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Sketcher

The Sketch workbench draws flat outlines on a plane, holds them with constraints and dimensions, and hands their closed areas to the features that build solids.

Creating a sketch, choosing its plane and closing it again are described in Editing. This guide covers what happens while a sketch is open. Every number here can be a formula (Variables and formulas), and every tool has a sketch.* command behind it (Scripting).

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

Drawing

Pick a tool from the toolbar's geometry row (the Geometry panel with Tool panels on in Preferences › General › Interface) or by its key, then click in the view. A panel's caption opens its full tool menu; use the checkboxes to pin tools, or right-click a pinned button to unpin it. Reset pins restores the workbench's defaults. A card by the cursor names the tool, says what the next click does and lists the keys that apply. Escape drops a typed value first, then a half-drawn shape, then the selection.

A drawing tool stays in hand after its shape, ready for the next; Escape or a right click goes back to Select. With Continue drawing off (Display & snapping fold, Preferences › Sketch) each finished shape goes back to Select, a line after its first segment.

Tool Key Variants
Point O
Line L
Polyline P
Arc A Center and endpoints, Three points
Circle C Center and rim, Three points
Ellipse E Center and axes, Three points, Arc of ellipse, Arc of parabola, Arc of hyperbola
B-spline B Open, Periodic, Through points, Closed through points
Path
Rectangle R Two corners, Center and corner, Rounded, Three corners, Center and two corners, Frame
Regular polygon G Triangle to octagon (the Tool section sets any count from 3 to 12)
Slot S Straight slot, Arc slot
Text

A tool's variants open from the dropdown beside its button. The task panel's Tool section holds the options of the tool in hand: a polygon's sides, a slot's width, a rounded rectangle's radius, a frame's wall, a B-spline's degree, whether it is closed and whether its clicks are points it passes through.

A polygon's second click is a corner. With Across flats on in its Tool section, the click is the middle of a side instead: the polygon is sized by the circle inside it, the width across its flats (a hex nut trap's), and a second construction circle on the same centre touches the sides, so a diameter on it holds that width. A typed radius is then that circle's.

A rectangle's preview is the rectangle the click makes. A rounded rectangle whose corners do not fit its radius, or a frame with no room for its wall, draws dashed, and the click adds nothing.

A shape's sizes go in the card by the cursor before its last click (Tab moves on, Enter holds them by dimensions). A tool whose clicks set the whole shape stores it at its last click. One that leaves more to set (a rounded rectangle's radius, a frame's wall, an offset's distance, a corner's fillet or chamfer, a text) keeps it waiting in the panel's Tool section after the click: the section's fields now edit that result, and the view shows it solved as they change. A value that does not fit says why and holds OK back. One click makes one result: further clicks do not start another until it is put away. Only the section's Cancel drops it and leaves the sketch as it was; OK, Enter, Escape, a click in the view, another tool or finishing the sketch all store it as one undo step, as the section has it. Escape also puts the tool down; after the others the tool stays in hand when Continue drawing is on. An edit from elsewhere (an undo) puts it away. A recording of it is the sketch.draw call with that setting.

Paths and nodes. A spline can be edited by its nodes, as vector drawings edit paths. Double click a spline in the Select tool: it shows its nodes as squares, the curve kept; one that is not yet a chain of cubic pieces is rewritten as one (more control points, the same curve; a spline drawn through points stops passing through them, and one with weights is refused). Click a node to pick it: its two handles show, each joined to it by a line. Drag the node and its handles come with it; drag a handle and the node stays put. A node is Smooth (its handles held in one line through it, so the other handle turns with the one dragged), Symmetric (mirrored through it) or a Corner (each handle on its own). Right click a node for a menu of the three, its own ticked; nodes that were smooth on the curve come out smooth. Escape, another tool or a click on anything else ends the edit. The Path tool draws a path directly: click to place a corner node, press and drag to place a smooth node and pull its handles out (the other mirrored), click the first node to close the path, and Enter, a right click or a second click on the last node finishes it open. A closed path's first and last nodes are one point, so it closes a profile.

A spline drawn through points keeps passing through them as they move. While a constraint reads the curve (a point on it, a tangent, its length) or one of its control points, the solve moves the controls with the points, so the constraint holds on the curve as it is stored.

