Drawings¶
Documents a part or assembly on sheets: views projected from the model, dimensions and annotations on them, and a title block filled in from the model's properties. A drawing references its models' files. When a model is saved, its views are updated.
File > Make Drawing… for a drawing of the active part or assembly, or File > New Drawing… for an empty one.
img/drawings/drawing-window.png
A drawing of a part with front, top, right and isometric views, the View Layout tab of the command panel, and the drawing's design tree.
Creating a Drawing¶
- Make Drawing
-
File > Make Drawing…. Creates a drawing of the active part or assembly, with its front, top and right views laid out by the sheet's projection angle and an isometric view in the corner they leave, at the largest standard scale that fits above the title block. A drawing shows the model as saved: if it has unsaved changes, a dialog offers to Save it first. With no part or assembly active, select a file. An assembly's drawing also gets a BOM table and balloons on its isometric view.
If the model already has a drawing, open in a tab or saved beside it under its name, a dialog offers to Open Drawing or create a New Drawing.
- New Drawing
- File > New Drawing…. Creates a drawing with one empty sheet and opens the Model View page to select a model and place its views. See Model View. You can also drag a part or assembly from the Open Parts list or the file explorer onto the sheet: on an empty sheet it is placed as its standard views, else as a front view where it is dropped.
Both first ask for the Template and Size. Each template is shown as its first sheet on the size chosen. A template sets the sheet format, the drafting standard and any title block values saved with it, and some set a size of their own. The template and size used last are chosen. Templates come with SpryCAD and from the company standards library. See Title Block.
Press Ctrl+S to save. A drawing is saved as a .sdrw file. Make Drawing offers to save it beside its model,
under the model's name.
The Drawing Tabs¶
While a drawing is active, the command panel shows its own tabs in place of a part's:
| Tab | Commands | See |
|---|---|---|
| View Layout | Model View, Standard 3 View, Projected View, Auxiliary View, Section View, Detail View, Break, Broken-out Section, Crop View, Hide/Show Edges, Update Views | Model View, View Properties |
| Annotation | Dimensions, Model Items, Auto Arrange, Note, Hole Callout, Center Mark, Centerline, Area Hatch, Datum Feature, Feature Control Frame, Surface Finish, Weld Symbol, Balloon, Auto Balloon, BOM Table, Hole Table | Dimensions, Annotations, Area Hatch, Balloons, Tables |
| Drawing | Line Weights, Drafting Standard, Layers, Release Revision, Follow Latest, Export PDF, SVG and DXF, Print | Drafting Standard, Layers, Revisions, Export and Print |
| Sheet Format | Add Sheet, Sheet Properties, Edit Sheet Format, Save Format to Library, Save as Template | Sheets, Sheet Format |
| Sketch | Sketch tools, on the sheet or on a view | Sketches on Drawings |
While a sketch is open, only the Sketch tab is shown. While the sheet format is edited, only the Sheet Format tab is shown, with the format's own commands.
The Drawing Design Tree¶
The design tree shows, from the top:
- Drawing row
- The drawing's name, with its revision once released. Right-click it for the drawing's menu.
- Sheets
- One row per sheet, with its size and scale. Select a sheet to show it. Right-click it for the sheet's menu.
- Views
- Under each sheet, its views, each with its name and kind: an orientation such as Front, Projected, Section A-A, Detail B or View C. The tooltip gives the model's file, and whether the model is pinned to a revision. A view whose model could not be loaded is red; it is shown as last saved.
- Sketches
- The sketches drawn on the sheet or on a view. A sketch with references to edges the model no longer has is red, with their count. Double-click a sketch to edit it.
- Dangling annotations
- Annotations whose edges are gone from the model, listed in red to find and delete.
Select a view or an annotation in the tree to select it on the sheet and open its page. Press Del to delete the selected sheet, view, sketch or annotation.
Drawing Menu¶
Right-click the drawing row:
| Item | Does |
|---|---|
| Properties… | The drawing's own title block values. See Title Block |
| Add Sheet | See Sheets |
| Update Views | Loads every model again and updates the views |
| Drafting Standard… | See Drafting Standard |
| Layers… | See Layers |
| Release Revision… | See Revisions |
Sheet Menu¶
Right-click a sheet in the design tree, or its tab below the graphics area: Rename…, Sheet Properties…, Edit Sheet Format, Move Up and Move Down (Move Left and Move Right on a tab), Add Sheet and Delete Sheet. See Sheets.
Working on the Sheet¶
The graphics area shows the sheet flat: drag with the middle button to pan, Shift + middle drag or the wheel to zoom, and double-click the middle button to fit the sheet. The views cannot be rotated.
- Click
- Selects a view or annotation and opens its page in the property panel.
- Double-click
- On a note, dimension or hole callout, edits its text; on another annotation, opens its page. On a view, opens a sketch on it. On a sketch, edits it.
- Drag
- Moves the view or annotation under the pointer.
- Right-click
- The menu of what is under the pointer: a view, an annotation or a hatch. On the paper, the sheet's menu: Model View, Standard 3 View, Sketch on Sheet, Sheet Properties…, Add Sheet and Delete Sheet.
When the Model Changes¶
A drawing shows its models as saved. When a part or assembly it shows is saved, open drawings update their views and the status bar names the models. Dimensions and annotations stay on the edges they reference; one whose edge is gone is dangling, drawn in red and listed in the design tree.
A released drawing pins its views to the revisions of their models, so later changes to the models do not reach it until Follow Latest. See Revisions.