Schematic - General

Parent page: Schematic Preferences

Summary

The Schematic – General page of the Preferences dialog provides controls to configure the basic setup of schematic-based documents and the Schematic Editor workspace. 

Access

The Schematic – General page is part of the main Preferences dialog (File |

Options/Controls

Options

• Drag Orthogonal - When dragging components with this option enabled, any wiring that is dragged with the component is kept orthogonal (i.e. corners at 90°). If this option is disabled, wiring dragged with a component will be repositioned obliquely.
  • Drag Step - Determines the distance between the steps created when dragging an object with parallel connection lines over the range of Smallest to Large.

• 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 a component when the component is dropped onto a wire.
• Convert Cross Junctions - Enable this option so that when the addition of a wire would create a four-way junction, it is instead converted into two adjacent three-way junctions. When this option is disabled, 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 the option is enabled, the wiring cross-overs will be displayed with little bridges on the currently focused schematic sheet.

Auto-Increment During Placement

• Primary - Enter a value to auto-increment component pin designators as pins are sequentially placed for a component. With the value set to 1 for example, the designators of a sequence of placed pins would be 1, 2, 3, etc. Note that the designator of the first pin would be set to 1 in the Pin Properties dialog as the pin is placed.
• Secondary - Enter a value to auto-increment component pin names as pins are sequentially placed for a component. With the value set to 1 for example, the designators of a sequence of placed pins would be D1, D2, D3, etc. Note that the name of the first pin would be set to D1 in the Pin Properties dialog as the pin is placed. If set to -1, the pin name would decrement – D8, D7, D6, etc.
• Remove Leading Zero - Enable this option to remove leading zeros from the string of numbers. For example if it was 002 and the option is enabled, the leading zeros would be removed for a result of 2.

Alpha Numeric Suffix

Multi-part components can use either a Numeric or Alpha part identifier suffix (for example, U1:1 or U1A). Select the preferred style from the drop-down list.

• Alpha - Select this option to use an alpha component suffix - U1A, U1B, etc.
• Numeric, separated by a dot - Select this option to use an numeric component suffix with dot separator - U1.1, U1.2, etc.
• Numeric, separated by a colon - Select this option to use an numeric component suffix with colon separator - U1:1, U1:2, etc.

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 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 from the component outline to the start of the pin number text.

Default Font for Primitives

Click the Change button to configure the font used for all primitives on schematic documents.

Default Power Object Names

• Power Ground - When placing a Power Ground style power port in a schematic, its net name will default to this value. If the field is empty, then the last valid value will apply to any new ports of this style. The default name is GND.
• Signal Ground - When placing a Signal Ground style power port in a schematic, its net name will default to this value. If the field is empty, then the last valid value will apply to any new ports of this style. The default name is SGND.
• Earth - When placing an Earth power port in a schematic, its net name will default to this value. If the field is empty, then the last valid value will apply to any new ports of this style. The default name is EARTH.

Defaults

• Template - Use this field to set the default template file that will be used to create new schematic sheets. Choose from the drop-down menu list of predefined templates based on standard page sizes. To not use a template, set the field to No Default Template File.

Port Cross References

• Sheet Style -  Choose one of the following sheet styles for the cross referencing of ports on a schematic sheet or schematic sheets within a project.
  • None - No sheet style is added in the cross reference string of all ports.
  • Name - Names of the sheets to which the ports are linked are added in the cross reference strings.
  • Number - The sheet numbers of the sheets to which the ports are linked are added in the cross reference strings.

The design project needs to be compiled first before any cross references can be added to the ports. Sheet Numbers can be defined in the SheetNumber entry under the Parameters tab in the Document Options dialog:
Project | Content | .

• Location Style - Choose one of the following location styles for the cross referencing of ports on a schematic sheet or schematic sheets within a project.
  • None - No location style is added in the cross reference string of all ports.
  • Zone -The reference zone numbering (the sheet borders have the zones) is added in the cross reference strings of all ports that are associated to the parent objects, such as the location of sheet symbols.

  • Location X,Y - The locations of the ports are published in brackets in the cross reference strings for all ports that are associated to the parent objects, such as the location of sheet symbols. Note that the design project needs to be compiled first before any cross references can be added to the ports.

Imperial Unit System

• Use Imperial Unit System - Enable this option to use imperial units in schematic projects.
• Imperial unit used - From the drop-down list, choose one of the available imperial units: Mils, Inches, Dxp Defaults (10 mils), or Auto-Imperial. If Auto-Imperial is selected, the system will switch from Mils to Inches when the value is greater than 500 mils.

Metric Unit System

• Use Metric Unit System - Enable this option to use the metric units for schematic projects.
• Metric unit used -  From the drop-down list, choose one of the available metric units: Millimeters, Centimeters, Meters, or Auto-Metric. If Auto-Metric is selected, the system will switch from Millimeters to Centimeters when the value is greater than 100 cm.

Unit System

Reports the current default unit setting for new documents and indicates a pending unit change.