创建原理图中的电路连接

Net labels identify and electrically connect different points in a schematic.

Summary

Electrical connectivity between schematic component pins can be created by placing a wire between those pins. This is called physical connectivity since the pins are physically connected with a wire. Connectivity also can be created logically by using suitable net identifiers, such as net labels. As well as providing a human-friendly identifier for a net, a net label allows you to connect points on a circuit without actually physically wiring them together.

Availability

Net labels are available for placement in the Schematic Editor only in the following ways:

• Choose Place » Net Label from the main menus.
• Click the Net Label button () in the graphic objects drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the top-most item on that section of the Active Bar.)
• Right-click in the design space then choose Place » Net Label from the context menu.
• Click the  button on the Wiring toolbar.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter net label placement mode with a net label floating on the cursor:

• Press Tab to open the Net Label mode of the Properties panel with the Net Name field selected and ready for editing; enter the new net name.
• Position the net label so that its bottom-left corner touches the object to which you want to assign it then click or press Enter to place the net label.
• Continue placing further net labels, or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement while the net label is still floating on the cursor and before the center point of the net label is anchored are:

• Press the Tab key to pause the placement and access the Net Label mode of the Properties panel in which its properties can be changed on the fly. Click the design space pause button overlay ( ) to resume placement.
• Press the X or Y keys to flip the net label along the X-axis or Y-axis.
• Press the Spacebar to rotate the net label counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in increments of 90°.

Considerations during placement:

• The electrical hotspot on a net label is the lower left corner, therefore, this corner must touch the wire, bus, or signal harness for a valid connection to be made.
• If the Net property of the net label is entered before it is placed and the value entered has a numeric ending, each subsequent net label will auto-increment this numeric value. This behavior is configured in the Auto-Increment During Placement options on the Schematic – General page of the Preferences dialog. For net labels, only the Primary field applies; the Secondary field applies when the object has multiple fields, such as a Pin.

Graphical Editing

The net label can be edited graphically using what is known as in-place editing. To edit a net label string in place, click once to select, pause then click a second time to enter edit mode.

 Click once to select the string.

 Pause, then click a second time to enter in-place edit mode.

 The string has been selected, ready to type in a replacement string. The Net Label can be edited in-place.

Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

Notes

• Net labels create logical connectivity within a single schematic sheet; they do not create connectivity between schematic sheets. To do this, Ports must be used.
• To negate (include a bar over the top of) a net label, use one of the following methods:
  • Include a backslash character after each character in the net name (e.g., E\N\A\B\L\E).
  • Enable the Single '\' Negation option on the Schematic - Graphical Editing page of the Preferences dialog, then include one backslash character at the start of the net name (e.g., \ENABLE).
• When individual nets form a bus, there are specific requirements as to how they are named. For more information, refer to the Bus page.
• Net identifiers of different types do not automatically connect to one another even if they share the same name. For example, a net label named AGND will not automatically connect to a power port named AGND; a wire must be placed to connect them.

Location

• (X/Y)
  • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • Y (second field) - the current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
• Rotation - use the drop-down to select the rotation. 

Properties

• Net Name - use the drop-down to select the net name or enter the name directly.
• Font - use the controls to select the desired font, font size, color, and attributes to bold, italicize, etc., if desired.
• Justification - select the justification by clicking on an arrow that corresponds with the desired justification, or the circle to center.

Off Sheet Connectors are used to create connections between schematic sheets.

Summary

An off sheet connector is an electrical design primitive. Off sheet connectors are used to connect nets across multiple schematic sheets that are descended from the same parent sheet symbol.

Availability

Off sheet connectors are available for placement in the Schematic Editor only in the following ways:

• Choose Place » Off Sheet Connector from the main menus.
• Right-click in the design space then choose Place » Off Sheet Connector from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter off sheet connector placement mode with an off sheet connector floating on the cursor:

• Press Tab to open the Off Sheet Connector mode of the Properties panel with the Net Name selected and ready for editing; enter the new net name.
• Position the off sheet connector so that its electrical hotspot (the end held by the cursor) touches the wire to which you want to connect then click or press Enter to effect placement.
• Continue placing further off sheet connectors or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement while the off sheet connector is still floating on the cursor are:

• Press the Tab key to pause the placement and access the Off Sheet Connector mode of the Properties panel in which its properties can be changed on-the-fly. Click the workspace pause button overlay ( ) to resume placement.
• Press the X or Y keys to flip the off sheet connector along the X-axis or Y-axis.
• Press the Spacebar to rotate the off sheet connector counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in increments of 90°.

