Attribute List

Depending on the Mode and filter buttons, the following attributes can be displayed in the Attributes dialog. The Display label and Attribute label values are displayed for each attribute in the Attributes table. The Display label value is shown in the Customize Table Configuration Dialog and Constraint Browser dialogs for the relevant attribute. The Attribute label value provides a more detailed description of the attribute. To display the attributes for a particular mode and attribute type, click the relevant link below.

Mode	Attribute type
Signal	Differential Pair
	E-Net
	Net
	Component
	Pin
	Pin pair
Class/Group	Net class
	E-Net class
	Differential pair class
	Net group
	Differential pair
	E-Net
	Net
Skew Group	Skew Group
	Pin Pair
Component	Component
	Pin
Part	Part
	Part pin

Mode: Signal

Attribute type: Differential Pair

Display label	Attribute label	Description	Associated Attribute Types
Clearance Class	Clearance Class	For the signals that you select in the Signals tree, this attribute allows you to specify a clearance class that you create in the Clearance Class Manager dialog. This dialog allows you to create clearance classes, and specify the design rule stack referred to between nets in each one.	Differential pair class, E-Net class, Net class, Differential pair, E-Net, Net.
Color	Color	For a selected signal, this attribute allows you to specify a color in the displayed Select color dialog. All items with the selected signal are displayed in the color that you specify.	Differential pair class, E-Net class, Net class, Component, Differential pair, E-Net, Net.
Coupled Length	Coupled Length	For the differential pair, the total length of routes is displayed that meet the track spacing requirements for differential pairs. These requirements are set in the Track spacing column in the Rule Editor Dialog: Differential Pairs Tab. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair.
Coupled Ratio (%)	Coupled Ratio (%)	For the total length of routes in a differential pair, the percentage is displayed which meet the track spacing requirements for differential pairs. These requirements are set in the Track spacing column in the Rule Editor Dialog: Differential Pairs Tab. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair.
Max. (Ω)	Differential Impedance Max. (Ω)	Allows you to specify the maximum differential impedance value that is permitted for the differential pair.	Differential pair class, Differential Pair, Pin Pair.
Min. (Ω)	Differential Impedance Min. (Ω)	Allows you to specify the minimum differential impedance value that is permitted for the differential pair.	Differential pair class, Differential Pair, Pin Pair.
Violated Length	Differential Impedance Violated Length	For the differential pair routes, the total length is displayed that violates the differential impedance value in the design. If values are entered for Min (Ω) and Max (Ω), then the Violated Length value for the relevant design is displayed when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair, E-Net, Net, Pin Pair.
Match Ratio (%)	Differential Impedance Match Ratio	For a differential pair, the percentage of the routes is displayed that does not violate the differential impedance value in the design. When you click Update values in Constraint Browser, differential impedance is calculated using the layer stack and material values in the design. The match ratio is not displayed if the minimum and maximum values of the differential impedance are not set. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair.
Differential Pair Class	Differential Pair Class	Using the Differential pair class dialog, specify a differential pair class that you create in the Differential Pair Class Manager dialog.	Differential Pair.
Differential Pair Rule Stack	Differential Pair Rule Stack	For a differential pair, this attribute allows you to specify a differential pair rule stack from the Rule library. These are created in the Rule Editor Dialog: Differential Pairs Tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	Differential pair class, Differential Pair, Pin Pair.
Total Length	Differential Pair Total Length Actual	Allows you to display the total length of all routes in the differential pair when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair.
Hole/Area Design Rule Stack	Hole/Area Design Rule Stack	Allows you to specify a Hole/Area Design Rule Stack from the Rule library, for the signals that you select in the Signals tree. This defines the minimum clearances between holes and layout areas, and conductor types. These are created in the Rule Editor dialog, Conductor Clearance tab, Hole/Area sub tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Actual	Length Difference between Positive/Negative Actual	Allows you to display the maximum difference in length between the positive and negative tracks of a differential pair. Click Update values in Constraint Browser to display this value. If it is greater than the value specified in the Max. field (Length Difference between Positive/Negative Max.), then it is shown in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair class, Differential Pair.
Max.	Length Difference between Positive/Negative Max.	Allows you to specify the maximum difference in length that is permitted between the positive and negative tracks of a differential pair. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential Pair.
Match Ratio for Differential Rule (%)	Match Ratio for Differential Rule (%)	For all routes in a selected differential pair, the percentage of their total length is displayed that does not violate the specified differential pair rule stack. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair.
Non-coupled Length	Non-coupled Length	For a differential pair, the total length of routes is displayed that do not meet the track spacing requirements for differential pairs. These requirements are set in the Track spacing column in the Rule Editor Dialog: Differential Pairs Tab. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair.
Max.	Pin Pair Delay Max.	This attribute allows you to specify the maximum propagation delay between the pins of the differential pair.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Min.	Pin Pair Delay Min.	This attribute allows you to specify the minimum propagation delay between the pins of the differential pair.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Max.	Pin Pair Length Max.	Allows you to specify the required maximum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Min.	Pin Pair Length Min.	Allows you to specify the required minimum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, E-Net, Net, Pin Pair, Skew Group.
Same Net Design Rule Stack	Same net Design Rule Stack	Allows you to specify a Same Net Design Rule Stack from the Rule library. This defines the clearance that is applied, by default, between conductors with the same net. These are created in the Rule Editor dialog, Conductor Clearance tab, Conductor sub tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Signal	Signal	Allows you to display the signal that is associated with the item that you select.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net. Pin Pair.
Topology Template	Topology Template	Allows you to assign a compatible topology template to the E-Net or differential pair that you select in the Signals tree. This can be done using the Assign Topology Template dialog, or by specifying its name in the Topology Template cell. This attribute is only available in a High Speed environment. Click in this cell to display the Assign Topology Template dialog. You can also copy and paste an existing value in this cell. If you attempt to specify an incompatible value, then a warning message is shown, and the value is not updated. An incompatible value may have a topology structure which does not match the selected E-Net or differential pair. For example, it may comprise a different number of ICs or passive components. When you enter a compatible topology template, it is automatically checked. If the topological structure of the relevant signal does not follow the assigned topology template, then the value in this cell is shown in red. The topology template is also checked whenever the following actions are performed. Constraint Browser is launched. The routing pattern is updated while Constraint Browser is displayed. The Update values command is executed in Constraint Browser. The Undo, Redo or Delete command is executed when the Topology Template field is displayed. When the topological structure of the signal matches the assigned topology template, the value in this cell is immediately shown in black.	Differential Pair, E-Net.
Violated Length for Differential Rule	Violated Length for Differential Rule	For a selected differential pair, this attribute allows you to display the total length of routes that violate the specified differential pair rule stack. This is displayed when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair.
Violated Length	Width Violation Length Actual	Allows you to display the length of track whose width is outside the values defined in the specified track width stack. This is selected in the Track Width Stack cell. Click Update values in Constraint Browser to display the Violated Length value. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair, E-Net, Net. Pin Pair.