Lines. The line tool chains: each click ends one segment and starts the next, and a right click, Enter or Escape finishes. Press on the end the tool is drawing from and drag: that segment is an arc tangent to the one before, and the tool goes on with lines from the arc's end. A first press dragged and let go draws one line to where it was let go.

Polyline. The polyline draws lines and arcs in one run. M switches the next segment in turn between a line, a tangent arc, a square arc and a reversed arc; each arc stays tangent to what comes before it. A click back on the first point closes the shape and ends the run.

Each segment of a line or polyline run is an undo step of its own. Backspace takes back the segment just drawn and the run goes on from where it started; Undo does the same, and a run whose start an undo or another edit took away ends, the next click starting afresh.

Typed values. While a shape is being drawn, the card by the cursor shows its sizes as they follow the cursor: a line's length and angle, a rectangle's width and height, a circle's diameter, an arc's radius and sweep, a polygon's radius and turn, a slot's length, angle and width. Before the first click it shows X and Y, so the first point can be typed too. Start typing and the value goes into the first field; Tab moves to the next. A field takes a number or a formula over the document's variables (Printer.wall * 2), worked out once as it is entered; the shape keeps no link to the formula. A typed field's lock shuts: it holds its value while the cursor moves. Escape empties the fields. The card stands on the side of the cursor where it hides the least of the sketch, and gives way to a dimension's card while one is open.

Some steps only place a point (a three-point shape's first point, an ellipse's axes); there the card says "Enter places it". A value that does not work out is named in the log and left in the field to be mended. Once a value is typed, moving the cursor back across the start does not flip the shape over.

Snaps, hints and auto constraints

The cursor is drawn to ends, midpoints, centres, curves, intersections and the sketch's axes. While a line is drawn it also snaps level or plumb with its start, parallel or square to a line it passes near, and onto a line's extension past its end. A dashed hint line shows which snap is taking the cursor, and the click leaves the matching constraint (horizontal, vertical, parallel, perpendicular, point on object). A direction that reaches a curve or an axis near the cursor lands where it crosses it, and the click leaves both (the hint names both, "Perpendicular to · On axis").

With no drawing tool in hand the same marks and names show what the cursor is on (an end, a centre, a line's middle, a curve, the origin or an axis) without moving anything, so you can see where a drag or the next shape would snap. While a constraint tool waits for picks the mark names what its click takes: a point, or the curve or axis itself (over a line's middle it says On curve, since the tool takes the line).

When several snaps are in reach, an existing point wins first (the new curve then shares it, so outlines close), then the origin, a crossing, a line's middle, a foot or touching point from the start, a curve or an axis, level or plumb, parallel or square, and last an extension. Of two alike, the nearer wins; of two as near, the line nearer the cursor, then the one further left and lower. Points lying on one spot go by which was drawn first. A curve whose points are missing, or a circle of negative radius, takes no snap.

A centre-point arc's end always lies on the arc's circle, so its click takes only snaps on that circle: a point standing on it, or where the circle crosses a line, circle, arc or axis near the cursor (held there). Anywhere else the end lands on the circle in line with the cursor and the cue names no snap.

Hold Shift while drawing a line and it leaves its start in whole steps of the angle snap step (15° to start with; 1°, 5°, 10°, 30°, 45° and 90° are offered), as far as the cursor reaches that way.

Arc helpers. While a drawing tool is in hand, the rest of each arc's circle, past its ends, draws as a dashed guide. A point dropped on it lands on the circle, marked where it lands, and with Auto constraints on is held on the arc by a point on object constraint (as a point dropped on a line's extension is held on the line).

The toolbar's Snap to objects and Grid buttons, and the drawing switches in the task panel's Display & snapping fold (Angle snap step, Show grid, Grid auto spacing, Snap to grid, Snap to objects, Reuse existing lines, Auto constraints, Arc helpers), turn these on and off.

Reuse existing lines. Off to start with, a shape drawn against a line draws its own line on top of it, even between the same two points (a second rectangle against the first one's wall). On, a line a drawing tool would lay between two points a line already joins is that line: the rectangles, polygons, slots' straight sides and a line or polyline segment repeating one all use it, and a point of the shape that lies exactly on that line's end is that end. A drawn line reuses only a drawn line and a construction line only a construction line; external geometry is never reused. The existing line keeps its constraints, and those the shape would add to it that the sketch already enforces (the second rectangle's vertical on the wall) are left out; typed values stay. Preferences › Sketch sets it for every sketch.

