Atlas Tech Talks · DFM Guide

When a hole tears out or a bend deforms it

A hole on a flat pattern looks harmless. It is a circle on a drawing, dimensioned to a couple of decimal places, and it usually goes in without incident. The trouble starts when that circle sits too close to something: the edge of the part, or a bend line. Put a punched hole a hair too close to a sheared edge and the punch shoulders the thin remaining web of material until it bulges, cracks, or tears clean through. Put a hole a little too close to a bend and the forming operation stretches the metal around it, pulling a clean round hole into a lopsided oval or a teardrop.

Neither failure shows up in CAD. Both show up on the shop floor, usually after the tooling is set and the first article is in an inspector’s hands. The fixes at that point are all expensive: move the feature and re-cut, add a secondary drilling operation after forming, or scrap and start over. The good news is that the spacing rules that prevent both problems are simple, well established, and tied directly to one number you already know: material thickness.

This guide lays out the two distances that matter most for hole placement in sheet metal: hole-to-edge and hole-to-bend. Both are practice-based DFM guidelines rather than a single stamped standard, so the numbers below are presented as the typical ranges the fabrication industry works to, with sources. Treat them as design starting points and confirm the tight cases with your fabricator.

Two different rules, two different failure modes

Engineers often lump “hole spacing” into one mental rule. It is actually two rules, because the two situations fail for different physical reasons.

Hole-to-edge distance governs what happens when a hole sits near the outside edge of the part. The failure mode here is a tear-out or bulge. When a hole is punched, the punch shears a slug out of the sheet, and the material immediately around the punch is pushed and stretched. If there is not enough solid material between the hole and the part edge to resist that force, the thin web deforms: the edge bulges outward, the wall between hole and edge thins, and in the worst case it splits. This is a blanking and shearing problem, and it is most severe when the hole is punched rather than cut.

Hole-to-bend distance governs what happens when a hole sits near a bend line. The failure mode here is distortion. When a flange is formed, the metal on the outside of the bend stretches and the metal on the inside compresses. That deformation is not confined to the exact bend line: it spreads into a zone on either side. Any hole that falls inside that deformation zone gets dragged along with the moving material and comes out oval, teardrop-shaped, or “pulled” toward the bend. This is a forming problem, and it happens whether the hole was punched, laser cut, or drilled, because the damage is done during bending, not during hole-making.

The practical takeaway: hole-to-edge is about surviving the punch, and hole-to-bend is about surviving the form. Keep them separate in your head, because the numbers and the fixes are different.

Minimum hole-to-edge distance

The rule of thumb: keep the distance from the edge of the hole to the edge of the part at least equal to material thickness, and preferably 1.5 to 2 times material thickness for punched holes. Industry DFM guides converge on this range. A minimum of one times material thickness (1T) from hole edge to part edge is a common starting guideline, while many fabricators call for at least 2T for punched holes near a blank edge to guarantee no bulge or tear-out. Fabcon publishes this as its “2xT edge rule”: place holes at least two times material thickness from edges (Fabcon, DFM Principles for Precision Sheet Metal).

The distance is measured from the nearest point of the hole to the nearest part edge, not from hole center. Threaded holes, extruded (formed) holes, and countersinks need more room than a plain clearance hole, because those features either concentrate more load in the surrounding wall or draw material during forming. When in doubt on a threaded or formed feature, move up to the 2T to 3T range.

The table below shows recommended minimum hole-to-edge distances by common steel sheet gauge, using 2T as the recommended punching minimum and 1T as the practical laser floor. Values are rounded and should be adjusted for softer or more brittle alloys.

Punching versus laser makes a real difference here. A CNC turret punch shears the hole with a hard tool, and that shearing force is exactly what threatens a thin edge web. Laser cutting removes material thermally with no side load on the surrounding metal, so it is more forgiving of holes near edges and can hold cleaner geometry at smaller edge distances. That is why the laser column above can run down near 1T while the punch column stays at 2T. A fabricator that cuts your part on a fiber laser can often accept edge distances a punch shop would reject. The reverse is also true: if the part is destined for a turret punch on a high-volume run, design to the punching minimums even if your quoting portal shows a laser price.

