Sketching
Starting and ending a sketch
Click a plane or a flat face, then click Sketch (Sketch tab), or right-click a face ▸ Sketch. Clicking a sketch tool such as Circle with no sketch open also starts a 2D sketch: pick a plane or flat face and the tool is ready. (For sketches in space, see the 3D Sketches chapter.) You can also start a feature such as Extrude without a sketch: RazorCAD asks you to pick a plane or face, you sketch, and when you exit the sketch the feature continues. If the profile is open you can keep editing or abort and keep the sketch.
- Esc ends the active sketch tool first; pressing it again closes the sketch and keeps it.
- Enter does not leave the sketch.
- The ✔ in the confirm corner, or Exit Sketch, closes the sketch.
- Ctrl+Z / Ctrl+Y undo and redo inside the sketch.
The sketch tool wheel
While sketching, press and hold the right mouse button. After a moment, or as soon as you start to drag, a wheel of sketch tools appears around the pointer. Keep the button held, move toward a tool (it highlights) and release to activate it. Releasing in the centre or pressing Esc cancels. A quick right click (press and release without moving) still opens the right-click menu.
Defined and under-defined sketches
Sketches are made of points, lines, arcs and circles held in place by relations and dimensions. A numerical constraint solver keeps them satisfied.
- Geometry is blue when under-defined and black when fully defined.
- The Property panel shows the remaining degrees of freedom.
- An under-defined sketch shows (-) in the tree. Construction lines only need to be positioned.
Sketch orientation
In the sketch Property panel, Rotate 90° turns the sketch axes about the sketch normal, and Flip Side looks at the sketch from the other side of the plane. Both are saved with the sketch.
Sketch tools
| Tool | Key | How it works |
|---|---|---|
| Select | S | Select entities, drag geometry |
| Line | L | Click a chain of points. Coincident, horizontal and vertical relations are added automatically; snapping to a midpoint or onto a curve adds those relations too. Double-click, Enter or Esc ends the chain. |
| Centerline | Construction line for symmetry, mirroring, gears or as a revolve axis | |
| Corner Rectangle | R | Built with horizontal and vertical relations |
| Center Rectangle | Also adds construction diagonals with a midpoint relation | |
| Circle | C | Centre, then radius |
| Centerpoint Arc | A | Centre, start, end; the direction follows the mouse |
| 3 Point Arc | Start, end, then a point it runs through | |
| Tangent Arc | From the end of a line or arc, kept tangent by a Tangent relation | |
| Ellipse | Centre, end of the major axis, then the minor radius. Trim it for an elliptical arc. | |
| Spline | N | See below |
| Point | Lone sketch points that stay, for example to place holes | |
| Straight Slot | Built with tangent and equal relations | |
| Polygon | P | Set the number of sides in the Property panel |
| Dimension | D | See below |
| Trim | T | See below |
| Extend | A line or arc end runs on to the first entity in its way and stays on it | |
| Split | Splits a line or arc in two at the click; the halves stay collinear or equal | |
| Project Edges | E | See below |
| Offset | O | See below |
| Mirror | Select the entities plus a centerline, then click Mirror | |
| Import DXF | See below | |
| Linear / Circular Sketch Pattern | Copies the selected entities with the relations and dimensions among them. A selected point is the circular pattern's centre. | |
| Make Block / Insert Block | Make Block saves the selection (with its relations) under a name in your settings. Insert Block places copies with a click, in any sketch, and can delete blocks from the library. | |
| Text | See below | |
| Gears | See the Gears chapter | |
| Airfoil | See the Airfoils chapter | |
| Sketch Fillet / Sketch Chamfer | Set the radius or distance, then click corners. The first one made gets the dimension; the others made before you leave the tool are made Equal to it, so one value changes them all. | |
| Intersection Curve | Projects the outline where the sketch plane cuts the bodies | |
| Construction Geometry | Q | Toggles the selected curves to or from construction (drawn dotted, ignored by features) |
| Display Relations | Shows or hides the relation glyphs | |
| Delete | Del | Deletes the selected entities or relations |
Dimension
Click a line, circle or arc (or two entities), then click to place the dimension.
- Moving the mouse switches between horizontal, vertical and aligned.
- Two lines give an angle; a point and a line give a perpendicular distance.
- Values accept equations, such as
width/2. - A dimension that would over-define the sketch is added as a driven (reference) dimension.
