Sheet Metal & Press Brake for Fusion 360 — User Guide

Sheet Metal & Press Brake turns an Autodesk Fusion sheet-metal part into what the press-brake operator needs, and makes the flat pattern match your own brake:

• Bend Sheet: the bends of the flat pattern in a suggested bend order, the back gauge X for every step, flip and rotate notes and checks, written as a shop PDF, a layered flat DXF and a bend-program CSV.
• Apply Bend Rule: a Fusion sheet-metal rule from your material, die and punch, so the flat pattern and its DXF match the brake.
• Calibrate from Test Bend: the real bend deduction and K-factor from one bent test strip.
• Press Brake Library: your machines, punches, dies and materials.

It also creates manufacturing-aware sheet-metal forms: louvers, lances, dimples, emboss/deboss forms, bridge forms, knockouts, extruded holes, reinforcing beads, and gussets, with Tab & Slot joints and a manufacturing export.

In the Design workspace, open the Sheet Metal tab and find the Press Brake panel. To reopen this guide from Fusion, choose About Sheet Metal and Press Brake, then Open Help.

Press brake: quick start

1. Open Press Brake Library once. The starter library holds published catalogue and standard values, each with its source in its notes: eight real machines, the tools of the three tooling systems and 23 sheet materials (see Starter library below). Add your own machine if it is not there, keep the tools you own (delete the others or leave them), and enter the load ratings stamped on your tools.
2. Select the part and run Apply Bend Rule. Pick the machine first (the die and punch lists show the tools that fit it), then the material, thickness, die and punch. The dialog shows the inside radius, the K-factor, the bend deduction at 90°, the minimum flange and the force per metre before anything changes. OK creates or updates a rule named after the setup (for example S235 3 mm V24) and makes it the part's active rule.
3. Optional: bend a test strip and run Calibrate from Test Bend. Apply Bend Rule then uses the measured values for that material, thickness and die.
4. Run Bend Sheet. Check the suggested bend order (Move up / Move down change it), read the checks, then choose a folder for the PDF, DXF and CSV.

Press Brake Library

Pick Edit or add an entry, a category and an entry (or + New entry), change the values and click OK. Lengths use the document units. The library is a local JSON file; import merges another library (an entry with the same id is replaced, a same-name entry is kept under a new name), export writes the whole library for another computer, and Restore the starter entries adds back deleted or changed starter entries without touching your own. Test-bend calibrations are stored in the same file and can be deleted there. A library saved by an earlier version loads as it is: its entries get the tooling system Other, and their outlines are drawn from their values until you give them their own.

Minimum inside radius by thickness. Material standards give the minimum radius per thickness band, in mm or as a multiple of t. Write the bands up to each thickness in mm: 1.5: 1.6 mm; 2.5: 2.5 mm; 3: 3 mm (EN 10025-2) or 3: 0.25 t; 6: 0.5 t; *: 1 t (EN 10149-2), * for any thicker sheet and - where the standard gives no value. The bands win over the single multiple of t. Where the standard splits by rolling direction, the starter values are for bend lines across the rolling direction; bends along it need a larger radius.

Tools made for one machine (the Langmuir Titan set, for example) name it under For machine: they are suggested first for that machine.

Tooling systems. European (Promecam), American and New Standard (Wila/Trumpf) tools do not fit each other's clamps. Bend Sheet and Apply Bend Rule list the punches and dies of the chosen machine's tooling system; a tool or machine set to Other fits every machine. Choose the machine first: a die or punch that does not fit it is replaced by the suggested one (a bending die near 8 × t, a straight punch). In an inch design the first American-tooling machine is the default.

Optional values are 0 when not given; the checks that need them are skipped and listed as not checked. Enter the load rating stamped on your own punches and dies: it is the limit the maker guarantees.

Tool and machine outlines

The collision checks, the 3D view and the 3D check need the outline of every punch and die and of the machine's upper beam and back-gauge finger. Every entry has one, from the best source there is:

• Its own outline: picked in a Fusion sketch with Outline from sketch, imported with Import from DXF... (a tool maker's CAD drawing) or entered as points. It always wins.
• The maker's drawing of a starter tool: UKB CAD drawings, and the AMADA, WILA, Wilson Tool and Langmuir drawings measured to scale: 37 of the 38 starter punches and 70 of the 87 dies. Most of the others are drawn from the maker's published dimensions. It is used while the entry keeps its catalogue values.
• Drawn from its values: a straight, acute, gooseneck or flattening punch from its height, width, angle, tip radius and relief; a 1-V, acute, multi-V or hemming die from its V, angle, shoulder radius, width and height. Change a value and the outline follows. A value the entry does not give takes a typical one, and the outline says so. An offset tool or a tool of style Other needs its own outline.
• The upper beam is drawn from the punch shoulder (its clamping face) on the tang axis, so it sits on whichever punch a step uses: the machine's own outline, else a clamp and beam from its upper clamp width and height and beam thickness, else the typical clamp of its tooling system. The starter machines carry their makers' clamp drawings where they are published (Durma, AMADA, SafanDarley, Bystronic, Langmuir), else an equivalent clamp (TRUMPF: the WILA clamp made to replace it; Harsle: a 100 mm European holder). An older beam outline drawn relative to the punch tip is still used as it was entered. Without a finger outline the back gauge is a typical two-step finger.

