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Editing workflow

How documents, bodies, sketches and features behave in the app.

Documents and tabs

Files and session

Import

File › Import, or a file dropped on the window, brings a file into the open document. STEP and IGES come in as solids, mesh files as mesh bodies, a .prtcad as linked parts (Assembly), a DXF drawing or a picture as a sketch (Sketcher).

A mesh keeps the colours its file gives it: a PLY's vertex or face colours (text or binary), an OBJ's materials and textures (the .mtl and pictures beside it), a 3MF's colour groups, materials and textures. A 3MF prepared for printing brings only what is printed: modifier, support blocker and enforcer, and negative volumes are left out, and the import's report says how many. A PLY with no faces is a point cloud, which is refused for now.

An STL file holds bare numbers, so importing one asks what units they are in (millimetres, centimetres, metres or inches; the last answer is offered first) and scales the mesh to millimetres. "Don't ask again" reads every later STL in that answer; Preferences › General › Files turns the question back on and sets the units it uses meanwhile. Other formats say their own units. A script names them with units (mm, cm, m, inch).

A mesh from a 3D scanner is a scan: Use as scan in the mesh body's menu (or pc.file.import{path = …, scan = true}) marks it so, and Not a scan sets it back, one undoable step either way. Its row carries a SCAN badge whose tip gives its triangles, points and the median spacing between them, and the units its file was read in when they were not millimetres. A solid cannot be a scan. Scans are what the inspection and mesh-editing tools of RFC 0004 work on.

Mark surface… in a scan's menu marks part of its surface by hand, for the tools that work on part of a scan. With Window, Brush (its diameter in millimetres) or Lasso chosen in the task, a drag over the view marks the triangles it covers and a drag with the right button or Alt rubs them out; Shift-drag turns the view. Only faces turned towards you are taken unless "Include faces pointing away" is on. Invert swaps marked and unmarked, leaving the border between them bare; Clear starts again. The marking stays with the tab when the task closes, until it is cleared or the scan gets a new mesh (a mesh step building, an undo, another client's change), which drops it; moving the scan keeps it. pc.scan.mark{body = …, box = …, ball = …, facing = …} marks from a script. The Inspection bench fits shapes to what is marked.

A FreeCAD file (.FCStd) comes in as printCAD's own history, rebuilt here rather than read as finished shapes, and where printCAD cannot rebuild something, as the shape the file saved for it, so every part looks whole:

The command behind it is project.import (Scripting).

The active body

Tools are enabled only when their input exists:

Tools Need
New sketch, primitives, datums A body
Pad A sketch, or a flat face of the solid
Revolution, loft, pipe, helix A sketch
Pocket A solid, and a sketch or a flat face of it
Groove, hole A sketch and an existing solid
Fillet, chamfer, draft, thickness, face tools, patterns, booleans A solid

A Design feature added to a surface body, or to an imported body that cannot take features (a mesh not yet converted, a part linked from another file), goes into a new body, and the log says so. Surface features go on a surface body, or on one holding only sketches and datums; elsewhere they start a new body (Surfaces).

Sketches

This section covers where a sketch goes and how its editing session runs. Drawing, constraints, regions, reference pictures, text and projected geometry are in the Sketcher guide.

Creating one. Design's New sketch switches to the Sketcher and shows a plane picker:

The sketch is added to the body, opened for editing, and the camera turns square to its plane.

Placement offset. The sketch panel's Placement fold moves it off whatever it was placed on, a base plane, a face, an attachment or a datum: along the normal, across the plane in x and y, and turned about the normal. A sketch a few millimetres above a plane needs no datum plane for it. Placing the sketch again elsewhere drops the offset.

A fully constrained sketch being edited: a plate with three holes and their dimensions

Editing one. Double clicking a sketch in the tree opens it the same way.

While editing, the view stays square to the sketch plane: pan, zoom and roll work, orbit and standard views do not.

Constraining to the model. A constraint or dimension tool pressed while the selection does not fit it yet stays armed (its button lit) and takes more picks: a click on the sketch adds an element, and a click on an edge of a solid adds that edge, or the vertex at its end when the click is there and the tool takes a point. Once two items are picked and fit, the edges are projected into the sketch as guides (an edge the sketch already holds is used again) and the constraint goes on: a distance from a point to a model edge, a point coincident with a model vertex, a circle tangent to a round edge. That is one undo step. Enter applies the tool to a single item, Escape or a right click puts it away.