Grid. Show grid lays a grid on the sketch plane, its lines along the sketch's axes from its origin. Three spacings draw at once, each ten times the last, and each fades in as zooming in spreads its lines apart, so the grid gets finer as you close in. With Grid auto spacing the spacings are powers of ten of a millimetre, as the view's own grid is; off, they count from Grid size (7.5 mm gives 7.5, 75 and 750 mm). Snap to grid lands a click on the finest lines drawn clearly, never on lines too faint to see.

Joining by dragging. Drag a point onto another point or onto a curve and hold it there a moment: when you let go, it is joined with a coincident or point-on-object constraint. How long it must rest is Preferences › Sketch › Drag constraint delay (400 ms to start). It needs Auto constraints on.

Constraints and dimensions

Select elements, then pick a constraint. A plain letter picks a drawing tool; Shift and a letter picks a constraint.

Constraint Key Variants
Coincident Shift+C
Point on object Shift+O Point on object, Midpoint
Horizontal Shift+H Horizontal, Horizontal or vertical (whichever is nearer)
Vertical Shift+V
Parallel Shift+P
Collinear Shift+J
Perpendicular Shift+N
Tangent Shift+T
Equal Shift+E
Symmetric Shift+S
Block Shift+B
Group Shift+G
Dimension Shift+D
Lock Shift+K
Horizontal distance Shift+L
Vertical distance Shift+I
Distance Distance, Gap between curves
Arc length
Radius Shift+R Radius, Radius or diameter by kind, An ellipse's minor radius
Diameter
Angle Shift+A Between two lines, To the X axis, To the Y axis, Where two curves meet, An arc's opening, By three points
Refraction

Dimension (Shift+D) gives whatever the selection takes: a length, a distance, a radius or an angle. Lock holds a point where it is, as two distances from the origin. Horizontal distance and Vertical distance take two points, a point (from the origin), a line (between its ends) or two lines (between the ends of each that lie nearest each other).

One dimension per size. A dimension the sketch already holds is not made again: the tool selects the one it holds and says so, and the command refuses it. This counts the same dimension in another form too: a circle's radius beside its diameter, a line's length beside the distance between its ends (a length typed while drawing is that distance), and a distance from A to B beside one from B to A. A reference dimension holds its size as much as a driving one, and so does one switched off; change the value of the one there, or make it driving, instead. Block fixes an element in place.

Coincident (Shift+C) joins points; on a point and a curve it puts the point on the curve, and on two or more circles, arcs or ellipses it makes them concentric, each centre on the first one's. Curves that share a centre already are left as they are, and the tool says so.

Collinear (Shift+J) puts two or more lines on one line: each after the first lands on the first one's line, wherever along it.

Symmetric takes two points and a line, three points (the last is the centre), or a curve and then a line: the curve's two ends mirror each other about the line.

Group (Shift+G) holds the selected elements together as one rigid piece. The piece keeps its shape but still moves and turns: drag any member and the whole group comes with it.

Waiting for picks. A constraint or dimension tool picked while the selection does not fit it yet stays armed (its button lit) and takes more clicks. A click on the sketch adds an element; a click on an edge of a solid adds that edge, or the vertex at its end. Once the picks fit, the model's edges are projected into the sketch as guides and the constraint goes on, all as one undo step. Enter applies the tool to a single item; Escape or a right click puts it away. Editing has more on this.

Continue constraining. A constraint tool puts itself away once its constraint is on. With Continue constraining on (Display & snapping fold, Preferences › Sketch) it arms again with nothing picked, so the next clicks get the same constraint, until Escape or a right click.