Press Brake Library shows each entry's outline under its values, blue when it is exact (its own or the maker's drawing) and orange when it is drawn from the values; the line above it says where it comes from. The checks list every outline that is not exact under Assumed, in the dialog and on the bend sheet. Auto tools + order tries tools with exact outlines first.

Tool length: one piece or a sectioned set

A punch or die is one piece of its Working length, or a Sectioned set: the pieces the shop has, in mm or with "in", horns marked L and R, 2x15 for two pieces, *x835 for as many 835 mm pieces as needed. AMADA's 800 mm set reads 100L, 10, 2x15, 20, 40, 50, 150, 300, 100R. For each step the add-in builds a station from the set the way press-brake controllers and offline programs do:

• It covers the bend line, short by at most the machine's Tool shorter than the bend line by at most (5 mm unless set: the Delem "tool length tolerance", the Cybelec "negative tolerance"). A short station is centred, half the shortfall at each end.
• It stops where the inside radius of a bend formed across its bend line starts, on its own side of the sheet: flanges formed up stop the punch, flanges formed down stop the die. A tool pushed into a formed radius bulges the corner. Tool end clear of a formed bend adds room for placing the part by hand.
• Between two formed bends (a box) it is as long as the room allows; otherwise it may run past the bend line and takes the fewest pieces, one solid piece when one covers it. Next to a single formed bend it is moved to the free side.
• Pieces butt. Gap between tool pieces at most, a multiple of the thickness, lets them spread to reach the length: up to 1 t on steel and 0.5 t on soft aluminium leave no visible mark (WILA).
• A horn goes at each end that faces a formed bend, then the long pieces at the ends and the short ones inside (AMADA, Cybelec). The horn's relief (setback x tip band x height, 35 x 10 x 35 for the AMADA AFH ear) lets the return of a formed wall pass: the 3D view and the 3D check model it. A horn without a relief is checked as a plain piece.
• Max force, sectioned and Max force on a horn are checked on the steps whose station uses the set or a horn.

The bend sheet, the PDF tools table and the CSV give each step's station, for example 295 mm (2.3 short): 100L + 50 + 15 + 15 + 100R. The starter tools carry their makers' pieces: AMADA's 800 mm set with ears plus solid 835 and 415 mm, WILA's /2 550 mm set with horns plus /1 515 mm pieces, Wilson Tool's X 35.875 in set with ears plus 36 and 18 in, the Langmuir Titan kits; the UKB tools stay one piece of 415 or 835 mm. A tool with neither a working length nor a set is taken as long as the bend line and listed under Assumed. Restore the starter entries loads the sets into a library saved before.

Starter library

The library includes 12 UKB stock-tool entries with sections sampled from original manufacturer CAD: four punch and two die shapes, each in 415/835 mm single-piece lengths. See tool sources. A Source URL field records the source of each entry. Installed holders, machine and backgauge geometry still need shop-specific data. Existing saved libraries are retained; restoring starter entries adds the new tools and resets edited starter entries. Duplicate custom reground starter tools first.

Every starter entry quotes its source in its notes. A value the source does not publish stays empty; it is never estimated. Where a tool's outline is drawn from its values, the typical value it takes is named in its outline line.

• Machines from the makers' data sheets: Langmuir Titan 25T (American tooling), TRUMPF TruBend 7036 and 5130 and SafanDarley E-Brake 35-1250 (New Standard), Durma AD-R 30100 (European), Bystronic Xpert Pro 100/3100, Amada HG-1003 and Harsle WE67K-100T3200 (tooling system not stated by the maker: Other).
• European (Promecam) tools from the AMADA NEW AFH catalogue: straight, sash, gooseneck, 30° and hemming punches; 1-V dies 88° V4–V25 and 85° V32–V80, 30° dies, the 4-V block V16/22/35/50 and hemming dies, with their load ratings.
• American tools from the Wilson Tool American Precision and Planed catalogues (punches, staged 1-V dies 1/4–2 in, 30° dies, hemming and flattening tools, 4-way blocks) and the Langmuir Titan 25T set (its punch and die guide, made for that machine).
• New Standard tools from the WILA catalogue: straight, gooseneck, 28° and flattening punches; 86° V4–V20 and 80° V24–V100 dies, 30° dies and a hemming die.
• Materials: S235JR, S275JR and S355J2C with the EN 10025-2 bending radii, A36 (ASTM A6), DC01 and A1008 cold-rolled, DX51D+Z and A653 galvanized, S355MC and S700MC (EN 10149-2), Hardox 450 (SSAB), stainless 304, 316L and 430, aluminium 1050A, 3003, 5052, 5754, 5083, 6061-T6 and 6082-T6 (EN 485-2), copper Cu-ETP and brass CuZn37. Rm is the middle of the standard's range. The air-bend radius share of V is the published one (The Fabricator, S. Benson; the Langmuir manual), else Benson's tensile scaling 0.16 × Rm / 413.7 MPa.

