Defining Schematic Preferences for Altium Designer

The pages in the Schematic category of the Preferences dialog provide access to preferences relating to features and functionality within the schematic editing domain.

General

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

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

Objects that are identified numerically will have their value incremented during repeated placement, based on the Primary and Secondary settings. For example, if Primary has a value of 1 and you press Tab during Net label placement and set the Net Name value to D01, the first net label placed will be labeled D01, the second will be D02, then D03, D04, and so on. Note that the numerical value must be the entire value or a suffix (it cannot be a prefix). Enter a negative number to decrement the value during placement.

• Primary – any object that is identified numerically will have its numerical identifier incremented by this value, if the value is edited during placement. Examples include Parts, Net Labels, Ports, Off Sheet Connectors, Sheet Entries and component Pins. 
• Secondary – any object that includes a secondary numerical identifier will have that numerical identifier incremented by this value. The Name field of Component Pins is a Secondary numerical identifier. 

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 that the ports are linked to are added in the cross reference strings.
  • Number – the sheet numbers of the sheets that the ports are linked to are added in the cross reference strings.
• 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.

Default Blank Sheet Template or Size

• Template – use the drop-down to set the default user template that will be used to create new schematic sheets. If No Default Template File is selected, a default blank schematic is created when you open a new schematic sheet. Use the Data Management – Templates page of the Preferences dialog to set the path to the templates directory.
• Sheet Size – use the drop-down to select the default blank sheet size that will be created every time you need to create a new schematic document. Sheet size can also be specified at the local document level using the Standard Page Options settings of the Properties panel in Document Options mode.
• Drawing Area – reflects the dimensions of the sheet size chosen in the Sheet Size field. This field is uneditable.

File Format Change Report

• Disable opening the report from older version – enable to NOT create a report when an older Altium Designer schematic file format document is opened. The report informs you that the document was created in an older version of the software and provides some information on features of the opened document that may be lost or have changed. This option is disabled by default.
• Disable opening the report from newer version – enable to NOT create a report when a newer schematic file format is loaded in Altium Designer. The report informs you that the document was created in a newer version of the software and provides some information on features of the opened document that may be lost or have changed. This option is disabled by default.

Graphical Editing

The Schematic – Graphical Editing page of the Preferences dialog provides numerous controls related to the editing of schematic-based documents directly in the design space.

The Schematic – Graphical Editing page of the Preferences dialog

Options

• Clipboard Reference – if this option is enabled, when you copy or cut a selection within the design space, you will be asked to select a reference point. This is useful when copying a section of circuitry that is to be pasted back into a schematic sheet. This reference point will be the point where the section of circuitry will be held when pasting. Note that the clipboard reference location is overridden by the nearest electrical hot-spot if the Object's Electrical Hot Spot option is enabled.
• Add Template to Clipboard – enable this option to also copy the current sheet template to the clipboard when you copy or cut from the current schematic sheet.
• Display Name of Special String – enable this option to display the names of the special string used by Text String objects as faint superscripts on the schematic sheet.
• Display Names of Special Strings that have No Value Defined – enable this option to display the names of special strings when they have no defined value. Disable this option to essentially hide these names, which can be of great benefit when several special strings with long names start to overlap.
• Center of Object – hold the object being moved or dragged by its reference point (for objects that have one, such as library components or ports), or its center (for objects that do not have a reference point such as a rectangle).
• Object's Electrical Hot Spot – hold the object being moved or dragged by the nearest electrical hot spot (for example the end of a pin). With this option enabled, the software moves the clipboard reference location of the object that is about to be pasted to its nearest electrical hot-spot.
• Auto Zoom – if this option is enabled, the schematic sheet is automatically zoomed when jumping to a component. Zoom level remains as it was if this option is disabled.
• Single '\' Negation – if this option is enabled, a net name can be negated by typing a backslash character before the first letter in the net name. This applies to ports, net labels, sheet entries, power ports, and harness entries.
• Confirm Selection Memory Clear – the selection memories can be used to store the selection state of a set of objects. To prevent inadvertent overwriting of a selection memory, enable this option.
• Mark Manual Parameters – parameters displayed with a dot denotes that auto-positioning has been turned off and that parameters are moved or rotated with its parent object (component, for example). To hide the dots, disable this option.
• Always Drag – if this option is enabled, every time you drag a component (or selection of components) on a schematic document, the electrical wiring stays connected. Press the Spacebar to rotate the component(s). Use Ctrl+Spacebar to toggle the wire start/end mode (corner modes).
• Shift Click To Select – enable this option if you want to use Shift+Click to select specific primitives in the design space. When this option is enabled, click the associated Primitives button to open the Must Hold Shift to Select dialog to access a list of primitives from which you can determine which are to use this Shift+Click method for selection.
• Click Clears Selection – enable this option if you want to deselect all design objects by clicking anywhere on the schematic design space. Regardless of the setting, you can deselect a selected design object by clicking on it.
• Place Sheet Entries automatically – enable this option if you want to have a sheet symbol generate a sheet entry with a matching net name automatically every time a new connection with a valid net name is wired to that sheet symbol. Otherwise, a connection with no net name wired to a sheet symbol will generate a sheet symbol with a system-generated net name.
• Protect Locked Objects – enable this option if locked objects are not to be moved and are to be ignored if they are part of a selection that is being moved. Disable this option and you will be prompted with a warning dialog if you attempt to move locked objects.

