands slightly proud; it would sit flush only in about 4 mm sheet (M6). For 3 mm sheet we also have a formed countersink to the full head diameter (Ø 12.8 / Ø 16.8) — if the head must sit flush, say so in the notes and we'll review it.

What to model

• A 90° cone with a through hole underneath, Ø 6.6 (M6) / Ø 9 (M8) to ISO 273.
• Cone depth at most 0.75 t: diameter at the surface = hole + 1.5 t (see table). Stamping cannot make a cone through the full thickness.
• 90° — that is what our tools are. The calculator recognises a 120° cone, but we make it only by arrangement.
• A stamped countersink opens on the punch side, i.e. opposite to where collars point. A countersink on the collar side is possible only in 3 mm sheet.

Holes, slots and distances

A hole at a catalogue size is punched in one stroke, anything else is laser-cut — the calculator prices both correctly, punching is just cheaper. The distances below are rules of thumb; the calculator does not check them, we do when preparing production.

Catalogue punch shapes

Full punch feature catalogue with drawings →

Chamfers and deburring

We do not machine edges. Laser and punch both cut square to the sheet, so a chamfer in the model will not be on the part — and the calculator may read it as something else. A laser-cut edge is practically burr-free; a punched hole keeps a small burr on the die side.

• Do not model chamfers on holes. A 90° cone — and 0.5 × 45° is a 90° cone — is read as a countersink and charged.
• Do not model chamfers on outer edges. The part then no longer has a uniform thickness and the calculator may measure it wrong.
• If edges must be broken, write it in the enquiry notes; on the drawing use ISO 13715 (e.g. “edges −0.3”). The machine has roller deburring; we use it by arrangement.
• Milled chamfers or custom countersinks are made by our sister site prototype.builders ↗.

Bends

We bend on a TruBend 5170 with the tools we own. The inner radius comes from the die, not from the model — set the bend radius in your CAD sheet-metal module from the table. A flange shorter than the minimum cannot rest on the die. Forces, lengths and acute angles are on the press-brake tooling page.

• A hole closer to the bend than 2 t + Ri is pulled into an oval during bending.
• A bend that ends inside the sheet needs a relief cut at least t wide and reaching past the end of the bend — otherwise the corner tears.

Press-brake tooling and what we can bend →