Editing a dimension. A new dimension opens a card by its label, the measured value in its Value field and selected, so typing replaces it: type a value or a formula and press Enter or OK (a click elsewhere in the view is OK too). The dimension is made only then; Escape or Cancel leaves it unmade, with nothing to undo. A double click on a dimension's label opens its card again, and so does a value or formula typed into its row in the constraint list. While the card is open the view shows the sketch solved at the value, and the line under the field says what it comes to; a value the sketch cannot take (a loop of formulas, an unknown name, a length below zero, constraints that cannot be met) says why on the card and holds OK back. OK is one undo step; Cancel and Escape leave the dimension as it was. For a circle, Measures switches between dimensioning the radius and the diameter; for an arc's length, between its length and its sweep in degrees. The card also offers the document's variables and "Save as variable" (Variables and formulas). Another tool, or an edit that changes the sketch under it, puts the card away. Drag a label to move it. A label you have not moved sits clear of what it measures: a length or distance, horizontal and vertical ones too, off the outside of the shape it belongs to, an arc's length outside the arc, an angle between its rays. Constraint symbols keep their size to the labels, so a larger label size (Preferences › Sketch) or UI scale makes them, and the area that takes a click on them, larger alike.

What is held. Geometry draws white while it can still move. An element nothing left free can move (a point fixed in both directions, a line whose ends both are, a circle whose centre and size are) draws blue, so the parts already done stand out while the rest of the sketch is still free. Once the whole sketch is fully constrained, everything draws green.

Renaming. A double click on a geometric constraint's glyph opens its row in the constraint list for a new name. A named dimension can be read by formulas elsewhere.

Big changes keep the shape. A dimension typed far from its value, or a drag that pulls the sketch a long way, can be met by the shape's mirror image as well as by the shape itself. When a change moves the sketch more than a twentieth of its size, the solver walks there in small steps from where the sketch stands, so a corner stays on the side it was on. A small change is solved in one step.

The task panel. Its header names the sketch, says what it stands on, and shows the solver's state as a pill (degrees of freedom left, fully constrained, conflicting); Cancel puts the sketch back as the session found it and Done keeps it. Under it, the Elements and Constraints lists, each folding on its own, share one filter: type a name, or choose Selected, Related to selection, Relations, Dimensions, Reference, Named, Parked, Normal geometry or Construction. An element row shows its size (a line's length, a radius, a point's place) and, before it, a badge for each constraint on the element or its points (four, then "+N"), coloured as the constraint's row; a constraint row names its kind and, as chips, the elements it ties ("Line 2", "Point 4"), its value plain until the row is hovered or selected, when the field and its fx show. Hovering a row lights what it stands for in the view; hovering a chip lights its element, here and in the view, and hovering a badge its constraint. Clicking a chip or badge selects what it names and scrolls its row into view. While a row, chip or badge is hovered, or while anything is selected, the rows related to it draw with a faint yellow tint and a bar at their left: a constraint's elements and the curves ending at its points, an element's constraints, its points and the curves sharing them. While a filter narrows the constraints, Delete N shown deletes every one it shows. A constraint row's menu activates or deactivates it, makes a dimension driving or reference (measured, not enforced), renames, parks or deletes it. Placement, Solver and Display & snapping fold away at the end, each with a one-line summary; Labels show, in Display, sets what a dimension's label reads: its value, its name, or both.

The toolbar's constraint row also has Toggle driving / reference, Toggle active, Park / unpark constraints (parked glyphs draw only while Show parked constraints is on), Remove axis alignment, and selectors for conflicting, redundant, malformed and under-constrained elements. Select origin, Select horizontal axis and Select vertical axis, in the toolbar's Reference group beside External geometry, add the sketch's origin or axis to the selection, so a constraint tool can take it without a click on it; while a constraint tool waits for its picks, they hand it the reference as its next pick. The badge in the view's corner gives the sketch's degrees of freedom, and the header's pill what the solver found; a conflict or redundancy also shows a card at the top of the panel, which selects what the offending constraints hold when clicked. The Solver fold holds how the solver runs (auto update, removing redundants, its step limit and tolerance). With Auto remove redundants on, a constraint added with a constraint tool takes away the older constraints it makes redundant, and a shape a drawing tool makes drops those of its own constraints the sketch already enforces (a rectangle drawn onto another's wall leaves out the vertical the wall holds already), keeping what the sketch held before; typed values always stay.