Graphical Editing

The off sheet connector can be edited graphically using what is known as in-place editing. To edit an off sheet connector string in-place, click once to select, pause, then click a second time to enter edit mode.

 Click once to select the string.

 Pause, then click a second time to enter in-place edit mode.

 The string has been selected, ready to type in a replacement string.

The Off Sheet Connector can be edited in-place.

Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

Location

• (X/Y)
  • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current workspace origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • Y (second field) - The current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
• Rotation - use the drop-down to select the rotation. Choices are: 0 Degrees, 90 Degrees, 180 Degrees, and 270 Degrees.

Properties

• Net Name - enter the net name.
• Cross Ref - this field displays cross reference values that are applied to the offsheet connector. 
• Style - use the drop-down to select the default from the available choices: Left or Right. Click on the color box to access a drop-down from which you can select the default color.

General (Net)

Displays the properties of the nets assigned to the off sheet connector. Update as needed.

Parameters (Net)

• Selection buttons - click the desired objects to display in the grid.  
• Add - use the drop-down to add the desired object(s) then define the values.

A placed Power Port

Summary

A power port is an electrical design primitive. It is a special schematic object used to define a power or ground net. Power ports allow you to conveniently indicate a power net at any location in the design, which can then be connected to pins or wires. Power nets of the same name automatically connect throughout the design, except in the following two situations:

• If a Power Port is specifically wired to a Port object, then that power net becomes local to that sheet - net connections beyond the sheet must then be defined by the wiring of the Port/Sheet Entry combination.
• If the Net Identifier Scope is set to Strict Hierarchical. This sets all power nets to be local within each sheet. Refer to the Options tab of the Project Options dialog to learn more.

Availability

Power ports are available for placement in the Schematic Editor in the following ways:

• Click Place » Power Port from the main menus.
• Click the  button on the Wiring toolbar to place a bar-style power port, pre-assigned to the VCC net.
• Click the  button on the Wiring toolbar to place a power ground style power port pre-assigned to the GND net.
• Click the Harness Entry button () in the graphic objects drop-down on the Active Bar located at the top of the design space. Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the top-most item on that section of the Active Bar.
• Click the  button on the Utilities toolbar to access a drop-down providing an array of power port commands, including the various styles and several net-pre-assigned power ports.
• Right-click in the design space then choose Place » Power Port from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter power port placement mode. A power port symbol will appear floating on the cursor.

1. Position the object then click or press Enter to effect placement.
2. Continue placing further power ports or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement while the power port is still floating on the cursor are:

• Press the Tab key to pause the placement and access the Power Port mode of the Properties panel from where its properties can be changed on the fly. Click the design space pause button overlay ( ) to resume placement.
• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement.
• Press the Spacebar to rotate the power port counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in increments of 90°.
• Press the X or Y keys to mirror the power port along the X-axis or Y-axis.

Graphical Editing

This method of editing allows you to select a placed power port object directly in the design space then change its location graphically. Power ports are fixed with respect to their size and shape. As such, editing handles are not available when the power port object is selected:

A selected Power Port

• Click anywhere inside the dashed box then drag to reposition the power port as required. While dragging, the power port can be rotated (Spacebar/Shift+Spacebar) or mirrored (X or Y keys to flip along the X-axis or Y-axis).
• The assigned net for a power port object can be edited in place by:
  1. Single-clicking the power port to select it.
  2. Single-clicking again (or pressing Enter) to enter the in-place editing mode. Sufficient time between each click should be given to ensure that the software does not interpret the two single-clicks as one double-click (which would open the Properties panel).
  3. To finish editing in-place text, press Enter or use the mouse to click away from the power port.

Power Port Styles

The following graphical styles of power port are available and can be set by editing the object's Style property in the Properties panel.

