How a Press Brake Works: Force, Tooling, and Accurate Bends
What a press brake does: turns flat sheet metal into controlled bends A press brake is a machine tool that…
For an initial check, calculate:
Minimum flange length ≈ 0.7 × V
Here, V is the actual opening of the selected V-die—not the material thickness or an assumed opening that may change during tooling selection. This estimate applies to a standard air bend near 90 degrees. By itself, it does not approve the part for production.
A flange must be long enough to remain supported on the die shoulder as the punch drives the sheet into the opening. If the flange is too short, its edge may slip into the V or lose stable support, resulting in an unreliable bend or preventing the bend entirely.
For example, with a 16 mm V-opening:
Minimum flange ≈ 0.7 × 16 mm = 11.2 mm
Treat 11.2 mm as an initial estimate of fit and support. Some references use a more conservative near-limit check of approximately 0.77V. For the same die, this gives 12.32 mm, commonly rounded to 12.3 mm. A flange near either limit requires a tooling-specific check because the punch radius, material thickness, bend angle, die shoulders, and part support can affect the workable minimum.
The calculated limit and the drawing dimension must refer to the same geometry. Shops and drawings may define a flange using an inside dimension, an outside dimension, a tangent point, or an edge-to-theoretical-sharp dimension. These values are not automatically interchangeable because material thickness and bend radius shift the reference point.
Before comparing a drawing dimension with 0.7V:
A direct comparison without this conversion may make a short flange seem acceptable or cause a flange that would actually fit to be rejected.
The expression 8T, where T represents material thickness, is commonly used as an initial guideline for selecting a V-die opening:
V ≈ 8T
It addresses a different question than 0.7V. The 8T guideline recommends a die opening, while the 0.7V rule determines whether the flange is long enough for the opening actually selected.
When both initial rules apply:
Minimum flange ≈ 0.7 × 8T = 5.6T
The 5.6T result is based on two assumptions: an 8T die opening and a flange estimate of 0.7V. If the die opening changes, the thickness-based result changes accordingly.
Thickness multiples are shortcuts associated with specific tooling assumptions or operating goals. They may indicate die selection, basic shoulder support, a preferred working margin, or another shop-specific threshold. Therefore, they are not interchangeable definitions of minimum flange length.
For example, 5.6T follows mathematically when V = 8T and the flange estimate is 0.7V. A 4T rule does not result from those same assumptions; it reflects a different die-opening ratio, geometry, or shop criterion. Before applying any thickness multiple, identify what the rule is intended to calculate.
The release check should focus on the actual setup: verify the punch and die, material thickness, bend geometry, dimension convention, backgauge contact, and tool clearance. Only then can the preliminary 0.7V estimate be used to support a manufacturability decision.
Let T represent the material thickness. Once the actual V-die opening is known, this table converts common die-opening ratios into preliminary minimum-flange estimates for a 90-degree air bend.
| Actual V-die opening | Calculation | Approximate minimum flange |
|---|---|---|
| 6T | 0.7 × 6T | 4.2T |
| 8T | 0.7 × 8T | 5.6T |
| 10T | 0.7 × 10T | 7.0T |
| 12T | 0.7 × 12T | 8.4T |
These values are planning estimates, not fixed limits for every press brake operation. Use the row corresponding to the die opening actually installed, then verify the punch and die, material, bend geometry, backgauge contact, and tool clearance.
With an actual opening of V = 6T:
Minimum flange ≈ 0.7 × 6T = 4.2T
A smaller V-opening results in a shorter estimated minimum flange, but it also affects the required forming force and the resulting bend geometry. Before using 4.2T as a design target, confirm that the material and tooling are suitable for the 6T opening.
With V = 8T:
Minimum flange ≈ 0.7 × 8T = 5.6T
The 5.6T value applies only when the selected opening is eight times the material thickness. It should not be applied to a job that ultimately uses a different die.
With V = 10T:
Minimum flange ≈ 0.7 × 10T = 7T
In this case, the flange requires an estimated bend-line-to-edge length equal to seven times the material thickness. Increasing the opening from 8T to 10T therefore raises the estimate from 5.6T to 7T.
With V = 12T:
Minimum flange ≈ 0.7 × 12T = 8.4T
Under this rule, a wider opening requires a longer flange because the sheet must span a greater distance while remaining supported by the die shoulders. A flange that works with a smaller die may become too short if the tooling selection changes.
