Properties Panel

The Properties panel displays the properties associated with an object that is selected on the eCADSTAR Schematic Editor or Symbol Editor canvas, and allows you to change the properties where applicable. Toggle on the Properties panel by clicking View > Display > Property. Alternatively, click Property on the status bar.

  • When multiple objects of the same type are selected, the same items are displayed as when a single object is selected.
  • Properties of multiple objects can be changed simultaneously.
  • For the Coordinates, User Attributes and SPICE Attributes properties, click either "+" or "-" to toggle the display of child objects. The specified setting is saved until the application is restarted.

Component properties are displayed in the following order.

  1. System defined properties, not including SPICE related properties.
  2. User defined attributes
  3. SPICE related properties

If you right-click a row which has an attribute defined as a hyperlink in the Attribute Manager dialog, then you can launch the hyperlink by clicking Open Hyperlink on the assist menu. This is also possible in eCADSTAR Schematic Viewer. If multiple cells are selected that have different values or If a hyperlink is not specified, then this command is made unavailable. The hyperlinks are launched in your default browser.

Item   Description
Property   Shows the properties associated with the object that you select on the canvas. User-defined attributes are also listed in eCADSTAR Schematic Editor. User-defined attributes are specified in the Attribute Manager dialog, in eCADSTAR Library Editor. The relevant values are set in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, User Part Attributes section.
Value   Shows the values associated with each property. The type of cell varies depending on the associated property. Set a value as follows for each type of cell. properties cannot be set when a command is running.
  Numerical field A cell containing a real number or integer. Click the cell to set a value.
  Box A cell containing multiple options. Select a value from the box.
  Text pad A cell with a character string. Click the cell to enter a character string to the text pad.
  Enter a value directly, or select a value from the dialog that is displayed by clicking .
Control For certain rows, the control column determines how the Value column behaves when updated. Details are provided on a row-by-row basis below.

 

Note
  • For items that are split over multiple sheets, such as net sub circuits or multiple gated items: when adding a value, it is added only to the selected item, and not to the associated ones. For example, if you apply a design rule stack value to a sub circuit on sheet 001, it is not automatically applied to a sub circuit on sheet 002. It is recommended to add the value in Constraint Browser, which applies it to all relevant sub circuits, and gates. Alternatively, enter these values manually for each sheet and item. However, for a multi-gated part, the Fitted attribute applies to all gate components.
  • If you change the Reference Designator value for a gate component, then the value is updated for all parts in the design with that Reference Designator value.

 

The properties displayed in the Properties panel vary depending on the object that you select on the canvas. A selection of important properties are shown below.

When a component is selected

When a net or bus is selected

When a pin is selected

When a property viewer is selected

When text is selected

When a figure is selected

When a circle is selected

When a simulation frame is selected

When a text frame is selected

When a component is selected

Item     Description
Property     The properties are listed that are associated with the component selected on the canvas. If you specify SPICE attributes in the Library Editor Panel: Parts Tab or the Part Editor Panel: SPICE Tab for a part, then the specified values are shown in the relevant SPICE columns when the part is added to the canvas. For further information on SPICE attributes, see: Understanding SPICE Controller.
Note
The SPICE attributes that you specify in this panel are not added to the library. When simulating with parts, it is recommended to add them to the library instead. However, this is not necessary when simulating only with symbols.
  Reference Designator   Specify the reference of the component. If you specify a Reference Designator value that already exists on any sheet in the design, then a warning dialog is displayed which shows the duplicate value. However, it is not displayed if the value exists within a block in the design.
  • Click Yes in the dialog to keep the duplicate value.
  • Click No in the dialog to discard the duplicate value.

If you update this value for a gate component, then the value is updated for all parts in the design with that Reference Designator value. Gate components are components that have the same Reference Designator value.

