Drawings
RazorCAD makes 2D engineering drawings of parts and assemblies, saved as .rdrw files and opened in their own tab.
Starting a drawing
- Start window ▸ New Drawing, or File ▸ New Drawing, opens the set-up dialog (below) and then an empty sheet.
- File ▸ Make Drawing from Part (in a part), or Make Drawing from Assembly (in an assembly): after the set-up dialog, places the standard three views at a scale that fits, clear of the title block.
- A drawing can show assemblies as well as parts: every component is drawn where it sits, through its sub-assemblies, in the configurations shown; suppressed and hidden components are left out. Big assemblies (more than about 200 solids) are drawn fast from the parts' display meshes: lines, circles and arcs as exact as the 3D view's, and where an edge turns hidden to about two thousandths of the view's size. A site layout of thousands of solids then takes seconds a view instead of many minutes. In a view's properties, Hidden lines chooses Automatic, Exact or Fast; section and flat-pattern views are always exact.
Drawings are opened, saved and listed in the recent files like parts.
The sheet and its template
The default template is A3 with an ISO 5457 frame (zones and centring marks) and an ISO 7200-style title block: title, drawing number, material, scale, size, units, projection symbol, drawn / checked / approved, date, mass, company, revision, sheet n of m and general tolerances. Sheet sizes A0 to A4, landscape or portrait.
Drawing templates
A drawing template (.rdrt file) keeps a drawing's set-up: its sheets (size, orientation, scale, projection), the drawing settings (text height, decimals…), the title block's standing entries (company, drawn / checked / approved by, finish, tolerances, revision) and notes placed on the sheet. Views, parts and part-specific entries (title, drawing number, material, mass, date) are not kept.
- File ▸ Save as Template… in a drawing saves one, by default to
Documents\RazorCAD\Templates. Opening a .rdrt file edits the template in its own tab. - The New Drawing dialog lists your templates (from the Templates folder, or Browse… for one anywhere) and the standard ones: A4 portrait and landscape, A3, A2, A1 and A0 landscape, and A3 and A4 in third angle projection. Set the drawing name, title, drawing number, drawn by and company, and the first sheet's size, orientation, scale and projection. Tick Use this template as my default to have it chosen first next time. Double-click a template to create the drawing at once.
- Change Template… (File menu, Sheet tab, or right-click the drawing in the tree) switches an existing drawing to another template. Views, dimensions and annotations stay; company, tolerance and finish come from the new template, and the old template's notes are replaced. Undo goes back.
- Company sheet formats: a template can carry its own border, title block and logo in place of the standard ISO one, used on sheets of its size and orientation. Its text shows the drawing's properties, and can be set in a font installed on the PC; PDF exports embed the font. Drawing Properties lists the title block's own fields.
Changing the projection (Change Template or Sheet Properties) lays the views out again for the new projection, so a top view stays a top view.
Working on the sheet
| Action | How |
|---|---|
| Zoom | Mouse wheel |
| Pan | Middle or right drag, or left drag on empty paper |
| Fit the sheet | F |
| Move views and annotations | Drag them |
| Edit | Double-click a view for its properties, a dimension or note to edit it |
| Menus | Right-click |
| Delete | Del |
| Undo / Redo | Ctrl+Z / Ctrl+Y |
View Layout tab
| Command | What it does |
|---|---|
| Model View | Pick an open part or assembly, or browse for its file (.rcad or .rasm), pick the orientation (front, back, top, bottom, left, right, isometric, dimetric, trimetric or flat pattern) and click on the sheet. Then move around it to place projected views. |
| Standard Views | Three views laid out for first- or third-angle projection |
| Projected View | A view aligned with its parent |
| Flat Pattern | A sheet metal body unfolded (see below) |
| Section View | Horizontal or vertical cutting line, hatched cut faces, A-A labels and arrows, flip |
| Detail View | A circle with a letter, 2:1 by default |
| Auxiliary View | Looks square at an inclined edge, so it shows its true shape |
| Break | Leaves out the middle of a long part; dimensions across the break keep the true length |
| Crop View | Shows only the area you draw round |
| Update Views | Re-reads the parts and redraws the views |
A broken or cropped view can be put back to whole from its right-click menu. Section views hatch each body or component with its own angle and spacing.
Views are hidden-line projections computed by the geometry kernel.