For T = 2 mm and an actual V = 16 mm, the opening is:
V ÷ T = 16 mm ÷ 2 mm = 8T
Use the 8T row or calculate it directly:
Minimum flange ≈ 0.7 × 16 mm = 11.2 mm
The table produces the same result:
5.6T × 2 mm = 11.2 mm
Use 11.2 mm as the initial manufacturability screen, measured according to the same flange-dimension convention used by the shop. Before releasing a flange near that value, confirm that it remains supported on the die shoulders and can contact the backgauge without colliding with the punch, die, or surrounding part geometry.
A short flange becomes unstable when its edge can fall into the V rather than remaining supported on the die shoulder. Once that support is lost, the tooling no longer controls the material as intended, so dimensional fit alone cannot confirm that the bend is manufacturable.
In air bending, the sheet initially spans the die opening as the punch presses it into the V. The contact points on the die shoulders support the sheet as it rotates and the bend forms.
The flange must therefore extend far enough from the bend line to its outer edge to maintain stable contact with the shoulders throughout the forming stroke. It must be long enough to bridge the tooling as the bend forms, not merely long enough to enter the space between the punch and die.
If the flange is too short, its edge can move beyond the supporting shoulder and drop into the die opening. This changes the contact geometry during the stroke: the flange may slide rather than rotate predictably around the bend region.
The resulting unsupported load can curl the edge, distort the leg, or twist the part. Because the point at which support is lost may vary with placement and normal setup variation, the final bend angle may also differ from part to part. A successful trial bend alone does not establish a repeatable production setup when the flange is operating at the support limit.
The V-die opening determines the distance the sheet must bridge. A wider opening places the die shoulders farther apart, requiring a longer flange to maintain support. A narrower opening brings the shoulder closer to the bend line and may allow a shorter flange, provided the punch, die, material, forming force, and required bend geometry are compatible.
This is why the actual installed opening governs the preliminary minimum-flange check. The estimate represents a geometric support condition; it does not guarantee that every bend above the calculated value will run reliably.
Thickness still matters because it affects which die openings and punch geometries are suitable for the job. Thicker sheet commonly requires a wider opening, which then increases the flange length needed for shoulder support. Two parts with the same material thickness can therefore have different practical minimum flange lengths when formed with different dies.
Do not approve a short flange based on thickness alone. First select a suitable punch and die for the material and bend, then check the flange against the actual opening and verify shoulder support, backgauge contact, bend-sequence clearance, and tool clearance.
A thickness-based rule can screen a design, but it cannot approve it. The usable minimum depends on the actual V-die opening, punch geometry, material, bend angle, and forming method. Select tooling that can produce the specified bend without excessive force, unacceptable marking, cracking, or interference, then calculate the flange requirement against that tooling. As a practical next step, assess the ADH Machine Tool WC67K Series NC press brake and its proposed tool set against the required bend geometry, force, support, and clearance before releasing the design.
Define the bend before selecting the tools:
For concrete tooling and equipment specifications covering CNC bending and related sheet-metal processes, use the ADH Machine Tool downloadable product resources to compare suitable options for the defined bend requirements.
Also confirm the material direction, surface-finish requirements, and any bend-radius tolerance that could limit the tooling choice. These details can rule out a setup that appears acceptable based on thickness alone.
Do not choose the smallest available opening simply to make a short flange pass. A narrower opening may reduce the geometric flange requirement, but it also increases forming-force demand and can alter the resulting radius, shoulder pressure, surface marking, and cracking risk.
A wider opening generally reduces the required force but spans more material, increasing the flange length needed for stable support. Choose the opening by evaluating these constraints together:
The selected opening is a tooling decision, not a value that should be adjusted solely to make the flange calculation pass.
The punch tip must be compatible with the required radius, material, die opening, and forming method. An unsuitable tip radius can concentrate strain, promote cracking, or leave an imprint on the bend. A punch that is too broad or has the wrong profile can also interfere with an adjacent flange, return, embossment, or previously formed bend.
Check the entire punch profile, not just the tip. The punch angle, width, height, and relief determine whether the tool can reach the bend throughout the stroke. Where nearby geometry causes interference, an acute, gooseneck, or relieved profile may be necessary, but any substitution must still satisfy the radius, force, and tooling-capacity requirements.