Finishing. Done in the task panel's header, or Enter, ends the edit and returns to the workbench you came from. Escape in the view drops what is in progress first: a typed value, a half-drawn shape, the selection.

The sketcher's task panel: what the solver says, its settings and the constraints

Datums

Design's datum tools add a plane, line, point or coordinate system to the active body. The task panel's Attached to list places it: on a base plane, or by a mode built from what is selected on the body. A mode whose picks are missing is greyed, its tooltip saying what to select first.

Mode Select first Places it
On a face A face On the face, tangent to it where it is curved
Through three points, through two points Edges or a face, if any Through the points, the unpicked ones near the datum
Square to an edge, along an edge, tangent to an edge An edge At or along the edge
Where two planes meet On the line two planes share
Midway between two planes Two faces Halfway between parallel faces; between faces at an angle, on the plane bisecting it
Centre of a curve A circular edge At the circle's centre, square to it
Centre of mass At the body's centre of mass, on its axes of inertia
On a datum, another body's origin On that datum or origin plane
Square to a face A face Along the face's normal
Through a line and a point, where a line meets a plane An edge Through the line
Where two lines cross Two edges Where the lines pass nearest

Each reference row in the panel swaps what the datum stands on: Use selected face or Use selected edge takes the current pick, and a plane row also takes a base plane or an earlier datum plane. The midway plane's two rows each take a face, a base plane or a datum plane, so it can stand between a face and a datum. Between faces at an angle it takes the bisector passing between them, through the material where they are two faces of one solid, its x-axis along the line where they meet.

References on the body's own solid follow it: when a feature before the datum changes, the rebuild finds each face and edge again, by name, and the datum moves with them, along with the sketches and features built on it. The offset, turn, tilt and flip in the panel move the datum from where its mode places it. pc.design.datum makes the same datums from a script (Scripting).

Design features

  1. A tool such as Pad adds the feature, hides the sketch it uses, and opens the feature's task panel.
  2. Changes in the panel apply to the model as you make them.
  3. Done keeps the feature. Cancel removes a new feature, or restores an existing one to how it was when the panel opened. Both sit in the panel's header, beside the feature's name and its state (live preview, rebuilding, or a failed rebuild).

Everything done in one task panel is one undo step. While the panel is open, the material the feature adds or takes away is drawn as a translucent preview.

A pad's preview, drawn see-through The Pad task panel

View handles. While its task is open, a feature shows a dot at the end of each number it can show in the view: a pad's or pocket's length (and the second side's), a hole's depth, a thread's length along its face, a revolution's or groove's angles on an arc round its axis, a draft's angle, a primitive's sizes, a fillet's radius or a chamfer's size. One more dot sets where it starts: a pad's, pocket's or hole's start offset, from its profile or from the plane or face it starts on, and a revolution's or groove's start angle; those go either side of zero. Drag a dot to set the number: in steps of 1 mm or 5°, or with Shift held in fine steps of 0.1 mm or 1° (Preferences › Design sets all four). A drag stops on a number's limit even where that is no whole step (a revolution's 360°, a draft's 45°, a fillet's largest size); only typing goes past one. Every number field in the app does the same: dragged, it stops at its range or limit, and the mouse wheel's steps land on it. The number shows beside the dot and the status bar names it with its steps while it is held. A pad's, pocket's, hole's, revolution's or groove's dot turns the feature the other way when clicked, or when dragged back through its start. A number a formula sets has no dot. A pad's or pocket's length snaps to a flat face square to its way, of any body shown, when its dot comes within a few pixels of that face's plane; the face lights while it holds, and Alt drags past it. While a dot is held, typing a number opens a field beside it; Enter sets it, and text that is no number sets the number's formula. The dot being edited is drawn lit: the one held, the one whose typed value is still open, or the one whose field the task panel last changed. A fillet's or chamfer's dot stands on its edges whether they were picked one by one, taken with their faces or all taken.

Number fields in task panels step with the mouse wheel over them: a whole unit a notch, a tenth with Shift.

