Solid Features
Live previews
While a feature's Property panel is open, the model is rolled back to just before that feature and the feature is shown in colour: yellow for material it adds and red (seen through the body) for material it removes. Fillets and chamfers show the material they add or remove; reference geometry being edited is drawn in orange. Click ✔ (or Enter) to finish.
Every value field accepts numbers or equations (see Equations in the Evaluate chapter).
Extrude and Extrude Cut
Extrudes a sketch profile into a solid, or cuts it out.
End conditions:
| End condition | Meaning |
|---|---|
| Blind | A set depth |
| Mid Plane | The depth split equally on both sides of the sketch |
| Through All / Through All – Both | Through every body, in one or both directions |
| Up To Vertex | Click a model vertex or choose a reference point |
| Up To Surface | Click a flat model face or choose a plane; angled surfaces are supported and the extrusion is trimmed to the surface |
| Offset From Surface | As Up To Surface, at a set distance from it |
Options:
- Merge result (boss): untick to keep the new material as a separate body even where it touches. A boss that doesn't touch existing material makes a new body anyway.
- Thin Feature: makes a wall of the given thickness from the profile; direction one side, other side or mid-plane. Open sketches switch it on automatically.
- Feature Scope (cuts): All bodies by default; untick it and click the bodies to cut.
Revolve and Revolve Cut
Revolves a profile about an axis: the sketch axes, any line in the sketch (such as a centerline), a reference axis, a straight model edge or a cylindrical face (click it in the view). Cuts have the same Feature Scope option as extruded cuts.
Sweep and Sweep Cut
Sweeps a profile along a path.
- Profile: a sketch, or Circular with a diameter (useful for springs).
- Path: a sketch chain or a helix.
- Thin option.
Loft and Loft Cut
Blends between two or more profile sketches, in order. A third or later profile shapes the middle.
- A circle is split into as many equal arcs as the other profile has corners.
- Profiles with different segment counts give an error naming the sketches.
- Options: straight (ruled) sides, Thin.
Hole
Hole (Features tab, Insert ▸ Features ▸ Hole…) makes standard holes.
| Type | Sizes |
|---|---|
| Hole (clearance) | ISO 273 close, normal or loose fit, for M2 to M24 |
| Counterbore | For socket head cap screws (ISO 4762) |
| Countersink | ISO 10642, 90° |
| Tapped hole | ISO metric or Unified (inch), drilled at the tap drill size; the thread is shown as a cosmetic thread and given in drawing callouts |
| Custom sizes | Your own diameters and depths |
- Blind with a 118° drill point, or Through All; reversible.
- Place holes at clicked points on a flat face, or exactly at the points and circle centres of a sketch on the face.
- Holes work on sheet metal too, and a drawing's Hole Callout reads their size from the feature.
Helix
Pick a sketch with a circle; it sets the axis and diameter. Define the helix by pitch and revolutions, pitch and height, or height and revolutions. Options: start angle, clockwise, reverse. Use a helix as a sweep path for springs and coils.
Thread Cut and Thread Extrude
Click a bore (Thread Cut) or a shaft (Thread Extrude).
- The size is chosen automatically from the diameter, or choose a metric (ISO) or inch (Unified) standard size, or custom. Coarse / UNC sizes are preferred.
- Optional pitch; left-hand option.
- Length: the whole face, a depth, or up to a plane or face. Threads never reach past the ends of their face.
- The bore or shaft is resized to the thread size if needed (a bore to the minor diameter, a shaft to the major). A bore that would break out of the body is refused.
- Threads run all the way to the ends: grooves run out into open air, otherwise the thread is cut off flush with the end.
Cosmetic Thread
Cosmetic Thread (Features tab, Insert ▸ Features ▸ Cosmetic Thread…) marks a bore or shaft as threaded without modelling the thread, so it costs nothing to rebuild. Use it where the thread only needs to be shown and called out.
- Click the bore (internal thread) or the shaft (external thread). The thread starts at the end nearest the click; Start from the other end reverses it.
