Built in Nampa, Idaho. Shipped nationwide. View current offers →
Skip to clearance checker
Design tools / Sheet metal bending Xeon NC

Reverse bend.Clearance checker.

Give an already-formed flange room to move. Compare your geometry with our punch profiles, inspect the bend in 3D, and find a workable combination of base and flange dimensions.

Check your part Explore tooling

Powered by Xeon NC

01 / Configure & compare

Check your return flange.

Your part & tooling

Xeon NC tooling library
The result screens the punch profile at the final inside angle. The rounded 3D sheet and forming motion help explain access; they do not check the full motion, die, clamps, or part-on-part collisions. Tool-angle and tonnage compatibility still need review. See model limits.
02 / Bending design guide

Make room for the next bend.

A reverse bend is any bend that has to be formed while a previously formed flange is standing up next to the punch. Channels, trays, offsets, Z-sections, return flanges and hems all create the same situation: by the time the last bend goes in, part of your part is already occupying the space the tool needs.

A standing flange needs room beside the punch throughout the bend. If it occupies the same space as the tool, the part needs a different punch, geometry, or bend sequence. This checker focuses on that geometric access question; material and tonnage limits still need a separate review.

What makes this hard to eyeball is that the part moves during the bend. At the bottom of the stroke the base of the part is folded into a V around the punch tip, so the two legs are tilted upward — roughly 45° each for a 90° bend. Every flange already standing on those legs gets swung up and inboard, toward the punch body, exactly when clearance is tightest. A flange that looks like it has an inch of room in the flat CAD view can be touching the tool at the bottom of the stroke.

What the checker does: it takes the actual traced cross-section of each punch in our tooling library, folds your part the way the brake folds it, and finds the tallest return flange that still misses the tool. Same geometry engine, same tool profiles as our 3D Bend Simulator.
03 / Bending design guide

Reading the Envelope

Open “Cross-section & clearance envelope” below the 3D view to compare punches. The horizontal axis is your inside base dimension — how much flat sits between the new bend line and the flange that is already formed. The vertical axis is the tallest that already-formed flange can be. Each curve is one of our punches.

A point under a curve clears that punch profile in the final-angle model. A point above it indicates interference. Your part is the black dot; leave room below the curve for your safety margin.

Three features of the curves are worth understanding, because they explain most of what happens to real parts.

  • Near the origin, every curve collapses. With a short base dimension the flange is close to the punch tip, where the tool is a solid wedge. There is no relief available that close in — the punch has to be that shape to press the radius. This is why a narrow channel with tall legs is the hardest thing to ask for.
  • Then the curves jump. Once the base dimension is past the widest point of the tip wedge, the flange clears into the relieved section of the punch and the ceiling suddenly becomes the full working height of the tool. The jump is a real cliff edge, not a gradual improvement, and it lands in a slightly different place for every punch.
  • At the far right, the curves flatten or dip. The top of the tool is not straight — the head flares out where it seats into the clamp. A very tall flange a long way out can catch that flare, which is why the curves stop rising and in one case turn back down.
Leave margin. The default 0.05″ is there for a reason. Actual sheet runs to mill tolerance, the backgauge places to a real tolerance, and springback compensation drives the punch slightly deeper than the nominal angle needs. A design that clears by only 0.002″ in the model leaves very little allowance for production variation.
04 / Bending design guide

Where the Limit Comes From

The result uses a simplified 2D cross-section. These four steps explain the clearance calculation.

Reverse Bend Clearance Model ──────────────────────────────────────────────────────── 1. Punch frame: tip at the origin, tool axis vertical. Profile = DXF trace of the real tool. 2. Leg tilt: β = 90° − A_new / 2 (A_new = angle being formed now) At the bottom of the stroke the sheet wraps the punch tip, so each leg rises at β from horizontal. For A_new = 90°, β = 45°. 3. Formed corner: P = d · (cos β, sin β) d = inside base dimension 4. Flange direction: v = rotate(leg direction, 180° − A_old) Flange occupies P → P + F · v Max flange height F is the largest F for which the segment P → P + F·v does not intersect the punch profile.

Step 2 is the one people miss. In the flat CAD view the base is horizontal and the return flange points straight up, comfortably clear of everything. At the bottom of the stroke that base is folded into a 90° V, both legs are at 45°, and the return flange has rotated 45° toward the punch along with the leg it sits on. For a 90°/90° part this works out to a memorable rule of thumb: the flange can be about as tall as the base is long, before you consider which punch is in the machine.

Step 4 is why acute angles hurt twice. An already-formed flange at 60° instead of 90° does not just stand up — it leans back over the base, directly into the space the punch body needs. Change the return flange bend angle in the checker from 90° to 60° and watch the ceiling drop.

Everything the model needs about the tool comes out of the traced profile: the wedge half-angle near the tip, the tip radius, where the relief starts, how tall the relieved section is, and where the head flares. The calculation uses the sampled tool profile.

05 / Bending design guide

Our Punch Library, in Clearance Terms

The five punches in our library, described by what they can reach around rather than by what radius they press. Full geometry and photos are in the Press Brake Tooling Library; these are the numbers that decide a reverse bend.

Punch Tip R / angle Relief starts at Relieved height What it is for

Relief starts at is how far the flange has to be from the punch centreline before it stops fouling the tip wedge and gets into the relieved section. Relieved height is how tall it can then be before it reaches the tool head. Both are measured off the traced profile.

