The Radius Callout Decides Three Things at Once

Bend radius looks like housekeeping in a CAD dialog box. It settles three separate outcomes at the same time: whether the outer fiber of the flange tears, what length of strip the blank requires, and how far the finished angle opens once the tool lets go.

Forming references treat the minimum radius as a limit rather than a preference, and they express it as a multiple of material thickness. One thickness on 2 mm steel means an inside radius of 2 mm, while half a thickness on the same stock means a 1 mm radius. Writing the limit in multiples of T lets one rule travel across gauges, because outer-fiber strain scales with thickness in the same way.

Three failure modes come out of one tight radius. Cracks open on the outside of the bend when the surface runs out of stretch. Wrinkles and a distorted profile appear on the inside, where the metal has been compressed past what the tool can hold. Any angle that lands short of target is telling you the elastic part of the deformation recovered after the punch released.

Radius also sits at the centre of the drawing conversation with a supplier. A forming shop receives a radius, a material grade, a temper and a thickness, and those four values pick the tooling. Change any one of them and the setup changes with it.

Inside a stamping program, bending runs as one forming operation among several rather than as a separate job shop service. The custom sheet metal bending page describes where that operation sits and what forms alongside it.

Inside Radius or Outside Radius: What the Drawing Actually Controls

Two radii describe every bend, and only one of them belongs on the drawing. Inside radius is the value read across the concave face, where the punch nose sits. Outside radius is read across the convex face, and it runs one material thickness larger than the inside figure.

By convention, a callout that reads only bend radius means the inside value. Forming charts and die design follow the same convention, because the punch nose and the die opening are what physically establish the geometry. Any drawing that intends the outside radius has to say so in words.

Misreading the convention costs one full thickness on every bend. On 2 mm stock, a supplier who reads an intended outside radius as an inside radius forms a bend 2 mm tighter than the design allows, and the outer fiber pays for it. Thin stock hides the error well enough to survive a first article, then turns up later as cracks in a batch.

Naming the convention in a drawing note takes one line of text and removes an entire class of first-article arguments, while also protecting the flat pattern, because the K-factor is indexed to the inside radius rather than to whatever number happened to be quoted.

The Neutral Axis and the K-Factor

Metal across a bend does not behave as one block. Fibers on the outside stretch in tension, fibers on the inside compress, and between the two runs a band that holds its original length. That band is the neutral axis, and its arc length becomes the developed length of the bend in the flat blank.

Three zones across one bend. The neutral axis sits inside the bend area rather than at mid-thickness, and its position shifts as the radius changes, so the value is calculated rather than assumed.

K-factor locates that band. Take the offset from the inside face to the neutral axis, divide it by the sheet thickness, and the result is K. Published sheet metal values fall roughly between 30 and 50 percent. The figure climbs as the radius grows against the thickness, so a tight bend on thin stock pulls the band inward while a generous radius lets it settle closer to the middle of the section.

Those bands are typical rather than universal. Exact figures depend on the alloy, the temper, the die and the forming method, and published tables from different sources disagree at the edges. Direction of travel is the dependable part of the story, and it runs one way: radius up, K-factor up, bend allowance up.

K-factor belongs to a material and a process rather than to a drawing template. A CAD library ships with a default value that is general-purpose rather than specific to your alloy, temper and die. Two suppliers can cut identical flanges to two different flat lengths while both follow the drawing, because each used a different K-factor and neither wrote it down.

Shops do not recalculate a customer K-factor. Whatever the model used goes straight to the laser or the strip layout, and the error arrives as flanges that measure short or long on the first article, with the blame heading toward the tool rather than the model.

From K-Factor to Flat Blank: Bend Allowance and Bend Deduction

Three numbers connect the radius on a drawing to the blank that gets cut. Bend allowance is the arc length along the neutral axis through the bend. Outside setback is the distance from the bend apex to the tangent point along the flange. Bend deduction is twice the setback minus the allowance, and that result comes off the total of the outside flange dimensions to give the flat length.