- Size, pitch, left-hand and length (whole face, depth, or up to a plane or face) as for Thread Cut. The feature's note says when the face is not the size the thread expects (a bore about the minor diameter, a shaft the major).
- In the model it shows as a thin helix on the face. Tapped holes made with the Hole feature show their threads the same way.
- On drawings it is drawn by convention: from the side, thin lines at the thread's other diameter and a line where it ends, dashed for a hidden bore; end on, a three-quarter circle. A view's Cosmetic threads box turns them off.
- Hole Callout on a bore with a cosmetic thread gives the thread, for example "M10×1.5 THRU ALL / TAP DRILL Ø8.5 THRU ALL".
Wrap (Emboss / Deboss)
Pick a sketch (outlines and/or text) and a face, flat or curved. The sketch is projected along its normal onto the face and raised (emboss) or sunk (deboss) by the depth.
Patterns and Mirror
Patterns and mirrors copy features or bodies. Any feature that changes the bodies at a place can be copied: extrudes, cuts, holes, fillets, chamfers, drafts, domes and sheet metal forms. A feature without a shape of its own (such as a fillet) is run again on the matching edges or faces of each copy.
| Feature | Copies |
|---|---|
| Linear Pattern | Along one or two directions (X, Y, Z or any reference axis) |
| Circular Pattern | Round an axis (X, Y, Z or any reference axis) |
| Mirror | About a plane or flat face |
| Sketch Driven Pattern | At every point (or circle centre) of a sketch |
| Curve Driven Pattern | Along a sketch, 3D sketch or helix, spaced evenly to the end or at a set distance; moved, or turned to follow the curve |
| Fill Pattern | On a square or staggered grid over a flat face, kept a margin from its edges (for example a perforated panel) |
Patterns of cuts are cut out in one operation, and patterns of added features (bosses, pins, ribs) are fused into the body in one operation, so large patterns rebuild quickly. A plate with 200 bosses builds in about 2 seconds.
A pattern or mirror of a sheet metal feature that makes a body (Base-Flange, SM-Extrude, Lofted-Bend, Transition) copies that body as it is at the pattern, with the flanges and cuts added to it so far. Each copy is sheet metal with its own flat pattern. A mirrored copy's flat pattern is the mirror image, with its bends going the other way. A mirrored lofted bend becomes a plain solid.
Fillet
Open the feature and click edges on the model. The model is rolled back to just before the feature so every edge can be picked; tick Preview to see the result. The radius accepts equations.
- Edges are remembered by type, direction and position, and found again after parameter changes.
- Where a fillet can't be added on top of earlier fillets (a corner where several blends meet), RazorCAD recomputes it together with the preceding fillets in one operation.
- Where two blends exactly meet (for example R2 on both edges of a 4 mm wall) the result is a full round.
- Variable size: a radius at the start and another at the end of each edge.
- Face fillet: pick faces instead of edges; the edges where they meet are rounded.
Chamfer
Click edges as for a fillet. Chamfer types: equal distance, distance + angle or two distances. Flip direction swaps the sides.
Shell
Click the faces to remove and set the wall thickness, inward or outward. Where a fillet or chamfer is smaller than the wall, the outside keeps it and the inside gets a sharp corner.
Draft
Pick a neutral face, then the faces to tilt by an angle. Reverse tilts them the other way.
Rib
An open sketch line is thickened and filled out until it meets the model, either in the sketch plane (for example a gusset across a bracket corner) or square to it.
Dome
A spherical cap or half ellipsoid on round faces, or a smooth dome filled over any other flat outline. Reverse presses it in.
Move Face
Push or pull flat faces along their normal, or turn a face about one of its edges. The neighbouring faces follow.
Scale
Scales every body by one factor, about the origin or about the centre of the bodies.
Long operations
If a feature takes more than a few seconds, a banner above the model says what is being worked on ("Still working on Extrude Cut1 (12 s)…") with a Stop button (also next to the progress bar). Stop restarts the geometry kernel: a feature you are still editing is cancelled and a finished feature is suppressed, so you can unsuppress it to try again.