Minimum hole size and hole-to-edge distance in stamping

Why small holes are a tool problem

A punching tool is a column in compression. As the hole gets smaller relative to its length, the punch becomes slender and is more likely to buckle or snap. The length is set by the die and the stripper, so a small hole in a thick sheet gives a high length-to-diameter ratio. That is the real limit, not a single diameter number.

The slug also has to clear. A small slug can jam in the die, be pulled back into the strip or weld itself to the punch. The clearance around a small punch is small, so a slight misalignment or a worn punch will rub and heat. A hole that is made successfully on the first article can still fail in production if the punch is not guided and lubricated.

The working rules

For a conventional stamping die, a practical starting point is a hole diameter equal to or greater than the sheet thickness. That keeps the punch stiff enough for mild steel and gives the slug a chance to clear. A hole smaller than the thickness is possible, but it needs a review of the punch material, the guidance and the strip.

The edge distance is the distance from the hole edge to the part edge, not the centre distance. As a starting point, keep it at or above one thickness. A hole closer than that leaves a weak wall that can tear or bulge during punching. A hole-to-hole web should also be at least one thickness, and more if the material is hard or the holes are close to a bend.

These are starting points, not rules that apply to every material. A soft copper part can go below them, and a hard stainless part should stay above them. The table below gives a practical range by material.

The strip layout can raise or lower the limit. A punch that is supported by a strong stripper and guided close to the work will survive a smaller hole than a punch that is unsupported. A station with a lot of surrounding cuts may weaken the strip and let the material move, which changes the effective edge distance. If a hole is close to the limit, show it on the strip layout and ask the toolmaker how the punch will be guided.

How the material changes the limit

Mild steel is forgiving. It shears cleanly with a reasonable clearance and does not work-harden much, so a hole at one thickness is usually reliable. Stainless steel is different. It work-hardens at the cut edge, which raises the force on the next stroke and wears the punch. The same hole that works in mild steel may need a larger diameter or a tougher punch in 304.

Copper and brass are soft and shear easily, so the hole can be smaller than the thickness. The risk is the slug and the smear. Copper can pick up on the punch and close a small hole, and a soft slug can deform instead of clearing. Aluminium has a similar galling risk and needs a polished punch and the right lubricant.

High-strength steel raises the punch load and the wear. The limit moves up, and the tool may need a premium punch steel or a coating. If the part is also thick, the length-to-diameter ratio becomes the deciding factor.

Edge distance and tear-out

A hole close to the edge leaves a narrow wall. During punching, the material around the hole is pushed outward, and a thin wall can bulge or tear. The risk is higher if the hole is near a bend, because the bend adds strain in the same region. Keep the hole at least two thicknesses from a bend line, and more if the bend radius is tight.

The part edge itself should have a radius at the corners. A sharp corner concentrates stress and wears the die. A small radius, around half the thickness or more, makes the punch easier to maintain and the part stronger. If the function needs a sharp corner, a secondary operation or a different process may be better.

Design fixes when the hole is below the limit

The first fix is to increase the hole or the edge distance if the function allows. That is free and always worth checking. If the hole must stay small, a stepped punch can help: the punch has a short small-diameter section and a larger shank, which reduces the length-to-diameter ratio and resists buckling.

A second fix is to move the small hole to a secondary operation. A drilled or laser-cut hole after stamping can be cheaper than a fragile punch and the downtime it causes. A third fix is to change the process: laser cutting or EDM can make a small hole in a flat part with no punch at all. The trade-off is the piece price and the edge quality.

For a very small hole in a thick part, a pilot hole and a shave may be needed. That is a two-step route, but it can hold a tighter hole and a better edge than a single punch. The cost has to be compared with the risk of a broken punch in production.

Tool maintenance is part of the answer. A small punch should be checked for wear at a shorter interval than a large one, and the die should be cleaned before a slug can build up. A spare punch kept at the press is cheaper than a stopped line. If the hole is critical, add a plug gauge to the setup check so the operator can catch a drift before the run produces scrap.

• Increase the hole or the edge distance if the function allows
• Use a stepped punch to shorten the slender section
• Move the hole to a drill, laser or EDM operation
• Use a pilot hole and a shave for a tight small hole
• Review the strip layout to give the punch more support

Inspection and tool life

Inspect the small holes first, because they are the features most likely to drift. Measure the diameter at the top and the bottom of the hole, and check for a taper or a burr. A hole that is undersized at the bottom may be a sign of a worn punch or a slug that is dragging. Check the edge distance on the first and last part of a run.

Track punch life. A small punch wears faster than a large one, and the wear shows as a change in hole size or a burr. Ask the supplier for the punch replacement interval and keep a spare. If the hole is critical, add it to the first article and to the in-process check plan.

What to put on the drawing

State the hole diameter with a tolerance, the edge distance and the web between holes. If the hole is at or below the process limit, say so and ask for a DFM note rather than assuming it can be punched. Mark the holes that are functional and the ones that are only for location or clearance.

For a part with several small holes, give the datum scheme and the position tolerance. A hole that is dimensioned from a feature made at another station can accumulate error. A hole dimensioned from the datum that the die uses is easier to hold and easier to inspect.

Where a hole is below the limit, mark it as a special characteristic rather than tightening the tolerance. A note that says the hole may be made in a secondary operation gives the supplier a route without a fragile punch. That is clearer than a general tolerance that quietly applies to a feature the die cannot hold.

• Hole diameter and tolerance
• Edge distance and web width
• Distance from the hole to any bend line
• Datum scheme and position tolerance
• Which holes are functional and which are clearance
• Whether the hole can be made in a secondary operation