Note
The warning dialog is not displayed if a duplicate Reference Designator value is assigned to empty gates or empty power boxes.
  Gate Number   For Gated Components, the Gate Number will be shown. This corresponds to the Gate selected on the sheet. For components that do not consist of any gates, No value will be shown in this row.
  Coordinates   Allows you to set the X and Y coordinates of a component selected on the canvas in eCADSTAR Schematic Editor, including a part, connector or block. In Symbol Editor, these values are also editable. Click either "+" or "-" to toggle the display of the X and Y rows. The specified setting is saved until the eCADSTAR application is restarted.
Either type or paste a numeric value in the relevant box. If a component cannot be moved to the specified coordinates because of a net or component conflict, for example, then the coordinate values are not changed. If multiple objects of the same type are selected, then their coordinate values cannot be set.
Note
  • The coordinates of objects in multi-instanced blocks are not editable, with the exception of property viewers.
  • The Coordinates column can also be added to Component Browser in eCADSTAR Schematic Editor and eCADSTAR Schematic Viewer. This shows the position of the relevant component on the canvas. In the Component Browser, Coordinates column, use the Filter row to list only components located in a particular part of the canvas. Components are displayed whose X or Y coordinate value matches the value specified in the Filter row.
    X Specify the coordinate of the component in the X direction.
    Y Specify the coordinate of the component in the Y direction.
  Angle   Allows you to specify the angle at which the component is displayed on the eCADSTAR Schematic Editor canvas.
  Mirror   Specify whether a selected component, connector or block is flipped in the vertical plane.
  • ON: the selected component or connector is flipped in the vertical plane.
  • OFF: selected component or connector is not flipped in the vertical plane.
  Scale   Allows you to specify the scale of the component.
  Part name   Displays the part name for a selected component.
  • For sheet/global/power/ground connectors, you can edit the Net Name (Part Name) value. See: Net label or Bus label.
  • For hierarchy connectors, you can edit the Pin Label (Part Name) value.
  Symbol name   Allows you to change the symbol name for a selected component, connector or block. Select a value using the Change Symbol dialog. This is displayed when you point the cursor in this box, and then click the displayed button.
  Symbol Alternate   For a selected component or connector, you can select an alternate symbol name if available. Select a value using the Change Symbol dialog. This is displayed when you point the cursor in this box, and then click the displayed button.
  Number of Pins   Displays the number of pins on the component.
  Component Type   Displays the component type.
  Bit Count   The total number of bits associated with the component.
  Color <DEF>   Allows you to specify the color of the component on the schematic sheet. Click to display the Select color dialog.
  Instance Net Label   Displays the instance net label associated with the component.
  Comment   Displays comments that are associated with the component.
  Block Name   Displays the name of the block
  Hierarchy Type   Shows whether the block symbol is a definition block, which can be reused in the design. This is specified in theBlock Symbol dialog.
    Multi-Instanced The new block symbol is a definition block. It can be reused in the design by selected it in the Add Block, or Change Block command. When it is updated, all instance blocks that are added to the design based on this block are also updated. To do this, select Check Hierarchy Update and then select Update All Instances or Update Instance.
     Single-Instanced The new block symbol is used only on the displayed canvas. It cannot be reused in the design by selecting it in the Add Block or Change Block command.
  Value   Displays the value that is specified for the component in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Value column.
  Description   Displays the description of the component that is specified in the Library Editor Panel: Parts tab, Description column. This might include the type of component, and its specification. For a selected block, you can edit this value.
  Component Group   Define the name of a component group in this cell to associate the component with it. When you forward annotate into eCADSTAR PCB Editor, the specified component group appears in the Component Group Settings dialog. Component groups allow you to move multiple components as a single group on the eCADSTAR PCB Editor canvas.