Modifying

Tool Key What it does
Fillet Rounds a corner, or joins two curves with an arc (variant: Chamfer)
Trim T Removes the span clicked, or every span a drag crosses
Extend Extends a curve's end to the next curve
Split Splits a curve where you click
Copy, Move, Rotate, Scale Copy, move, turn or size the selection from a base point or pivot
Offset Copies each selected curve or chain at a distance
Symmetry Mirrors the selection about a line, two points or a point
Rectangular array Copies the selection into rows and columns
Join curves Merges a chain of curves into one B-spline

Fillet and Chamfer take a radius or length in the Tool section, and Keep it leaves the corner as a construction point on both curves, with its constraints. A click on a corner (or on the second curve) does not cut at once: it waits in the Tool section, which names the two curves, and the view shows the corner cut and solved as the radius, length or Keep it change. A size the curves cannot take says why and holds OK back. As with a shape, only Cancel drops it; OK and everything else cut it as one undo step. The size carries on to the next corner. A script's sketch.draw with tool = "fillet" still cuts at once, and a recording of it is that call with the size applied.

Spline edits. Raising a spline's degree and inserting a knot keep the curve. Lowering the degree, lowering a knot's multiplicity and removing a knot fit the nearest curve, and the log gives the largest deviation found by sampling every span, in mm. A projected spline follows its source and takes none of these edits. Convert to B-spline keeps a point held on the curve held on the spline, as long as the point lies on the spline's span.

Trim and Extend at the axes. By default the sketch's axes do not cut. Press U while Trim or Extend is in hand, or tick Cut at the axes (U) in the Tool section, and the two axes cut as curves do; an end left on an axis is held on it. Trimming the middle of a line leaves two pieces held collinear, so they stay on one line.

Patterns. Move, Rotate and Scale take a number of copies. For Move and Rotate:

Offset copies the selected curves to the side of its click. Several curves or chains (circles, or an outline and the holes in it) are copied each on its own in one step: the closed ones all grow or all shrink as the one nearest the click does, and an open one goes to the click's side. A closed chain of lines and arcs shrunk past a narrow part splits there into the loops that keep the whole distance from it. The copies wait in the Tool section, whose distance, Round, Both sides and other switches change them in the view; as with a shape, only Cancel drops them, and OK and everything else copy at what the section shows, carried on to the tool. A frame round any outline is its offset with the original kept. Offset can also replace the original, or stay held to it by one dimension (both in the Tool section). Symmetry can keep the original and hold the image to it with symmetric constraints. Copies, patterns and arrays keep text as text.

Manual dimension labels move, turn, mirror and scale with their geometry, including labels on copies. Their text size stays set by Appearance. Automatic labels are placed for the current view. A dimension spanning selected and unselected elements keeps its placement.

Selecting and viewing

Regions and profiles

A closed sketch shades every region its curves close, the same way while it is edited and out of editing, so it looks alike as it opens and closes. The regions a plain Pad takes (every loop, a loop inside another a hole) shade a little stronger than the rest, such as the ring between two loops inside a third. A curve's loose end, which the profile leaves out, has a red ring once no shape is being drawn.

A Pad, Pocket, Revolution or Groove made from a sketch whose curves stop just short of each other (ends within half a percent of the sketch's size) joins those ends in the same step, as Repair sketch would, and its task says what it joined, with Undo the join to put the sketch back. Cancel puts it back too. A sketch the join cannot close is left alone, and the feature names its loose ends.

Curves may cross, branch or leave a spur. Every closed area between them is a region: two overlapping circles make three, the lens and two crescents. Pad, Pocket, Revolution and Groove take every region by default, and can take only the ones you click in the view or tick in their task, so two crossing circles can pad just their overlap (Editing).

Out of editing, each region can be picked. The region under the pointer lights in the hover colour; click it to pick it alone, Ctrl+click to add or take away regions, and picked regions draw in the selection colour. Pad, Pocket, Revolution and Groove started then take exactly the picked regions. The curve under the pointer lights on its own, the rest of the sketch staying plain, and Ctrl+click on it picks the curve itself. A click on the sketch's lines or its tree row selects the whole sketch, and with the whole sketch a Pad takes what it always took. A Pipe started with curves picked runs along those curves alone (Editing).

Validate sketch reports stray points, constraints naming missing geometry and whether the sketch closes, and selects what it finds. Check wall thickness marks where the profile gets thinner than Preferences › Sketch › Minimum wall.

