Distance

distance is the general linear dimension: point to point, point to line, line to line, or anything to a circumference. Dimensions are constraints with a value — they do not just relate two entities, they hold the relationship at a number, and that number is what you edit later.

In the viewport

1. Click the entities to measure: two points, a point and a line, a line and a circle, two parallel lines, two circles — or a single line for its own length.
2. Click Dimension. For a pair of points that is not axis-aligned, move the cursor to choose the measure — above or below the pair gives the horizontal distance, beside it the vertical one, inside or diagonal the aligned (straight-line) one — and click to place the label.
3. Type the value and press Enter. The statement is written after the geometry, the solver applies it, and the label stays on screen.

Shortcuts: double-click a line to dimension its length; double-click a dimension label to edit its value in place. Dimension labels can be hidden with the sketch dialog's Show constraints → Dimensional toggle.

A line picked: Dimension is enabled. It is the one button that is always available; with nothing picked it arms and waits for two picks.

Before

The base is drawn 70 long and the rise 25 tall, with no dimensions.

Afterdistance(base.start(), base.end(), 100)

Stretched to 100 × 45 by the two dimensions, whose labels stay on screen.

The code behind it

The guesses draw the base 70 long and the rise 25 tall; the two distance statements stretch them to 100 and 45. Combined with horizontal / vertical, a point-pair distance acts as a width or height.

l-profile.part.js

import { sketch, line } from 'fluidcad/core';
import { coincident, horizontal, vertical, fix, distance } from "fluidcad/constraints";

sketch("xy", () => {
    const base = line([0, 0], [70, 0]);
    const rise = line([70, 0], [70, 25]);
    coincident(base.end(), rise.start());
    horizontal(base);
    vertical(rise);
    fix(base.start());
    distance(base.start(), base.end(), 100);
    distance(rise.start(), rise.end(), 45);
})

In code

distance(p1, p2, 100)            // point ↔ point, straight-line
distance(p1, p2, 100, 'x')       // point ↔ point, measured along X only
distance(p1, p2, 45, 'y')        // ... along Y only
distance(p, l, 20)               // point ↔ line, perpendicular
distance(l1, l2, 30)             // line ↔ line (pair it with parallel)
distance(l, c, 130)              // line ↔ circle/arc, to the near side of the circumference
distance(l, c, 170).max()        // ... to the far side
distance(c1, c2, 5)              // circle ↔ circle, gap between circumferences
distance(origin(), p, 40)        // from a datum

Each form removes 1 DOF. The value may be a number or a param() so the Parameters panel can drive it.

Near side and far side

A distance from a line or point to a circle or arc measures to the circumference, not the center — the near side by default. Chain .max() for the far side. In the viewport the side you touch on the circle decides: a click on the side facing the other entity measures near, a click on the opposite side measures far; the timeline row's menu offers Use min/max tangent to flip a committed one.

The code behind it

gauge.part.js

import { sketch, line, circle } from 'fluidcad/core';
import { vertical, fix, distance, diameter } from "fluidcad/constraints";

sketch("xy", () => {
    const wall = line([0, 0], [0, 100]);
    const near = circle([140, 30], 40);
    const far = circle([140, 70], 40);
    vertical(wall);
    fix(wall.start());
    distance(wall.start(), wall.end(), 100);
    diameter(near, 40);
    diameter(far, 40);
    distance(wall, near, 130);        // to the near side of the circumference
    distance(wall, far, 170).max();   // to the far side instead
})

To measure to the center instead, dimension the center point: distance(wall, c.center(), 150).

Degrees of freedom

Every sketch entity carries parameters — a line has 4 (two endpoints), a circle 3 (center and radius), an arc 5, a point 2. Each constraint removes some; the tables on each page say how many. The sketch status readout shows the balance:

• Under-constrained — degrees of freedom remain. The geometry rests at its guesses and can still be dragged; the solver re-solves live while you drag, honouring every constraint. This is a fine working state.
• Fully constrained — zero DOF. Every entity is locked and renders green. This is the goal for production parts: the sketch is completely determined by its dimensions, so an edit anywhere has one predictable outcome.
• Over-constrained / conflicting — the diagnostics name the conflicting or redundant statements by file and line, and the affected geometry renders red. Remove the surplus statement.

Constrain the shape first (coincident, horizontal, tangent, …), then the size (dimensions), then the position (fix or a datum), and watch the counter fall to zero.

See also

• Diameter, Radius, Angle
• Parameters — driving a dimension from the Parameters panel