Order matters when the numbers are worked by hand. Fix the radius first, read the K-factor from the radius-to-thickness ratio, work the allowance and the setback from there, and leave the flat length until last. Working backwards from a target flat length usually means iterating until the two agree.

Recording the figure used at step two is what makes the calculation traceable later, because that is the step where two engineers most often disagree without noticing.

Two 90 degree bends on 5 mm cold-rolled steel show how much the radius carries. Both parts have outside flanges of 40 mm and 30 mm, so the flange sum is 70 mm in each case. Only the inside radius moves, and the K-factor is held at 40 percent so that the radius stays the single variable.

Second row carries the lesson. Nothing changed except the inside radius, and the blank came out 2 mm shorter at a single bend. Four bends at the generous radius therefore consume about 8 mm less strip than the same part drawn at one thickness, and every flange dimension on the drawing deserves a second look whenever the radius moves.

Real parts usually show a wider gap than this comparison does, because published tables raise the K-factor as the radius grows. Holding K constant keeps the arithmetic readable and still makes the point that radius and flat pattern are joined. A late radius change therefore rewrites the flat pattern, and the flat pattern is what the die is cut from.

Minimum Inside Radius by Material: The Table Designers Actually Need

Published forming references converge on a set of working ranges, and most of them express the limit as a multiple of thickness. Ranges below cover the grades a stamping shop processes. Conservative ends apply when the temper is hard, the bend runs with the grain, or the tooling is not yet known.

Rows marked case by case are the ones where published multipliers disagree or where the temper decides the answer, so treat those as confirmation items with the forming source rather than as numbers to write straight onto a drawing.

Two rows deserve a second look. Hardened 6061 is the outlier of the aluminum family, and published guidance puts it at several times the radius that soft aluminum or mild steel needs, which explains why it keeps appearing in cracked-flange stories. Ferritic stainless such as 430 sits below 304 on ductility even though both carry the stainless label, so a radius approved on one grade does not transfer to the other.

A radius table is not a test bend

A table like this is a starting point for a drawing callout rather than a substitute for a test bend. Where a part sits near the limit, one coupon from the actual coil settles more than a page of charts, and it costs almost nothing at the quotation stage.

Material selection touches everything else on the part, which is why precision metal stamping parts are usually reviewed as a package. Radius, hole position, material thickness, corner design and forming sequence all move together during DFM, and the cheapest changes are the ones made before tooling is released.

What Moves the Minimum: Temper, Work Hardening and Thickness

Three variables move a minimum radius further than the alloy name does, and all three are visible on the paperwork before a price is issued.

Where a drawing lands on a hardened aluminum grade with a one-thickness radius, the fix is a material or temper decision rather than a better punch. That decision belongs to the designer, and a factory cannot make it on the designer behalf without changing the part.

Ronghai processes carbon steel grades including SPCC, SPCD, SPCE, Q235 and Q345, stainless grades including 201, 304, 316 and 430, aluminum in 5052, 6061 and 6063, copper alloys, galvanized steel, HSLA and spring steel. Formability across that list runs from excellent on carbon steel to moderate on spring steel, which is a useful first screen before any radius is fixed.

Hole placement, corner design and material utilization sit in the same review, and the 10 DFM rules for stamping parts cover how those checks run alongside the radius decision.

Grain Direction: The Difference Between Half a Thickness and One

Rolled sheet shows a direction of grain left by the mill. A bend line set across that direction stretches fibers lying sideways to the bend, and that is the favorable case. Bend lines set parallel to it stretch fibers end to end, and that is the case that cracks.

Illustrative ranges for mild steel quoted in published forming guidance and fabricator data. The gap between the two rows is the price of orientation, and it gets paid on the drawing rather than at the press.

Gap between those rows is a design lever rather than a defect. On formable alloys, grain direction can move the safe minimum from around half a thickness to a full thickness. Harder tempers go further, and there the orientation can decide whether the flange forms or fractures. Any part with bends running in two directions usually has one orientation that is worse than the other, and that is the bend worth checking first.