Once the actual V-die opening is known, use the planning estimate for a 90-degree air bend:
Estimated minimum flange = 0.7 × actual V-die opening
For a hypothetical setup with a 24 mm opening:
Estimated minimum flange = 0.7 × 24 mm = 16.8 mm
The 16.8 mm result is the calculated geometric minimum for that opening, not a machine limit or a production guarantee. If the shop switches to a 30 mm opening, the estimated minimum becomes 21 mm. The flange must be reevaluated rather than approved based on the previous result.
Apply the shop’s established flange-dimension convention consistently. A measurement taken from the bend line is not interchangeable with an outside dimension unless bend deductions and the drawing convention are handled correctly.
A flange designed exactly at 0.7V provides no allowance for setup or process variation. Tool wear, variation in sheet thickness, part-positioning error, springback, and inconsistent backgauge contact can turn a marginal trial bend into an unstable production process.
No universal margin is suitable for every material, machine, tolerance, and batch size. Establish it with the fabricator based on the selected tooling and required process capability. If no extra length is available, treat the feature as a near-limit condition that requires a documented machine-and-tooling trial rather than assuming the formula has approved it.
Tool selection therefore determines only the theoretical minimum. Release still requires confirmation that the flange can contact the backgauge, clear the punch and die throughout the full stroke, and withstand the planned bend sequence on the available press brake.
A flange that meets the geometric estimate can still fail in production. The backgauge may not locate it consistently, nearby geometry may interfere with the tooling, a cutout may eliminate critical support, or the required force may exceed the setup rating. Treat the estimate as permission to evaluate the actual operation, not as permission to release the drawing.
For a near-limit flange, the fabricator should establish the production margin and trial requirements for the selected machine, tooling, material, tolerances, and batch size. The trial should verify stable positioning, full-stroke clearance, acceptable dimensions and bend angle, sufficient support, and permitted forming force.
The backgauge fingers require a stable surface to establish the bend-line position. Verify that they can physically reach the intended gauging surface without entering the die space, contacting nearby features, or requiring the operator to balance the blank on an edge.
Contact must also be repeatable. A very short flange, tapered edge, rounded corner, notch, or flexible sheet may contact the gauge differently from one cycle to the next. This can cause variations in flange length and bend angle, even when the flange is nominally long enough for the die.
Evaluate the setup on the actual press brake, including the gauge-finger shape, support arms, tooling position, and planned bend sequence. If stable contact cannot be achieved, possible remedies include changing the gauging surface or bend sequence, adding a temporary locating tab, using a dedicated fixture, or forming a longer flange and trimming it afterward. For operations that require repeatable setups and CNC-controlled bending, the ADH Machine Tool CNC press brake provides a relevant production solution within the company’s CNC-based sheet metal equipment portfolio. Each remedy or equipment choice alters the process and must be included in the manufacturing plan.
Checking clearance only at the bottom position is insufficient because the workpiece rotates as the ram moves. During this rotation, the part may strike the punch body, die shoulders, punch holder, ram, backgauge, or machine frame before it reaches the required angle.
Model or trial the entire motion using the actual punch and die profiles, including their holders. Pay particular attention to return flanges, hems, boxes, channels, and deep parts. The punch tip may reach the bend line while the wider punch body or holder collides with an existing wall.
A relieved or gooseneck punch may provide the necessary clearance, but it is not an automatic substitute. Its radius, angle, load rating, and compatibility with the die must still meet the bend specification.
The bend sequence determines the geometry surrounding each bend when it is formed. A blank that clears the tools during the first operation may become impossible to position after an adjacent wall or return lip is formed.
Review each bend in sequence and track how the part enters, rotates within, and exits the tooling. Account for embossments, louvers, hardware, offsets, and previously formed bends, as any of these can obstruct rotation or prevent the workpiece from resting correctly on the die.
Changing the sequence may resolve one collision while creating another or eliminating the surface required for backgauging. If no sequence works, the design may require greater spacing, a shorter return, a different tool profile, a removable tooling section, or a separate forming operation. The bend simulation and shop trial must reflect the planned production sequence rather than an isolated bend.
Support depends on the material that actually contacts the die shoulders, not on the flange’s nominal outline. A hole, edge notch, or cutout near the bend can leave part of the workpiece unsupported, allowing it to dip, twist, or slide as the punch applies force.