• Display Strings As Rotated – enable this option to display strings at their rotation angle (including upside down and left-reading). Disable this option to have strings always kept as right-reading, as they are rotated.

  Note that this option is not available if the operating system supports DBCS (e.g., if Japanese or Chinese locale is set for the host OS).
• Reset Parts Designators On Paste – enable this option to reset component designators when pasting onto a schematic sheet. When components are pasted, their designators will be reset to "?".
• Sheet Entries and Ports use Harness Color – enable this option if you want Ports and Sheet Entries to change color to match the color of the Signal Harness. If you specify a color for the Signal Harness, the Port or Sheet Entry will change to match. Disable this option if you prefer your Port and Sheet Entries to maintain their default color.
• Net Color Override – enable this option to view net highlighting. When this option is disabled, the Net Color Override dialog will appear if you attempt to highlight nets.

• Double Click Runs Interactive Properties – enable this option to either open the Properties panel when editing placed objects using double click, or disable it to open the modal dialog when editing placed objects using double click.

  Right-clicking on a placed object then choosing Properties from the context menu will result in the modal dialog opening if the Double Click Runs Interactive Properties option is disabled. The Properties panel will appear instead if this option is enabled.

• Show Pin Designators – enable to display the pin designators in the design space.

Auto Pan Options

• Enable Auto Pan – check to enable auto-panning.
• Style – auto-panning comes into effect when the cross-hair action cursor is active and you move the cursor to the edge of the view area. If auto-panning is on, the sheet will automatically pan in that direction. Set this field to control cursor movement during auto-panning. The options are Auto Pan Off, Auto Pan Fixed Jump (pans the sheet by a fixed step, which is set in the Step Size field – the cursor remains at the edge of the view area), and Auto Pan ReCenter (pans the sheet by a fixed step, which is set in the Step Size field – the cursor is re-centered in the view area after the pan).
• Speed – drag this bar to set the auto-panning speed. The further to the left, the slower or finer the auto-panning movement.
• Step Size – enter a value to set the size of each auto-panning step. The step size determines how fast the document pans when auto-panning is enabled. The smaller the value, the slower or finer the auto-panning movement.
• Shift Step Size – enter a value to set the size of each step when the Shift key is held during auto-panning. This determines how fast the document pans when auto-panning is enabled and the Shift key is pressed. The smaller the value, the slower or finer the auto-panning movement.

Color Options

• Selections – this field shows the current color used as the highlight color for selected items. When an object on a schematic sheet is selected, it will be highlighted using this color. Click the field to access the Choose Color dialog in which you can change the color as required.
• Special Strings with No Value – this field shows the current color used as the highlight color for special strings that have no assigned value. A special string that has no assigned value on a schematic sheet will be highlighted using this color. Click the field to access the Choose Color dialog, from where you can change the color as required.

Cursor

• Cursor Type – select an option from the dropdown list to set the style of the "crosshair" editing cursor. This cursor is displayed when you are performing any editing action in a schematic document. The following options are available: Large Cursor 90 (cursor takes the form of a horizontal and vertical line extending from the edge of the document area); Small Cursor 90 (cursor takes the form of a small cross made with a horizontal and vertical line); Small Cursor 45 (cursor takes the form of a small cross made with 45 degree lines); Tiny Cursor 45 (cursor takes the form of a tiny cross made with 45 degree lines).

Compiler

The Schematic – Compiler page of the Preferences dialog provides numerous controls related to schematic compilation and validation.

The Schematic – Compiler page of the Preferences dialog

Errors & Warnings

Errors & Warnings – the schematic objects that have an error or warning can have a wriggle underlined with specified color on the schematic sheet. You can toggle the display and the color of the wriggle for an object depending on the Level of violation by clicking on one of the fields in the Display column and one of the fields in the Color column.

Auto-Junctions

• Display On Wires – enable to display the system-generated junctions for wire objects.
  • Size – choose the size of system-generated junctions for wire objects.
  • Color – click to change the visibility or color of system-generated junctions.
  • Drag Color – click to change the color of the hotspots used to provide visual feedback on where new auto-junctions to join intersecting wires will be created while performing a drag operation.
• Display On Buses – enable to display the system-generated junctions for bus objects.
  • Size – choose the size of system-generated junctions for bus objects.
  • Color – click to change the visibility or color of system-generated junctions.
  • Drag Color – click to change the color of the hotspots used to provide visual feedback on where new auto-junctions to join intersecting buses will be created while performing a drag operation.
• Display When Dragging – enable to display the hotspots used to provide visual feedback on where new auto-junctions will be created while performing a drag operation.

Compiled Names Expansion

The project is automatically compiled after every edit action that you perform, or whenever you run the Project » Validate command. Once the project has been compiled, multiple document tabs appear at the bottom left of the schematic editor design space. The left-most (Editor) tab displays your original, logical schematic. To the right of this tab there will be a tab for each compiled (physical) schematic - one tab in a standard design, or multiple tabs in a multi-channel design (a tab for each channel). Learn more about dynamic compilation, and examining the connectivity in the compiled project.

The compiled schematic is displayed when you click on the Compiled tab. The amount of dimming applied is configured in the System - Navigation page of the Preferences dialog (hover the cursor over the image to display).

On a compiled tab only the components are available for editing, so all other design objects are dimmed (to indicate that they cannot be edited). The dimming level is configured in the System – Navigation page of the Preferences dialog.

The options below apply to how the objects are displayed on the compiled tabs:

Display the expanded compiled names of the following objects – enable the below listed desired objects:

• Designators – when a design project is compiled, all the logical sheets are expanded into physical sheets, and as a consequence, some nets are also expanded to reflect on the expanded physical sheets. Enable this option to allow component designators on physical sheets to acquire expanded net information when logical sheets are expanded into physical sheets. The drop-down menu controls how the expanded compiled names of designators are displayed after the project is compiled.
  • Display superscript if necessary – when the logical designator name and the compiled designator name differ, then the superscript is displayed.
  • Always display superscript – display superscript text for designators.
  • Never display superscript – never display superscript text for the designators.
• Net Labels – when a design project is compiled, all the logical sheets are expanded into physical sheets, and as a consequence, some nets are also expanded to reflect on the expanded physical sheets. Enable this option to allow net labels on physical sheets to acquire expanded net information when logical sheets are expanded into physical sheets. The drop-down menu controls how the expanded compiled names of net labels are displayed after the project is compiled.
  • Never display superscript – never display superscript text for the net labels.
  • Always display superscript – display superscript text for net labels.
  • Display superscript if necessary – when the logical net label name and the compiled net label name differ, then the superscript is displayed.
  Note that the Net Labels option also determines the expansion of Power Port objects.
• Ports – when a design project is compiled, all the logical sheets are expanded into physical sheets, and as a consequence, some nets are also expanded to reflect on the expanded physical sheets. Enable this option to allow ports on physical sheets to acquire expanded net information when logical sheets are expanded into physical sheets.
• Sheet Number – when a design project is compiled, all the logical sheets are expanded into physical sheets, and as a consequence, some nets are also expanded to reflect on the expanded physical sheets. Enable this option to allow sheet number parameters on physical sheets to acquire expanded net information when logical sheets are expanded into physical sheets. The drop-down menu controls how the expanded compiled names of sheet number parameters are displayed after the project is compiled.
  • Never display superscript – never display superscript text for the sheet numbers.
  • Always display superscript – display superscript text for sheet numbers.
  • Display superscript if necessary – when the logical sheet number and the compiled sheet number differ, then the superscript is displayed.
• Document Number – when a design project is compiled, all the logical sheets are expanded into physical sheets, and as a consequence, some nets are also expanded to reflect on the expanded physical sheets. Enable this option to allow document number parameters on physical sheets to acquire expanded information when logical sheets are expanded into physical sheets. The drop-down menu controls how the expanded compiled names of document number parameters are displayed after the project is compiled.
  • Never display superscript – never display superscript text for the document numbers.
  • Always display superscript – display superscript text for document numbers.
  • Display superscript if necessary – when the logical document number and the compiled document number differ, then the superscript is displayed.

