TOOL DESIGN

Sheet Metal Design Guidelines for Stamping: A DFM Checklist

October 21, 2026 · Atharva Engineers


Most of a stamped part's cost is decided when the drawing is made. A few design rules make the difference between a simple, robust progressive die and a complicated, fragile one. These are the checks we run on every drawing before quoting. They are rules of thumb: material, thickness and tolerance can change them, so always confirm with your toolmaker.

In the guidelines below, t is the material thickness.

Holes and slots

  • Minimum hole diameter: at least 1 × t for mild steel; larger for stainless and high-strength steels. Smaller holes need fragile punches.
  • Hole to edge distance: at least about 1.5–2 × t, or the edge bulges and the hole distorts.
  • Hole to hole distance: at least about 2 × t between holes.
  • Holes near bends: keep holes at least about 2 × t plus the bend radius away from the bend line, or they stretch into ovals.

Bends

  • Inside bend radius: at least about 1 × t for mild steel and CRCA; harder or high-strength materials need more. Work out flat lengths with our bend allowance calculator.
  • Minimum flange length: a common guide is at least about 2.5–3 × t plus the bend radius, so the material can be held while it bends.
  • Bend relief: add a relief cut where a bend meets an edge, to stop tearing at the corner.
  • Grain direction: bends across the rolling direction are less likely to crack. The strip layout can orient critical bends correctly if they are marked on the drawing.

Corners and profiles

  • Avoid sharp internal corners. Small radii make punches and dies stronger and last longer.
  • Avoid long, narrow tabs and slots. They need slender punches that break, and parts that distort.
  • Keep part outlines nest-friendly. Shapes that interlock on the strip save material. See 5 ways to reduce sheet metal cost.

Tolerances

  • Apply tight tolerances only where function needs them. Stamping holds cut features accurately, but formed dimensions vary more because of springback and material variation.
  • Dimension from a datum that the tool can reference, such as a pierced hole, rather than from a bent edge.
  • State burr direction and maximum burr height for edges that matter, especially on electrical parts. See controlling burrs and the punch and die clearance guide.

Forming features

  • Embosses and ribs: keep depth modest relative to thickness, and leave distance from edges and bends.
  • Deep draws: avoid where a shallow form will do. Deep drawing needs special material grades and extra stations.
  • Extruded holes and tapping: confirm with the toolmaker early; they affect strip layout and station count.

Before you send the drawing

  1. Material grade, thickness and temper stated
  2. Critical dimensions and tolerances marked
  3. Burr side and limit defined where needed
  4. Finish or plating specified
  5. Annual volume stated, because it decides the type of tool

Our RFQ checklist has a ready-to-use template.

Want a second opinion on manufacturability? Send us your drawing. With the quotation, we point out where small design changes can make the progressive tool simpler and the part cheaper.

Free calculators: Press Tonnage Calculator Bend Allowance Calculator Die Clearance Calculator
Let's get started

Send Us Your Drawings

Get a technical evaluation and commercial quote within 24 hours.