Setting Up a Schematic Document

Now reading version 15.1. For the latest, read: Setting Up a Schematic Document for version 24
 

Parent page: Capturing Your Design Idea as a Schematic

Grids and Cursors

Before placing objects in the Schematic Editor, set the grids to enable easier placement. Altium Designer offers three grid types: visible grids for navigation, snap grids for placement, and electrical grids for aiding the creation of connections. Grids are document options, meaning that they are saved with the individual design, and therefore, grid settings may differ between one design document and the next. Set the grids initially in the General region of the Document Options mode of the Properties panel.

The Visible Grid appears whenever the zoom level allows them to be sufficiently spaced, displayed as either lines or dots. To turn the visible grid on or off in the current document, click the toggle Visible Grid button ( ) in the panel, choose the View » Grids » Toggle Visible Grid command from the main menus or use the Shift+Ctrl+G keyboard shortcut.

The Snap Grid is the grid that the cursor is locked to when placing or moving schematic design objects. The current value of the snap grid is displayed on the left-hand side of the Status Bar. You can also use the View » Grids » Set Snap Grid command to set a specific value for the snap grid through the Choose a snap grid size dialog.

Electrical grids override snap grids since they allow connections to be made to off-grid parts. Enable Snap to Electrical Object Hotspots (can be toggled using the View » Grids » Toggle Electrical Grid command from the main menus or the Shift+E shortcut) so that when moving an electrical object in the design space, if it falls within the electrical grid range of another electrical object to which it could connect, it will snap to the fixed object and a hotspot (red cross) will appear. The electrical grid should be set slightly lower than the current snap grid or else it becomes difficult to position electrical objects one snap grid apart.

Grids can be quickly modified or toggled between enabled and disabled through keyboard or mouse shortcuts, for example, press G/Shift+G to cycle forward or back through the Snap grid settings defined on the Schematic - Grids page of the Preferences dialog for the current measurement system in force (Imperial or Metric). You can also use the View » Grids » Cycle Snap Grid and the View » Grids » Cycle Snap Grid (Reverse) commands from the main menus. If you change the grid size in this manner, your entered setting (through the Choose a snap grid size dialog) will be lost since cycling only involves the currently chosen preset interval settings.

You can change the Cursor type to suit your needs in the Cursor region of the Schematic - Graphical Editing page of the Preferences dialog. For example, a large 90 degree cross that extends to the edges of the design window (Large Cursor 90 option) can be useful when placing and aligning design objects.

Altium components are designed on an Imperial grid, be aware that their pins will not fall on logical grid increments if you choose to use a Metric grid. You can use an Imperial grid with a Metric sheet, the sheet Template and Units are set in the Document Options mode of the Properties panel, which is displayed when there is nothing selected on the schematic sheet.

Properties Panel

When the active document is a schematic document (*.SchDoc) and no design object is selected in the design space, the Properties panel presents the Document Options.

The following collapsible sections contain information about the options and controls available under the panel's General tab:

The following collapsible section contains information about the options and controls available under the panel's Parameters tab:

When a design object is selected, the panel will present options specific to that object type. The following table lists the object types available for placement on a schematic sheet – click a link to access the properties page for that object.

Arc Bezier
Blanket Bus
Bus Entry Comment
Compile Mask Designator
Ellipse Graphic
Generic Component Harness Connector
Harness Connector Type Harness Entry
Net Label No ERC
Note Offsheet Connector
Parameter Parameter Set
Part Polygon
Polyline Port
Power Object Probe
Rectangle Round Rectangle
Sheet Entry Sheet Symbol
Sheet Symbol Designator Sheet Symbol Filename
Signal Harness Text Frame
Text String Wire
Pin  
If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Note

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.

Content