Sketch relations and dimensions — PartCraft help

Relations fix how geometry sits relative to other geometry. Dimensions fix sizes. To add a relation, select items with the Select tool (SS) and choose its button in the right panel; to add a dimension, use the Dimension tool (DD) or the dimension buttons in the right panel. How to work with them: Fully define a sketch.

"Curve" below means a circle or an arc. The origin counts as a point.

Relations

Button	Symbol	Select	Effect
• Coincident	• (shown only when selected or in trouble)	Two points	The points meet
• Coincident	•	A point and a line	The point lies on the line (or its extension)
• Coincident	•	A point and a curve	The point lies on the circle or arc
H Horizontal	H	A line, or two points	The line is level, or the two points are at the same height
V Vertical	V	A line, or two points	The line is upright, or the points are one above the other
∥ Parallel	∥	Two lines	The lines run the same way
⊥ Perpendicular	⊥	Two lines	The lines meet at a right angle
T Tangent	T	A line and a curve	The line touches the curve without crossing
T Tangent	T	Two curves	They touch, outside or inside, as drawn
T Tangent	T	A spline and a line, arc or spline that meets one of its ends	The spline leaves that end in the other curve's direction
= Equal	=	Two lines	Same length
= Equal	=	Two curves	Same radius
◎ Concentric	◎	Two curves	Same center
◎ Concentric	◎	A point and a curve	The point sits at the curve's center
M Midpoint	M	A point and a line	The point sits at the line's middle
↔ Symmetric	↔	Two points and a line	The points are mirror images about the line (Mirror adds these)
⚓ Fix	⚓	A point, a line, a curve or a spline	Holds it exactly where it is now (a spline: its points)

Lines here include centerlines. Drawing adds some relations for you: snapping to a point makes it coincident, snapping to a curve puts the point on it, nearly level or upright lines get H or V, and a rectangle comes with its four corners joined, two H and two V.

Fix is a quick way to stop something moving, but the part then cannot follow a dimension change elsewhere. Prefer dimensions to the origin.

Dimensions

Button	Select	Measures	Shown as
Distance	A line	Its length	Distance 40
Distance	Two points	The straight distance between them	Distance 40
Distance	A point and a line	The distance from the point to the line, square to it	Distance 40
Distance	Two parallel lines	The gap between them	Distance 40
Horizontal distance	Two points, or a line	The left-right distance only	Horizontal distance 40
Vertical distance	Two points, or a line	The up-down distance only	Vertical distance 40
Radius	A circle or arc	Its radius	Radius R10
Diameter	A circle or arc	Its diameter	Diameter ⌀20
Angle	Two lines that are not parallel	The angle between them, 0 to 180 degrees	Angle 30°

With the Dimension tool, PartCraft picks the kind from what you click and where you place the number:

You click	You get
One line	Its length; for a slanted line, horizontal if the number goes above or below it, vertical if to the side
One circle	Diameter
One arc	Radius
Two points	Distance; horizontal or vertical as for a slanted line
A point and a line	Distance from the point to the line
Two lines	Angle, or the distance if they are parallel
A point and a circle	Nothing: "Those items cannot be dimensioned together." Dimension to the circle's center point instead

Offset (shown as the distance) is made by the Offset tool: it holds a copied line parallel at that distance, or a copied arc or circle concentric with a radius that much bigger or smaller. The other pieces of the same offset carry an O relation and follow the one Offset dimension. See Splines, trim, offset and other sketch tools.

Dimension values are millimeters (or degrees), never negative. Radius and diameter must be more than zero. A value of 0 is allowed for distances: two points 0 apart are coincident.

How solving behaves

Least movement. When a value changes, the solver moves the geometry as little as possible. A line whose length changes grows equally at both ends if nothing holds either end.
No flipping. Distances from a point to a line, horizontal and vertical distances, angles and tangency remember which side they were made on. Changing a value never flips the geometry to the other side.
Conflicts leave things alone. If relations contradict each other, the sketch stays exactly as it was and the conflicting ones turn red.
Redundant relations (implied by others) are named in the status bar ("is already implied. Delete it.") and the feature still builds, with a warning.
Tangent joints. Where a fillet arc meets its lines at a shared end point, tangency is solved in a form that stays well defined there, so sketch fillets do not read as over defined.

Not available yet

Collinear, coradial and pierce relations; a point on a spline; driven (reference) dimensions; ordinate and arc-length dimensions; equations between dimensions. Use Parallel plus a 0 distance for collinear lines.