  Placement Group   Define the name of a placement group in this cell to associate the component with it. The specified placement group is added to eCADSTAR PCB Editor when you forward annotate. Placement groups are used by the Gather Components command.
  Fitted   Specify whether a component is mounted on the board by selecting YES or No. Selecting YES specifies that it is mounted on the board. For a multi-gated part, the status of all gate components is updated.
  Reference Designator Prefix   Displays the prefix for the reference designator of components. This is specified in the Library Editor Panel: Parts tab, Reference Designator Prefix column.
  Start Value for Reference Designator   For a selected block, this field allows you to specify the start value of the reference designators of its associated components. This value is applied instead of the value in the Sheet Settings dialog, Properties tab, Start Value for Reference Designator field.
  Part Number   Displays the part number of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Part Number column.
  Manufacturer   Displays the Manufacturer for the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Manufacturer column.
  Manufacturer Part Number   Displays the Manufacturer Part Number for the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Manufacturer Part Number column.
  Vendor Name   Displays the Vendor Name that is associated with the component in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Vendor Name column.
  Vendor Reference   Displays the Vendor Reference that is associated with the component in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Vendor Reference column.
  Tolerance   Displays the tolerance for the setting in the Value cell. The Tolerance setting is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Tolerance column.
  Wattage   Displays the electrical power of the component, expressed in watts, that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Wattage column.
  Frequency   Displays the frequency of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Frequency column.
  Voltage Rating   Displays the voltage rating of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Voltage Rating column.
  Current Rating   Displays the current rating of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Current Rating column.
  Max. Operating Temperature   Displays the maximum operating temperature of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Maximum Operating Temperature column.
  Min. Operating Temperature   Displays the minimum operating temperature of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Minimum Operating Temperature column.
  Dimensions   Displays the dimensions of the component that are specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Dimensions column.
  Package Type   Displays the type of package for the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Package Type column. A package type has a defined set of physical dimensions that the component has to conform to. Typically, the pitch spacing, height and general shape of the component is defined. for each package.
  Terminal Pitch   Displays the distance between the pins on the component that are specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Terminal Pitch column.
  Mounting Type   Displays the mounting type that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Mounting Type column. Mounting types for a component might include "through-hole" or "surface mount".
  Gender   Displays the gender of the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Gender column. The gender of a component can be specified as "male" (plug) or "female" (socket).
  Number of Rows   Displays the number of rows of pins on the component that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Number of Rows column.
  Part Class   Displays the class that is specified for the part in the Library Editor Panel: Parts tab, Part Class column. The following values can be specified.
  • Antenna
  • Capacitor
  • Connector
  • Crystal
  • Diode
  • Filter
  • Fixing
  • Inductor
  • Integrated Circuit
  • Jumper
  • Power Convertor
  • Regulator
  • Resistor
  • StarPoint
  • Switch
  • TestPad
  Part Acceptance Status   Displays the approval status of the component. This is specified in the Library Editor Panel: Parts tab, Part Acceptance Status column. The following values can be specified.
  • Approved
  • Unapproved
  Part Acceptance Reason   Displays the reason for non-approval of the part that is entered in the Library Editor Panel: Parts tab, Part Acceptance Reason column.
  Device Type  