Regions. A sketch's curves may cross, meet three or more at a point, or leave a spur: every closed area between them is a region (two overlapping circles make three, the lens and two crescents). By default a feature takes them all, a loop inside another loop being a hole. A pad, pocket, revolution or groove can take only some. Before starting it, click a region of the closed sketch in the view to pick it alone, and Ctrl+click to add or take away more: the feature starts with exactly those, so a disc inside a ring picked together with the ring pads the whole disc. A click on the sketch's lines, or on its row in the tree, selects the whole sketch again. With its task open, click a region on the sketch's plane to take it alone, Ctrl+click to add or take away one; the regions left out show shaded. The task panel lists the same regions as checks. A region keeps its name while the sketch's dimensions change; pc.sketch.regions lists them for scripts, and the feature's regions field holds the names it takes.

Ctrl+click on a curve of a closed sketch picks that curve beside its regions. A revolution or groove started with a straight curve picked turns about it (its axis set to that sketch line). A pipe started with curves of a sketch picked runs along those curves alone, one chain of them, and takes the body's latest other sketch as its profile; its task lists the path sketch's curves as checks, every one ticked while the pipe takes the whole sketch, and the feature's path_curves field holds the ones it takes.

Where it starts. A pad, pocket or hole starts on its sketch's plane. Its Start at list moves the start to a datum plane of the body, the plane of another of its sketches, or Selected face (a flat face clicked in the view first). Start offset moves it on from there, either side of zero. A revolution's or groove's Start angle turns where it starts about its axis.

Primitives. The additive and subtractive primitives (the toolbar's Primitive lists) are a box, cylinder, sphere, cone, torus, ellipsoid, prism, wedge or tube: a hollow cylinder with an outer and an inner radius and a height, standing on its placement like the cylinder. A subtractive tube cuts a ring-shaped groove and leaves the core. A tube whose inner radius is not below its outer fails on the feature.

Keep what it shares. A pocket, a groove, and a loft, pipe or primitive that cuts, can keep only the material it shares with the body, cutting the rest away, instead of cutting its own shape out: tick Keep what it shares in its panel. A cutting helix has the same as Keep inside.

A tilted axis. A revolution, groove or helix can turn about an edge, a datum line or a borrowed edge that does not lie in the sketch plane: tick Project onto the sketch, and it turns about the axis's shadow on the plane. Without it, an axis that leaves the plane is refused on the feature.

Boolean tolerance. Every feature that fuses or cuts has an Advanced group under its panel with a Tolerance. Faces closer than it are joined by the fuse or cut, closing a small gap or sliver between them. Empty leaves it automatic, and Automatic puts a stated one back. It takes a formula, and the property panel lists it as Boolean tolerance.

Imported and converted solids take features too. The first feature added to one (a pocket, a fillet) gives the body a Base shape feature first: the imported solid, kept as what the body's history starts from. The body stays one body; its history reads Base, then the feature. Cancel on that first feature, or deleting the Base once nothing follows it, makes the body the plain imported solid again. Repair shape on such a body mends its base, and the features build again on it.

Replace shape… (a body's menu, in the tree or the view) reads the shape from another file: its first solid becomes the base, and the features after it build again on the new shape, finding their faces by name. On a body without features it simply replaces the shape. It clears the undo history, as an import does.

Fillet and chamfer work on the picked edges, or every edge of a picked face, and with nothing picked ask for a pick first. With Follow tangent edges on they take every edge that runs on smoothly from them too (the round of a filleted corner and the sides past it). A chamfer by two distances, or by a distance and an angle, measures its first distance on one face of the edge (Flip direction takes the other) and keeps it on that side all along a tangent chain, even where the faces change from a flat side to a round and on. A chamfer's Auto, a new one's, bevels its size each way, but a face too narrow for it takes the bevel only as far as it goes while the other face's leg goes on, edge by edge; its handle drags until every face has run out. A chamfer by two distances has a handle on each face, each stopping where its face runs out.

A fillet's Type is Auto for a new one: one radius, but on a single edge a face too narrow for it takes the round only as far as it goes, while the other face's contact goes on growing, the round turning elliptical, until that face runs out too; its handle drags that far. Radius is the plain round. Two distances meets one face Distance 1 from the edge and the other Distance 2 (Flip direction swaps the faces), with a handle on each face that stops where that face runs out. Its Profile is Elliptical, the round stretched to the two distances, or Conic, whose Rho sets how full it is: near 0 almost a bevel, 0.5 a parabola, near 1 almost the sharp edge. Two distances round several edges together where they run on from each other as one tangent chain, or meet three at a time at a box's corner; any other meeting of such rounds at a vertex is refused with the reason. A round over several edges has its handles on the first, each stopping where the nearest face of any edge runs out.