Where orientation gets decided

Nesting decides which case a part gets. Inside a progressive die, the strip layout fixes the orientation of every part cut from the coil, so a rotation introduced to improve material utilization also rotates the grain direction of the critical bend. That trade deserves a look before the layout is frozen, because a coupon that bends cleanly in one orientation can crack in production at the other.

Designs that depend on bending with the grain have spent their own margin. Where a critical bend cannot be reoriented, grain direction belongs on the drawing as a note, so the strip layout has to respect it rather than optimize around it.

Hole-to-Bend Distance: Decoding the 3T Rule

A bend does not deform only the bend line. The worked zone spreads to either side of it, and any hole sitting inside that band moves with the material as the flange forms. What comes back is an oval, a teardrop, or a hole stretched toward the bend, and the cause lies in forming rather than in how the hole was made. Punching, laser cutting and drilling all produce the same result once a hole sits too close.

Published fabrication guidance gives the clearance as a formula rather than a constant, with the measurement taken from the nearest point of the hole rather than from its centre.

Thickness and inside radius are the two inputs, which is why the rule of thumb that circulates as keeping holes three thicknesses away from the bend line only holds when the inside radius equals one thickness. Increase the radius and the clearance grows with it. A 2 mm part with a 6 mm inside radius needs 10 mm of clear metal between the hole and the bend line rather than 6 mm.

Slots and tapped holes are more sensitive than clearance holes. The formula steps up for large features, and a hole sized for a shoulder bolt, or one matching a fixed pattern on a mating part, becomes a reject once it ovals, while an oversize clearance hole may tolerate the same distortion without complaint.

Stamping holds an advantage here that a press brake does not. Inside a progressive die, the pierce station and the form station occupy separate positions in the strip layout, so the distance between a hole and a bend line is set while the layout is being drawn. Where a hole genuinely has to sit close to a bend, piercing after forming is the remaining route, and that adds an operation along with its cost.

Springback: Why the Angle Opens After the Ram Lifts

A flange formed to a right angle rarely stays at a right angle. Once the punch backs off, the elastic share of the deformation returns and the angle opens. Springback is a material property rather than a fault, and the tool has to push past the target so the part relaxes back onto it.

Ordering the common materials helps. Recovery is smallest on soft low-carbon steel and on soft aluminum grades in the 3003 family, with AL5052 sitting in the middle. High-strength aluminum such as 6061 in T6 and work-hardening stainless such as 304 recover noticeably more, often by several degrees.

Three ways to compensate in a die

Forming method matters as much as the alloy. Air bending returns the most, while bottoming and coining pin the radius down and return less. Inside a stamping die, the compensating options are an overbend built into the form station, a restrike or coining station that settles the angle after forming, or a die correction made at tryout once the recovered angle has been measured.

Ronghai evaluates forming quality and springback during tool tryout, and necessary modifications are completed before sample production begins. A first article that follows then carries the angle the customer approved rather than the angle the die produced on its first stroke.

None of this means a supplier is struggling when the first stroke misses the target angle. Springback is what the material does, and the useful conversation is about how much overbend the tooling carries and how the recovered angle gets measured.

Above Three Millimeters: Where the Rules Shift

Thick stock changes the arithmetic in three places at once. Outer-fiber strain rises for a given radius, the force needed to form the bend rises, and the tooling has to be stiffer to hold the geometry. Published guidance for mild steel puts a half-millimeter sheet in a 1 mm to 2 mm radius range and 3 mm stock in a 6 mm to 9 mm range, and that spread is the material answer rather than a conservative habit.

Where the geometry will not allow the radius the thickness needs, the escapes are usually one of three. A bend can be made in several small increments rather than in one sharp stroke, which spreads the strain across more deformation. Grade can be swapped for one with more elongation, which buys radius at the cost of strength. Annealing restores ductility, and it adds a heat treatment step along with the handling around it.

