Schematic Preferences

Created: January 17, 2024 | Updated: March 11, 2026

Altium Essentials: Schematic Preferences

This content is part of the official Altium Professional Training Program. For full courses, materials and certification, visit Altium Training.

Watch Now

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.

The Schematic – General page of the Preferences dialog

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

Options
Break Wires At Autojunctions	Enable 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 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 a component is dropped onto a wire.
Components Cut Wires	Enable this option to configure what occurs when a component is dropped onto a wire. The wire is cut into two segments and the segments are automatically terminated onto any two hot pins of the component. The Optimize Wires & Buses option must first be enabled.
Enable In-Place Editing	When this option is enabled, the focused text field can 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. When this option is not enabled, you cannot edit the text directly; you have to edit it from the Properties panel. You can only graphically move this text field.
Convert Cross-Junctions	Enabling this option signifies 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 signifies 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 the 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 When this option is enabled, the port is automatically drawn to suit the I/O type attribute. The direction that an input or output port is drawn will depend on which side of the sheet the port is currently placed (left or right) when the Unconnected Left to Right option is disabled. Unconnected Left To Right - when this option is enabled, unconnected ports are always displayed in a left-to-right direction (referred to as a right style).
Port Direction	When this option is enabled, the port is automatically drawn to suit the I/O type attribute. The direction that an input or output port is drawn will depend on which side of the sheet the port is currently placed (left or right) when the Unconnected Left to Right option is disabled. Unconnected Left To Right - when this option is enabled, unconnected ports are always displayed in a left-to-right direction (referred to as a right style).
Drag Orthogonal	When 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). When this option is disabled, wiring dragged with a component will be repositioned diagonally. Drag Step - select the desired size from the drop-down.

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	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.

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.

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 - choose one of the following sheet styles for the cross referencing of ports on a schematic sheet or schematic sheets within a project.
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 - choose one of the following location styles for the cross referencing of ports on a schematic sheet or schematic sheets within a project.
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.

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

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

Options
Clipboard Reference	If 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 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 to display the names of the special string used by Text String objects as faint superscripts on the schematic sheet.
Center of Object	Enable to 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	Enable to hold the object being moved or dragged by the nearest electrical hot spot (e.g., 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	When 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	When 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	To prevent inadvertent overwrite of a selection memory, enable this option. Selection memory can be used to store the selection state of a set of objects.
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	When this option is enabled, when you drag a component (or selection of components), 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 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 in which you can specify which are to use the `Shift+Click` method for selection.
Click Clears Selection	Enable 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 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 the 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	When enabled, 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 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 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 to have ports and sheet entries 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 to view net highlighting. When this option is disabled, the Net Color Override dialog will open when you attempt to highlight nets.
Double Click Runs Interactive Properties	When enabled, the Properties panel will open when editing placed objects using double-click; when disabled, the modal dialog will open 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 open 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	Auto-panning comes into effect when the cross-hair action cursor is active and the cursor is moved to the edge of the view area. If auto-panning is on, the sheet will automatically pan in that direction.
Style	Use the drop-down 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 the 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.

When the Use Document Font option is enabled, the title font used is that defined by the document options (the Document Font entry in the General region of the General tab of the Properties panel when no object is selected in the design space).
When the Use Document Font option is disabled, use the provided options to choose the desired font type, size, color, and text attributes.

Color Options
Selections	This is 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 a dialog in which you can change the color as required.
Special Strings with No Value	This is 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 a dialog in which you can change the color as needed.
Cursor
Cursor	Use the drop-down to select the style of the "crosshair" editing cursor. This cursor is displayed when performing any editing action in a schematic document.

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

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

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 is 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.

On a compiled tab, only the components are available for editing and 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 compiled tabs.

Display the expanded compiled names of the following 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.
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.
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.
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.

