Key takeaways
- State the material standard and grade with the thickness range, because a 0.1 mm variation in a 1.5 mm sheet moves each 90° bend allowance by 0.07 mm.
- A ±1° bend angle tolerance puts 1.75 mm of variation at the end of a 100 mm leg, so flange dimensions need a stated datum rather than a default.
- Write edge requirements as a number: 0.1 mm maximum burr on coated-contact edges, 0.3 mm elsewhere, with the edge class marked on the view.
- A note that contradicts a view is read in favour of the view, so fix the view rather than adding a note that argues with it.
- Notes repeated on every drawing belong in a numbered standard-note block, referenced by document number and revision, not retyped per sheet.
Two drawings of the same bracket reach two fabricators. Both show the same geometry, the same material and the same three bends. One carries a complete set of drawing notes for sheet metal and comes back with a price and a delivery date; the other comes back with eleven questions, and the part that is eventually made has a 0.6 mm radius on the inside of the bends, a burr on the edge that faces a painted panel, and a coating thickness nobody can measure.
The difference is the note block. Views carry geometry; notes carry the decisions about surfaces, edges, joints, finishes and evidence, and those decisions are where most rework originates. A drawing with a complete note block is a document a tool room, a welder and an inspector can each read and act on without calling the designer.
This guide sets out the ten drawing notes for sheet metal that remove the most rework, in the order a shop reads them, with the number each one turns on. It assumes the part is a laser-cut or stamped, formed and welded assembly in CRCA, stainless or aluminium, and it treats general tolerancing as a default rather than a specification. The other design rules sit in the design and CAD hub.
Why the note block, not the geometry, decides the quote
Geometry is unambiguous in a modern drawing; a 120 mm hole is a 120 mm hole. Notes are where the ambiguity lives, and every ambiguity becomes a question at quotation, a decision at the machine, or a concession at inspection.
A missing radius note does not stop production. It hands the choice to whoever sets the press brake, and the punch that is already in the machine decides the radius. A missing burr note hands the choice to whoever runs the deburring station, and if there is no deburring station the burr ships. That is the mechanism: an unwritten requirement is not a default requirement, it is a delegated decision.
The ten notes below are ordered by the operation that consumes them, so the block reads as a route: what the part is made from, how it is formed, how its edges are treated, how it is joined, how it is finished, how it is marked, how it is checked and how it is packed.
The ten drawing notes for sheet metal, in order
| # | Note | What it prevents | Ganesh limit or note |
|---|---|---|---|
| 1 | Material grade, standard and thickness range | Parts made from an unstated grade with different formability | CRCA, stainless and aluminium from 0.8 mm to 40 mm; grade and standard named on the drawing |
| 2 | Minimum inside bend radius | Cracking at the outside of a tight bend | 1.0t minimum for CRCA to 3.0 mm; radius set by the punch, so state the value |
| 3 | Grain direction relative to bend lines | Split flanges on tight bends in half-hard sheet | Bends across the rolling direction where the radius is under 1.5t |
| 4 | General tolerance and datum scheme | Two fitters measuring from different edges | ±0.5 mm typical; tighter on named features by agreement |
| 5 | Edge and burr limits with edge classes | Burrs scoring a coated mating face; cuts in handling | 0.1 mm maximum on coated-contact edges, 0.3 mm elsewhere |
| 6 | Weld size, type and finish treatment | Over-welding, distortion, unmeasured "grind flush" | Symbols to ISO 2553; fillet 3–5 mm typical; flush means ±0.2 mm |
| 7 | Coating system, DFT and masking | Thin patches, painted threads, coated earth studs | Seven-tank pretreatment, 18 ft × 14 ft powder booth, DFT checked |
| 8 | Marking, position and depth | Untraceable parts; marking on a visible or mating face | Laser etch 0.1 mm deep or ink; position stated on a view |
| 9 | Inspection and evidence | A first article that checks the wrong features | FAI and PPAP available; critical characteristics listed on the drawing |
| 10 | Packing reference and quantity per pack | Damage in transit; miscounts at goods-in | Pack specification by number, not prose; dunnage pitch stated |
1. Material, standard and thickness range
Write the grade and the standard, not just "MS 1.5". CRCA to IS 513 is not one material: the drawing quality designation changes formability, and a part designed for a drawing grade that is made from a commercial grade will split at a tight bend or tear at a drawn corner. State the standard, the designation and the thickness with its tolerance.
The tolerance matters because thickness drives bend allowance. Bend allowance is θ(R + Kt) for a bend angle θ and K-factor K, so for a 90° bend at K = 0.44 a 0.1 mm change in thickness moves the allowance by 1.5708 × 0.44 × 0.1 = 0.069 mm. That is small on one bend and 0.21 mm across a part with three, which is why a flange stack that is dimensioned to the inside of the bend can miss a ±0.5 mm mating face without anyone making a mistake.