Another consequence of heavy gauge sits outside the bend itself. Thickness variation in the incoming coil moves the formed dimensions, and the effect is larger on thick stock because the same variation represents a bigger share of the section. Incoming inspection covers thickness, width, flatness and hardness for exactly that reason.

Heavy gauge also narrows the choice of tooling. Higher forming loads demand more guide rigidity and a stiffer structure, and a form station that works comfortably on thin stock can need a redesign before it will hold the same geometry on 4 mm.

What to Put on the Drawing: A Radius Checklist

Eight lines of drawing text remove most of the radius arguments that reach the tool room, and none of them adds engineering work at the design stage.

Ronghai inspects bend angle at first article and again during in-process and final inspection, so a drawing that states the radius, the angle and their tolerances gives the inspection plan something to measure against. General tolerances on stamped parts follow the customer drawing, with published capability figures of 0.05 mm for general work and 0.02 mm where a part needs precision, on stock from 0.3 mm to 20 mm. The guide to realistic stamping tolerances covers how those bands are chosen and what each step costs.

Two drafting habits cause most of the trouble. Dimensioning to the formed part without developing the flat pattern produces a blank of the wrong length, and every callout can look correct while the parts come out over or undersize. Setting the radius at the published minimum with no margin leaves nothing for material lot variation, tool wear or grain effects, and the minimum then behaves as a cliff edge rather than a target.

Minimum radius is the number at which the material still forms on a good day. A drawing that sits on it has spent its margin before the first coil is opened, and a supplier who accepts that drawing without comment has taken on a risk that was never theirs to carry.

Working With a Stamping Supplier on Bend Radius

Four questions get to the useful answers when a program moves from drawing to tooling, and the replies say more about a supplier than the price does.

Send the drawing and the model together with the material grade, the thickness, the annual volume and the tolerances that will actually be inspected, and the radius question gets answered during engineering review rather than at the press. Ronghai runs bending alongside blanking, piercing, forming, deep drawn stamping parts and coining, so a part that needs a generous radius in one station and a tighter one in another becomes a tooling question rather than a process limit.

The Radius Callout Decides Three Things at Once

Bend radius looks like housekeeping in a CAD dialog box. It settles three separate outcomes at the same time: whether the outer fiber of the flange tears, what length of strip the blank requires, and how far the finished angle opens once the tool lets go.

Forming references treat the minimum radius as a limit rather than a preference, and they express it as a multiple of material thickness. One thickness on 2 mm steel means an inside radius of 2 mm, while half a thickness on the same stock means a 1 mm radius. Writing the limit in multiples of T lets one rule travel across gauges, because outer-fiber strain scales with thickness in the same way.

Three failure modes come out of one tight radius. Cracks open on the outside of the bend when the surface runs out of stretch. Wrinkles and a distorted profile appear on the inside, where the metal has been compressed past what the tool can hold. Any angle that lands short of target is telling you the elastic part of the deformation recovered after the punch released.

Radius also sits at the centre of the drawing conversation with a supplier. A forming shop receives a radius, a material grade, a temper and a thickness, and those four values pick the tooling. Change any one of them and the setup changes with it.

Inside a stamping program, bending runs as one forming operation among several rather than as a separate job shop service. The custom sheet metal bending page describes where that operation sits and what forms alongside it.

Inside Radius or Outside Radius: What the Drawing Actually Controls

Two radii describe every bend, and only one of them belongs on the drawing. Inside radius is the value read across the concave face, where the punch nose sits. Outside radius is read across the convex face, and it runs one material thickness larger than the inside figure.

By convention, a callout that reads only bend radius means the inside value. Forming charts and die design follow the same convention, because the punch nose and the die opening are what physically establish the geometry. Any drawing that intends the outside radius has to say so in words.

Misreading the convention costs one full thickness on every bend. On 2 mm stock, a supplier who reads an intended outside radius as an inside radius forms a bend 2 mm tighter than the design allows, and the outer fiber pays for it. Thin stock hides the error well enough to survive a first article, then turns up later as cracks in a batch.