What this means in practice

  • OW202/S is the default for most of our gauges and is already an offset tool — its body sits back behind the tip line, which is why it handles ordinary return flanges without a tooling change.
  • OW200/S is the gooseneck. Its 86° tip is fatter close in, so it is worse than the acute punch at very small base dimensions, but its throat clears far more once you are past it. It is the tool for a tall return flange on a reasonable base — and, as covered below, the wrong tool when flanges stand on both sides.
  • OW300/S is the same gooseneck 80 mm taller. This is the deep-box and deep-tray tool — the only one that clears flanges taller than about 190 mm.
  • OW203/S is the heavy R4 punch for plate. Its 60° included angle makes it the worst of the set for clearance, which is the trade for pressing a soft radius in 1/4″ material.
  • OW202/K is the short 120 mm body. Useful for shallow parts, but its low head means tall flanges run out of room sooner.
06 / Bending design guide

One Flange vs. Two: Why Hat Sections Are Harder

Switch the checker between Formed flange on one side and Formed flange on both sides and the ceiling drops sharply. Understanding which of the two your part is doing matters more than any other input on the panel.

First, which case are you in?

The check is about flanges that are already formed when the current bend goes in. The material on the far side of the bend line being formed right now is not a problem — it is wrapping the punch tip, which is what it is supposed to do.

  • One side is the normal case, and it covers more parts than people expect — including the last bend of a plain U-channel. When you form the second leg of a channel, only the first leg is standing; the second one is being created by the stroke you are in.
  • Both sides is the harder case: a bend that goes in between two flanges that already exist. Hat sections, top-hat stiffeners, trays already flanged at both ends, and any part where the bend order forces the middle bend to come last.

Why the second flange costs so much

Our punches are relieved on one side — the body is set back behind the tip line on the working side and full width on the other. With one formed flange we simply turn the relief towards it and you get the generous curve. With flanges on both sides only one of them can be in the relief. The other is up against the full body of the tool, and that side sets the limit.

The gooseneck punches show this most dramatically, and in a way that inverts the usual advice. An OW200/S has an 86° included tip — almost the same angle as the 90° V your part is folded into at the bottom of the stroke. On the relieved side that hardly matters. On the unrelieved side the punch flank ends up running very nearly parallel to the leg of your part, a couple of degrees apart, so the already-formed flange on that side is effectively touching the tool from the moment it exists. For a two-flange bend the gooseneck is the worst tool in our library, and the acute 28° OW202/S — whose flank sits far inside the V — is the best. The checker's table shows this directly.

Design consequence: if a bend has to land between two existing flanges, decide early whether the flanges are short enough to clear, because your options at the brake are limited. Growing the base dimension a quarter inch is usually free at the design stage and can be the difference between a part we form in one setup and a part that becomes a weldment. It is also often possible to re-order the bends so the middle one is not last — ask us before you commit to the geometry.
07 / Bending design guide

If It Doesn't Clear

A red verdict is not the end of the part. In rough order of how little it costs you:

  • Grow the base dimension. The cheapest fix by a wide margin, and often invisible to the function of the part. Because the curves have a cliff edge, a very small increase can take you from impossible to comfortable — the checker will tell you the minimum base dimension for your flange height.
  • Shorten the return flange. Equally cheap if the flange is there for stiffness rather than for a fastener.
  • Open the return flange angle. If the already-formed bend is acute, bringing it to 90° stops it leaning into the tool and buys a surprising amount of room.
  • Let us change the punch. Free, and often enough on its own — the checker shows which of the five clears. A gooseneck or the tall OW300/S may pick up a part the default tool cannot.
  • Re-order the bends. Sometimes forming the return flange last instead of first removes the conflict entirely. This is our problem to solve, not yours, but it is worth knowing it exists as an option.
  • Split the part. If nothing clears, the geometry becomes two parts and a joint. Better to find that out now than after tooling up.
Related reading: Part-on-Part Collision covers the mid-stroke case where the part hits itself rather than the tool, Picking Tooling for the Bend explains how punch and die selection sets your radius, The Bend Affected Zone covers feature clearance near the bend line, and Bending Ontology & Material Specs has the per-material bend deduction data.
08 / Bending design guide

Model Assumptions

Stated plainly, so you know what the green verdict is and is not promising.

  • It checks the punch only. Interference with the die, the backgauge fingers, the machine bed or the operator's hands is not modelled. Downward-facing flanges near the die shoulder are the usual case this misses.
  • It checks the part against the tool, not against itself. Part-on-part collision is a separate question with its own guide and 3D viewer.
  • The corner is idealised as sharp. The reported envelope uses sharp corners. Actual bend radii change the geometry and need to be considered when reviewing a close fit.
  • The flange is checked on its inside face. Material thickness is drawn in the cross-section but the binding surface is the face towards the tool, which is the one that touches.
  • Bottom of stroke, fully formed. The check is made with the part at its final angle and the punch at depth. The bend is a continuous motion and clearances change through it; a part that only just clears at the bottom of the stroke deserves a real simulation, which is what our programmers run.
  • Tools are treated as flippable. We orient the relief towards the flange, which is what the shop does. OW203/S is symmetric so orientation is irrelevant to it.
  • Profiles are 2D cross-sections. Segmented tooling, tool gaps along the bend line and features that vary across the width of the part are outside this model.

Use this as an early geometric screen. Send the folded model for confirmation of tooling compatibility, overbend, machine access, and the complete bend sequence.

The 3D preview adds sheet thickness and rounded corners for clarity. Its width is illustrative. The reported limits continue to use the sharp-corner, inside-face envelope described above; the animation is not a collision check through the full stroke.

From geometry to a confirmed bend sequence

Let’s review
your part.

Upload the folded model and include your critical dimensions. Our team reviews the bend sequence and tooling before production.

Upload your design