How close can a hole be to a bend?

Use the number on your material page.

Every Xeon NC material page publishes a row called Min Hole / Cutout from Bend Line for the exact gauge you are ordering. That value already accounts for the tooling we will use, and for almost every material we form it is the larger of the two constraints in play.

The value equals roughly 0.63 × the V-die opening, measured from the edge of the hole to the bend centerline on the flat pattern. For 0.060″ mild steel formed in our 12 mm die, that is 0.298″. Put the hole edge that far from the bend line and neither failure mode described below can reach it.

If you want to understand why that number is what it is—or you need to defend a feature that has to sit closer—the rest of this guide takes it apart.

Three ways to state the same distance.

Most disagreements about hole spacing are not disagreements about the number. They are disagreements about where the two ends of the tape measure go.

Published rules of thumb are quoted from the bend line, from the bend tangent, to the hole center, and to the hole edge—often without saying which. Those choices differ by more than the tolerance on the feature. Everything in this guide is measured from the edge of the hole to the bend centerline, on the flat pattern.

The hole pulls toward the bend.

This is the failure mode everyone knows, and it is real—it is just not usually the binding one.

During forming the outer fiber of the bend stretches and the inner fiber compresses. That strain does not stop cleanly at the tangent line; it fades out across a corridor of permanently deformed material on both flanges. Inside that corridor, the metal flows toward whatever is weakest. A hole is a void with no material to resist, so the strain concentrates around it: the hole elongates along the bend axis, shifts off its nominal position, and the surrounding face dishes.

The result is a fastener that will not seat, a dowel that will not locate, and a hole diameter that no longer matches the drawing. The practical threshold is the inside radius plus two material thicknesses, and stiffer, less ductile material needs more room.

DistortionLeft: the hole sits inside the deformation corridor and ovalizes as material flows into it. Right: the same hole moved clear of the corridor forms round and stays on position.

This is the rule behind quote warning codes 3243 and 4243, documented in the DFM rules and error code lookup. The bend-affected zone guide goes deeper on the deformation field itself.

The part is standing on two lines.

In air bending the sheet touches the tooling in exactly three places: the punch nose, and the two die shoulders at ±V/2 either side of the bend line. Those shoulders carry the entire forming load.

Put a hole on a shoulder and the geometry stops being a stress-concentration question and becomes a contact question. The sheet is being pressed against a hardened steel edge at that exact location, with tonnage behind it. The hole rim gets dimpled, the edge of the opening rolls, and the flange can collapse locally—independently of anything the bend-affected zone is doing.

This is why the die opening, not the bend radius, sets the real floor. And because the die opening grows with material thickness, the keep-out grows with it too.

Three contactsThe Xeon NC bend simulator marks them directly: two shoulder points where the sheet rests on the die, and one punch contact at the nose. The shoulder markers are the lines a hole must stay off.

The number is already published for your gauge.

You do not have to derive any of this. Open the material page for what you are ordering and read the bend data table.

The hole clearance and the minimum flange are the same value because they describe the same physical fact: the strip of sheet that has to lie flat and unbroken across the die shoulder. A flange shorter than that has nothing to sit on. A hole inside it removes the material that would have been sitting there.

Stop measuring. Look at it.

The Xeon NC bend simulator draws the die shoulder keep-out directly onto your flat pattern as a hatched red band, and flags any hole that lands inside it.

This turns the whole question into something you can see instead of something you have to calculate. Build the profile, place the hole where the design wants it, and the tool tells you whether the die can live with it.

✗ Rejected / 0.158″ from the bend line

A Ø0.25″ hole on 0.060″ mild steel, placed 0.158″ from the bend centerline. It overlaps the hatched band, so the simulator turns it red and labels it in shoulder zone. It is also excluded from the exported STEP cutouts.

✓ Accepted / 0.315″ from the bend line

The same hole moved out to 0.315″. It clears the die shoulder band and also clears the 0.298″ published minimum for this gauge, so it has deformation margin as well. The flag disappears.

Note what the two frames have in common: the band did not change. It is a property of the die, which is a property of the thickness. The only thing that moved was the hole.

Formed resultSwitch to 3D View to see the accepted hole on the folded part. Holes that fail the shoulder check are deliberately left out of the 3D mesh and the STEP export, so an empty face is itself a signal.

Every die band, all three numbers.

All distances are from the hole edge to the bend centerline on the flat pattern. Design to the fourth column.

Two things are worth reading off that table. First, the design minimum beats the deformation rule in almost every band, which is why one number is enough for most parts. Second, the exceptions are all heavy stainless—0.075″ and 0.188″ 304 and 316—where the 3T corridor finally overtakes the die. On those two gauges, use the deformation value.

The keep-out also scales hard with thickness. Going from 16 gauge to 3/16″ plate multiplies the required clearance by two and a half, because the die opening did the same. A hole pattern that was comfortable on a thin prototype can be illegal on the production gauge.

Four honest options.

Sometimes a mating part fixes the hole and the bend, and there is no room between them. That is a legitimate design problem with real solutions—none of which is pretending the clearance is fine.

For the related case where a formed flange collides with tooling or with the part itself, see the part-on-part collision guide. For two perpendicular flanges meeting at a box corner, see how to keep corner flanges from colliding. For choosing the radius that sets these numbers in the first place, see the bend radius guide.

Seven lines before you upload.

Each one takes seconds in the simulator or on the material page, and each one prevents a warning on the quote.