Apply Bend Rule

Air bending forms the inside radius from the die: Ri = V × the material's air-bend ratio (about 0.16 for mild steel, 0.21 for 304 stainless, 0.14 for 5052 aluminium). The punch tip radius is used when it is larger. The K-factor is the test-bend value when there is one, else the material's K-factor, else auto: DIN 6935, K = (0.65 + 0.5 log₁₀(Ri/t)) / 2, at most 0.5.

The rule sets the bend radius and the K-factor, and Fusion recalculates the flat pattern: BA = θ (Ri + K t), OSSB = (Ri + t) tan(θ/2), BD = 2 OSSB − BA. Bends that keep their own radius (bend overrides, or a body converted to sheet metal) are listed after OK; their flat follows the K-factor but not the press-brake radius. The setup is remembered on the component for Bend Sheet. A thickness different from the part's rule asks before it changes the sheet thickness.

Calibrate from Test Bend

Cut a strip and measure its length. Bend it once on the die, about 90°. Measure the outside of both legs, to the outside of the bend (calipers over each leg), and the bend angle: 90 for a right angle, or 180 minus the angle measured between the legs. The add-in computes the bend deduction (both legs minus the flat length) and the K-factor that gives it with the die's inside radius, and stores both for that material, thickness, die and punch. A new test bend of the same setup replaces the older one.

Auto tools + order and section geometry

Auto tools + order tries the punch and die chosen in the dialog first, then straight punches and dies near 8t; acute tools only when the part has an acute bend. It tries both gauge sides (the side with the shorter X first, as the plan itself chooses) and other bend orders, with a few good tool pairs before the whole library. Candidates rank by the checks their own tools leave open and by their warnings, then by tool changes; tools with exact outlines are tried first. Gaps of the machine (ratings, X range) apply to every candidate and do not rank them. It stops as soon as no better plan can exist, and once it has a plan it stops after about 2 seconds; at most it takes 8 seconds or 1,200 candidates, and Cancel stops it at once. While searching, steps are checked with 2 mm motion samples; the chosen plan is checked again at the normal 0.5 mm, and a step that collides there is rejected and the search continues. When the part's flat body can be refolded, a plan the sections clear is then folded in 3D through every step, as Check all steps in 3D does (a few seconds a step, not counted in the 8 seconds). A step whose part meets the upper beam or clamp is searched again with taller punches or in another order, one that meets the punch or die with other tools; when no plan clears in 3D, the plan with the fewest such steps is kept and its 3D check says which steps need other tools. The PDF tooling table and CSV list each step's tools. Provisional means data or rule checks remain incomplete. A search limit is not proof that special tooling is necessary.

In Press Brake Library, an outline is JSON [[x,z],...] in mm. Punch origin is its lowest tip; die origin is the V centre at shoulder level. The upper beam is drawn from the punch shoulder (z = 0, the clamping face) on the tang axis (x = 0); gauge coordinates are relative to X at shoulder level: draw the gauge finger with its stop face on x = 0 and its body toward +x, where the edge of the sheet rests on that face. A punch or die with neither a working length nor a sectioned set is taken as long as the bend line, and without a gauge retraction the finger stays at X during the bend; both are listed under Assumed. Library versions 1 to 5 load in version 6 without changing old values.

Import from DXF... under each outline field reads a closed outline from a 2D DXF drawing in millimetres or inches, such as a tool maker's CAD file. Centre lines and other dashed lines, text, dimensions and circles are skipped; arcs become chords within 0.005 mm, and an outline over 256 points is simplified with the tolerance reported. Draw the punch tip down and the die V up, as in the press: the punch origin moves to its lowest tip point and the die origin to the centre of its widest top opening at shoulder height. Beam and gauge outlines keep the drawing's coordinates. Check the outline before OK saves the entry.