Variable runs the radius along the edges, taken as one run end to end: Start radius at one end, End radius at the other, smoothly between and never past them. Start from the other end turns the run round. + Radius between adds a radius at a place along the run, At its share of the run's length from the start (0.5 halfway), in the widest gap so far; × takes one away. The edges must make one run, a tangent chain or edges picked end to end; edges that branch at a vertex are refused. The radii are set in the panel only, as the view has no handle for a place along the run, and Corners does not apply.

Corners says how a vertex closes where the rounds or bevels meet. A fillet's Setback stops each round short of the corner and fills the gap with one smooth patch; Rolling ball runs every round into the corner, the rounds meeting along the curves where they cross and the ball's sphere or torus closing what is left, on corners of three edges between flat faces (other corners say so). A chamfer's Point mitres the bevels into one point; Facet ends them on a small flat facet, a triangle where three meet (not yet on a padded solid's corners).

Overflow says what a round or bevel does where it reaches more than its own two faces. Every switch is on at first, and the first that works is used; with none that works, the feature fails and says why.

A chamfer has Blend into round and Trim through only. Every fillet along edges shows Overflow. A round of one radius takes every switch, with Setback or Rolling ball corners, and so does a Variable round holding one radius all along and Two distances that are equal with the Elliptical profile. A radius that varies, two different distances, the Conic profile and a rolling-ball corner joining convex and concave rounds take Trim through alone: the other switches change nothing there, and with Trim through off a round that would change another face fails and says so.

A fillet's Edges choice Between two faces rounds between two picked faces that need share no edge: the ball rolls between them, and the round fills or takes off what lies between it and where the faces' surfaces meet, such as a step from a tall block down to a low one across a groove.

A fillet's or chamfer's size never drags past what builds. When its task opens or its edges change, the largest size that builds on them is worked out beside the preview, and dragging the size, by its dot or in its field, stops there: in 1 mm steps with a largest of 5.3 mm a drag up goes 4, 5, 5.3 and back down 5.3, 5, 4. A chamfer by two distances keeps their ratio, so both sizes stop at the same scale. Only a size typed past the largest fails.

When a fillet or chamfer fails, its error names the edges that cannot take it ("edge 2 of 3: …"), they draw red while the feature is selected or its task is open, and the task lists them. The task also gives the largest size that fits every edge, with Use to set it, and what each failing edge takes alone. Leave these edges sharp (in the task and the feature's tree menu) takes the failing edges out of the feature in one step that undo puts back; the feature never builds part of its edges on its own.

An angle bracket with the fillet in its inside corner painted

Delete faces takes picked faces out of the solid and closes each opening from the faces around it: a bore, a boss or a round taken away, on any solid, an imported one included. What the kernel does not close yet it refuses by name, on the feature.

Offset faces pushes or pulls picked faces along their outward normals (negative into the material; a bore offset in widens), and Move faces shifts them, or turns them about an axis; in both the faces around them follow on their own surfaces. The distance, the move and the angle take formulas.

Offset solid grows the whole solid by a distance, or shrinks it with a negative one: every face moves that far along its outward normal and the faces around it follow, corners staying sharp. A 10 mm box offset by 1 mm is 12 mm each way, and a hole in it narrows by 2 mm. Use it for a cavity with clearance (a body offset and cut from another with Boolean) or a socket with play. The kernel offsets flat, cylindrical, conical, spherical and toroidal faces; a solid with a free-form face (a spline pad, a loft, an ellipsoid), or one a shrink would collapse, fails on the feature with the kernel's reason.

Thread cuts a thread into a round face of the solid, a shaft's outside or a bore's inside, to a standard size or a pitch and depth of your own, for its whole length or part of it, with a chamfered start or a run-out end, or only shown as a cosmetic thread. docs/HOLES.md (Threads on a face) describes it.

