Keep the nearest edge of a hole at least 2.5 times the material thickness plus the bend radius away from the bend line. On 2 mm steel with a 2 mm inside radius, that's about 7 mm.
Closer than that and the bend drags the hole out of shape. Round holes turn oval, the edge nearest the bend bulges, and bolts that should drop straight through suddenly need a file. It's a design issue, not a cutting one: the laser cut the hole perfectly, then the press brake pulled it. Here's a table to design against, why it happens, and what to do when the hole really has to be close.
Why holes near a bend distort
When sheet bends, the metal near the bend line stretches on the outside and compresses on the inside. That deformation doesn't stop dead at the bend line. It spreads a short way into the flat flange on either side.
A solid flange doesn't care. A hole sitting in that zone does. The metal around it has less material to resist the pull, so the hole stretches towards the bend. The closer it sits, the worse it gets, and on very close holes the edge of the hole can even fold up with the bend.
You'll usually see one of three things:
- Oval holes. The hole is longer in the direction across the bend.
- A bulge or kink in the flange edge beside the hole.
- A wandering bend line. The hole weakens the sheet along the bend, so the fold follows the path of least resistance.
All three get worse with thicker material and harder alloys.
Minimum hole distance table
These figures use the 2.5T + R rule of thumb with an inside radius equal to the thickness, which suits mild steel and soft aluminium. Stainless and harder aluminium normally get a bigger radius, so add the extra radius to the distance.
| Thickness | Inside radius (about 1T) | Minimum distance, hole edge to bend line |
|---|---|---|
| 1 mm | 1 mm | 3.5 mm |
| 1.5 mm | 1.5 mm | 5.25 mm (call it 5.5) |
| 2 mm | 2 mm | 7 mm |
| 3 mm | 3 mm | 10.5 mm |
| 4 mm | 4 mm | 14 mm |
| 6 mm | 6 mm | 21 mm |
Example: a 3 mm 304 stainless bracket with a 5 mm inside radius. 2.5 × 3 = 7.5, plus 5 = 12.5 mm. So the hole edge should be at least about 12.5 mm from the bend line, a couple of millimetres more than the mild steel figure.
These are rules of thumb, not hard limits. A small hole may get away with a little less. A big hole, or one that has to hold a tight fit, deserves a little more.
Watch the flange length too
Hole distance and flange length are linked. If the flange is short, there may not be room for the hole at a safe distance and enough metal beyond it.
Say you have a 2 mm flange that's 15 mm long and you want an 8 mm hole in it. The hole needs to start 7 mm from the bend line, and an 8 mm hole then reaches 15 mm. There's nothing left at the edge. You'd either need a longer flange or a smaller hole. A good starting rule for the edge side is to keep holes at least one material thickness from the flange edge as well.
So check both: distance to the bend, and distance to the edge. Our guide to minimum flange length gives the bending side of that equation, and minimum hole size for laser cutting covers small holes and edge distances.
Slots and cut-outs near bends
Slots follow the same rule, but their direction matters.
- Slots running parallel to the bend behave like a row of holes. Keep the nearest edge at the minimum distance.
- Slots running across the bend (perpendicular to it) are worse, because the end of the slot sits in the deformation zone. Either stop the slot short of the danger zone or run it right through the bend as a deliberate relief.
- Large rectangular cut-outs in a flange near a bend can let the whole bend line bow. Keep them back, or break the bend into separate sections.
If a cut-out has to reach the bend, it should go all the way through it and act as a relief notch rather than stopping just short. Stopping a few millimetres short is the worst of both worlds. Our post on bend relief explains how to size those notches.
When the hole really has to be close
Sometimes a hole simply can't move. A hinge, a mounting pattern on an existing frame, or a cable gland near a corner. Here are the usual fixes, roughly from cheapest to most expensive:
- Make the hole a slot. If it's a bolt hole, elongating it slightly along the direction of distortion hides the stretch, and a washer covers it.
- Add a relief slot along the bend line. A narrow laser-cut slot along the bend, beside the hole, takes the stretching instead of the hole. It weakens the bend locally, so it isn't always appropriate.
- Accept the oval. On a clearance hole that's well oversized, a little distortion may not matter. Say so on the drawing so nobody chases it.
- Drill or cut the hole after bending. This guarantees a round hole in the right place, but it's a separate operation and adds cost. Worth it for precision holes only.
- Move the bend. Sometimes the cleanest answer is to change the part so the bend sits elsewhere.
Dimensioning holes on bent parts
How you dimension holes matters as much as where they are. Dimension holes from the nearest bent face, or from an edge on the same flange, rather than from the far end of the part through several bends. Every bend adds a little variation, and measuring across bends stacks it up.
For hole-to-hole fits, like a bracket that must bolt to a frame, keep the matching holes on the same flange if you can. Holes on the same flat face are laser cut in one go and stay accurate to each other.
Sending the part
Send a STEP model of the bent part or a dimensioned PDF, plus the material, thickness, and quantity. If any hole is closer to a bend than the table suggests, flag it in the notes and we'll come back to you with options before anything is cut.
Read more about our CNC bending service, or start a quote for CNC bending with cutting and bending on the same order.