2. Minimum inside bend radius, and who chooses it
A press brake produces the inside radius of the punch, not the radius drawn in CAD. A 1.5 mm CRCA part drawn with a 0.5 mm inside radius will be formed with whatever tooling is in the machine, and a 0.5 mm radius on 1.5 mm sheet is 0.33t — below the 1.0t that drawing-quality CRCA needs, so the outside fibre tears across the grain on the first sharp bend. A part that fails at the press is a part that fails on the day of the first delivery.
The drawing states the minimum inside radius, and for CRCA up to 3.0 mm that is 1.0t. Below that, the tooling has to be right and the material has to be a drawing grade. The same note should reference the hole and slot distance from the bend line, which has its own rule and its own article: hole-to-bend distance in sheet metal design.
3. Grain direction
Sheet is rolled, and the properties differ along and across the rolling direction. A bend whose line is parallel to the rolling direction puts its maximum strain across the weak axis, and a tight radius there splits sooner than the same radius across the grain. On 1.5 mm CRCA at a 1.0t radius the difference is small; on 3.0 mm, or on stainless and half-hard aluminium, it decides whether the part forms at all.
State the bend line relationship, and show the rolling direction on the flat pattern with a grain arrow if the part has any tight radius.
4. General tolerance and datums
ISO 2768-1 covers general tolerances where the drawing does not call out a specific tolerance, and that is exactly its role here: it sets a default for the features nobody cared to tolerance. It does not replace a datum scheme. Two holes that locate a bracket to a frame need a position tolerance from a stated datum, because a general tolerance measured from two different edges accumulates in both directions.
For sheet metal, ±0.5 mm is the working default on a laser-cut part, and features that matter are called out individually. The datum should be the face that locates the part in the assembly, not the drawing's bottom-left corner.
The principles for how a tolerance applies when the drawing is silent are set out in ISO 8015, which establishes that dimensions apply independently unless a relationship is stated. A fabricator who assumes a different rule will inspect the part differently, which is how a good part is rejected.
5. Edge and burr, written as a number
"Deburr all edges" is not a requirement, because it cannot be measured and therefore cannot be rejected. Write a limit and an edge class: 0.1 mm maximum burr on every edge that contacts a coated face, a gasket or a hand, and 0.3 mm maximum elsewhere, with the edge class marked on the view.
The physical reason is that a 0.2 mm burr under a 160 kg stack load scores a painted face in transit, and a burr on a handle edge cuts a glove. The requirement costs a deburring pass, so it should be written only where it is needed — a burr limit on every edge of a large panel adds work for no benefit.
6. Welds: size, type and what "flush" means
A weld symbol states the joint, the weld type, the size and the length. Without a size, the welder uses what the joint will take, which on 1.5 mm sheet is usually too much and pulls the part out of square.
For sheet metal assemblies, 3–5 mm fillets are typical, and an intermittent weld needs its pitch and length stated: 20 mm weld at 100 mm pitch is a different structure from a continuous seam. Spot welds need a nugget diameter and a pitch. And "grind flush" needs a number, because flush to ±0.2 mm is a different operation from a blended toe; on a visible face the first is a finishing step and the second is a paint defect waiting to happen.
7. Coating, DFT and masking
State the system, the colour, the gloss, the dry film thickness and the masking. Powder at 60–80 µm is the usual industrial specification; below 60 µm the film can show the substrate profile and lose corrosion performance, and above 100 µm it chips at the edges and bridges close-fitting holes.
Masking is the note that gets forgotten. Threads grow by 0.12–0.16 mm on an M6 thread at that film thickness, so a coated rivet nut will not accept its bolt. Earth studs must stay bare. Any mating face that sets a clearance must be masked. The coating line runs a seven-tank pretreatment, and the substrate it produces is part of why the film adheres — a part that skips a stage and gets a thicker coat still fails, which is why the note specifies the system and not just the thickness. The related failure is covered in powder coating laser-cut edges.
8. Marking
Every part needs a part number, a revision and a date or lot code. Laser etching at 0.1 mm depth survives coating and is legible after years in service; ink does not survive a pretreatment line. State the position, because a mark on a visible face is a cosmetic defect on a painted panel and a mark on a mating face is a high point.
9. Inspection and evidence
Say what has to be measured and what has to be recorded. A first article inspection on a new part should cover the critical characteristics listed on the drawing, dimensioned from the datum, and it should be repeated after any change that affects the flat pattern. PPAP is available where the customer's own quality system requires it; the drawing should say so, because it changes the paperwork and the timing of the first delivery.
10. Packing and quantity per pack
The pack is part of the specification. Reference a packing specification by number and revision, state the quantity per pack, and state the dunnage pitch where the parts are flat panels. A drawing that leaves packing silent gets a pack designed at the dispatch bay on the day, which is where panel damage begins.
The worked example: three bends and one missing note
Take a 1.5 mm CRCA channel, 300 mm wide, with three 90° bends and a 100 mm flange on each side that has to mate with a bracket at ±0.5 mm. The drawing shows the flange dimensions to the inside of the bend and no bend angle tolerance.