- Circles and arcs: dimension from a circle or arc to another circle, arc, point or line by clicking both. The Modify box offers Center (centre to centre), Min (nearest) and Max (farthest). Min also measures the gap between concentric circles. Switching keeps the geometry in place and shows the new value.
- Outside references: you can also click model edges, model vertices or entities of earlier sketches. RazorCAD creates linked construction geometry and dimensions to it, so the dimension follows the model. Example: "keep this hole 25 mm from the right edge" still holds after the width changes.
Trim
Power trim: hover over a segment and it turns red; click to remove it up to the nearest intersections. Lines are shortened or split, circles become arcs, and new end points get on-curve relations.
Offset
Click a line, arc or circle and its whole connected chain is offset. Move the mouse to the side and distance you want and click, then type the exact distance. Corners are re-trimmed or extended.
- You can also click a model edge (with Select chain, the connected edges lying in a plane parallel to the sketch, such as a face outline) or a curve of another sketch.
- Linked offset (default): the offset follows its source, including model edges when the model changes, and one dimension drives the chain (relation "Offset ⇉").
- Untick it for a single offset: plain geometry with no link.
- While the tool is active, the faces the sketch plane cuts are highlighted and the cut outline is drawn in teal. Clicking it offsets the whole outline.
Project Edges
Click a model edge, or an entity of an earlier sketch, to project it into this sketch. Or select edges first and then click Project Edges (or press E): they are projected at once. Projected geometry is drawn in purple, is linked and updates when the source changes (relation "On Edge ⇲"). The ends of projected lines are joined to each other and to sketch geometry already there, so the edges of a face give a closed outline ready to extrude. While the tool is active, the outline where the sketch plane cuts the bodies is drawn in teal; clicking it converts the whole outline. This works for solids and surfaces.
Spline
Click the points the curve runs through (they snap like line points), then double-click, Enter or Esc to finish, or click the first point again to close it. Drag a point to reshape the curve, or drag the curve to move it; deleting a point takes it out of the spline. Splines make profiles on their own or with lines and arcs and are exact curves for extrudes, revolves, cuts, lofts and sweep paths. Lines can be trimmed where they cross a spline.
Import DXF
Import DXF brings a DXF file into the open sketch: lines, arcs, circles, polylines with arcs, ellipses and elliptical arcs, splines, points and blocks. The file's units are converted to millimetres. You can scale it and place it as in the file, centred, or by its corner.
Text
Click Text on the Sketch tab, then click to place. The panel sets the text, font (the PC's installed fonts), height (capital-letter height), angle, bold and italic. Drag the text to move it. Text extrudes as a boss or cut; text inside an outline is cut out of it. To put text on a curved face, use Wrap (Features chapter).
Relations
Select entities (Ctrl+click for several). The Property panel lists the relations that apply:
| Selection | Relations offered |
|---|---|
| 1 line | Horizontal, Vertical, Fixed |
| 2 or more points | Coincident, Horizontal, Vertical |
| 2 or more lines | Parallel, Perpendicular, Collinear, Equal, Horizontal, Vertical |
| Point + line | Coincident (on line), Midpoint |
| Point + circle/arc | Coincident (on curve) |
| Line + circle/arc | Tangent |
| Circles/arcs | Equal, Concentric, Tangent |
| 2 points + line | Symmetric (about the line) |
| 3 lines | Symmetric (two lines about a centerline) |
Relations are shown as small green glyphs next to the geometry. Click a glyph to select it, then press Del to remove it. Hovering a glyph highlights the entities it ties together. Redundant or conflicting relations are refused with a message.
How profiles are found
Profiles are found automatically from all non-construction geometry and sent to the kernel as exact lines, arcs and circles. Intersections are split, dangling lines are ignored and nested loops become holes. A full circle (or arcs that make one) becomes a single closed curve, so an extruded circle has one continuous cylindrical face.
Showing and hiding sketches
Sketches absorbed by a feature are hidden by default. Right-click a sketch in the tree ▸ Show / Hide, or use its eye in the tree.
Change Sketch Plane
Right-click a sketch ▸ Change Sketch Plane… and pick another plane or flat face for it, for example to repair a sketch whose plane was deleted ("The reference plane is missing"). Its curves keep their sketch coordinates. Only planes above the sketch in the tree are offered.