Outline from sketch, under the entry, reads the outline of a punch, a die or the machine's upper beam or back-gauge finger (chosen under it) from a sketch in the open design: click inside the closed outline, or pick its curves one by one. Regions picked together join into one outline (a tang drawn as its own region, say), construction lines are skipped, and until the curves close the dialog names the open ends. The sketch is read in millimetres as the Front, Right or Top view (whichever faces it) shows it, with the design's up axis up, so draw the tool as you see it there: the punch tip down and the die V up, anywhere in the sketch. For the upper beam the sketch origin is the punch shoulder on the tang axis, and for the gauge finger it is X at shoulder level. The picture above updates at once; on a punch, set Height so its dashed line sits at the shoulder. A maker's STEP model becomes an outline by projecting its end face into a sketch.

The solver samples the bending stroke, gauge retraction and punch withdrawal, including sheet thickness and the radii of already formed bends. It checks each tool's station against the bends formed at its ends (see Tool length). Every part of the sheet moves at most 0.5 mm between two checks: material near the bend line moves little and is checked less often than the flange ends. At most 3,600 samples per phase, with a 0.02 mm penetration tolerance. Insufficient sampling, oblique/non-90-degree end walls and interrupted sections remain incomplete. This is sampled 2D plus axial checks, not full 3D collision certification or a solution for arbitrary loading/unloading paths.

Signed CW/CCW handling preserves arbitrary angles. Per-bend radii come from native bend extents using the component rule K-factor; a bend whose extents cannot be resolved uses the rule radius and is flagged on the sheet. Check any bend-specific unfolding override. Test-bend data matches the exact punch as well as material, thickness and die.

PDF/CSV/DXF are staged together and published with a hash manifest. An ordinary publication failure restores the old files. Stale companions from a previous export must be included or exported to a different folder. Stored step tools and gauge sides reload with the part; changing the global setup resets them.

Bend Sheet

Bend Sheet works on any Fusion sheet-metal part, with or without forms. A part without a flat pattern gets one from its largest planar face. Forms made by this add-in are suppressed while the flat is read and restored afterwards; each form is then placed in the flat by measuring its flange with the temporary markers Manufacturing Export uses, so the checks see where it is. Bend Sheet is not blocked by the forming-tool qualification that Manufacturing Export checks.

The bend table. Bends are numbered B1, B2… from left to right in the flat seen from its top face. UP folds the flange toward that face, DOWN away from it; an UP bend is made with that face up, toward the punch. Flange lengths are the outside lengths of the finished part on each side of the bend, to the next bend or the edge.

Bend order. The suggestion bends outer flanges first (a bend with a free flange on one side), groups bends of the same direction to save flips, and bends short before long. Select a row and use Move up or Move down; Suggested order restores the suggestion. The order and the press-brake setup are remembered on the component.

Back gauge. For every step the part is laid on the die as it is at that moment, with the earlier bends formed. X is measured from the bend line to the farthest point of each side: the free edge of a flat side, or the outside of a formed flange (for a 90° flange: the flat distance to its bend line plus half its bend deduction). The side whose X fits the machine's back gauge range goes to the gauge, the smaller X first. The handling column says when to flip the part over, turn it end for end or rotate it by the stated signed angle (CW/CCW).

Checks. Every step is checked for a flange shorter than the die minimum (0.7 × V), a force above the die or punch limit per metre or the machine limit (F = 1.42 × Rm × t² / V kN per metre of bend), a part longer than the bed, a formed flange taller than the punch (collision risk) and a formed flange hanging down closer than V to the bend line (short Z bends). The part is checked for holes or cut-outs closer than 2.5 t + Ri to a bend line, an inside radius below the material minimum, a bend that closes sharper than the die or punch angle (air bending cannot close a bend below the die angle: use acute tools), and a flat made with a different radius or K-factor than the press-brake setup. Problems show in the dialog and on the sheet; a check that needs a missing library value is listed as not checked.

Forms near a bend. A form made by this add-in that reaches into a bend zone is an error: the bend crushes it or pulls it out of shape. A form closer to where the bend starts than 3 t + R (Mate) is a warning; a louver made in a press-brake louver die keeps 15.88 mm (Protocase). Every step also carries the forms' cross-sections on its flanges through the section check, so a form that rests on the die shoulders, hangs into the V, meets the punch or the back gauge is reported by name, for example Step 2 (B2): The louver 8c4508 is in the way of the die before the bend starts. Each form goes where the panel of the flat it lies on goes (a form beside a tab stays with the sheet it is joined to). A form on a wall already formed across the bend (a box's end wall) is not in the step's section: the section check says so and the 3D check covers it. A form that cannot be placed in the flat (on a rolled face, or spread over two flanges) is listed so it can be checked by hand, and a gusset across a bend is listed with the tooling its bend needs.