Minimum hole-to-bend distance

The rule of thumb: the edge of the hole should sit far enough from the bend line that it stays outside the deformation zone. The industry formula, used by fabricators for decades, ties that distance to both material thickness and the inside bend radius.

For holes smaller than roughly 1 inch (25 mm) in diameter:

d = 2T + R

For larger holes and for slots (roughly 1 inch / 25 mm and up):

d = 2.5T + R

where d is the minimum distance from the edge of the hole to the bend line, T is material thickness, and R is the inside bend radius (V&F Sheet Metal, Bend Sizes and Hole Positions). Some shops publish a simplified version, “keep the hole at least 3T from the bend line,” which is really the 2T + R formula evaluated at the common case where the inside radius equals material thickness (R = T). A more conservative simplification seen in DFM guides is a clearance of 3 to 4 times material thickness between the hole edge and the start of the bend zone (Yijin Solution, Sheet Metal Design Guidelines).

The table below works the formula for common steel gauges, assuming a typical inside bend radius equal to material thickness (R = T). If your actual inside radius is larger, add the difference. Distances are measured from the hole edge to the bend line (the tangent point of the inside radius on the flat).

What happens inside the zone. When a hole falls inside the deformation band, the forming operation pulls the near wall of the hole toward the bend while the far wall lags. The hole elongates in the direction of the bend and takes on a teardrop or oval shape (V&F Sheet Metal). For a plain clearance hole this may be cosmetic and tolerable. For a hole that has to be tapped, that has to pass a shoulder bolt, or that mates to a fixed pattern on another part, an ovalled hole is a reject. Slots are more sensitive than round holes, which is why the formula bumps up to 2.5T + R for larger features, and why some shops push slots out to 4T + R.

Hole-to-hole and hole size minimums

Two more constraints round out the picture.

Minimum hole diameter. For punched holes, the general guideline is that hole diameter should be at least equal to material thickness. A 0.060 in (16 ga) sheet needs punched holes no smaller than about 0.060 in in diameter. Go smaller and the punch pin, which is now thinner than the material it is shearing, is at high risk of deflecting or snapping (DFMPro, drawing on Gerald Davis’s sheet metal design guidelines). Some DFM checkers set the default even more conservatively, flagging any punched hole whose diameter is less than twice the material thickness. Laser cutting escapes this limit because there is no pin to break: a fiber laser can produce holes well below material thickness, down to roughly 0.5 mm on thin gauges, though very small holes on thicker stock suffer from kerf taper and rougher walls (Yijin Solution).

Hole-to-hole spacing. Keep at least material thickness, and preferably 2T, of solid metal between adjacent holes. Punching two holes with only a sliver of material between them invites the same web bulge and tear-out you see with a too-close edge, and on a punch it can also distort the first hole when the second is struck. The 2T spacing guideline mirrors the hole-to-edge rule for the same physical reason: the wall between features needs enough material to resist the shearing load.

Why the numbers are what they are

The spacing minimums are not arbitrary safety margins. They fall out of how the metal actually moves.

Punch shear and material flow. When a punch drives through sheet, it does not cleanly slice a circle. It shears: the material rolls over at the top, fractures through the middle, and leaves a burr at the bottom. Around that shearing action, the metal is displaced sideways and stretched. That displaced material has to go somewhere. When there is a full field of metal around the hole, the displacement is absorbed with no visible effect. When the hole is near an edge, the only place for the displaced material to go is out toward the free edge, which bulges. Shrink the web further and the stretch exceeds what the material can take, and it tears. The 1T to 2T edge minimum is the amount of surrounding material needed to absorb punch displacement without bulging.

The deformation zone. Bending is bulk plastic deformation, and it is not confined to a razor-thin line. The metal yields and flows across a band whose width scales with thickness and radius. Outside that band the metal is essentially undisturbed. The 2T + R formula is an estimate of how far the disturbed band reaches: roughly the inside radius plus a couple of thicknesses of surrounding stretch. Put a hole beyond that reach and it never feels the forming strain, so it stays round. Put it inside and it is part of the material that flows.

