Altium Designer Documentation

Defining General Schematic Preferences for Altium Designer

Created: 17.03.2021 | Updated: 25.09.2021

Parent page: Accessing, Defining & Managing System Preferences

The Schematic - General page of the Preferences dialog

Summary

As its name suggests, the Schematic – General page of the Preferences dialog provides numerous general controls related to editing schematic-based documents directly in the design space. 

Access

The Schematic – General page is part of the main Preferences dialog that is accessed by clicking the  control in the upper-right corner of the design space then selecting the General entry under the Schematic folder.

Options/Controls

Units

  • Select Mils or Millimeters, whichever is desired.

Options

  • Break Wires At Autojunctions - Enable this option to break wires at autojunctions (autojunctions are automatically inserted when two wires/buses/signal harnesses are connected in a T-type fashion or when a wire/bus/signal harness connects orthogonally to a pin or power port/bus power port).
  • Optimize Wires & Buses - Enable this option to prevent extra wires, poly-lines, and buses from overlapping on top of each other. Overlapping wires, poly-lines, or buses are removed automatically.

    You need to enable this option to have the ability to automatically cut a wire and terminate onto any two pins of this component when this component is dropped onto this wire.

  • Components Cut Wires - Enable this option to drop a component onto a schematic wire. The wire is then cut into two segments and the segments are terminated onto any two hot pins of the component automatically. You will need to enable the Optimize Wires & Buses option first.
  • Enable In-Place Editing - If this option is enabled, the focused text field may be directly edited within the Schematic Editor rather than in a dialog box. After focusing on the field you want to modify, click it again or press the F2 shortcut key to open the field for editing. If this option is not enabled, you cannot edit the text directly and you have to edit it from the Parameter Properties dialog. You can only graphically move this text field.
  • Convert Cross-Junctions - Enabling this option denotes that when the addition of a wire would create a four-way junction, it is instead converted into two adjacent three-way junctions. Disabling this option denotes that when a four way junction is created, the two wires crossing at the intersection are not joined electrically and if the Display Cross Overs option is enabled, a cross-over is shown on this intersection.
  • Display Cross-Overs - When this option is enabled, the wiring cross-overs will be displayed with small bridges on the currently focused schematic sheet.
  • Pin Direction - Enable this option to display the direction of pins of components on a schematic document. The pin direction is indicated by the orientation of a triangle symbol. 
  • Sheet Entry Direction - Enable this option to display the direction of sheet entries on a schematic document.  
  • Port Direction - Enable this option to allow port styles to be determined by the I/O type attribute of corresponding ports. 
    • Unconnected Left To Right - Enable this option and those unconnected ports on a schematic document are displayed in a left to right direction (as a right style).
  • Drag Orthogonal - If this option is enabled, when you drag components, any wiring that is dragged with the component is kept orthogonal (i.e., corners at 90 degrees). If this option is disabled, wiring dragged with a component will be repositioned obliquely. Click the check box to toggle its status.
    • Drag Step - Select the desired size from the drop-down. Options include: Smallest, Small, Medium, and Large.

Include with Clipboard

  • No ERC Markers - Enable this option to include No ERC Markers in the clipboard. 
  • Parameter Sets - Enable this option to include Parameter Sets in the clipboard. 
  • Notes - Enable this option to include Notes in the clipboard.

Alpha Numeric Suffix

Each part in a multi-part schematic component is uniquely identified by an alphabetic or numeric suffix. Use this drop-down to choose how the suffix is presented:

  • Alpha - choose this option to use an alphabetic suffix with no separator (e.g., R12A, R12B, R12C). The setting will be applied to all currently open sheets.
  • Numeric, separated by a dot '.' - choose this option to use a numeric suffix with a dot separator (e.g., R12.1, R12.2, R12.3). The setting will be applied to all currently open sheets.
  • Numeric, separated by a colon ':' - choose this option to use a numeric suffix with a colon separator (e.g., R12:1, R12:2, R12:3). The setting will be applied to all currently open sheets.

Pin Margin

  • Name - Normally, component pin names are displayed inside the body of the component adjacent to the corresponding pin. This option controls the placement of component pin names. It specifies the distance (in hundredths of an inch) from the component outline to the start of the pin name text. 
  • Number - Normally, component pin numbers are displayed outside the body of the component directly above the corresponding pin line. This option controls the placement of the pin numbers. It specifies the distance (in hundredths of an inch) from the component outline to the start of the pin number text. 

Auto-Increment During Placement

  • Primary - Enter a value to auto-increment on pin designators of a component when you are placing pins for a component. This is used for building components in the Library editor. Normally you would use a positive increment value for pin designators and negative increment value for pin names. For example: 1, 2, 3 for pin designators and D8, D7, D6 for pin names results in Primary = 1 and Secondary = -1. Set the Name to D8 and Designator to 1 in the Pin Properties panel page in pin mode before you place the first pin.
  • Secondary - Enter a value to auto-increment on pin names of a component when you are placing pins for a component. This can be used for building components in the Library editor. Normally you would use a positive increment value for pin designators and negative increment value for pin names. For example: 1, 2, 3 for pin designators and D8, D7, D6 for pin names results in Primary = 1 and Secondary = -1. Set the Name to D8 and Designator to 1 in the Pin Properties panel page in pin mode before you place the first pin.
  • Remove Leading Zeroes - Enable this option to remove leading zeroes from the string of numbers. For example, if the string is 000467 and the option is enabled, the string will become 467 with the leading zeroes removed.

Port Cross References 

To configure port cross reference settings, visit the Project Options - Options dialog.

Обнаружили проблему в этом документе? Выделите область и нажмите Ctrl+Enter, чтобы оповестить нас.

Связаться с нами

Связаться с нашими Представительствами напрямую

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
Вы сообщаете о проблеме, связанной со следующим выделенным текстом
и/или изображением в активном документе: