Schematic Editor: Application Settings

The Application Settings dialog allows you to specify the color of items that are previewed on the canvas, and set the position of property viewers. You can configure settings for rotating, copying, pasting and deleting objects on the canvas. Synchronization, Reference Designator and backup options can be specified, and DRC and Check Mode settings can be configured. It also allows you to configure SPICE Controller. Launch this dialog by clicking File > Configuration > Application Settings on the ribbon in eCADSTAR Schematic Editor or eCADSTAR Schematic Viewer.

Display Settings

Advanced

Check

SPICE Controller

Display Settings

Value		Description
Select Preview		Allows you to specify the color of items that are previewed on the canvas when the cursor is hovered over them.
	Color button	Displays the Select color dialog. Specify the preview color by selecting it in the dialog, and then clicking OK. When you hover the cursor over items on the canvas, they are displayed in the color that you specify.
Selected		Allows you to specify the color of items that you select on the canvas.
	Color button	Displays the Select color dialog. Specify the color for selected items by clicking it in the dialog, and then clicking OK. Items that you select on the canvas are displayed in the specified color.
Property viewer		Allows you to specify the position of Property Viewers that are displayed on the canvas. To display a Property Viewer, right-click the relevant row in the Properties Panel and select Display Viewer on the assist menu.
	Origin	Allows you to specify the origin of the property viewer by selecting an item in the Origin box. The origin is indicated by a red square. The position of the property viewer is defined in relation to its origin.
Marks		Allows you to specify whether marks are displayed on the schematic sheets for unconnected pins and net nodes. These marks are helpful when creating a schematic sheet, but are not typically required after the schematic sheet has been created.
	Unconnected pins and Net nodes	Selected: marks are displayed on the schematic sheets for unconnected pins and net nodes. These marks are displayed when the schematic sheet is printed. Not selected: marks are not displayed on the schematic sheets for unconnected pins and net nodes. These marks are not displayed when the schematic sheet is printed. Note You must close and then reopen the schematic sheet to apply the above changes.

Advanced

Value		Description
Rotate		When objects are rotated on the canvas, this setting allows you to specify whether they are rotated around their center or their origin.
	Rotate around center	Selected: objects are rotated around their center. Not selected: objects are rotated around their origin.
Copy		When a net is copied, this setting allows you to specify whether the associated net label is also copied.
	Copy with Net Label	If user-defined net names are copied. Selected: the net label of the net is copied, as well as the net. eCADSTAR is immediately updated to show the copied net label. Not selected: the net label of the copied net is not copied. If system-defined net names are copied. Selected: the system generated net labels are not assigned automatically to the net. Instead, they are assigned when they are saved. This prevents the same net label being auto generated by multiple users, which could result in nets merging when saved. Not selected: the net label of the copied net is not copied.
Paste		Allows you to specify whether information regarding design variation is kept when a component is copied and pasted on the same sheet, and when a circuit block is copied and pasted.
	Retain variation information	Selected: information regarding design variation is kept when a component is copied and pasted on the same sheet, and when a circuit block is copied and pasted. Not selected: information regarding design variation is lost when a component is copied and pasted on the same sheet, and when a circuit block is copied and pasted.
Component to Net Interaction		When placing a symbol over a net on the canvas, this section allows you to specify whether it is automatically connected to the relevant net. It also allows you to specify whether it is connected to the net in series or parallel.
	Auto Connect	Selected: if you place a symbol over a net on the canvas, then it is automatically connected to it. This is illustrated in the following example. Not selected: if you place a symbol over a net on the canvas, then it is placed over the net, but is not connected to it. This is illustrated in the following example. However, if you select Split Net, then it is automatically connected, in series, to the net.
	Split Net	Selected: if you place a symbol over a net on the canvas, then it is automatically connected, in series, to the net. This is illustrated in the following example. Not selected: if you place a symbol over a net on the canvas, and Auto Connect is selected, then it is automatically connected, in parallel, to the net. This is illustrated in the following example.
Delete		Allows you to specify whether connected nets are also deleted.
	Delete connections with Component deletion	Selected: when a component is deleted, connected nets are also deleted. Not selected: when a component is deleted, connected nets are not deleted.
Synchronization		Allows you to synchronize the net label of a net, and the part name of a power supply, ground, sheet connector, hierarchy connector or global connector that is connected to the net. You can also synchronize the bit count when pin labels are set for symbol pins in Symbol Editor.
	Port Net label	If selected, then signal names are synchronized when a connection is made between a net and a sheet connector, hierarchy connector or global connector. On a net, the signal name is the value of the Net Label attribute. On a sheet connector, hierarchy connector or global connector, the signal name is the value of the Part Name attribute. Unassigned Net label or Part Name attributes are replaced by assigned values. Previously-assigned Net label or Part Name attributes are not changed.
	Do Not Target Hierarchy Connector in Net/Bus and Port Net Label	If selected, hierarchy connectors are not synchronized but all other attributes are synchronized (Power/Ground/Sheet Connector/Global Connector).
	Bit count when the Symbol Pin name is changed	If selected, bit counts are synchronized when symbol pins are connected. A symbol pin can represent multiple physical pins in Symbol Editor.
Reference		Allows you to specify the number of digits in the numeric part of the auto-generated values for Reference Designator.
	Number of digits in Reference Number	Specify the number of digits in the numeric part of the auto-generated values for Reference Designator.
Backup		Allows you to specify the interval at which schematic data is backed up.
	Auto-backup interval (minutes)	Specify the interval, in minutes, at which the schematic data that you are editing is automatically backed up.