Tear-out mechanics. Both failure modes are the same phenomenon at different scales: a thin ligament of metal loaded beyond its capacity. Whether it is the web between a hole and an edge under punch load, or the wall of a hole inside a bend under forming load, the metal fails when the local strain exceeds its ductility. More ductile alloys (soft aluminum, mild steel) tolerate tighter spacing; harder or more brittle materials (spring steel, some stainless tempers, hardened aluminum) need more room. That is why every table here is a starting point, not a guarantee: ductility moves the line.

How to fix a too-close hole

When a review flags a hole that violates one of these minimums, there are five standard moves, roughly in order of preference:

• Move the hole. The cheapest fix is almost always to shift the feature to a legal distance. If function allows even a small relocation, take it.
• Add a relief. For a hole near a bend, a relief notch or slot at the bend can keep the forming strain from reaching the hole, or a bend relief can prevent tearing at the corner. This preserves the hole location while changing where the metal flows.
• Cut it on a laser instead of punching it. If the violation is a hole-to-edge or hole-diameter issue, switching from turret punch to laser removes the shearing load entirely and often makes a marginal design legal. This does nothing for hole-to-bend, which is a forming problem.
• Redesign the flange. Shortening a tall flange, opening the inside radius, or relocating the bend can pull the deformation zone away from the hole.
• Drill or tap after forming. When the hole absolutely has to be near the bend and has to stay accurate, leave it off the flat pattern and add it as a secondary operation after the bend is formed. This is the most reliable fix for accurate tapped holes near bends, and also the most expensive, because it adds a setup and an operation (V&F Sheet Metal).

Pitfalls that bite engineers

• Holes in the bend zone. The single most common issue. A hole that looks comfortably placed on the flat pattern lands inside the deformation band once the flange is up. Always check hole-to-bend with the 2T + R formula, not by eye.
• Threaded holes too close to edges. A clearance hole might survive at 1T from an edge, but a tapped hole needs full thread engagement in undistorted material. Give threaded and formed holes the 2T to 3T treatment.
• Dimensioning to the wrong reference. Hole-to-edge is measured from hole edge to part edge, and hole-to-bend is measured from hole edge to the bend line (the tangent of the inside radius). Dimensioning center-to-center or center-to-bend hides the real clearance and lets a violating hole slip through.
• Assuming laser and punch have the same minimums. They do not. Laser is more forgiving on edge distance and hole size; punch is not. A design that quotes fine on laser can fail on a punch line, and high-volume parts often move to punching for cost.
• Ignoring the deformation zone on tall flanges. A tall flange with a large radius has a wider deformation band. The 2T + R distance grows with R, so a generous inside radius pushes holes farther from the bend than a sharp one would.

Hole placement in the Atlas world

At Atlas, hole spacing is one of the first things flagged in DFM review, because it is one of the cheapest problems to fix on a drawing and one of the most expensive to fix after tooling. When a flat pattern comes in, the review checks every hole against the edge, against its neighbors, and against every bend line it sits near, using the same 2T edge and 2T + R bend guidelines laid out above, adjusted for the specific alloy and temper on the job.

The cut method matters to that review. Atlas runs both laser and punch capability, so a hole that is marginal for one process may be perfectly fine on the other. Where a design pushes edge distance or hole size below punching minimums, moving the part to the laser is often the clean answer, and the review will say so rather than send back a redesign request. Where the problem is a hole inside a bend deformation zone, no cut method saves it, and the recommendation is to relocate the hole, add a relief, or drill and tap after forming. Post-form tapping is a standard Atlas operation for accurate threaded holes that have to live near a bend.

How Atlas helps you place features right

The fastest path to a clean part is to catch spacing issues before the tooling is set, and that is exactly what the Atlas DFM review is for. Send the flat pattern and the bend layout, and the feedback comes back with specific numbers: which holes are too close to which edges or bends, how far they need to move, and whether a process change (laser instead of punch, or a secondary drilling operation) solves it without a redesign. The goal is not to send a design back with a list of rejections. It is to get the part manufacturable with the fewest changes to the engineer’s intent, and to flag the cases where a tapped hole near a bend should simply be added after forming.

