Sheet metal fabrication from concept to packing: the full process

A sheet metal part passes through many hands before it reaches the customer, and each stage relies on the one before. A missing bend relief in the model becomes a torn corner on the press brake; an unmasked thread becomes a nut that will not start.

This article walks through the nine stages in order, with what goes in, what comes out and what to check. The first three stages are design and engineering, which is where SMDE works. The other six are carried out by fabricators and finishers on their own equipment, but design decisions set the limits for all of them.

1. Concept design

The concept stage asks: can this be made from sheet, and roughly how? Start from the space available, the loads, the mounting, the environment and the quantity. A sketch or block model is enough to agree the envelope, material and joining method.

Quantity matters early: five brackets and five thousand can justify very different designs. Decide the likely finish now too, because it affects material choice; anodising, for example, only applies to aluminium.

2. Detail design: 3D parts and assembly

Detail design turns the concept into a 3D model of every part and the assembly. Use the sheet metal tools in your CAD package so flat patterns are developed from bend data. The features that most often cause trouble on the shop floor are:

• Bend radius: model the inside radius the fabricator's tooling produces. In air bending it comes from the V-die opening.
• K-factor or bend table: use the fabricator's bend data. A wrong K-factor moves every flange after the first bend.
• Reliefs: add bend and corner reliefs where bends stop short of an edge or flanges meet; a width of at least T is a common rule of thumb.
• Holes near bends: keep hole edges clear of the bend, typically at least 2 to 2.5 × T plus the inside radius, or they will distort.
• Minimum flange length: a flange must reach past the die shoulder. Around 0.7 × V for a 90° bend is a common rule of thumb.
• Hardware: self-clinching nuts, studs and standoffs need a minimum sheet thickness, edge distance and a sheet softer than the fastener. Take these from the manufacturer's data.
• Tolerances: apply a general tolerance, such as a class from ISO 2768-1, and tighten only what matters. Dimensions across several bends hold looser than cut features, because errors add up.

Design the assembly for the steps that follow: tab-and-slot joints to locate parts for welding, clearance for torches, spanners and rivnut tools, and holes sized for coating (stage 7).

3. Preparing 2D DXF files of each part

Most fabricators program their laser or punch from DXF files. A clean DXF is a flat pattern and nothing else: the geometry the machine should cut, with any bend and etch information kept apart so it cannot be cut by mistake.

• Export one DXF per part, at 1:1 in millimetres. Check one known dimension after export, because unit errors are easy to miss.
• Put cut geometry, bend lines and etch marks on separately named layers. Agree layer names and colours with the fabricator if they have a convention.
• Remove dimensions, notes, borders and title blocks, and check contours are closed with no duplicate lines. Anything left in the file may be cut.
• Show bend direction (up or down) and angle, either on the bend layer or on the accompanying drawing.
• Name files consistently with part number and revision, for example TRAY-012_REV-B_2.0MM_S275.dxf, so the material and thickness are visible before the file is opened.
• Send a bill of materials with part numbers, revisions, materials, thicknesses, finishes and quantities per assembly and per batch.

Nesting, arranging parts on the sheet to minimise waste, is usually done by the fabricator in their own software, but you can help: state the grain or brushing direction where it matters, and say whether a part can be rotated.

4. Cutting by laser or punching

The flat blanks are cut on a fibre laser, a CNC turret punch or a combination machine. Laser cutting suits profiles and short runs; punching suits repeated holes, louvres, extrusions and other formed features on longer runs. The choice deserves its own discussion, which you will find in our article on laser cutting vs punching.

Cut parts usually need deburring. Sharp edges and dross cut hands, scratch mating parts and spoil coatings, since powder pulls thin on a sharp edge. If edges must be broken to a specific size, say so on the drawing.

5. Bending on an accurate CNC press brake

Bending is where design errors usually show up first. A CNC press brake controls the punch depth (Y axis), which sets the angle in air bending, and the back gauge fingers (X and R axes), which locate the sheet relative to the bend line.