Note
A license is required to access the variation functionality in eCADSTAR.

Check

Value		Description
DRC		Allows you to specify whether components that are not fitted to the board are checked by the DRC command.
	Check not fitted components	Selected: components that are fitted and not fitted to the board are checked by the DRC command. Not selected: only components that are fitted to the board are checked by the DRC command.
	Use E-Net for Matrix and Conflicting Pin Types checks	Selected: the DRC checks that are defined in the DRC Settings Dialog, Conflicting Pin Types and Connection Matrix fields are performed using the relevant E-Net, rather than the logical net. Not selected: the DRC checks that are defined in the DRC Settings Dialog, Conflicting Pin Types and Connection Matrix fields are performed using the relevant logical net, rather than the E-Net.
Check Mode		Allows you to identify overlapping nets, and nets that have the same value for Net Label, but are not connected.
	Net overlap check	Selected: overlapping nets are identified. This includes the same net or different nets. Not selected: overlapping nets are not identified.
	Net label mismatch check	Selected: connections are not permitted between nets that have different values for Net Label. Not selected: connections are permitted between nets that have different values for Net Label.

SPICE Controller

LTspice Setting

Value

Description

Executable path

Displays the path to the LTspice executable file that you specify. Click

and browse to the required *.exe file in the Select executable path dialog. It is recommended that you download the LTspice application from the Analog Devices website.

Note
Before you execute a simulation, specify this path and then restart eCADSTAR.

Select the LTspice executable file (*.exe) in the displayed Select executable path dialog.

Command-line arguments

Specify the command-line arguments that are passed to the simulator.

Note
It is recommended that -ascii is specified. This converts the data for the Operating Point Display into ASCII format. This enables it to be back annotated from the LTspice application into eCADSTAR Schematic Editor.

The following command-line arguments are supported.

Value	Description
-ascii	Use ASCII .raw files.
-b	Execute in batch mode. For example, "scad3.exe –b deck.cir" will leave the data in the file deck.raw.
-big	Start as a maximized window.
-encrypt	Encrypt a model library.
-FastAccess	Batch conversion of a binary .raw file to Fast Access format.
-ini <path>	Specify an .ini file to use other than %WINDIR%\scad3.ini.
-max	See: -big.
-netlist	Batch conversion of a schematic to a netlist.
-nowine	Prevent use of WINE(Linux) workarounds.
-PCBnetlist	Batch conversion of a schematic to a PCB format netlist.
-registry	Force LTspice to store user preferences, MRU, etc. in the registry instead of the %WINDIR%\scad3.ini file.
-Run	Start simulating the schematic opened on the command line without pressing the Run button.
-SOI	Allow MOSFET's to have up to seven nodes, even in subcircuit expansion.
-uninstall	Execute one step of the uninstallation process.
-wine	Force use of WINE(Linux) workarounds.

Include file

Allows you to add and delete library files, and order them in the Include file table. These are text files that may comprise analysis statements, circuit nets or device models. In the SPICE Controller Manager, add them to the Analysis tree by clicking Insert Analysis Conditions, and then selecting Include files in the Analysis Conditions dialogs. These files are listed in the displayed Select an Include file dialog. If specified, then they are added when the simulation is performed.

Include file table

Displays the library files that you specify using the Add and Browse buttons. Use the

and

buttons to specify the search order for these files. The most trusted library file should be listed first.

Add

Adds a blank include file to the Include file table, in an editable state. Specify the path to an include file, and press Return. The path is shown in the table.

Browse

Allows you to browse to an include file in the displayed Select include file dialog. The path to the selected file is shown in the table.

Delete

Deletes the selected include file. You can delete multiple items using the Ctrl or Shift keys, or by dragging the cursor.

Moves the selected item up one row in the Include file table. You can select multiple items using the Ctrl or Shift keys, or by dragging the cursor.

Moves the selected item down one row in the Include file table. You can select multiple items using the Ctrl or Shift keys, or by dragging the cursor.

Subcircuit

Allows you to add and delete subcircuit files, and order them in the Subcircuit table. This allows you to simulate part of a hierarchical design as a subcircuit.

Subcircuit table

Displays the subcircuit files that you specify using the Add and Browse buttons. Use the

and

buttons to specify the order in which they are listed.

Add

Adds a blank subcircuit file to the Subcircuit table, in an editable state. Specify the path to a subcircuit file, and press Return. The path is shown in the table.

Browse

Allows you to browse to a subcircuit file in the displayed Select subcircuit dialog. The path to the selected file is shown in the table.

Delete

Deletes the selected subcircuit file. You can delete multiple items using the Ctrl or Shift keys, or by dragging the cursor.

Moves the selected item up one row in the Subcircuit table. You can select multiple items using the Ctrl or Shift keys, or by dragging the cursor.

Moves the selected item down one row in the Subcircuit table. You can select multiple items using the Ctrl or Shift keys, or by dragging the cursor.

Value	Description
OK	Saves the settings in the Application Settings dialog, and closes the dialog.
Cancel	Closes the Application Settings dialog without saving your changes.
Apply	Saves the settings in the Application Settings dialog. The dialog remains open.