Frequently asked questions

How far from the edge should a hole be?

Keep the edge of the hole at least one material thickness (1T) from the part edge as a floor, and 1.5 to 2 times material thickness for punched holes to be safe against bulge and tear-out. Threaded and formed holes should get 2T to 3T.

How close to a bend can I put a hole?

Use d = 2T + R for holes under about 1 inch in diameter, and d = 2.5T + R for larger holes and slots, where d is measured from the hole edge to the bend line, T is thickness, and R is the inside bend radius. When the inside radius equals thickness, that works out to roughly 3T.

Why did my hole go oval after bending?

It sat inside the bend deformation zone. The forming operation stretched the metal around the hole and dragged the near wall toward the bend, pulling a round hole into a teardrop or oval. The fix is to move the hole outside the 2T + R distance, add a relief, or drill it after forming.

What is the minimum hole size for punching?

As a general guideline, a punched hole diameter should be at least equal to material thickness. Smaller than that, the punch pin is thinner than the sheet it is shearing and risks deflecting or breaking. Some DFM checkers flag anything under twice thickness.

Does laser cutting change the rules?

For hole-to-edge, hole-to-hole, and minimum hole size, yes. Laser removes material thermally with no side load, so it tolerates smaller edge distances and much smaller holes than punching. For hole-to-bend, no. That is a forming problem, so the 2T + R rule applies no matter how the hole was made.

How much space do I need between two holes?

Keep at least material thickness, and preferably 2T, of solid metal between adjacent hole edges, for the same reason as the edge rule: the wall between features needs enough material to resist the punch or forming load.

Do slots follow the same rule as round holes?

Slots are more sensitive to bend distortion than round holes, which is why the hole-to-bend formula steps up to 2.5T + R for slots and larger features, and some shops push slots to 4T + R near a bend.

Should I dimension to hole center or hole edge?

For these spacing checks, think in hole edges. Hole-to-edge is hole edge to part edge, and hole-to-bend is hole edge to bend line. Dimensioning to center hides the true clearance and can let a too-close hole pass review.

Final thoughts

Hole spacing is one of the highest-leverage things an engineer controls on a sheet metal part, because the rules are simple and the cost of ignoring them is high. Two distances carry most of the weight: keep holes at least 1T to 2T from edges so they survive the punch, and keep them at least 2T + R from bend lines so they survive the form. Everything else, the minimum diameters, the hole-to-hole spacing, the slot adjustments, follows from the same physics of shearing and material flow. Design to these starting points, dimension to hole edges, tell the shop whether the part is punched or lasered, and send the tight cases through DFM review before the tooling is set. The holes that never make it to a scrap bin are the ones that were placed right on the flat pattern.

Engineer’s Bookmarks: External References

• Fabcon, DFM Principles for Precision Sheet Metal Manufacturing (the 2xT edge rule and hole-to-bend guidance)
• V&F Sheet Metal, Bend Sizes and Hole Positions (the d = 2T + R and d = 2.5T + R hole-to-bend formulas)
• Yijin Solution, Sheet Metal Design Guidelines (hole diameter, edge distance, and 3 to 4T bend clearance)
• DFMPro, What’s In DFM Sheet Metal Design (minimum hole diameter vs thickness, drawing on Gerald Davis’s design guidelines)
• Paragon Metal Fabricators, Design for Laser Cutting (laser DFM: holes at least 2T from bend lines, bend relief)
• JC Proto, Sheet Metal Hole Tolerances: Laser vs Punch vs CNC (process comparison for hole quality)
• Xometry, Minimum Bend Radius Reference Table and Calculator (inside bend radius reference feeding the R term)
• ASM Handbook, Volume 14B: Metalworking, Sheet Forming (ASM International) for the underlying blanking, shearing, and bending mechanics
• Machinery’s Handbook (Industrial Press) for sheet metal gauge, bend allowance, and punching references