Naming the convention in a drawing note takes one line of text and removes an entire class of first-article arguments, while also protecting the flat pattern, because the K-factor is indexed to the inside radius rather than to whatever number happened to be quoted.

The Neutral Axis and the K-Factor

Metal across a bend does not behave as one block. Fibers on the outside stretch in tension, fibers on the inside compress, and between the two runs a band that holds its original length. That band is the neutral axis, and its arc length becomes the developed length of the bend in the flat blank.

Three zones across one bend. The neutral axis sits inside the bend area rather than at mid-thickness, and its position shifts as the radius changes, so the value is calculated rather than assumed.

K-factor locates that band. Take the offset from the inside face to the neutral axis, divide it by the sheet thickness, and the result is K. Published sheet metal values fall roughly between 30 and 50 percent. The figure climbs as the radius grows against the thickness, so a tight bend on thin stock pulls the band inward while a generous radius lets it settle closer to the middle of the section.

Those bands are typical rather than universal. Exact figures depend on the alloy, the temper, the die and the forming method, and published tables from different sources disagree at the edges. Direction of travel is the dependable part of the story, and it runs one way: radius up, K-factor up, bend allowance up.

K-factor belongs to a material and a process rather than to a drawing template. A CAD library ships with a default value that is general-purpose rather than specific to your alloy, temper and die. Two suppliers can cut identical flanges to two different flat lengths while both follow the drawing, because each used a different K-factor and neither wrote it down.

Shops do not recalculate a customer K-factor. Whatever the model used goes straight to the laser or the strip layout, and the error arrives as flanges that measure short or long on the first article, with the blame heading toward the tool rather than the model.

From K-Factor to Flat Blank: Bend Allowance and Bend Deduction

Three numbers connect the radius on a drawing to the blank that gets cut. Bend allowance is the arc length along the neutral axis through the bend. Outside setback is the distance from the bend apex to the tangent point along the flange. Bend deduction is twice the setback minus the allowance, and that result comes off the total of the outside flange dimensions to give the flat length.

Order matters when the numbers are worked by hand. Fix the radius first, read the K-factor from the radius-to-thickness ratio, work the allowance and the setback from there, and leave the flat length until last. Working backwards from a target flat length usually means iterating until the two agree.

Recording the figure used at step two is what makes the calculation traceable later, because that is the step where two engineers most often disagree without noticing.

Two 90 degree bends on 5 mm cold-rolled steel show how much the radius carries. Both parts have outside flanges of 40 mm and 30 mm, so the flange sum is 70 mm in each case. Only the inside radius moves, and the K-factor is held at 40 percent so that the radius stays the single variable.

Second row carries the lesson. Nothing changed except the inside radius, and the blank came out 2 mm shorter at a single bend. Four bends at the generous radius therefore consume about 8 mm less strip than the same part drawn at one thickness, and every flange dimension on the drawing deserves a second look whenever the radius moves.

Real parts usually show a wider gap than this comparison does, because published tables raise the K-factor as the radius grows. Holding K constant keeps the arithmetic readable and still makes the point that radius and flat pattern are joined. A late radius change therefore rewrites the flat pattern, and the flat pattern is what the die is cut from.

Minimum Inside Radius by Material: The Table Designers Actually Need

Published forming references converge on a set of working ranges, and most of them express the limit as a multiple of thickness. Ranges below cover the grades a stamping shop processes. Conservative ends apply when the temper is hard, the bend runs with the grain, or the tooling is not yet known.

Rows marked case by case are the ones where published multipliers disagree or where the temper decides the answer, so treat those as confirmation items with the forming source rather than as numbers to write straight onto a drawing.

Two rows deserve a second look. Hardened 6061 is the outlier of the aluminum family, and published guidance puts it at several times the radius that soft aluminum or mild steel needs, which explains why it keeps appearing in cracked-flange stories. Ferritic stainless such as 430 sits below 304 on ductility even though both carry the stainless label, so a radius approved on one grade does not transfer to the other.