Repair

Repair sketch (the sketch row of the toolbar) puts right what stops an outline from closing or solving: ends that nearly meet (within the snap reach) become one point, curves of no length and doubled curves go, and constraints left naming nothing, or the same thing twice, go with them. An arc whose two ends meet becomes the circle it nearly was, keeping what named it. Drawn ends stay drawn. The log says what it did. Imported outlines need it most.

Reference pictures

File › Import takes a PNG or JPEG as a reference picture. It lies on the plane of the sketch being edited (else in a new sketch), shown while the sketch is edited, to draw over. It only draws: no profile and no constraint come of it. Seen at an angle, it draws in true perspective.

The task panel's Reference images section sets each picture's middle, width, turn and opacity, and removes it.

Calibrate sizes a picture from a length you know on it: click the two ends of that length on the picture, type the real length (a value or a formula), and Apply. Two options go with it:

File › Import also reads a DXF drawing into a new sketch.

A picture's scale

A picture placed without a width takes the size its file states (a PNG's or JPEG's resolution), and says so: until it is measured against something of known size, an UNCALIBRATED mark stands on its corner with where its scale came from. Calibrate it by a distance (the panel's Calibrate: two points and the length between them) or by a circle: pc.sketch.calibrate_image{sketch = s, x = …, y = …, diameter = 10} fits the circle whose rim the point is on (a gauge pin or a washer laid on the glass beside the part) and scales the picture about its centre.

A scanner's sensor and its carriage may not agree, a picture coming out a little stretched one way. pc.sketch.calibrate_axis{sketch = s, from = {x, y}, to = {x, y}, length = 100, axis = "y"} scales the picture along one of its own axes only: calibrate across with a ruler laid along the rows, then down with one laid along the columns. Every measure reads the picture as stretched. pc.sketch.save_scanner_profile{sketch = s, name = "flatbed 600"} keeps what a calibrated picture's pixels measure (in the configuration folder's scanner_profiles.json), and a later picture whose file states the same resolution takes that scale when it is placed without a width, or sketch.image{profile = …} names one.

Squaring a picture

pc.sketch.align_image{sketch = s, origin = {x, y}, toward = {x, y}} moves and turns a picture so the first point is the sketch's origin and the second lies along +x from it (a sheet's edge, a part's datum). pc.sketch.turn_image{sketch = s, quarters = 1} turns it by quarter turns about the origin, and mirror = true shows a part scanned face down as it is.

Edges of a picture

A picture of a part on a flatbed scanner is a measurement once it is calibrated. Its edges are found as it loads, to a tenth of a pixel, and drawn over it in the external colour while the sketch is open. Fit to a picture's edge (External geometry row) fits a click: it starts from a dozen edge points at the click and runs on both ways while each next point keeps to the shape, so a line stops at a corner and a circle runs round its whole rim. It takes the shape that runs further, logs how far the points stray (σ), and refuses a line on a curve or a circle on less than 8° of round.

While a picture's edges are found, a click of Point, Line, Polyline, Arc or Circle by three points, or B-spline lands on the nearest edge within the snap reach, anywhere along it to a fraction of a pixel, and a loupe beside the cursor shows the picture round the point magnified four times, its edges and the point crossed. A point, a curve's end or a crossing within reach still wins. Hold Alt to place the click where it is. pc.sketch.fit_edge{sketch = s, x = …, y = …, kind = "circle"} does the same from a script; with box = {{x, y}, {x, y}} it fits every edge point in the box instead, leaving out the points that stray past three times the median stray (a burr, a speck of dust, a neighbouring edge) and answering how many went.

pc.sketch.image_objects{sketch = s} finds the separate parts on the sketch's pictures: the picture is split into part and ground by its grey level, and each part is measured in millimetres where the picture lies. You get its area (holes left out), its holes, centroid, the diameter of a disc of the same area, its widest and narrowest caliper widths and the direction of its long axis; outlines = true adds its boundary. Lay a handful of washers on the glass and read them all at once.

pc.sketch.bolt_circle{sketch = s, circles = {…}} puts the circle through the centres of three or more circles (a flange's bolt holes) as construction, with how far each hole strays from it and its angle round it.

pc.sketch.image_profile{sketch = s, x = …, y = …} reads the part nearest a point as its radius against angle round its centroid and counts the profile's peaks that stand out by at least prominence (0.2 mm): a gear's teeth or a knurl's ridges, with their pitch and the profile's inner and outer radius.