You can change the Device Type of the selected component.

  • Active: active component
  • Passive: passive component
  Passive Type   Displays the type of passive component. These are specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Passive Type column. The following values may be displayed.
  • Capacitor: defines the selected part as a capacitor.
  • Resistor: defines the selected part as a resistor.
  • Inductor: defines the selected part as a inductor.
  • Diode: defines the selected part as a diode.
  • Other Passive: a passive type that has at least two nodes, and may contain a more or less complex inner circuitry.
  • None: if selected, then passive series pins in the component are not considered.
  • Undefined: if selected, then the part is not defined as a passive component.
  Passive Connectivity   If this value is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, then a list of connected passive pin pairs are displayed that are separated by the "space" character.
  Allow Testpoints   Displays whether testpoints can be generated for the part. This value is specified in the Allow Testpoints field in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab.
  Solder Method   Displays whether the solder method for the part is restricted to "Reflow" or "Single Reflow", or whether it is set to "Any", to allow any method of soldering. This value is specified in the Solder Method field in the Library Editor Panel, Parts tab, or the Part Editor Panel, Properties tab.
  Use in Schematic   Displays whether the part can be back annotated into eCADSTAR Schematic Editor. This value is specified in the Use in Schematic field, in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab.
  Use in Layout   Displays whether the part can be forward annotated into eCADSTAR PCB Editor. This value is specified in the Use in Layout field, in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab.
  Use in Parts List   Displays whether the part appears in the part lists that you generate in eCADSTAR. This value is specified in the Use in Parts List, in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab.
  XY location label   Allows you to manually create an XY location label for a sheet connector or global connector. This shows the connected sheets for the connector. You can also do this automatically using the Cross Reference command. The XY location label field is not editable for power and ground connectors.
Specify the path by entering an alphanumeric value, such as '100'. If the connector is in a hierarchical block, the location label would appear as follows.
BLK1/001
BLK1/BLK3/001
  User Attributes   Click the associated "+" or "-" icon to toggle the display of user-defined attributes. The specified setting is saved until eCADSTAR Schematic Editor is restarted. These attributes are specified in the Attribute Manager dialog, in eCADSTAR Library Editor. The relevant values are set in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, User Part Attributes section.
Note
For multi-gated components that have the same part and reference designator, you can set the value of an attribute in all associated components. They must be in the same circuit in the current variant, and can be within an instance block (a definition block is treated as a circuit).
You can do this in Component Browser or the Properties panel in eCADSTAR Schematic Editor.
The following attributes can be set.
  • User defined attributes.
  • The System attributes Component Group and Placement Group.

SPICE attributes cannot be set.

  • If an attribute value is set for multiple components that each have different part names or reference designators, but all contain multi-gated parts, then all sets of components are updated.
  • If all relevant sheets are in the same circuit but a component is not in the active sheet, then the attributes are not updated if a sheet is locked by another user. An error message is also displayed. This occurs even if the locked sheet does not contain an affected component.
  SPICE Attributes   Click the associated "+" or "-" icon to toggle the display of SPICE Attributes. The specified setting is saved until eCADSTAR Schematic Editor is restarted.
    SPICE Element Name In the SPICE circuit, the prefix of this value represents a specific SPICE element. For example, "IC1" (prefix "I") represents a current source in SPICE.  To represent a subcircuit, change it to "XIC1" (prefix "X"). You can also specify a prefix using the SPICE Element Header attribute. For more information, see Understanding SPICE Controller, Simulation Properties for Components and Pins.
    SPICE Simulation Value Allows you to specify the electrical characteristics of a passive device. For resistors, capacitors and coils, set values for resistance, capacitance and inductance, respectively. The value that you specify overrides the "Value" property for the device.
    SPICE Model Name This is a dedicated LTspice property which defines the electrical characteristics of active elements. It provides the device model name that is used for analyzing active elements such as transistors or various types of IC. To be used in the analog unit, you must add the device model as an include file in the Schematic Editor: Application Settings dialog.
    SPICE Element Header Adds a prefix to the Reference Designator property. In the SPICE circuit, the prefix represents a specific SPICE element. For example, "IC1" (prefix "I") represents a current source in SPICE. See Understanding SPICE Controller, Simulation Properties for Components and Pins.
    SPICE Substrate Connection Node For BJT, JFET, or MOSFET devices, this specifies the net to connect to a substrate pin. Set the net name to specify a substrate (bulk) connection target. You cannot set it for a device model in subcircuit (.SUBCKT) format, even if the device type is BJT, JFET, or MOSFET.
    SPICE Parameter 1 - 10 Allow you to specify additional parameters, such as a temperature dependence for a resistor. These parameters are dependent on the device type. For example, the temperature coefficient for passive devices (up to the second order) is enabled. For active devices, physical information for semiconductors is enabled. The items that are enabled depend on the SPICE type or version. Many of these parameters can be omitted.  For more information, see Understanding SPICE Controller, Simulation Properties for Components and Pins.
Value     For the component selected on the canvas, the values are listed that are associated with each property.