3D view of a step

Under 3D view, Show the selected step in 3D draws the step selected in the bend table beside the model: the part refolded from its flat to that point of the stroke, with the earlier bends formed, the punch, die and back-gauge fingers swept along their lengths, and the upper beam see-through. Motion (%) runs the stroke as the checks do: the back gauge retracts, the punch bends the part, then withdraws. Where the part cuts into a tool at that moment, the volume they share is drawn in solid red and the tool turns see-through red. The view opens at the first contact found, by the 3D check when it has run, else by the section check; Go to the contact returns to it. When the flat cannot be refolded (a bend not joined to its flanges in the flat), the view shows the section across the bend swept along it, with the formed end walls of a box: the model the section check uses. Nothing is added to the design: the graphics go and the camera returns when the box is cleared or the dialog closes.

3D check

Check all steps in 3D checks every step of the part's plan with the real part. The flat body is cut at the bend zones and folded step by step in the order of the table, and at every 5° of each bend and through the withdrawal it is tested against the punch, die and upper beam as solids (their outlines along their lengths); a contact is then narrowed to a fraction of a degree. A contact counts when the part and a tool share more than 1 mm³ and the shared part is more than a skin (a mean section across the bend line above 0.05 mm²: a sheet lying on a long die only touches it). This finds what a section across the bend cannot show, for example a return at the top of an end wall that hangs over the end of the punch. The check takes a few seconds a step, shows its progress and can be cancelled. Each contact is listed in the checks, for example Step 5 (B3), 3D check: the flange at B6 meets the punch at the start of the bend; a contact made by a form names the form (the louver 8c4508 meets the die). The bend sheet prints the result as 3D check. The result belongs to the plan: a new order or another tool clears it. Not checked in 3D: the back-gauge fingers (the part lies against them), the bend zone being formed, springback and the deflection of tools and machine. A step with a tool that has no outline, a hem or no V die is reported as incomplete.

Outputs, for the selected part or all sheet-metal parts in the design:

• Bend sheet PDF: on every page a header with the design, date and page number; for each part its material, thickness, die, punch and machine, the flat with numbered bend lines and UP/DOWN, the bend table in bend order with X, gauge and handling, the checks, and a side view of every step on the die. Where a collision was found, the side view also draws the part and the tool in red at that moment, with the angle.
• Flat DXF, one per part: layer CUT with the outline and holes, BEND with the bend lines, ETCH with short marks at both ends of each bend line and the part ID in a single-line font (for a plasma scriber or a laser), NOTES with texts such as B1 UP 90°. Only CUT is a cutting layer.
• Bend program CSV: step, bend, angle, direction, die, punch, X, gauge, handling and force, to type into the brake controller.

Forms

Before creating a form

1. Activate the sheet-metal component you want to modify.
2. Confirm the target body is a Fusion sheet-metal body.
3. Finish native flanges, manufacturing cutouts, and Tab & Slot joints, including joint edits, before creating forms.
4. Select a planar or analytical cylindrical face in Create Form. For a planar target, the add-in can create the baseline automatically. A fully cylindrical target must already have a native Fusion flat pattern. Louvers, bridges and lances need a planar face: a rolled part is punched flat before it is rolled. A gusset across a bend takes the bend's own face.
5. For the first form on a cylindrical fixture, select a persistent vertex, sketch point, or construction point as X=0/Y=0 and enter the common fixture datum ID. Later forms reuse and verify that reference.

Commands

Tab & Slot joints

1. Activate the owning sheet-metal component. Open Tab and Slot and choose Create new joint.
2. Select a straight free Tab edge and the perpendicular planar Mate face that will receive the matching slots.
3. Choose Number of tabs or Tab pitch. Set tab width, start/end margins, and Projection beyond mate, the extra tab length beyond the mating sheet thickness. Both sheet gauges are detected.
4. Set positive Slot clearance (each side). This is fit clearance on each side of the tab, not laser kerf compensation. Preview shows opaque resulting sheets with joined tabs and cut slots. Adjust the preview, then click Create Joint. Only participating originals are hidden temporarily; turning Preview off or choosing Cancel restores their previous visibility.

To edit, select a joint face or owned timeline feature before opening the command, or choose Edit existing joint and select the joint. Saved references and dimensions load automatically. Enable Replace edge / mate references only when both inputs need re-selection, then click Update Joint.

Supported joints use native Fusion sheet-metal bodies in the same component at a straight 90-degree connection, including an open corner of one folded body. Select native geometry inside the active owning component. Curved or bevelled ends, cross-component references, and flat-pattern geometry are excluded. Layouts allow up to 50 tabs; pitch mode centres the fitting set within the requested minimum margins.

Enclosure example

1. Use native Fusion sheet-metal base and flange tools to build the enclosure. Add cutouts and Tab & Slot joints, then finish their dimensions.
2. Create a louver and repeat it with Pattern Form, using an array or a selected louver region. Add extruded holes for tapped collars: choose the thread and the tap (forming or cutting) and the bore, pre-hole and collar are filled in; the model has no thread.
3. Run Audit Forms, review the native Fusion Flat Pattern, and use Fusion Drawing for assembly views, dimensions, and fabrication notes.
4. Use Manufacturing Export for the Punch Map and outputs supported by the part and its qualification. Check the mapping scope below before selecting an annotated handoff.