Text

The Text tool writes text on the sketch: click where its baseline starts. The text then waits in the Tool section, whose text, font, size and other fields change it in the view as they are set; OK (or Escape, a click in the view, another tool) writes it, and Cancel drops it. Another text takes another use of the tool. A text is one object standing on a point: a click on any of its letters selects it whole, dragging moves it, and constraints go on its point (fix it, put it on a line, dimension it from an edge), never on the letters. The letters are closed outlines that pad, pocket and export as any profile does; they are made from the text each time the sketch is read, so the text stays editable.

The Tool section's Layout buttons say where new text goes:

The Align buttons put each line at the start, middle or end of its room (along the curve, from the point), as a text editor's do; the Up and down buttons put the lines on the baseline, or with their top, middle or bottom on the point (in a frame, at its top, middle or bottom); Line spacing is a share of the font's own.

The Tool section (and, with a text selected, its Text section) sets the text, the font, its size, spacing and angle. The font is one of the bundled IBM Plex faces, an installed font chosen by family, or a font file. An installed font or a font file is kept in the document, so the text rebuilds the same on another computer. Size, spacing and angle can be set by a formula (Variables and formulas), and the text itself can show one: REV {Part.rev} writes the variable's value and follows it, {Width * 2:1} writes one decimal, and {{ or }} is a brace. A length shows in millimetres, an angle in degrees.

Explode to curves in the Text section turns a text into plain lines and splines, which can then be edited one by one; the text itself is gone. The curves keep the names the letters had, so a pad built from the text keeps its faces.

External geometry

External geometry (X) brings a solid's edges into the sketch, projected onto its plane. Click edges, or a face for every edge around it; Ctrl picks more. Its Intersection with faces variant takes faces instead and adds the curves where they cross the sketch plane. External from a sketch or datum brings in another sketch's curves or a datum's line, point or crossing.

Projected geometry is drawn in the external colour. It is a guide (dashed) until it counts in the profile (solid): Construction (N), or Toggle external geometry in profiles, switches the selected projections between the two. New projections follow the construction mode: guides in it, counting out of it. Projected geometry is never dragged.

Projected geometry follows its source: when the solid, sketch or datum changes, the projection is brought up to it without the sketch being opened, including edges of the sketch's own body, keeping the constraints on it where the shapes are the same kind. When what it came from is gone, the elements stay where they were, their rows in the task panel's Elements list read "lost", and the sketch's row in the tree shows a warning badge saying how many were lost. Edit the sketch to remove or replace them.

Sketching on a scan

Select an Inspection section or fitted plane and Create sketch puts the new sketch on it, in a body of its own. While a sketch is open, every visible scan its plane crosses shows the cut as a dashed line: the slice of the scan at the sketch plane, moving with the plane and with the scan when it is aligned. Place the sketch on a fitted plane, a coordinate plane or at an offset to choose the slice.

Fit the scan's section (External geometry row) turns every slice into lines and arcs end to end, each scan point within 0.1 mm of its piece, a closed slice closing so it pads at once. Sharp corners the scan rounds off come back sharp, lines within 3° of the sketch's axes turn onto them, and slices shorter than 1 mm are left out. In Construction mode the pieces come in as construction, to draw over. pc.sketch.fit_scan{sketch = s, tolerance = 0.05, axis_snap = 0} changes those.

The slice draws in the fitting colour where it lies within the Scan fit range (Preferences › Sketcher › Printing, 0.1 mm) of the sketch's curves, and in the conflict colour where it strays, and the status bar counts the points within range: draw or dimension, and see at once where the sketch leaves the part.

Each fitted piece keeps the slice points along it. Constraints and dimensions are always met exactly; the points then decide what they leave free, by least squares. Dimension a fitted outline 20 × 30 and it stays where the scan is, square to its sides, rather than wherever the solver last left it. A dimension the rest cannot meet is reported as a conflict, never bent to fit the points.

