Tutorials PartCraft help Walkthroughs
Draw your first sketch
Open a sketch on a plane or a flat face, draw lines, rectangles, circles, arcs, points and centerlines, round a corner, select, drag and delete.
Written for PartCraft 0.3. The same help is inside the app: press F1.
Every solid starts as a sketch: a flat drawing on a plane. This walkthrough covers the drawing tools. Tying the sketch down with relations and dimensions is in Fully define a sketch.
Start a sketch
You can sketch on a base plane or on any flat face of the part.
- Pick where to sketch:
- a base plane: click Front plane, Top plane or Right plane in the history, or click the plane in the view;
- a flat face: click the face in the view. The whole face highlights.
- Choose Sketch in the toolbar or press SS. (With a face picked you can also choose Sketch on this face in the right panel; with a plane, Sketch on it.)
The view turns square to the plane, the sketch tools appear in the toolbar, and the Line tool is ready. If you press Sketch with nothing picked, the base planes show and the status bar says "Click a plane or a flat face to sketch on. Esc stops."
A sketch on a face follows that face. If the face was made by a sketch edge or an extrude's end, the new sketch moves when the feature changes (a deeper pocket takes the sketch on its floor with it). If the panel says the face is "Fixed where picked", the sketch stays where the face is now.
The drawing tools
Each tool has a toolbar button and a key. Choose the same button again, press SS, or press EscEsc to go back to Select.
| Tool | Key | How to draw |
|---|---|---|
| Line | LL | Click the start, then click each next point. Lines chain end to end. End the chain with EscEsc, ReturnEnter, a right-click or a double-click. Clicking an existing point also ends it |
| Rectangle | RR | Click one corner, then the opposite corner. You get four lines joined at the corners, two horizontal and two vertical |
| Circle | CC | Click the center, then a point on the circle |
| Arc | AA | Click the center, then the start, then the end. The arc runs the way you move the pointer round the center |
| Point | PP | Click. A point on its own marks a hole center for Hole |
| Centerline | NN | Like a line, one segment at a time. Drawn dashed; it is construction geometry, used as a revolve axis or a reference |
| Fillet | FF | Click a corner where two lines meet, type the radius, press ReturnEnter |
| Spline | BB | Click the points the curve passes through; ReturnEnter ends, a click on the first point closes it. See Splines, trim, offset and other sketch tools |
| Trim | TT | Click the piece of a curve to remove, up to the nearest crossings |
| Dimension | DD | See Fully define a sketch |
While you draw, a small label next to the pointer shows the length, the size or the diameter.
More, at the end of the sketch tools, holds the control-point spline, Extend, Offset, Mirror, Polygon, Slot, the sketch patterns and Project edge: see Splines, trim, offset and other sketch tools.
Snapping
Snapping adds relations for you, so the sketch stays joined when it moves:
- On an end point or the origin, a small square shows. The new point is made coincident with it.
- On a line, circle or arc, a small cross shows. The new point is put on that curve.
- A line within 3 degrees of horizontal or vertical snaps to it and gets a horizontal or vertical relation. The label shows "H" or "V".
To avoid a snap, zoom in so you click farther from the point or curve.
Round a corner
- Press FF or choose Fillet.
- Click the corner point where two lines meet.
- A box opens with a suggested radius. Type the radius and press ReturnEnter.
Both lines are trimmed and joined by a tangent arc with a radius dimension. Messages you may see: "A fillet needs a corner where exactly two lines meet." and "That radius is too big for these lines."
Construction geometry
Construction lines, circles and arcs are dashed and gray. They guide the sketch but are not part of the profile that gets extruded or revolved.
- Select the lines, circles or arcs.
- Press QQ or choose Construction. Press it again to switch them back.
Select, drag and delete
Press SS (or EscEsc until no tool is active) for Select.
- Click a point, line, circle, arc, relation symbol or dimension to select it. ⇧Shift+click adds to the selection or takes away. On Windows and Linux ⌃Ctrl+click does the same; on a Mac, ⌘+click.
- Drag on empty space to draw a window: everything fully inside it is selected.
- Drag a point or a line to move it. The solver keeps every relation and dimension as it moves, so only free geometry moves. Drag a circle's edge to change its radius.
- Drag a dimension's number to move the label.
- Press fn DeleteDelete or DeleteBackspace, or choose Delete in the right panel, to delete the selection. Deleting geometry deletes the relations on it.
Zoom and pan in the sketch
- Roll the wheel to zoom at the pointer.
- Drag with the middle or right button to pan.
- Fit in the toolbar or the right panel fits the sketch in the view. In a sketch the FF key is the Fillet tool, not Fit.
Close the sketch
Choose Exit in the toolbar or Exit sketch in the right panel, or press EscEsc until the sketch closes. Each EscEsc first cancels what is in progress, then returns to Select, then clears the selection, and the next one closes the sketch.
The sketch stays selected, so the next Extrude or Revolve uses it.
What makes a good profile
Extrude and Revolve use every closed loop of the sketch's solid (non-construction) lines, circles, arcs and splines. Loops inside loops become holes.
- Every end must meet exactly one other end. "The profile is open: an end at (12.5, 40) is not joined to anything." names the place.
- No three ends may meet at one point: "The profile branches at (0, 20): more than two ends meet there."
- Points and construction geometry are ignored by the profile.