Rib grows a web from an open line or chain of lines and arcs in a sketch, the classic stiffener between two walls of a printed part. Draw the line where the web's free edge goes, on a plane through the part (the middle of a bracket, across a channel), select the sketch and choose Rib. The line's ends run on along it until they meet the solid, and the web fills between the line and the solid on the side where the solid closes it in, Thickness thick: on Both sides of the sketch plane, or all of it on One side or the Other side. Along the normal instead thickens the line in its plane and runs it along the plane's normal until it meets the solid: a web drawn on a plane above a floor stands down onto it, and one drawn between two plates reaches both. Across the plane, a line drawn above walls shorter than it runs on over their tops: the web then fills down between them and onto their tops, ending square where the solid ends along the line, flush with the walls' outer faces. A line that meets no solid, or a sketch that closes, fails on the feature. A rib is copied by Mirrored and the patterns like any other feature.

Scale body scales the whole solid about a point: by one Factor, or with Per axis by one along each of the body's X, Y and Z. It scales About the body's origin, the middle of the solid's bounding box, or a datum's origin (a datum point, a coordinate system). The inch → mm preset sets the factor to 25.4 for a part modelled in inches, and mm → inch goes the other way. Equal factors keep a cylinder a cylinder; unequal ones stretch it into a free-form surface, which some later features (an offset) cannot take. (The Scaled pattern is another thing: copies of a feature, each larger.)

Project sketch onto faces carries a sketch along its plane's normal onto picked faces of the solid, flat or curved: a label or a logo on a cylinder's wall. Select the sketch in the tree (and the faces, or add them in the task), then choose the mode: Split lines divides the faces along the sketch's curves and leaves the solid as it is (faces later features and colours can take), Emboss raises the regions the curves enclose out of the faces by the height, and Deboss sinks them in. Put the sketch beside the faces rather than through the solid: each curve lands on the side nearest the sketch. Carried straight onto a round wall, the sketch keeps its look from in front, but on the wall its widths stretch toward the sides.

Tick Wrap onto the curved surface to wrap the sketch onto the surface instead. The sketch's middle lands where the straight projection would put it, and the rest is laid onto the surface from there.

On a cylinder or cone the sketch is unrolled, as a paper label goes on a can: every length in the sketch is the same length on the wall. Its width runs round the axis and its height along it (on a cone, along the slope). A rectangle as wide as the wall's circumference goes all the way round, so a band or a scale can wrap much further than a straight projection reaches. The sketch's plane must run along the axis, not across it; a sketch that would reach more than once round is refused.

A sphere, a torus or a free-form face cannot take a flat sketch without stretching it, so the sketch is laid on as a flat sheet: every length running out from its middle is kept, and lengths across those lines stretch with the surface's curvature, little for a label small beside the surface. On a sphere of radius 10 a 6 x 4 rectangle covers 23.8 mm². The picked faces must all lie on one surface.

Recognize holes reads the body's solid for round holes: full bores open at one end or both, ending flat or in a drill point. It deletes their faces (one Delete faces feature) and drills them again as Hole features, one per set of alike holes on one plane, from a hidden sketch of their centres, so a recognized hole's diameter, depth and point are numbers to change like any hole's. Bores it cannot describe (a counterbore, a countersink, a slot) are left as they are and counted in the log. On an imported solid it gives the body its base shape first.

Patterns repeat features (the selected one, else the body's last that adds or cuts): Mirrored across a plane (the features picked in the tree, several with Ctrl, or with the body itself picked the whole body; its Originals list changes it after), Linear pattern along a line, Polar pattern about an axis, Circular pattern in concentric rings (each ring stepped out from the axis by the ring spacing, with a count of its own), Point pattern at a sketch's points (a copy at each point after the first, moved by how far it is from the first, so the original belongs on the first point drawn), and Path pattern along a sketch's chain of curves or an edge of the solid. Linear and polar patterns take Uneven spacing or Uneven steps, a gap of its own from each occurrence to the next; over the overall length or angle the gaps must add up to it, or the pattern is refused. A path pattern spreads its occurrences over the whole path (evenly round a closed one) or spaces them a distance apart along it; the original stands for the path's start, or its end with From the path's end, and each copy moves from there to its place, turned as the path turns with Turn with the path. An edge is found again on the solid as it stands where the pattern does in the history, so the copies follow the edge when the features before it change. Multi transform chains steps of every kind, a path among them, each applied to every occurrence before it. Fill pattern covers a region with copies in a Grid (a spacing along the rows and one between them) or a Honeycomb (each copy one spacing from its six neighbours): for vents and lightening holes. The region is a sketch's area (its regions chosen as a pad's are) or a flat face of the solid picked in the view, its outer edge bounding it. The lattice passes through the original and runs along the sketch's x axis (the body's X laid on a face), turned by Angle; the arrows on the original drag the spacings. A copy is made where all of it lies inside, at least Margin from the edge, and with Trim at the edge the copies the edge passes through are made too, trimmed to the region. The copies are the original's tool built once and moved, put in by one boolean, so a few hundred holes build in a second or two; more than 2000 are refused, with the spacing to widen. With a mirror's or pattern's task open, a dot stands at each occurrence, the original among them; click one to leave it out or bring it back. A skipped one draws crossed out, and the panel's Skipped row lists them, each with a button bringing it back and Clear bringing back all.