Manufacturing output

The CSV is the readable Punch Map for the shop and Excel. The optional JSON preserves stable IDs, form parameters, positions, orientations, and audit data as a machine-readable traceability/archive file; the add-in does not import it. Neither file becomes a Fusion native flat-pattern annotation. The optional DXF is Fusion's current native flat while only the add-in's forms are temporarily suppressed. Independent features created before the forms remain; dependent downstream features cause the transaction to abort. The Punch Map carries the forming-tool semantics.

A flat-safe DXF transaction stops and restores the design if suppressing the forms makes a downstream feature unhealthy. Place cuts or other manufacturing features that must appear in the DXF before the forms in the timeline. Restore failures are reported and never shown as a successful export. DXF currently requires exactly one sheet component with forms in the active design. For a multi-component design, disable Clean native flat DXF, Same-datum CUT/FORM DXF + shop PDF, and Annotated blank handoff, then export face-local CSV with or without JSON.

Enable Annotated blank handoff (SVG + datum schedule) for one native sheet-metal component: a validated unbent prism, or planar flanges of a folded part with a valid native flat pattern. The add-in maps the actual blank outline and tool locations to one shared datum. The SVG shows numbered locations, headings, tool sides, bend lines and a tool schedule; this option also includes JSON.

On a folded part, three temporary registration holes measure each planar flange's position and heading in Fusion's native flat. The add-in removes those holes and verifies restoration before publishing any output. The mapping tolerance is 0.005 mm. Fusion supplies the bend allowance and flat geometry; the add-in does not infer them or calculate forming strain.

Every instance in one form definition must lie on the same bounded planar flange, with its complete tool footprint clear of bends, edges and holes. Use separate definitions for different flanges. Curved form hosts, unsupported blank geometry, unresolved references, and registration or restoration failures stop the handoff; no guessed map is substituted. To export only face-local metadata, explicitly disable the mapped outputs.

CSV x_mm and y_mm are face-local coordinates. When the annotated handoff is selected, handoff_x_mm, handoff_y_mm and handoff_rotation_deg match the SVG datum. FW-BLANK-XY starts at the lower-left outline bounds; its axes follow the first form frame for an unbent blank and the native flat frame for a folded part. The optional native Fusion DXF still has its own origin and orientation; register the two datums before combining coordinates. Geometric validation does not qualify a physical forming process.

Production export checks the stored tooling qualification and model state. For review of unqualified tooling, select Reference-only package (not for manufacturing). It includes CSV and JSON, may include the annotated SVG when its geometry is valid, marks the package UNVERIFIED_DO_NOT_MANUFACTURE, and disables native DXF.

Punch Map columns for the shop: form_direction (out of or into the face the form was placed on), form_height_mm with height_datum (from the sheet face the form rises from to its top), made_by, louver_ends, progressive_hits, thread, knockout_trade_size, a bead path as lines and arcs (path_segments, path_length_mm, path_min_radius_mm, nibble_hits), do_not_mirror, and shop_checks with the makers' limits found for that form. With the annotated handoff they add the form as loaded (handoff_form_loaded UP, DOWN or CUT), the hit order, the open side of louvers and lances, and the forms that need an auto-index station.

Keep the .manifest.json revision file with every selected package file. Existing outputs are confirmed and replaced together. If you omit a companion that already exists under the same base filename, choose a new base filename or include that companion to avoid mixing old and new release files.

Common-datum manufacturing handoff

Manufacturing Export enables CUT/FORM DXF + PDF by default. For a validated unbent blank or registered planar flanges of one folded sheet component, the CUT/FORM DXF, vector PDF, annotated SVG, CSV handoff coordinates and JSON share FW-BLANK-XY, millimetres and one package revision. Keep the revision manifest with the complete package.

Load the blank sets which face of the blank is up on the punch press; Auto puts most forms up (makers form up whenever possible and form down last). Every form is then UP or DOWN as loaded, with its height. The hit order punches the cuts first, then the forms up, then the forms down, one tool at a time in one direction (AMADA), louvers from their open side toward their root (Conic). Tool stations: fixed stations are keyed at 0, 90, 180 and 270°, so a form at any other angle is marked for an auto-index station. The DXF, PDF, SVG and the CSV handoff coordinates show the blank from above as loaded: with the +N face down they show the -N face, turned over left to right (X from the other edge, angles 180° minus the model's). The sheets say not to mirror the blank: the forms are directional.

Punch press. The export checks the punch-press job with the settings in this group and lists the findings in the shop PDF and SVG (the CSV adds the station and the checks of each form). They are warnings: nothing is blocked. Station sizes gives each one-hit tool the smallest station that takes it: thick turret A to E (Mate Ultra TEC sizes; a form about 12.7 mm under its station, extrusions from C, knockouts by the AMADA table), with an F station, or TRUMPF tool sizes 0 to 2 or with size 5. A tool larger than the largest station is flagged. A stripper holds the sheet on the die through every stroke (Mate, TRUMPF), so a form made UP under a later hit's stripper, or made DOWN over a later hit's die, is flagged as pressed flat; the tools are taken as discs of the station's stripper and die. Hit order: Avoid crushing where possible makes such a hit before the form it would land on, within the forms up and within the forms down, where such an order exists; otherwise the finding says to relieve the tool or space the forms. Clamped edge, Clamp dead zone (72 mm, TRUMPF closed clamps) and Clamp centres (97 mm either side by default) flag forms where no tool can punch with the clamps closed.

Show the job in 3D reads the blank once (the forms are suppressed and put back) and draws the job beside the model: the blank as loaded, the forms made before the hit, the hit's forming tool between its station's stripper and die, the forms still to come as outlines and the clamps' dead zone. Hit steps through the hits in order and Stroke (%) moves the hit's tool from open to the bottom of its stroke. A tool that lands on a form turns red with the form. The camera comes back when the view is switched off or the dialog closes.

The DXF CUT layer contains the blank perimeter, existing through-holes, the pre-holes of extruded holes and the slits of louvers formed in a press-brake die (cut first, formed after). Analytic circles and circular arcs remain analytic; supported noncircular curves use the stated chord tolerance. FORM_UP and FORM_DOWN contain the tool-centre crosses and heading marks of the forms made up or down as loaded (and a bead's path), FORM those of knockouts, which are cut in place; NOTES contains instance numbers with the tool, the direction and the hit. BEND holds the native flat bend lines, which also appear in PDF and SVG. Only CUT is a cutting layer; never send BEND or the forming marks as cutting paths. Forming marks locate operations, not die geometry or stretched material. Tab & Slot geometry created before forms remains in the native blank.

The PDF shows the blank and numbered form locations, followed by a paginated coordinate schedule with tool codes, revisions, tool sides and form directions. Its diagram fits the page; use dimensions and coordinates, not the printed scale. Native flat DXF remains optional and uses Fusion's independent datum. Unsupported geometry or failed registration stops the common-datum package. Reference-only output includes a clearly marked PDF but never a cutting DXF. Production output still requires documented tooling qualification and a passing audit; flat registration does not change that requirement.

Fill a louver region

1. Create closed region and optional keep-out sketches on the same planar sheet face plane, before any forms in the timeline.
2. Create a seed louver. Open Pattern Form, select that definition and choose Louver region.
3. Select a fill profile and optional keep-out profiles. Set X/Y pitch, edge margin and grid angle, then click Rebuild Pattern.

The grid is anchored at the seed. Every accepted louver's complete tool footprint must fit inside both the selected region and the sheet material, clear all holes, explicit keep-outs and other stored forming footprints. The calculation adds a small geometric tolerance; documented tool edge and pitch limits remain enforced. A layout is limited to 100 accepted forms and 25,000 candidate grid positions.

Region references and grid settings are stored with the form. Reopening Pattern Form restores them; rebuild keeps stable IDs for unchanged grid slots. Rebuild after editing region sketches or other forms. Audit blocks stale region references or changed forming keep-outs before release. Deleted references must be selected again. This is an explicit rebuild workflow, not an automatic Fusion native feature recompute.

Tool Library

Create Form includes ten factory presets and a local user library. Select a preset to load it; enter a name to save/update it. You can also delete a selected preset or import/export the complete versioned JSON library. Imported name collisions are renamed instead of silently deleting local tooling data.

Filter presets by material/condition, documented thickness range, tool or machine text, and qualification. Thickness zero means all gauges. A nonzero thickness excludes presets without a documented range. Qualified filters include only definitions whose geometry still matches their qualification fingerprint. The ten factory presets are reference examples, not certified tooling. Save supplier-supported or shop-qualified data with the actual material, tool ID, revision and source document/page; import/export lets a shop reuse that evidence without inventing limits.

Planar folded geometry is a drafted, hollow approximation built with supported Fusion Loft (Join/NewBody), Combine Cut, and Extrude Cut features. Analytical cylindrical geometry uses Fusion Emboss and bounded owned cuts. Fusion determines the final surface wrap, so a qualified cylindrical process must include measurement of the committed Fusion result. It is not a native forming-tool feature and does not simulate forming strain, material thinning, springback, or a physical press-tool radius; it also creates no native flat-pattern forming annotation. For dimple/emboss/deboss, the catalog size defines the base and the draft, the wall's angle from vertical, reduces the crown by depth × tan(angle) per side; AMADA's standard tools need 30° or more, the default. Validate catalog dimensions against the actual material and physical tooling before release.