Inspect support across the full bend length. Pay particular attention to interrupted edges and large corner reliefs, especially where the remaining material forms narrow tabs. Features near the bend may also distort as the material stretches and flows, even when sufficient support remains to complete the bend.
Possible corrections include relocating the feature, reducing its size, retaining temporary support tabs, creating the feature after forming, or choosing a different process. Do not assume that one adequately supported section of the flange will stabilize all interrupted sections.
Before comparing a drawing dimension with a minimum flange requirement, determine what the dimension represents. A flange may be dimensioned to an inside surface, an outside surface, a bend tangent, or an outside mold line. These values are not interchangeable.
The flat pattern is developed using bend allowance or bend deduction. Bend allowance accounts for the developed length through the bend region, while bend deduction converts specified formed dimensions into the required flat length. Both depend on the shop’s material and tooling assumptions, including thickness, inside radius, and bending behavior.
Confirm that the released flat pattern is based on the same tooling assumptions used for the flange check. Changing the die can alter the formed radius and bend deduction, affecting both the final dimension and the amount of straight material available for gauging and die support. Recalculate the flat pattern instead of adjusting the brake program to compensate for an incompatible blank.
Use the tooling manufacturer’s chart for the selected material, thickness, die opening, bend length, and forming method. Compare the required force with the capacity of the press brake and the ratings of the punch, die, holders, and sectional tooling. Machine capacity may also depend on the load’s position and distribution across the bed, so total press capacity alone is insufficient. For long-workpiece applications that require a CNC-based bending solution, the ADH Machine Tool tandem press brake provides a relevant option to evaluate against these tooling, force, and load-distribution requirements.
If the required force exceeds any applicable rating, do not approve the setup. A wider die opening may reduce the force, but it also changes the formed radius, bend deduction, and minimum usable flange. Changing the punch, reducing the length formed in each operation, or choosing another forming process may likewise introduce new dimensional or support constraints.
When the flange is close to any practical limit, conduct a documented trial using the intended setup and inspect more than the first successful part. Acceptance criteria should address gauge repeatability, bend angle, flange dimension, feature distortion, marking, clearance, and permitted load. Manufacturer data and demonstrated process capability take precedence over a general estimate. If they indicate that the setup is unsuitable, the flange requires redesign or a different forming method, material assumption, or bend rule. For help evaluating the intended setup, tooling, automation options, or machine requirements, contact ADH Machine Tool, whose R&D capabilities include press brakes, laser cutting, industrial automation, and intelligent equipment.
The 0.7V estimate applies to one specific case: a typical 90-degree air bend in which the sheet remains supported by the shoulders of a V-die. If the included angle, forming method, inside radius, material behavior, or surrounding part geometry changes, the estimate may no longer reliably predict adequate support or clearance.
Do not address these exceptions by applying an arbitrary percentage to 0.7V. First classify the operation, then evaluate the selected punch, die, material, and full forming motion. This distinction matters because some exceptions require a longer flange, while others call for different tooling, a revised sequence, or an entirely different process.
An acute bend has an included angle of less than 90 degrees. As the bend closes, the flange rotates farther toward the punch and must remain supported while clearing the punch body, die, and any previously formed walls. Therefore, the standard 0.7V estimate may be too short.
Some tooling guidance recommends approximately 1.1 times the die opening or more for certain acute-die applications. Treat this value as tooling-specific guidance rather than a universal replacement rule. The required length depends on the target angle, die angle and opening, punch profile, material thickness, and the way the workpiece contacts the die shoulders throughout the stroke.
An obtuse bend, with an included angle greater than 90 degrees, also differs from the standard case. It may seem less restrictive because the flange rotates through a smaller angle, but the support position, backgauge contact, and dimension used to define the flange still vary with the geometry. Use an angle-specific calculator or the tooling manufacturer’s method, then examine the actual contact points instead of assuming that 0.7V remains conservative.
Air bending forms the angle primarily by controlling punch penetration without pressing the sheet fully against the die faces. Bottoming presses the material more completely into the die, whereas coining applies much higher localized pressure to imprint the tooling geometry into the bend.
These processes change where the material contacts the tools, how the radius forms, and how much force the operation requires. A flange that seems adequate under an air-bend estimate may interfere with the die, fail to seat properly, or exceed the rating of a punch, die, holder, or machine when bottomed or coined.