Generators (the toolbar's Generators list) make a sketch from a few numbers, set in its panel or with formulas: an involute gear to pad, a chain sprocket to pad, a stepped shaft to revolve, and a shaft's keyway to pocket. Each asks for its plane as a new sketch does.

A gear with a keyed bore and a chain sprocket, each a generated sketch padded

Split… (a body's menu, in the tree or the view) cuts a body into two pieces, each a body of its own: a part bigger than the bed, or one that prints without supports in two halves. It cuts across the middle of the solid, square to its longest side, and opens the first piece's task, where Cut by is a plane (a base plane, a datum plane or a sketch's plane of the body split, or a picked face) moved by Offset, or a sketch of the body whose profile is carried through the whole solid. The pieces build as the cut changes; Cancel takes them away. Each piece starts with a Clone of the body split and a Split feature keeping its side (in front of the plane or inside the profile, or with Keep the other side the rest), so editing the body split rebuilds the pieces. The body split is hidden, and the pieces stand where it stood. A change to one piece's cut is made to every piece of the split. From a script, design.split.

Separate pieces (a body's menu, in the tree or the view, offered when its solid is in more than one piece) makes each piece a body of its own: a plate pocketed through into two, a set of parts modelled in one body. Each piece starts with a Clone of the body and a Piece feature keeping the solid nearest a point on that piece, so editing the body rebuilds them; the body itself is hidden and the pieces stand where it stood. An edit that changes how many pieces there are does not add or remove bodies: each keeps the piece nearest its point. From a script, design.separate.

Section across X, Y or Z to sketch (a body's menu, in the tree or the view) cuts the solid with a plane through its middle, square to that axis, and keeps the outline as a new sketch on the plane, in a body of its own placed where the cut body stands: the outer boundary and every hole, each curve exact (lines, arcs, circles, ellipses, splines) and their ends joined, so a closed cut pads or pockets as drawn. The sketch is taken once and does not follow the solid. From a script, design.section takes any plane (a base plane, a datum plane or a sketch's plane) with an offset, and makes several parallel cuts with count and spacing, each a sketch of its own.

Borrowed geometry brings another body's sketch, or faces and edges of its solid, into this body, where the two bodies sit (Borrow geometry in Design; design.borrow). It follows its source, or keeps a frozen copy. A borrowed face is:

A borrowed edge is an axis to turn about, a direction to pad along, or a pipe's path.

The tree

The feature tree of the bracket: its sketches, pad, holes and fillet in order

Notes

A note puts a line of text on a face, an edge or a point of a body: a leader from the point to a label that reads its number and text (#3 Round this edge). There are two ways to make one:

A note moves with its body and follows its face or edge when the body is rebuilt. When an edit takes that face or edge away, the note is lost: it stays where it was, drawn red, and its tree row says Lost. A note on a spot the part hides from the view draws faint, its leader dashed. Each note keeps its number; a note taken away leaves its number unused.

The tree lists a body's notes under it, in an Annotations row: a resolved note is crossed out, a question still open shows ?. A double click or Edit note… opens one in the task panel, Open card on its card, Resolve and Reopen mark it, and its eye hides it. View › Annotations shows or hides every note at once (the note tool shows them while it is armed). A STEP export carries the shown notes with their text, on the faces they point at. How an agent reads and answers notes is in AI agents.

Rebuilding

Undo

Undo steps back through the recorded edits by applying their inverses. Each mouse gesture or command is one step, and the history keeps 64 steps. In a sketch's editing session every edit (a line drawn, a constraint added) is a step of its own. Imports, deleting a body that has anything in it, Replace shape, converting a mesh, refining and repairing a shape clear the history.

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