Quickstart: an angle bracket

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Prefer being shown? Bear can walk you through this very bracket inside the app: start the tutorial, or press Tutorial in the status bar.

A 120-degree angle bracket: rounded bend, rounded corners, two countersunk screw holes. Draw it sloppily, let the constraint solver square it up, then change the bend angle afterward without redrawing.

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1. Set up parameters

In the Parameters pane, click + and add:

Name	Value
leg	50mm
width	40mm
thick	5mm
hole	5mm
bend	4mm
bend_angle	120deg

Any dimension field accepts these names and arithmetic like leg - thick. Typing name=value in a dimension field creates a parameter on the spot. More in Parameters & units.

2. Draw the profile — roughly

Press L (Line) and click on the ground plane. Clicks chain segments; snapping closes the loop back at the start.

Draw the cross-section as six lines: a long base leg, a short end cap, back along the inside of the base, up the inside of the tilted leg (roughly 120° from the base), a short end cap, and back down to the start. Don't be precise — the next step squares it up. When the loop closes, the profile fills in.

3. Square it up with constraints

Press C (Constraint). For each constraint, select the line(s), then press its number key:

First pin it down: select the bend corner and the origin, press 4 (Coincident). Then:

1. Bottom base line + the X axis: 1 — Parallel (this makes it horizontal).
2. Bottom + inner base lines: 1 — Parallel.
3. The two tilted leg lines: 1 — Parallel.
4. Base end cap + bottom base line: 2 — Perpendicular.
5. Leg end cap + outer leg line: 2 — Perpendicular.

Now exact sizes with the Dimension tool (D): click a line, type the value, Enter:

• both outer legs: leg
• both end caps: thick

For the bend angle: select the bottom base line and the inner leg line, press D, type bend_angle, Enter.

4. Extrude it

Esc to leave the sketch, then E (Extrude). Click the profile face, type width, Enter.

5. Round the bend

With no sketch open, press F (Fillet):

1. Click the inside edge of the bend, type bend, Enter.
2. Click the outside edge, type bend+thick, Enter.

The two rounds are concentric, like bent sheet metal.

6. Cut the screw holes

Drill from the inside face of the base flange — where the screw heads sit:

1. Press S (Sketch), click the inside face of the base flange.
2. Press O (Circle). Click near the flange's tip, type hole for the diameter, Enter. Place a second circle beside it.
3. Position them with the Dimension tool (D): click a circle's center and a face edge, type the distance.
4. Esc, then E to extrude. Click both circles, drag the handle into the bracket (or type thick + 1), pick Cut, Enter.

7. Countersink the holes

Press K (Chamfer) and click the rim of one hole — where the hole meets the inside face. Shift+click the other rim, type 1.2, Enter.

8. Round the corners

Press F (Fillet), click a vertical edge at a flange tip, Shift+click the others, type 2, Enter.

9. Engrave a label

Press T (Text) and click the outer face of the base flange. Type BearCAD and center it on the face. Press E (Extrude), click the text, push the handle into the face (type 1), pick Cut — engraved letters.

10. Change your mind

Open the Parameters pane and change bend_angle from 120deg to 150deg. The whole part rebuilds — bend, holes, countersinks, rounds and all.

11. Export

File → Export → STL… (3D printing) or STEP… (other CAD apps).

Every screenshot on this page is generated automatically from docs-site/screenshots/quickstart.lua.

If something goes wrong

• Esc cancels what's in progress; again returns to Select.
• Undo (⌘/Ctrl+Z) reverts whole steps.
• The status bar explains what the active tool expects next.
• A red conflict means contradictory constraints — delete the most recent one.