Note

To negate a power port (include a bar over the top of its name), use one of the following methods:

• Include a backslash character after each character in the net name (e.g., V\C\C\3\).
• Enable the Single '\' Negation option on the Schematic - Graphical Editing page of the Preferences dialog, then include one backslash character at the start of the net name (e.g., \VCC3).

Location

• (X/Y)
  • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • Y (second field) - The current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial;  include the units when entering a value whose units are not the current default. 
• Rotation - use the drop-down to select the rotation. 

Properties

• Name - the name of the power port. Use the eye icon to show/hide the name.
• Style - use the drop-down to select the style of the power object. The preview image updates according to your choice. Click the color box to choose the color.
• Font - use the controls to select the desired font, font size, color, and attributes to bold, italicize, etc., if desired.

General (Net)

Displays the properties of the nets assigned to the power port. Update as needed.

Parameters (Net)

• Selection buttons - click the desired objects to display in the grid.  
• Add - use the drop-down to add the desired object(s) then define the values.

Wires are used to create electrical connectivity in a schematic.

Summary

A wire is a polyline electrical design primitive that is used to form electrical connections between points on a schematic. It is analogous to a physical wire.

Availability

Wires are available for placement in the Schematic Editor only in the following ways:

• Choose Place » Wire from the main menus.
• Click the Wire button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar).
• Click the button on the Wiring toolbar.
• Right-click in the design space then choose the Place » Wire command from the context menu.​
• Using the Ctrl+W shortcut.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter wire placement mode. Placement is made by performing the following sequence of actions:

1. Click or press Enter to anchor the starting point for the wire.
2. Position the cursor then click or press Enter to anchor a series of vertex points that define the shape of the wire.
3. After placing the final vertex point, right-click or press Esc to complete placement of the wire.
4. Continue placing further wire objects or right-click or press Esc to exit placement mode.
5. Use the Backspace or Delete keys to remove the last wire segment placed.

Placement Modes

When placing a wire, there are three 'manual' placement modes, two of which have Start and End sub-modes. The mode specifies how corners are created when placing wires and the angles at which wires can be placed. During placement:

• Press Shift+Spacebar to cycle through the modes.
• While in the 90 Degree or 45 Degree mode (known as true orthogonal modes), press Spacebar to cycle between the Start and End sub-modes.
• During placement, the current placement mode is displayed in the Status bar. You can change modes at any time during wire placement.
• In modes other than Any Angle, the line segment attached to the cursor is a look-ahead segment. The segment you are actually placing precedes this look-ahead segment.

45 degree mode

90 degree mode

Any angle mode

Auto Wire mode

Guided Wiring

Schematics have a definable electrical grid that makes it easy to define electrical connections between objects. As you are placing a wire, when the wire falls within the electrical grid range of another electrical object, the cursor will snap to the fixed object and a Hot Spot (blue cross) will appear.

The Hot Spot guides you to where a valid connection can be made and automatically snaps the cursor to electrical connection points.

The electrical grid can be defined on the General tab of the Properties panel in Document Options mode. It is recommended that you set the electrical grid to be slightly smaller than the current snap grid or it can become difficult to position electrical objects one snap grid apart.

Graphical Editing

This method of editing allows you to select a placed wire object directly in the design space and change its size and/or shape graphically.

When a wire object is selected, the following editing handles are available.

A selected Wire ready for graphical editing.

• Click and drag A to reposition the end points of the wire.
• Click and drag B to move a wire vertex. The end points will remain anchored.
• Click and drag on a wire segment to grab that segment and reposition it. The end points and other vertices will remain anchored.
• Right-click on a vertex point then choose the Edit Wire Vertex n command to access the Vertices tab of the Wire dialog with the entry for the nth vertex selected ready for editing.
• Click and hold on a vertex then press Delete on the keyboard to remove that vertex.

Information About Dragging

• While dragging, hotspots are used to provide a visual indication of where auto-junctions are going to be created.
• Unnecessary/redundant auto-junctions are removed after dragging has ceased.