Evaluate the flange using the actual matched tool set and forming method. Verify the tool angles, punch radius, die geometry, material thickness, required force, and full-stroke clearance. The 0.7V estimate may still be useful as an early warning, but it cannot validate a bottoming or coining setup.
A large inside radius cannot be created simply by replacing the punch with one having a larger radius in an otherwise standard setup. The material must wrap around the punch while remaining supported, and the punch body must clear the flange as it rotates. The process may require a wider V-die, radius tooling, staged forming, or another specialized method.
A wider opening places the die shoulders farther apart. This generally increases the straight-edge length required to prevent the flange from dropping into the opening, so a design may achieve the desired radius but lose flange manufacturability. The modified radius also affects the flat pattern and final flange dimensions.
Confirm the intended radius-forming method before finalizing either the die opening or the blank dimensions. The key question is whether the actual leg remains supported and clears the tooling throughout the full stroke, not whether its nominal dimension satisfies a standard 90-degree calculation.
Material thickness alone does not define forming behavior. Stainless and high-strength materials may require more force and exhibit greater springback than lower-strength material of the same thickness. A shop may address this with a different die opening, punch radius, angle-compensation method, or forming process.
Each response affects another constraint. A wider die opening can reduce the required force, but it also increases the preliminary minimum-flange estimate and may change the formed radius. A tighter setup used to control geometry may increase tool loading or mark the material. Adding a nominal flange margin without resolving these conflicts does not make the operation suitable.
No single additional safety percentage applies to every demanding material. Use material-specific tooling data and verify the proposed setup against allowable loads and dimensional requirements. Where production variation is important, the margin must be based on demonstrated capability with the specified material and setup, not on a generic allowance.
These features are sequences or compound forms, not isolated 90-degree flanges. A hem typically includes an initial acute bend followed by closing or flattening. An offset or Z-bend creates two closely spaced bends whose spacing must accommodate the offset tooling or planned sequence. Channels and tight returns can trap the punch, collide with the holder, or eliminate the surface required for backgauging.
Evaluating each leg independently using 0.7V overlooks these interactions. Model or trial the entire operation with the actual tool profiles and bend order. Check where the part rests, how it is gauged, whether each leg remains supported, and whether the formed shape can enter and exit the tools.
This is also where the rule’s apparent simplicity becomes dangerous: every individual flange may pass its arithmetic check while the part is still impossible to form. Once the job has been identified as an exception, the next decision is practical: increase the flange or bend spacing, change the punch or die, revise the bend sequence, or assign the feature to a process designed for that form.
When a flange is below the preliminary minimum for the selected V-die, first determine what prevents the bend. The edge may not be supported by the die shoulders, the backgauge may lack sufficient surface to locate the part, or a previously formed wall may collide with the punch, holder, or die. Each type of failure requires a different remedy.
Begin with the least disruptive approved change: a narrower die to provide support, a revised bend order to provide clearance, or temporary material for gauging. If standard tooling still cannot produce the feature reliably, assess specialty or custom tooling. Every change introduces new constraints, so recalculate the setup and inspect the complete forming motion before releasing the design.
A narrower V-die lowers the preliminary minimum-flange estimate because its shoulders are closer together. For a typical 90-degree air bend, the familiar 0.7V estimate can be recalculated using the proposed opening, but satisfying that calculation does not by itself approve the substitution.
The narrower opening concentrates the forming force over a smaller area. Verify the required tonnage against the allowable load for the press brake, punch, die, holders, and tooling length. A machine with sufficient total capacity may still be unsuitable if the rating of a tool or holder would be exceeded.
Also verify the bend that the smaller opening will produce. Narrower dies tend to create tighter inside radii and increase strain on the outside of the bend. This can increase cracking risk in hard alloys, stainless steel, or material bent tightly relative to its thickness. The different radius may also affect the flat pattern and finished flange dimensions.
Higher contact pressure can produce more pronounced die marks. Determine whether this is acceptable for polished, prefinished, aluminum, stainless, or cosmetic parts. Protective covers or suitable tooling may reduce marking, but they can also affect angle consistency and should be included in the trial setup.
Approve the narrower die only when its rating, expected radius, material compatibility, surface finish, and dimensional effects all meet the job requirements. It is a calculated setup change, not a universal solution for a short flange.