A radius table is not a test bend

A table like this is a starting point for a drawing callout rather than a substitute for a test bend. Where a part sits near the limit, one coupon from the actual coil settles more than a page of charts, and it costs almost nothing at the quotation stage.

Material selection touches everything else on the part, which is why precision metal stamping parts are usually reviewed as a package. Radius, hole position, material thickness, corner design and forming sequence all move together during DFM, and the cheapest changes are the ones made before tooling is released.

What Moves the Minimum: Temper, Work Hardening and Thickness

Three variables move a minimum radius further than the alloy name does, and all three are visible on the paperwork before a price is issued.

Where a drawing lands on a hardened aluminum grade with a one-thickness radius, the fix is a material or temper decision rather than a better punch. That decision belongs to the designer, and a factory cannot make it on the designer behalf without changing the part.

Ronghai processes carbon steel grades including SPCC, SPCD, SPCE, Q235 and Q345, stainless grades including 201, 304, 316 and 430, aluminum in 5052, 6061 and 6063, copper alloys, galvanized steel, HSLA and spring steel. Formability across that list runs from excellent on carbon steel to moderate on spring steel, which is a useful first screen before any radius is fixed.

Hole placement, corner design and material utilization sit in the same review, and the 10 DFM rules for stamping parts cover how those checks run alongside the radius decision.

Grain Direction: The Difference Between Half a Thickness and One

Rolled sheet shows a direction of grain left by the mill. A bend line set across that direction stretches fibers lying sideways to the bend, and that is the favorable case. Bend lines set parallel to it stretch fibers end to end, and that is the case that cracks.

Illustrative ranges for mild steel quoted in published forming guidance and fabricator data. The gap between the two rows is the price of orientation, and it gets paid on the drawing rather than at the press.

Gap between those rows is a design lever rather than a defect. On formable alloys, grain direction can move the safe minimum from around half a thickness to a full thickness. Harder tempers go further, and there the orientation can decide whether the flange forms or fractures. Any part with bends running in two directions usually has one orientation that is worse than the other, and that is the bend worth checking first.

Where orientation gets decided

Nesting decides which case a part gets. Inside a progressive die, the strip layout fixes the orientation of every part cut from the coil, so a rotation introduced to improve material utilization also rotates the grain direction of the critical bend. That trade deserves a look before the layout is frozen, because a coupon that bends cleanly in one orientation can crack in production at the other.

Designs that depend on bending with the grain have spent their own margin. Where a critical bend cannot be reoriented, grain direction belongs on the drawing as a note, so the strip layout has to respect it rather than optimize around it.

Hole-to-Bend Distance: Decoding the 3T Rule

A bend does not deform only the bend line. The worked zone spreads to either side of it, and any hole sitting inside that band moves with the material as the flange forms. What comes back is an oval, a teardrop, or a hole stretched toward the bend, and the cause lies in forming rather than in how the hole was made. Punching, laser cutting and drilling all produce the same result once a hole sits too close.

Published fabrication guidance gives the clearance as a formula rather than a constant, with the measurement taken from the nearest point of the hole rather than from its centre.

Thickness and inside radius are the two inputs, which is why the rule of thumb that circulates as keeping holes three thicknesses away from the bend line only holds when the inside radius equals one thickness. Increase the radius and the clearance grows with it. A 2 mm part with a 6 mm inside radius needs 10 mm of clear metal between the hole and the bend line rather than 6 mm.

Slots and tapped holes are more sensitive than clearance holes. The formula steps up for large features, and a hole sized for a shoulder bolt, or one matching a fixed pattern on a mating part, becomes a reject once it ovals, while an oversize clearance hole may tolerate the same distortion without complaint.

Stamping holds an advantage here that a press brake does not. Inside a progressive die, the pierce station and the form station occupy separate positions in the strip layout, so the distance between a hole and a bend line is set while the layout is being drawn. Where a hole genuinely has to sit close to a bend, piercing after forming is the remaining route, and that adds an operation along with its cost.