AutoFocus

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

The Schematic – AutoFocus page of the Preferences dialog

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

Dim Unconnected Objects
On Place	Enable to not dim all of the connected objects of a net when 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 aid in the placement of electrically-aware objects.
On Edit Graphically	Enable to dim all unconnected objects on the schematic sheet when you resize a connected object.
On Move	Enable to dim all unconnected objects when moving an object connected to a network of connected objects.
On Edit In Place	Enable to dim unconnected objects on the schematic object when editing the connected object.
Thicken Connected Objects
On Place	Enable to thicken the surrounding connected objects when placing a new object on a network of the connected objects. You can change presets for the electrical grid on the Schematic - Grids page of the Preferences dialog to aid in the placement of electrically-aware objects.
On Edit Graphically	Enable to thicken all the connected objects of a network on the schematic sheet when resizing a connected object.
On Move	Enable to thicken the surrounding connected objects when moving an object connected to a network of connected objects.
Delay	Move the sliding bar to the right to increase the time delay before connected objects are thickened.
Zoom Connected Objects
On Place	Enable to zoom in all the connected objects of a network when placing an object on the network. You can change presets for the electrical grid on the Schematic - Grids page of the Preferences dialog to aid in the placement of electrically-aware objects.
On Edit Graphically	Enable to zoom in all the connected objects of a network when resizing a connected object of the network.
On Move	Enable to zoom in the surrounding connected objects when moving an object connected to a network of the connected objects.
On Edit In Place	Enable to zoom in to the connected object being edited.
Restrict To Non-net Objects Only	Enable to zoom in to the non-net objects being edited. The On Edit In Place option must be enables to access this option.

Library AutoZoom

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

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

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

Imperial Grid Presets

The table contains lists of imperial values (in mils) 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 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 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 to select from a sub-menu of grid presets to restore the presets for the Snap Grid, Snap Distance, and Visible Grid.

When in the Schematic editor, use G/Shift+G to cycle forward or backward 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). For more information about schematic grids, refer to the Setting Up a Schematic Document page.

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

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

Cutting Length
Cutting Length	Choose to snap the cutter to an entire wire segment.
Snap Grid Size Multiple	Choose to size the cutter 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 to create a fixed-length cutter; enter the value in the field to the right. Values are entered in terms of default units (1 Unit = 10mil).

Regardless of the size of cutter with options other than Snap To Segment, the cutter will shrink to accommodate smaller-sized wire segments in their entirety as it passes over them as though Snap To Segment was selected.

Show Cutter Box

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

If the Show Cutter Box option is set to Never or On Wire, the cutting area will be distinguished in the design space through use of a central cross marker when the cursor is away from a wire segment.

Show Extremity Markers

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

If both cutter box and extremity markers are set to Never, passing the cursor over a wire segment will cause the relevant portion of the segment or its entirety to become highlighted, thus distinguishing the portion of wire that will be cut when clicked.

Defaults

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

The Schematic – Defaults page of the Preferences dialog

Some of this dialog's options/controls are straightforward and require no further explanation. Those that do are described below.

Default Primitives
Primitives	Use the drop-down to filter the listing of primitives.
Primitive List	This is the 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 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 following folder of the installation: Altium Designer Develop / Altium Designer Agile: `\Users\<ProfileName>\AppData\Roaming\Altium\Altium Designer <Solution> <GUID>` Altium Designer: `\Users\<ProfileName>\AppData\Roaming\Altium\Altium Designer <GUID>`

For more information about schematic design objects, refer to the QuickNav - Schematic Design Objects page.

Additional Controls
Permanent	When enabled, the default properties of all object types are locked and are not changed if an object's properties are edited during placement. When disabled, any changes made 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 made to the defaults are stored in this file when you exit.
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 action.
Reset All	Click to reset the properties of all objects to the system defaults.

Printer-friendly version

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

Feature Availability

The features available to you depend on which Altium solution you have – Altium Develop, an edition of Altium Agile (Agile Teams or Agile Enterprise), or Altium Designer (on active term).

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

Legacy Documentation

Altium Designer documentation is no longer versioned. If you need to access documentation for older versions of Altium Designer, visit the Legacy Documentation section of the Other Installers page.

Schematic Preferences

General

Graphical Editing

Compiler

Compiled Names Expansion

AutoFocus

Library AutoZoom

Zoom Library Components

Grids

Imperial Grid Presets

Metric Grid Presets

Break Wire

Show Cutter Box

Show Extremity Markers

Defaults

Content

Was this page helpful?