 When a net or bus is selected in eCADSTAR Schematic Editor

Item   Description
Property   The properties are listed that are associated with the net or bus selected on the canvas.
Net label or Bus label Displays the label that is associated with the net or bus.
For the Add Net, Net/Bus and Increment Net commands, and in the Net label, Bus label or Part name fields in the Properties Panel, if you attempt to change a label to one that already exists, then a confirmation dialog is immediately displayed. This asks whether to merge the nets.
  • Click Yes in the dialog to merge the nets.
  • Click No in the dialog to cancel the operation.

The dialog is shown if duplicate net labels exist for the following objects.

  • Net Bus Component: Sheet connector
  • Component: Global connector
  • Component: Power (Global connector)
  • Component: Ground (Global connector)

Duplicate net labels may be detected on all sheets in the circuit, including instance hierarchy. However, consider the following for global connectors.

  • The confirmation dialog is shown if the label of a global connector matches the label of a top sheet net.
  • The confirmation dialog is not shown if a net in the hierarchy that is not connected to a global connector matches the label of a net on the top sheet.
Note
If the bus name “X[1-4]” exists, and Use array syntax is selected in the Assignments dialog, then:
  • The confirmation dialog is shown for “X[1]”.
  • The confirmation dialog is not shown for “X1”.
If Use array syntax is not selected in the Assignments dialog, then:
  • The confirmation dialog is shown for both “X[1]” and “X1”.

For a connected net, if you specify a label when one is not already assigned, then the net names that are listed in the Net/Bus command, Suggested labels box, are excluded from this check. They are also excluded if the specified label is contained within the existing name. For example, if you specify a label for the highlighted bus below, then:

  • A warning is not shown for “A[1]”, ”A[2]”, ”A[1-3]” or “A[3-2]”.
  • A warning is shown for “A[4]”, ”A[1-4]” and ”A[4-2]”.

For an unconnected net, specified net names are not excluded from this check.

Note
The Control column determines how the Net Label behaves when updated:
  • When the check box is OFF, it changes the name on the selected items only.
  • When the check box is ON, it changes the name across the Whole circuit.
Instance Net Label Displays the instance net label associated with the net or bus.
Line Width Allows you to select the line width of the net or bus. To edit the line width values, right-click in this box and select Edit Line Width on the assist menu. The Line Width Tab dialog, Line Width tab is displayed
Color Click in the Value cell to display the Select color dialog.
  Net Type Allows you to set the net or bus to one of the following options:
  • SIGNAL: specifies that the net is not a power or ground net.
  • POWER: specifies that the net is a power net.
  • GROUND: specifies that the net is a ground net.
Note
When forward annotating or migrating a schematic design, an error message is displayed if this value does not match the type of symbol it is connected to. For example, if a ground net is connected to power symbol in the design.
 

Comment

In the Comment dialog, you can associate a comment with the net or bus. You can specify a value over multiple lines. This dialog is launched when you point the cursor in this box, and then click the displayed button.
  Clearance Class Allows you to assign a clearance class to the selected signal. Point the cursor in the Clearance Class row to display the button. Click this to launch the Clearance Class Dialog. Select a clearance class from the dialog to assign it to the signal.
  SPICE OP Voltage The Operating Point voltage for the selected net on the schematic sheet. This is simulated by the LTspice application. Operating Point voltage is used for analog simulation control units. Use it to set a voltage value to create adjusted results from calculations.
Value   For the net or bus selected on the canvas, the values are listed that are associated with each property.