Springback: Why the Angle Opens After the Ram Lifts

A flange formed to a right angle rarely stays at a right angle. Once the punch backs off, the elastic share of the deformation returns and the angle opens. Springback is a material property rather than a fault, and the tool has to push past the target so the part relaxes back onto it.

Ordering the common materials helps. Recovery is smallest on soft low-carbon steel and on soft aluminum grades in the 3003 family, with AL5052 sitting in the middle. High-strength aluminum such as 6061 in T6 and work-hardening stainless such as 304 recover noticeably more, often by several degrees.

Three ways to compensate in a die

Forming method matters as much as the alloy. Air bending returns the most, while bottoming and coining pin the radius down and return less. Inside a stamping die, the compensating options are an overbend built into the form station, a restrike or coining station that settles the angle after forming, or a die correction made at tryout once the recovered angle has been measured.

Ronghai evaluates forming quality and springback during tool tryout, and necessary modifications are completed before sample production begins. A first article that follows then carries the angle the customer approved rather than the angle the die produced on its first stroke.

None of this means a supplier is struggling when the first stroke misses the target angle. Springback is what the material does, and the useful conversation is about how much overbend the tooling carries and how the recovered angle gets measured.

Above Three Millimeters: Where the Rules Shift

Thick stock changes the arithmetic in three places at once. Outer-fiber strain rises for a given radius, the force needed to form the bend rises, and the tooling has to be stiffer to hold the geometry. Published guidance for mild steel puts a half-millimeter sheet in a 1 mm to 2 mm radius range and 3 mm stock in a 6 mm to 9 mm range, and that spread is the material answer rather than a conservative habit.

Where the geometry will not allow the radius the thickness needs, the escapes are usually one of three. A bend can be made in several small increments rather than in one sharp stroke, which spreads the strain across more deformation. Grade can be swapped for one with more elongation, which buys radius at the cost of strength. Annealing restores ductility, and it adds a heat treatment step along with the handling around it.

Another consequence of heavy gauge sits outside the bend itself. Thickness variation in the incoming coil moves the formed dimensions, and the effect is larger on thick stock because the same variation represents a bigger share of the section. Incoming inspection covers thickness, width, flatness and hardness for exactly that reason.

Heavy gauge also narrows the choice of tooling. Higher forming loads demand more guide rigidity and a stiffer structure, and a form station that works comfortably on thin stock can need a redesign before it will hold the same geometry on 4 mm.

What to Put on the Drawing: A Radius Checklist

Eight lines of drawing text remove most of the radius arguments that reach the tool room, and none of them adds engineering work at the design stage.

Ronghai inspects bend angle at first article and again during in-process and final inspection, so a drawing that states the radius, the angle and their tolerances gives the inspection plan something to measure against. General tolerances on stamped parts follow the customer drawing, with published capability figures of 0.05 mm for general work and 0.02 mm where a part needs precision, on stock from 0.3 mm to 20 mm. The guide to realistic stamping tolerances covers how those bands are chosen and what each step costs.

Two drafting habits cause most of the trouble. Dimensioning to the formed part without developing the flat pattern produces a blank of the wrong length, and every callout can look correct while the parts come out over or undersize. Setting the radius at the published minimum with no margin leaves nothing for material lot variation, tool wear or grain effects, and the minimum then behaves as a cliff edge rather than a target.

Minimum radius is the number at which the material still forms on a good day. A drawing that sits on it has spent its margin before the first coil is opened, and a supplier who accepts that drawing without comment has taken on a risk that was never theirs to carry.

Working With a Stamping Supplier on Bend Radius

Four questions get to the useful answers when a program moves from drawing to tooling, and the replies say more about a supplier than the price does.

Send the drawing and the model together with the material grade, the thickness, the annual volume and the tolerances that will actually be inspected, and the radius question gets answered during engineering review rather than at the press. Ronghai runs bending alongside blanking, piercing, forming, deep drawn stamping parts and coining, so a part that needs a generous radius in one station and a tighter one in another becomes a tooling question rather than a process limit.