Louvers, bridges and lances follow the punch-press tool: the raised part is the sheet itself, one gauge thick, and every lanced edge stays open. A louver is lanced along its front edge; the hood rises from the back root at the form angle (tool makers use 40–85°, 45° preferred), its crown stands over the front edge, both ends are drawn closed and the front is open over height − thickness. The open front is on the louver's +Y side before rotation: on a wall, rotate the louver so its front faces down, away from dust and dripping water. A bridge is lanced along both long sides and lifted by a ramp at each end, so it is open on both sides. A lance is cut on three sides and lifted by a ramp at its +X root; the free end draws back by height × tan(ramp angle ÷ 2). Height is measured top to top and must be at least 1.5 × thickness.

A louver's Ends are closed (drawn) or open: an open-end louver is cut along its front and both ends and only its back is bent, for more air on inside panels (Mate). Made by: a punch-press tool as long as the louver (one hit); a progressive tool that steps along it, for any length (give the tool length and the step: the thickness or less, Wilson; 0.8 mm, Mate), formed from the middle out; or a press-brake louver die, which forms a slit cut beforehand (the slit goes on the CUT layer; Protocase).

Beads along a path and gussets across a bend

A bead is made in one hit, nibbled hit by hit, rolled by a wheel tool or pressed by a press-brake rib die (Made by). A nibbled or rolled bead can follow a Bead path: sketch lines, arcs and circles on the face, end to end, rounded at least half the bead's width (a closed path makes a ring). The bead is swept along an owned copy of the path, with round ends where it starts and stops; give a rolled bead its wheel tool's smallest path radius (TRUMPF 30 mm, Mate 16-20 mm) and the path is checked against it. The Punch Map lists the path as lines and arcs; the handoff draws it.

A gusset Placed across a bend is a stiffening rib pressed into the inside of the bend in the bend stroke, with gusset tooling: a punch with the rib notch and a die with a beading bar (TRUMPF), or pressed after bending. Pick the bend's face; Length is each leg along the flanges from the inside corner, Width the rib's width. The rib is its own body in the inside of the bend: Fusion's flat pattern cannot unfold a bend with a rib pressed into it, and the blank is cut before the rib is pressed, so the sheet body and its flat stay as they are. It is one form (no placement pattern), it must lie on the bend and its legs on the flanges. Bend Sheet lists the gusset with the tooling its bend needs; the punch-press handoff leaves it out and the Punch Map keeps its row without handoff coordinates.

Tool makers' limits in Create Form

The Checks box under the form's description shows what tool makers publish for the form, while you edit it, and the result lists them after Create Form; Audit Forms measures them again. They are warnings: a shop with other tooling may still make the form.

• Height: louvers about 4 × thickness in mild steel, 3.5 × in stainless and aluminium (Conic); bridges 3 to 5 × by ramp angle (Conic); dimples 4 ×, embosses 3 × and at most 0.3 × the width (AMADA, Conic); beads 3 × and 0.4 × the width; extruded holes 2.5 × overall, from the far face (Mate; TRUMPF 2 ×); standard turret tools reach about 6.5 mm.
• Walls of dimples and embosses at least 30° from vertical (AMADA); louver form angle 40-85° from the sheet (Wilson).
• Extruded holes: a pre-hole at least the thickness (Mate, AMADA); a thread size for the bore and collar, up to the thickness Mate allows for it.
• Knockouts: the hole, not the conduit size (NEMA 71 nominal, or a cable gland); one tie up to 34.9 mm, two above (Mate); ties 2 × thickness (AMADA); a gap of at most 0.25 mm (NEMA 55). Trade size fills them in for the sheet.
• Distances on the face: 3 t to a sheet edge or cut-out, 6 t to another form, 3 t between louvers, 3 t + R to where a bend starts (Mate); 15.88 mm for a press-brake louver (Protocase).
• Rolled beads: up to 2 mm steel, 1.5 mm stainless, 2.5 mm aluminium (TRUMPF, Mate); progressive steps no longer than the thickness.

The material comes from the form's engineering profile (or the actual material); without one, mild steel is assumed.

Good practice

• Reuse the baseline flat pattern that Create Form creates or detects.
• Keep one associative cylindrical fixture zero and datum ID for all related forms; a deleted or moved datum blocks reuse and release.
• Resolve every Audit error before placement. The add-in blocks a new tool when another stored form overlaps it or its clearance record is damaged, stale, or incomplete.
• Use Edit Form instead of editing generated geometry directly.
• Read the Checks box before Create Form.
• Run Audit Forms before Manufacturing Export.
• Keep selected companion files and the package revision manifest together with the mandatory CSV.

Support: support@vanthanbk.com
Product: vanthanbk.com/company/sheet-metal-press-brake
Privacy: vanthanbk.com/privacy