AutoFocus

The Schematic – AutoFocus page of the Preferences dialog provides numerous controls related to auto-focus operations in the schematic.

The Schematic – AutoFocus page of the Preferences dialog

Dim Unconnected Objects

• On Place - enable this option to have the ability to not dim all of the connected objects of a net when you are placing an object on the net, dimming all other objects on the sheet.

  You can change presets for the Electrical Grid on the Schematic - Grids page of the Preferences dialog to help you with the ease of placement of electrically aware objects.
• On Edit Graphically - enable this option to have the ability to dim all unconnected objects on the schematic sheet when you are re-sizing a connected object. 
• On Move - enable this option to have the ability to dim all unconnected objects when you are moving an object connected to a network of connected objects on the schematic sheet. 
• On Edit In Place - enable this option to have the ability to dim unconnected objects on the schematic object when you are editing this connected object.
• All On - click to turn all the options related to dimming unconnected objects on the schematic ON.
• All Off - click to turn all the options related to dimming unconnected objects on the schematic OFF.

Thicken Connected Objects

• On Place - enable this option to have the ability to thicken the surrounding connected objects when you are placing a new object on a network of these connected objects on the schematic sheet.

  You can change presets for the Electrical Grid on the Schematic - Grids page of the Preferences dialog to help you with the ease of placement of electrically aware objects.
• On Edit Graphically - enable this option to have the ability to thicken all the connected objects of a network on the schematic sheet when you are re-sizing a connected object.
• On Move - enable this option to have the ability to thicken the surrounding connected objects when you are moving an object connected to a network of connected objects on the schematic sheet.
• Delay - the time delay before connected objects are thickened. Move the sliding bar to the right to increase the delay.
• All On - click to turn all the options related to thickening of connected objects on the schematic ON.
• All Off - click this button to turn all the options related to thickening of connected objects on the schematic OFF.

Zoom Connected Objects

• On Place - enable to have the ability to zoom in all the connected objects of a network when you are placing an object on this network.

  You can change presets for the Electrical Grid on the Schematic - Grids page of the Preferences dialog to help you with the ease of placement of electrically aware objects.
• On Edit Graphically - enable to have the ability to zoom in all the connected objects of a network on the schematic sheet when you are re-sizing a connected object of this network.
• On Move - enable to have the ability to zoom in the surrounding connected objects when you are moving an object connected to a network of these connected objects on the schematic sheet.
• On Edit In Place - enable to have the ability to zoom in the connected object that is being edited.
• Restrict To Non-net Objects Only - enable to have the ability to zoom in the non-net objects that are being edited.
• All On - click to turn all the options related to zooming connected objects on the schematic ON.
• All Off - click to turn all the options related to zooming connected objects on the schematic OFF.

Library AutoZoom

The Schematic – Library AutoZoom page of the Preferences dialog provides controls related to auto-zoom operations in the schematic.

The Schematic – Library AutoZoom page of the Preferences dialog

Zoom Library Components

Select one of the following options:

• Do Not Change Zoom Between Components
• Remember Last Zoom For Each Component 
• Center Each Component In Editor
  • Zoom Precision - slide to set the zoom precision. The further right, the higher the precision.

Grids

The Schematic – Grids page of the Preferences dialog provides the settings for the grid configuration in the schematic editor.

The Schematic – Grids page of the Preferences dialog

Grid Options

• Grid - select an option from the drop-down list to set the style of the visible grid for schematic documents. The following options are available:
  • Dot Grid - the grid is shown as dotted lines.
  • Line Grid - the grid is shown as solid lines.
• Grid Color - this field shows the current color used to draw the visible grid on schematic sheets (schematic editor and schematic library editor). Click the color sample box to open a dialog in which you can change the visible grid color. Note that if the current document is a schematic library component, grid color changes are not applied until you switch to a different library component. 