When a pin is selected

Item   Description
Property   The properties are listed that are associated with the pin selected on the canvas.
ID The symbol pin number. You can map this value to a footprint reference pin number in the Part Editor Panel.
Pin Number The footprint reference pin number. You can map this value to a symbol pin number in the Part Editor Panel.
Pin Label The notation that is displayed for the mapping of the selected pin.
  • If a gate is selected from a part with only a single gate defined in the library, then the Label information is displayed from the library pin details.
  • If the gate is selected from a part with multiple gates defined in the library, then the Gate Label information is displayed.
Pin Type Displays the pin type of the selected item. The following values may be displayed.

INPUT: the selected item is an input pin.

OUTPUT: the selected item is an output pin.

BIDIRECT: the selected item is a bidirectional pin.

POWER: the selected item is a power pin.

GROUND: the selected item is a ground pin.

NC: the selected pin is not connected.

UNDEFINED: the selected pin is not defined.
  Coordinates The X and Y coordinates of a pin that is selected on the canvas in Symbol Editor. These values are read-only. Click either "+" or "-" to toggle the display of the X and Y rows. The specified setting is saved until the application is restarted.
  Bit Count Shows the number of bits associated with the pin. A bit count of more than one enables a single pin object to represent multiple pins.
  Implied Power Signal In eCADSTAR Library Editor, this value is set in the Signal column for the pin. If the associated part is not instantiated into eCADSTAR Schematic Editor, then the value is allocated to the pin. If the part is instantiated into eCADSTAR Schematic Editor, then any signal that is connected to the pin will override this value.
  Pin Circuit Label If implied power is specified for a part in eCADSTAR Library Editor, then the embedded signal is displayed that is associated with the relevant pin. This attribute is not available in eCADSTAR PCB Editor.
  Placement Group Define the name of a placement group to associate the pin with it. The specified placement group is added to eCADSTAR PCB Editor when you forward annotate. Placement groups are used by the Gather Components command.
  Spice Pin Number Allows you to specify the pin sequence order that is defined in the SPICE model. This can be specified in both the part library and the schematic.
Value   For the pin selected on the canvas, the values are listed that are associated with each property.

When a property viewer is selected

Item   Description
Property   The properties are listed that are associated with the property viewer that you select on the canvas.
Coordinates Displays the X and Y coordinates of the property viewer that is selected on the canvas in eCADSTAR Schematic Editor or Symbol Editor. These values are editable. Click either "+" or "-" to toggle the display of the X and Y rows. The specified setting is saved until the eCADSTAR application is restarted.
Property Name Displays the property definition.
Value If appropriate, you can specify the text that is displayed in the property viewer.
Angle Allows you to specify the angle at which the text is displayed.
Origin Allows you to specify the origin of the property viewer by selecting an item in the Origin box. The position of the property viewer is defined in relation to its origin.
Font

Allows you to specify the font of the property viewer. Select a font from the displayed values. To edit a displayed font, right-click in this box and select Edit Font on the assist menu. The Assignments dialog, Font tab is displayed.
  Color <DEF> Allows you to specify the color of the property viewer. Click in the Value cell to display the Select color dialog.
Value   For the property viewer that is selected on the canvas, the values are listed that are associated with each property.

When text is selected

Item   Description
Property   The properties are listed that are associated with the text selected on the canvas.
Coordinates Displays the X and Y coordinates of the specified text. These values are editable. Click either "+" or "-" to toggle the display of the X and Y rows. The specified setting is saved until the application is restarted.
String In the String dialog, you can specify the text string that is displayed, over multiple lines. This dialog is launched when you point the cursor in this box, and then click the displayed button.
Angle Sets the angle at which the text is displayed.
Origin Allows you to specify the origin of the text by selecting an item in the Origin box. The position of the property viewer is defined in relation to its origin
Font Select a font from the displayed values. To edit a displayed font, right-click in this box and select Edit Font on the assist menu. The Assignments dialog, Font tab is displayed.
  Color Click in the Value cell to display the Select color dialog.
Value   For the text selected on the canvas, the values are listed that are associated with each property.

