Contact our corporate or local offices directly.
Before you start working with schematics, it is recommended to configure the settings of the schematic editor on the Schematic section pages of System Preferences (accessed by selecting File » System Preferences). On the Schematic – General page, you can define default units, schematic sheet size and other settings for a newly created schematic sheet.
A new schematic sheet can be created by selecting the File » New » Schematic command (1). Settings for the current schematic document are configured in the Document Options mode of the Inspector panel (2). In the General region of the panel, you can select units and set the grids to enable easier placement of design objects. In the Page Options region (3), you can select an existing schematic sheet template (Template), choose from standard sheet sizes (Standard), or set non-standard dimensions (Custom).
CircuitMaker tools allow you to capture electronic circuits of any complexity, from flat designs with a couple of components and connections, to complex hierarchical projects with structured connectivity across multiple sheets.
Electrical and graphical objects of the schematic editor can be placed by using commands from the ribbon's Home | Circuit Elements region (1) and Home | Graphical Elements region (2), respectively. Properties of a placed object selected in the design space can be changed in the Inspector panel (3) or in the ribbon's Home | Font and Home | Appearance regions (4).
There are some tools to facilitate your work with objects on a schematic sheet:
Selection Filter – allows you to define object(s) that can be selected on the sheet. You can choose all object types (All Objects) or some specific object types (Components, Ports, Texts, etc.).
Selection from left to right – click and drag a blue rectangle from left to right to select only those objects that are completely within the selection rectangle.
Selection from right to left – click and drag a green rectangle from right to left to select all objects that are within or touch the selection rectangle.
Ctrl+C / Ctrl+V / Ctrl+X – standard shortcuts to copy, paste, and cut selected objects. Commands are also available from the right-click menu.
Some other shortcuts useful when working in the schematic editor are listed in the Shortcuts section.
During schematic capture, you can use CircuitMaker community components available through the Libraries panel. You can search for the required component by specifying the category and/or using the search box. If a component has a schematic/PCB model added (such components are listed with the icon in the panel), this component can be placed on the schematic by dragging it or using the Place command from the component's right-click menu.
To define connectivity between component pins, you can use the tools provided in the ribbon's Home | Circuit Elements region. At the most basic level, you can create that connectivity by drawing a wire from one component pin to another by using the Wire object – this is referred to as physical connectivity.
After launching the wire placement command, the cursor will change to a cross-hair. When the cursor is near a component pin's electrical point, a red connection marker (red cross) will appear at the cursor location. This indicates that the cursor is over a valid electrical connection point on the component.
If the wire is forming a corner in the wrong direction, press Spacebar to toggle the corner direction. Press Shift+Spacebar to cycle through the wire placement modes. Use the Backspace or Delete keys to remove the last wire segment placed.
Connection within a schematic sheet can also be formed by placing a short Wire and a Net Label on each component pin – this is referred to as logical connectivity. For power nets global for the entire design, such as GND or VCC, you can also use Power Port objects. Some power ports with predefined styles and values are available in the Home | Circuit Elements | Power Port drop-down.
The Bus and Harness objects are used in more complex schematics. Buses are used to bundle a series of sequential nets, for example, an address bus or a data bus. Signal harnesses can be used to bundle any number of nets, buses and lower-level harnesses.
If the design does not fit onto a single schematic sheet, it can be spread over multiple sheets. Multi-sheet designs are implemented by placing a Sheet Symbol on the parent sheet, which represents and links to the child sheet. While you can place Sheet Symbols and define their properties manually, there are commands that allow you to build your multi-document structure quickly and efficiently. The commands you use will depend on your personal design methodology – which can be broadly classified as top-down, or bottom-up.
To build the structure in a bottom-up fashion, select the Sheet Actions » Create Sheet Symbol From Sheet command from the schematic sheet's right-click menu (1). In the Choose Document to Place dialog (2), select the schematic sheet that will be represented as a Sheet Symbol. The Sheet Symbol will include a Sheet Entry to match each Port it finds (3). The documents structure changes will be shown in the project tree within the Projects panel (4).
To build the structure in a top-down fashion, you can place a Sheet Symbol that represents a child schematic sheet to be created, then add the required Sheet Entries, then use the Sheet Symbol Actions » Create Sheet From Sheet Symbol command. A new schematic sheet will be created below the nominated sheet symbol. Ports are added to the child sheet to match any Sheet Entries found in the Sheet Symbol.
If Ports or Sheet Entries are added or removed at a later stage, they can be re-synchronized by using the Sheet Symbol Actions » Synchronize Sheet Entries and Ports command from the right-click menu of a Sheet Symbol. The Synchronize Ports To Sheet Entries dialog will open where the mismatches between the ports and the sheet entries are displayed. Use this dialog to ensure that all sheet entries on the sheet symbol are matched to ports on the referenced child sheet below, both in terms of name and I/O Type. Synchronization can performed by pushing properties of the selected sheet entry to the selected port or by pushing properties of the selected port to the selected sheet entry.
Design directives are objects that are placed on the schematic during design capture, providing a way of specifying instructions to be passed to the PCB. Design directive objects can be placed using the ribbon's Home | Circuit Elements | Directives drop-down:
_P, and a directive must be attached to each.
In properties of the selected Differential Pair or Net Class directive, a design rule can be added for the net to which the directive is attached. This rule will be transferred to the PCB during design synchronization.
When the schematic design is ready, you can then validate it by selecting Project | Validation | Validate (1). During validation, CircuitMaker checks the design for logical, electrical, and drafting errors in accordance with the settings on the Error Reporting and Connection Matrix tabs of the Project Options dialog (2). The errors and warnings found will be listed in the Messages panel (3). If there are no errors, the
Compile successful, no error found message will be shown in the panel.
While CircuitMaker provides an intuitive and user-friendly interface, you can become even more productive by using shortcut keys. Shortcut keys are more efficient than carefully positioning a mouse over a button or drilling through ribbons and menus.
The following is the list of some frequently used shortcut keys of the CircuitMaker's schematic editor:
Contact our corporate or local offices directly.