The angle defaults to whatever the brake holds, and ±1° is a normal machine capability. At the end of a 100 mm leg, 1° is 1.75 mm of lateral movement, because tan 1° × 100 = 1.75. The flange datum moves by that much before any thickness variation is counted. Add the three-bend thickness effect of 0.21 mm and the flange face is potentially 1.96 mm away from where the model put it.
Nothing was made badly. The part is inside every tolerance the drawing states, because the drawing stated none. The fix is two notes: "all flange dimensions to the outside of the bend" or a true-position dimension from the datum, and "bend angle ±1°, cumulative ±0.5° across the part". Both are one line, and together they turn a 2 mm argument into a 0.5 mm one.
The same arithmetic applies to the cumulative angle on a box: four bends at ±1° each can put the last flange 3.5 mm out at 50 mm from its bend, which is why a deep box with a closing seam needs a stated cumulative tolerance rather than a per-bend one. Bending tolerances and inspection covers how those limits are measured.
What Ganesh runs against a note block
Parts are cut on the 12 kW fibre laser with its 40 ft × 16 ft bed, formed on the 200 T, 5-axis brake with the 4,450 mm bed and Delem control to 10 mm, and welded on three CLOOS robotic MIG cells or at the 30+ manual stations. Press tools, fixtures and checking fixtures are built in the in-house tool room, which is what makes a stated radius and a stated weld size achievable rather than aspirational.
The note block is read at the manufacturability review before quotation: material and thickness against the forming route, radius against the available punches, burr against the deburring step, coating against the masking list. Drawings that arrive as PDF plus DXF or STEP with a complete note block move through that review in one pass. Customers including Mahindra, Godrej & Boyce and Indian Railways work to drawing sets that carry these notes, and the parts come back the same way. The manufacturing route behind the notes is described under sheet metal bending and tools and dies.
How to write the block so it survives revision
- Number every note and never reuse a number; add 11 rather than renumbering, so a reference in an email still points at the right note.
- Keep the sequence of operations, and keep it the same on every drawing.
- Put the notes that never change into a standard-note block with its own document number and revision, and reference it from the drawing.
- Never let a note carry a dimension; a note that repeats a dimension will eventually disagree with it.
- Delete a note that has been superseded rather than leaving it struck through, and record the deletion in the revision block.
- Keep the units and the number of decimal places consistent across notes and views.
The DXF and RFQ checklist lists the drawing fields that have to travel with the file, and a note block that matches it means the first review is about the part rather than the paperwork. Send the current revision through the quote form and the review comes back against your notes.
When a note is the wrong tool
Three cases. A requirement that applies to every part in the plant is not a drawing note; it belongs in the general specification the drawing references, and repeating it on 400 drawings guarantees that 40 of them carry an old version. A requirement that can be modelled is better modelled: a boss, a relief or a radius that exists in the geometry does not need a note to describe it. And a requirement that contradicts a view should be fixed in the view, because a note that argues with a dimension is a note that gets ignored.
What is left is the genuine note: the number that no view can carry, such as a burr limit, a coating thickness, a weld size, a marking depth or a packing pitch. Ten of those, written in order and kept under revision, are the difference between a drawing that is quoted once and a drawing that is questioned every time it is issued.
Frequently asked questions
What notes should every sheet metal drawing have?
Material grade and standard with a thickness range, minimum bend radius, edge and burr limits, general tolerance and datum scheme, weld size and finish treatment, coating system and masking, marking and traceability, inspection requirement, and packing reference. Ten notes cover the decisions that otherwise get made at the machine.
Should a sheet metal drawing reference ISO 2768?
Only for features with no individual tolerance. ISO 2768-1 covers general tolerances where the drawing does not call out a specific tolerance, so it sets the default for hole positions and cut-outs, and a fabricator still needs the critical features toleranced individually at ±0.5 mm or tighter.
How do you write a deburr note that can be inspected?
Give it a number and an edge class: 0.1 mm maximum on edges that contact a coated face or a hand, 0.3 mm maximum elsewhere, with the edge class identified on the view. A note that says 'deburr all edges' cannot be measured and therefore cannot be rejected.
What happens if the drawing note contradicts the view?
The view is normally read as taking precedence over a general note, which means a contradictory note is ignored rather than obeyed. The practical fix is to correct the view and delete the note, because a fabricator resolving the conflict by judgement will resolve it differently on the next order.
Where should the note block sit on the drawing?
Above the title block on the right-hand side, numbered, in the reading order of the operations: material, form, edge, weld, finish, mark, inspect, pack. A note read out of sequence gets applied out of sequence, and a packing note at the top of the list is the one the welder reads first.
Sources and further reading
- ISO 2768-1 — General tolerances for linear and angular dimensions without individual tolerance indications · reviewed 3 Nov 2026
- ISO 8015 — Geometrical product specifications: fundamentals, principles and rules · reviewed 3 Nov 2026
- IS 513 — Cold reduced carbon steel sheets and strips · reviewed 3 Nov 2026
Send the drawing and the note block
Send the current revision as PDF plus DXF or STEP. We will return the manufacturability points against your notes before the quotation, so the discussion happens once.
Request a quote