Imperial Grid Presets

The table contains lists of imperial values (in mils) for the Snap Grid, Snap Distance, and Visible Grid for schematic sheets. The values can be modified or the checkboxes can be enabled/disabled to toggle the visibility of each grid.

• Altium Presets - click this button to select from a sub-menu of grid presets to restore the presets for the Snap Grid, Snap Distance, and Visible Grid.

Metric Grid Presets

The table contains lists of metric values (in mm) for the Snap Grid, Snap Distance, and Visible Grid for schematic sheets. The grid values can be modified or the checkboxes can be enabled/disabled to toggle the visibility of each grid.

• Altium Presets - click this button to select from a sub-menu of grid presets to restore the presets for the Snap Grid, Snap Distance, and Visible Grid.

Break Wire

The Schematic – Break Wire page of the Preferences dialog provides controls related to the behavior of the cutting tool when using the Break Wire feature. While the tool is labeled Break Wire, it can be used to break wires as well as buses and signal harnesses.

The Schematic – Break Wire page of the Preferences dialog

Cutting Length

Select one of the following options to control the length of wire that gets cut:

• Snap to Segment - choose this option to have the cutter snap to an entire wire segment.
• Snap Grid Size Multiple - choose this option to have the cutter sized to a defined multiple of the current snap grid. Enter a value for the multiplier in the field to the right from 2 and 10 (inclusive).
• Fixed Length - choose this option to create a fixed-length cutter, the length of which is specified by entering a value in the field to the right.

Show Cutter Box 

Select one of the following options to control the display of the cutter box (dotted rectangular box) while in Break Wire mode:

• Never - never display the cutter box.
• Always - always display the cutter box, regardless of whether the cursor is over a wire segment or not.
• On Wire - only display the cutter box when the cursor passes over a wire segment.

Show Extremity Markers

Select one of the following options to control the display of extremity markers (at the ends of the cutter box) while in Break Wire mode:

• Never - never display the extremity markers.
• Always - always display the extremity markers, regardless of whether the cursor is over a wire segment or not.
• On Wire - only display the extremity markers when the cursor passes over a wire segment.

Defaults

The Schematic – Defaults page of the Preferences dialog provides controls and information related to primitives in the schematic.

The Schematic – Defaults page of the Preferences dialog

Default Primitives

• Primitives - use this field to filter the presented listing of primitives. Choose from: All, Drawing Tools, Other, Wiring Objects, Library Parts, Harness Objects,  and Sheet Symbol Objects.

• Primitive List - a list of primitives that can be used on a schematic sheet (filtered in accordance with the chosen entry for the Primitives field above). Click on the below listed Primitives to change the available default values as described.

  All primitive default values are saved in the Advsch.dft and Advsch.MMsdft files. These files are located in the \Users\<ProfileName>\AppData\Roaming\Altium\Altium Designer <GUID> folder of the installation.

  To view and edit the settings and options for each primitive, click on the desired entry in the Primitive List. Information for each primitive can be found at the following links:

  The links below provide information on all properties available for schematic objects. Note that some properties are only available in the Properties panel during or after the placement and are not available as default settings in the Preferences dialog.

  • Arc
  • Bezier
  • Blanket
  • Bus
  • Bus Entry
  • Comment
  • Designator
  • Ellipse
  • Graphic
  • Harness Connector
  • Harness Connector Type
  • Harness Entry
  • Net Label
  • No ERC
  • Note
  • Offsheet Connector
  • Parameter
  • Parameter Set
  • Part
  • Pin
  • 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

Additional Controls

• Permanent - if this option is enabled, the default properties of all object types are locked and are not changed if you edit an object's properties during placement. If this option is disabled, any changes you make to a particular object during placement (by pressing the Tab key while the object is floating on the cursor before placement to open the Properties panel) are used to update the default properties for that particular object type.
• Save as - click to save the current default object properties to a custom properties file (*.dft). You will be asked for a name and directory for the file. When the schematic editor server is started, the current defaults are read and any changes you make to the defaults are stored in this file when you exit. Use the Load button to load a previously saved set of default properties.
• Load - click to load a previously saved set of default object properties. You will be asked to navigate to and select a previously saved properties file (*.dft). After loading the properties file, close and reopen the Preferences dialog to show any changes made by the Load action.
• Reset All - click to reset the properties of all objects to the system defaults.