If you select variant text on the canvas, then Variant Text is shown in the Text row. You can edit the text value by pointing the cursor in the Value column, then clicking the button. Edit the value in the displayed Variant Text dialog.

When a figure is selected

Item   Description
Property   The properties are listed that are associated with the figure selected on the canvas.
Line Width Allows you to select the line width of the figure. To edit the line width values, right-click in this box and select Edit Line Width on the assist menu. The Line Width Tab dialog, Line Width tab is displayed.
Line Type Allows you to select the line type of the figure. To edit the line type values, right-click in this box and select Edit Line Type on the assist menu. The Line Type Tab dialog, Line Type tab is displayed.
  Color Click in the Value cell to display the Select color dialog.
Value   For the figure selected on the canvas, the values are listed that are associated with each property.

When a circle is selected

Item   Description
Property   The properties are listed that are associated with the circle selected on the canvas.
Line Width Allows you to select the line width of the figure. To edit the line width values, right-click in this box and select Edit Line Width on the assist menu. The Line Width Tab dialog, Line Width tab is displayed.
Line Type Allows you to select the line type of the figure. To edit the line type values, right-click in this box and select Edit Line Type on the assist menu. The Line Type Tab dialog, Line Type tab is displayed.
Radius Displays the radius of the circle.
  Color Click in the Value cell to display the Select color dialog.
Value   For the circle selected on the canvas, the values are listed that are associated with each property.

 

When a simulation frame is selected

Item   Description
Property   The properties are listed that are associated with the simulation frame selected on the eCADSTAR Schematic Editor canvas.
Coordinates Displays the X and Y coordinates of the selected simulation frame. These values are editable. Click either "+" or "-" to toggle the display of the X and Y rows. The specified setting is saved until the application is restarted.
Angle Specify the angle at which the selected simulation frame is displayed.
  Frame Type Displays the frame type as simulation.
  Line Width Allows you to select the line width of the figure. To edit the line width values, right-click in this box and select Edit Line Width on the assist menu. The Line Width Tab dialog, Line Width tab is displayed.
  Line Type Allows you to select the line type of the figure. To edit the line type values, right-click in this box and select Edit Line Type on the assist menu. The Line Type Tab dialog, Line Type tab is displayed.
  Color Specify the color of the selected simulation frame. Click in the Value cell to display the Select color dialog.
  Simulation Frame Name Enter an alphanumeric value for the name of the simulation frame.
Value   For the simulation frame that is selected on the canvas, the values are listed that are associated with each property.

 

When a text frame is selected

Item   Description
Property   The properties are listed that are associated with the text frame selected on the eCADSTAR Schematic Editor canvas.
Coordinates Displays the X and Y coordinates of the selected text frame. These values are editable. Click either "+" or "-" to toggle the display of the X and Y rows. The specified setting is saved until the application is restarted.
Angle Specify the angle at which the selected text frame is displayed.
  Frame Type Displays the frame type as text.
  Font Select a font from the displayed values. To edit a displayed font, right-click in this box and select Edit Font on the assist menu. The Assignments dialog, Font tab is displayed.
  Text Color Specify the color of the text in the frame. Click in the Value cell to display the Select color dialog.
  Line Width Allows you to select the line width of the text frame. To edit the line width values, right-click in this box and select Edit Line Width on the assist menu. The Line Width Tab dialog, Line Width tab is displayed.
  Line Type Allows you to select the line type of the text frame. To edit the line type values, right-click in this box and select Edit Line Type on the assist menu. The Line Type Tab dialog, Line Type tab is displayed.
  Frame Color Specify the color of the selected text frame. Click in the Value cell to display the Select color dialog.
  File Name Displays the path to the text file that you select in the Add Text Frame dialog, Text File Name box.
Value   For the text frame that is selected on the canvas, the values are listed that are associated with each property.

 

Related Topics
Design Tree
Changing a Reference Designator
Changing Multiple Reference Designators
Understanding SPICE Controller