Design values

Geometry fitted to a scan reads 19.98 where the part was drawn at 20. Select lines, arcs or circles while the sketch is open and each shows its size next to its probable design value (halves under 10 mm, whole millimetres above, radii to 0.5 mm). Dimension at design values holds the selected ones there with driving dimensions, or every unsized one when nothing is selected.

pc.sketch.candidates{sketch = s} lists the same sizes, and the relations the geometry nearly keeps but no constraint states yet (horizontal, vertical, parallel, perpendicular, equal, concentric), each with how far it is off: evidence to weigh, never applied on its own. pc.sketch.design_values{sketch = s, elements = {…}} holds sizes.

Saving as DXF, SVG or CSV

Save as DXF…, Save as SVG… and Save as CSV… (the sketch tools) write the open sketch at true scale in its own millimetres.

The DXF is R2000 with its unit declared. Lines, circles and arcs are written as themselves and other curves as polylines within 0.01 mm, on layer ELEMENTS; construction and guides go dashed on CONSTRUCTION, the pictures' edges, thinned to 0.01 mm, dashed on PICTURE_EDGES, and text blocks as text on NOTES. NOTES also holds a traceability line under the drawing: the scale, each picture's millimetres per pixel and where that came from (as given, the file's dpi, or what it was calibrated by), and the sketch's frame (its plane's origin and axes). pc.sketch.export_dxf{sketch = s, path = …, units = "inch"} writes it in inches; a DXF written comes back through File › Import.

The SVG is a millimetre a unit, y up as in the sketch, every curve a polyline within 0.01 mm, guides dashed, the traceability line under it: ready for a laser cutter or a plotter (sketch.export_svg).

The CSV starts with the traceability line (#), then a row per element (kind, id, drawn or construction, its points, radius and length) and per dimension (kind, id, name, driving or reference, value and unit); pc.sketch.export_csv{sketch = s} answers it as text.

Merge and carbon copy

Merge sketches makes a new sketch of this one and the sketches you tick; the originals stay as they are. Carbon copy copies another sketch's geometry into this one, with its constraints, as geometry of this sketch. Both need sketches on a parallel plane. Under a turn or a mirror between the planes, constraints stated against the sketch axes follow, and projected geometry stays projected from its solid, sketch or datum.

Mirror sketch makes a new sketch on the same plane with this one's geometry mirrored across its Y axis. Attach sketch moves the sketch onto the face selected on the solid, and Reorient sketch flips its normal or turns it 90°.

Preferences

Preferences › Sketch holds the workbench's settings.

Solver & constraints: Auto constraints, Drag constraint delay, Angle snap step, Continue drawing, Continue constraining, Hint lines (the dashed guides; off, the snaps still work), Arc helpers (the arcs' circles as guides and snaps), Avoid redundant auto constraints, Auto remove redundants, Reuse existing lines, Ask for a dimension's value, Snap to objects, Section view on open, Shade closed regions.

Printing: Minimum wall, for the wall thickness check.

Appearance:

Setting What it sets
Label size The size of the dimensions' values
Label face Monospace or Sans
Dimension lines How wide dimension, extension and leader lines draw
Dashed dimension lines Tones the dimensions down against the geometry
Axes How wide the sketch's axes draw while not picked
Dashed axes
Grid How much the grid's widest lines show, from faint to solid; finer ones show less
Grid lines Dotted, dashed or solid
Grid colour
Region shading How strongly closed regions are shaded

Colors shows the sketch palette.

Keys

The tool keys and M can be changed in Preferences › Keyboard; U, Tab, Enter, Escape and Backspace are fixed.

Keys Tools
O, L, P, A, C Point, line, polyline, arc, circle
E, B, R, G, S Ellipse, B-spline, rectangle, polygon, slot
T, X, N Trim, external geometry, construction
V View sketch
I Show or hide internal geometry
M Polyline: switch between lines and arcs
U Trim or Extend: cut at the axes
Shift+C, Shift+O Coincident, point on object
Shift+H, Shift+V Horizontal, vertical
Shift+P, Shift+N, Shift+T Parallel, perpendicular, tangent
Shift+J Collinear
Shift+E, Shift+S Equal, symmetric
Shift+B, Shift+G, Shift+K Block, group, lock
Shift+D, Shift+R, Shift+A Dimension, radius, angle
Shift+L, Shift+I Horizontal, vertical distance
Tab, Enter Next typed field; place and constrain
Escape Drop a typed value, then a half-drawn shape, then the selection
Backspace Line or polyline: take back the segment just drawn

While a value is being typed, number keys go to it.

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