If the flange has sufficient die support but the formed part collides with the tooling, changing the V-opening will not solve the actual problem. Review the bend sequence and trace the part through loading, forming, and removal. Performing the difficult bend earlier may provide clearance that is lost after an adjacent wall or return is formed.
Sequence changes affect more than access. Verify that a usable surface remains for each subsequent backgauge operation and that the operator can securely hold the evolving shape. Also recheck accumulated dimensions, because changing which bends are located from formed edges can alter how variation builds through the part.
Use a gooseneck punch when a straight punch or holder would contact a return flange, channel wall, or box side. Its recessed profile provides clearance for the formed wall, but the punch must still have the required tip radius and angle and remain within its load rating. Check clearance at full stroke and during part removal; clearance at the finished position alone does not eliminate the possibility of a collision earlier in the motion.
A flange may be geometrically formable yet too short to contact the backgauge consistently. In that case, add a temporary tab or sacrificial extension to the blank so the gauge fingers can locate against a larger, stable surface. Form the part using the extension, then remove it through a defined trimming operation.
Position the added material so it will not collide with the punch, die, gauge fingers, or adjacent features as the part rotates. The extension must locate the intended bend line without creating an ambiguous contact point. Removing it must also preserve the required edge condition and finished dimension without damaging the formed flange.
Document the tab geometry, gauging surface, trimming method, and inspection datum. Without these details, temporary material simply transfers the uncertainty from bending to trimming.
When conventional V-die support is still inadequate, select specialty tooling based on the failure mechanism.
These options do not maintain the assumptions underlying a standard V-die calculation. Follow the tooling supplier’s limits and evaluate the actual contact points, formed radius, required force, surface condition, and extraction path.
A near-limit calculation should result in a controlled test, not an informal production experiment. Use the specified material and thickness, the intended punch and die, the planned tooling protection, and the proposed bend sequence. A substitute material or wider test coupon may conceal the cracking, support, or gauging issue under investigation.
During testing, verify that the flange remains supported, the gauge contact is stable, and no part of the workpiece collides with the punch, die, holder, gauge, or machine throughout the complete stroke. After forming, inspect the bend angle, inside radius, flange dimensions, cracking, distortion, and surface marking. Repeat the bend enough times to determine whether the result is controllable rather than a single favorable outcome.
Record the successful tool identifiers, V-opening, punch radius, sequence, gauge method, machine settings, material specification, protective tooling, and inspection results. The tested setup—not the short-flange estimate alone—is what makes the part ready for production release.
Release the part only after the following five checks connect the drawing to a specific, workable press-brake setup. The flange estimate is an initial screening tool; the approved setup is the production requirement.
Begin with the material grade and actual thickness, required bend angle, and inside bend radius. These inputs affect tooling selection, formed geometry, and the required force.
Specify exactly how the flange is dimensioned: to the bend tangent, the inside intersection, or the outside edge. Do not compare a drawing dimension with a minimum-flange rule unless both use the same reference points.
Identify the intended punch angle and nose radius, the die angle and V-opening, and whether the operation uses air bending, bottoming, or coining. Confirm that the tools accommodate the specified material thickness and can produce the required angle and radius.
The 0.7 x V estimate serves as a starting point for a standard 90-degree air bend. Do not apply it unchanged to acute-angle work, bottoming, coining, wipe bending, rotary tooling, or other processes with different contact geometry.
For a standard 90-degree air bend, calculate:
Preliminary minimum flange = 0.7 x actual V-die opening
Use the opening of the die that will actually be installed, not a generic opening chosen from a thickness table. Keep the flange measurement convention consistent with the rule or tooling reference used for comparison.
A result close to the calculated minimum indicates a setup-risk part; it does not demonstrate that the bend will run reliably. Send the part for tooling review and, when necessary, conduct a controlled test using production material and the intended tools.
Check the complete setup before release:
If a narrower die, different punch, revised sequence, temporary gauge tab, or specialty tool is needed, repeat the calculation and every affected verification step. Any remedy changes the approved setup and may also affect the radius, force, surface condition, or dimensional result.
Record the material specification and thickness, bend angle and radius, flange measurement convention, forming method, punch and die identifiers, actual V-opening, calculated preliminary minimum, bend sequence, gauging method, and any handling or inspection requirements.
For a near-limit part, also document the verified machine settings and controlled-test results. Release the part based on this documented setup, not on 0.7 x V alone. If the tooling, material, or process changes, repeat the flange check and all affected setup validations.