View properties
Click a view to open its panel:
- Orientation, changeable after placing (also to and from Flat Pattern; projected and section views made from it are removed when it becomes a flat pattern, and Ctrl+Z brings them back).
- Display style: hidden lines removed, hidden lines visible, or wireframe; tangent edges and cosmetic threads on or off.
- Exploded (a view of an assembly that has exploded views): shows the view exploded as one of them. The components are where that exploded view moves them, the view keeps its place on the sheet, and its projected, section, auxiliary and detail views follow. Balloons on it pick the moved parts.
- Sheet scale or a custom scale; labels.
- Rotate View: −90°, +90°, 180° and 0° buttons and an angle box (degrees, counter-clockwise). Section lines, detail circles and annotations turn with the view.
Aligned views slide only along their alignment. Deleting a view deletes the views made from it.
Flat pattern views
A flat pattern view shows a sheet metal body unfolded with its outline and holes, bend lines (chain lines) with notes (UP / DOWN, angle, radius), optional bend region lines, and its flat size, thickness, number of bends and cut length underneath. It can be dimensioned (bend lines too) and exported to PDF. If the part has several sheet metal bodies, pick the body in the view properties. Instead of notes, the view can show a bend table: the bend lines numbered B1, B2… and a table of direction, angle and inside radius under the view. Forms, cross breaks and tabs and slots show as in the DXF.
Annotation tab
| Command | How |
|---|---|
| Dimension | Click a line for its length, a circle for its diameter (an arc: radius), two points, lines or circles for the distance between them (two lines at an angle: the angle), then click where the text goes. Horizontal, vertical or aligned depends on where you place it. Prefix, suffix, tolerance and override text can be set. |
| Note | Click on the sheet; click an edge first to add a leader |
| Baseline Dimension | Click the base edge or point, then each point or edge to dimension from it; the dimensions stack one above the other |
| Ordinate Dimension | Click the origin, then where the values line up, then the points to dimension |
| Chamfer Dimension | Click the chamfer edge and an edge next to it, then place the text ("3 × 45°") |
| Hole Callout | Click a hole. The callout gives its size and depth from the Hole feature (counterbore, countersink, tapped thread and tap drill) or its cosmetic thread, and how many of the same holes the view shows, for example "4× Ø6.6 THRU ALL / CBORE Ø11 DEEP 6.5". |
| Datum Feature | A datum letter in a box, with a triangle on the feature |
| Geometric Tolerance | A feature control frame: one of the 14 characteristic symbols, tolerance with Ø zone and material condition, and up to three datums |
| Surface Finish | A surface finish symbol with its roughness |
| Weld Symbol | Fillet, square, V, bevel or plug weld on a reference line with an arrow to the joint; arrow, other or both sides; all-around, field weld and tail |
| Center Mark | Click circles or arcs |
| Centerline | Click two lines (or two points); the centerline runs between them |
| Revision Table | Rows edited in one dialog; the latest revision goes into the title block |
| Cut List Table | The cut list of the part in the selected view (see the Fast Structure chapter); it updates when the part changes |
| Balloon | Click a part in a view, then where the balloon goes. The number is that part's item in the bill of materials, found from the part under the click (in a sub-assembly, the sub-assembly's item). Keep clicking for more; Esc ends. Where the part can't be told, it asks for the number. Right-click a balloon ▸ Item Number… to change it. |
| BOM Table | The bill of materials of the drawing's assembly: ITEM, QTY, PART and MATERIAL, at the top right of the sheet. Drag it anywhere; right-click it to show the sub-assemblies' parts (indented). It follows the assembly. |
Datum features, geometric tolerances, surface finish and weld symbols can each have a leader. Right-click one ▸ Edit… to change it.
Sheet tab
- Sheet Properties: size, orientation, scale, first or third angle.
- Title Block (Drawing Properties): title block fields, text height and decimals.
- Units: click MMGS / IPS in the status bar. An inch drawing gives lengths in inches with three decimals and its title block says "in"; angles are not converted.
- Change Template: see Drawing templates above.
- Add Sheet: drawings can have several sheets, shown as tabs under the sheet.
- Export PDF: vector PDF, one page per sheet.
- Export DXF: the current sheet as a DXF file, with layers for visible, thin, hidden and centre lines, text and hatching. A sheet format's logo is left out.
Views follow the part
Views and dimensions follow changes to the part or assembly, whether it is open in another tab or read from its file. A copy of the part is kept in the drawing so it still opens if the part file is missing.