• Bend sequence: earlier flanges must clear the punch, die and frame, so return flanges and deep boxes need checking before release.
• Angle measurement and correction: springback varies with material and batch. Operators check angles with a protractor, and some machines measure and correct during the stroke.
• Gauging: the cut edge against the finger must be square and long enough to rest on it.
• First-off inspection: measure the first part fully against the drawing before running the batch. If flange lengths are consistently out, the bend data in the flat pattern needs updating, not the gauge.

6. Welding

Welding joins formed parts into assemblies. MIG welding is quick and common for steel. TIG welding gives finer control and neater welds, and is widely used on stainless steel, aluminium and thin sheet. Resistance spot welding joins overlapping sheets without filler and with little visible marking on the far side, which suits enclosures and panels.

Heat causes distortion, and thin sheet distorts easily. Good weld prep and fit-up with small, even gaps, a jig to hold the parts, and short stitch welds in a balanced sequence all help. Specify only the weld needed; a continuous seam where a few stitches would do adds heat and distortion.

Welds may then be ground or dressed flush where visible or where parts fit against them, and spatter removed before coating.

7. Coating or anodising

Most parts need a finish for corrosion protection, appearance or both. The common options are:

• Powder coating: electrostatically applied and oven cured. Typical film thickness is around 60 to 120 µm, depending on the system.
• Wet paint: useful for large parts, small batches or specific paint systems. Film thickness depends on the primer and topcoat.
• Hot-dip galvanising: zinc coating for steel, applied by dipping, usually to EN ISO 1461. Thin sheet can distort in the bath, and closed sections need vent and drain holes.
• Anodising: an oxide layer grown on aluminium only. Typical decorative layers are around 5 to 25 µm, and as a rule of thumb roughly half grows outwards and half into the metal.

Every finish depends on pre-treatment: degreasing, cleaning and often a conversion coating or blast-cleaning. Laser-cut edges with oxide scale may need extra preparation.

For example, an M6 medium clearance hole of 6.6 mm with 0.1 mm of powder in the bore comes out at about 6.4 mm. The bolt still passes, but a hole sized closely to a dowel, a bush or a slide would not. Allow for coating on fits, and state on the drawing which areas must be masked: tapped holes, self-clinching nuts, earth points that need bare metal for electrical continuity, and mating faces.

8. Assembly with screws, nuts and fasteners

Assembly brings finished parts together with fixings. Self-clinching nuts and studs give strong threads in thin sheet; whether they go in before or after coating depends on the finish and fastener, so check the manufacturer's guidance. Rivnuts are fitted from one side and suit closed sections or coated parts.

• Torque: use the values from the fastener or insert supplier. Self-clinching and rivet nuts have torque-out limits, and overtightening spins them in the sheet.
• Threadlocker: specify it where vibration could loosen fixings, and say which grade, since some grades are meant to be removable and some are not.
• Inspection: check that every fastener is present and tight, parts move or close as intended, and earth continuity is tested where required.

9. Packing

Packing is the last chance to damage a part: a chipped coating on arrival undoes every stage before it.

• Leave protective film on stainless and pre-finished sheet where possible, and specify film that can be removed cleanly after the time in transit and storage.
• Use edge and corner protectors, and separate coated parts with foam, card or bags so they do not rub.
• Label each pack with part number, revision, quantity and destination; kit parts by assembly where that helps the customer.
• Choose boxes, crates or pallets for the weight and handling route, and avoid straps directly over coated faces.

Closing checklist

• Are the bend radius and K-factor in the model the fabricator's real values?
• Do reliefs, hole-to-bend distances and flange lengths meet the fabricator's limits?
• Are DXF files 1:1, in millimetres, on clean layers, with no dimensions and with revision in the file name?
• Does the BOM give material, thickness, finish and quantity for every part?
• Has the bend sequence been checked, and are welds specified only where needed?
• Are hole sizes and fits allowed for coating, and are masked areas marked?
• Are torque values, threadlocker and earth points specified?
• Are packing and labelling requirements agreed before the parts are made?

If you would like a second pair of eyes on a design before it goes to your fabricator, or need clean DXF files and fabrication drawings prepared, send us your drawings.

All insights