Indication of New Auto-Junction Creation

Depending on the affected wiring, performing a drag operation may result in the creation of auto-junctions at new locations. To provide visual feedback on where these new junction instances will be, hotspots are used. Enable the use of these hotspots and their color for wires and buses in the Auto-Junctions region on the Schematic - Compiler page of the Preferences dialog.

Selecting and Removing

With the wire selected, click on a segment to individually select that segment. This wire 'sub-selection' is distinguished by the associated editing handles becoming red in color.

Individual segment sub-selection.

The associated vertices for the segment can then be edited directly using the SCH List panel with any changes appearing immediately on the schematic.

You also can perform removal of selected wire segments with the tap of the Delete key. You can delete multiple segments across different wires - ensure that each is selected (Shift+Click twice on each subsequent segment to include it in the overall segment selection). Auto-junctions are also accounted for - allowing you to remove a segment of a wire up to that junction only (and including that junction if only two other wire segments would otherwise remain connected to it).

Autojunctions

A T-junction in a wire is automatically connected by a junction (Compiler-Generated Junction). If the Break Wires At Autojunctions option is enabled on the Schematic - General page of the Preferences dialog, an existing wire segment will be broken into two at the point where an autojunction is inserted. For example, when making a T-Junction, the perpendicular wire segment will be broken into two segments, one on each side of the junction. With the Break Wires At Autojunctions option disabled, the wire segment will remain unbroken at the junction.

General (Net)

Displays the properties of the nets assigned to the wire. Update as needed.

Vertices

• Width - use the drop-down to select the desired width. Click the color box to select the desired color for the object.
• Vertices Grid - lists all of the vertex points currently defined for the object in terms of:
  • Index - the assigned index of the vertex (non-editable).
  • X - the X (horizontal) coordinate for the vertex. Click to edit.
  • Y - the Y (vertical) coordinate for the vertex. Click to edit.
• Add - click to add a new vertex point. The new vertex will be added below the currently focused vertex entry and will initially have the same X,Y coordinates as the focused entry. Click to remove the currently selected vertex.

Parameters (Net)

• Selection buttons - click the desired objects to display in the grid.  
• Add - use the drop-down to add the desired object(s) then define the values.

The schematic compiler automatically adds junctions at each T-junction to complete the electrical connection.

Summary

A junction is an electrical design primitive. It is a small circular object used to join intersecting wires (or buses, or signal harnesses) on a schematic sheet. A Compiler generated junction is a junction that is automatically placed by the Auto-junctioning feature 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, power port or other electrical object.

Availability

This type of junction is placed automatically by the Schematic Editor's Auto-junctioning feature. As such, it is not a design object that can be accessed and placed by the user.

Placement

Compiler-generated junctions are placed automatically whenever a T-junction occurs during wiring, such as 2 wires/buses/signal harnesses meeting in a T, or a wire/bus/signal harness orthogonally crossing the end of a component pin or another electrical object, such as a Power Port.

Editing

A Compiler generated junction cannot be edited in the usual manner (via a dialog or graphically on the schematic sheet). The display properties of compiler generated junctions are configured on the Schematic - Compiler page of the Preferences dialog, as shown in the image below. Note that disabling the display of compiler generated junctions does not break the electrical connection at that junction point.

Configure the display options for compiler generated junctions (auto-junctions) in the Preferences dialog.

Indication of New Auto-Junction Creation

Depending on the affected wiring, performing a drag operation may result in the creation of auto-junctions at new locations. To provide visual feedback on where these new juntion instances will be, hotspots are used. Enable the use of these hotspots, and specify their color - for wires and buses - also as part of your preferences.

Control the display of predicted auto-junctioning during drag operations.

Example showing predicted new auto-junctions resulting from a drag operation.

Visual Indication of Connectivity Change

While dragging a component, it is possible to inadvertently drag a little to far, or off-course, resulting in an unintended auto-junction, and a potentially fatal change to the connectivity of a circuit. To provide a timely and graphical indication of the status of connectivity while performing a drag, a couple of icons are used:

- OK - the drag operation is not altering the connectivity of the circuit.

- Alert - the drag operation is causing a change to the connectivity of the circuit.

The applicable icon is displayed near to the cursor as you drag.

Providing a visual warning that a drag operation will result in a change to connectivity.