Attribute type: E-Net

Display label	Attribute label	Description	Associated Attribute Types
Max. (Ω)	Characteristic Impedance Max. (Ω)	Allows you to specify the maximum characteristic impedance for the E-Net or net that you select in the Signals tree in Constraint Browser.	E-Net class, Net class, E-Net, Pin Pair.
Min. (Ω)	Characteristic Impedance Min. (Ω)	Allows you to specify the minimum characteristic impedance for the E-Net or net that you select in the Signals tree in Constraint Browser.	Net.
Clearance Class	Clearance Class	For the signals that you select in the Signals tree in Constraint Browser, this attribute allows you to specify a clearance class that you created in the Clearance Class Manager dialog.	E-Net class, Net class, Differential Pair, E-Net, Net.
Color	Color	For a selected signal, this attribute allows you to specify a color in the displayed Select color dialog. All items with the selected signal are displayed in the color that you specify.	E-Net class, Net class, Component, Differential Pair, E-Net, Net.
E-Net Class	E-Net Class	Allows you to specify an E-Net class that you created in the E-Net Class Manager dialog. Specify a value in the E-Net class dialog.	E-Net.
Edge Style	Edge Style	For a selected E-Net or E-Net class, this setting allows you to specify the angle of the segment end of the lengthen pattern. The value that you specify is used in preference to the value specified in the Design Settings dialog, Lengthen section. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net.
Hole/Area Design Rule Stack	Hole/Area Design Rule Stack	For the signals that you select in the Signals tree, specify a Hole/Area Design Rule Stack from the Rule library. This defines the minimum clearances between holes and layout areas, and conductor types. These are created in the Rule Editor dialog, Conductor Clearance tab, Hole/Area sub tab.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Actual	Length Difference in Pin Pair Actual	Displays the maximum difference between the lengths in a Skew Group that is calculated when you click Update Values in Constraint Browser. If this value is greater than the Max. value that you specify, then it is shown in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net, Skew Group.
Max.	Length Difference in Pin Pair Max.	Allows you to specify the maximum difference between the lengths of pin pairs in a selected Skew Group.	E-Net class, Net class, E-Net, Net, Skew Group.
Max. Size	Max. Size	For a selected E-Net or E-Net class, this attribute allows you to set the maximum length applied between parallel routes when lengthening a routing pattern. The value that you specify is used in preference to the value specified in the Design Settings dialog, Lengthen section. This is illustrated below for the Accordion meander mode. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net.
Max. Via Count	Max. Via Count	Allows you to specify a maximum number of vias for a selected signal. If the calculated number of vias for the signal exceeds this value, then it is displayed in red in the Via Count cell.	E-Net class, Net class, E-Net, Net.
Meander Mode	Meander Mode	For a selected E-Net or E-Net class, this attribute allows you to specify the meander mode that is used to lengthen the E-Net. The value that you specify is used in preference to the value specified in the Design Settings dialog, Lengthen section. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net.
Min. Space	Min. Space	For a selected E-Net or E-Net class, this attribute allows you to set the minimum space applied between parallel routes when lengthening a routing pattern. The value that you specify is used in preference to the value specified in the Design Settings dialog, Lengthen section. This is illustrated below for the Accordion meander mode. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net.
Max.	Pin Pair Delay Max.	For the E-Net that you select in the Signals tree, this attribute allows you to specify the maximum delay that is permitted between the pin pairs.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Min.	Pin Pair Delay Min.	For the E-Net that you select in the Signals tree, this attribute allows you to specify the minimum delay that is permitted between the pin pairs.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Max.	Pin Pair Length Max.	For the E-Net, net or pin pair that you select in the Signals tree, this attribute allows you to specify the required maximum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Min.	Pin Pair Length Min.	For the E-Net, net or pin pair that you select in the Signals tree, specify the required minimum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Same Net Design Rule Stack	Same Net Design Rule Stack	For the signals that you select in the Signals tree, this attribute allows you to specify a Same Net Design Rule Stack from the Rule library. This defines the clearance that is applied, by default, between conductors with the same net. These are created in the Rule Editor dialog, Conductor Clearance tab, Conductor sub tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Net name	Shield Net name	Using the Net selector dialog, this attribute allows you to specify the signal name of the shield pattern. You can narrow down the signals displayed in the dialog by selecting or clearing the Ground, Power and Signals check boxes, and by filtering the displayed values using the Net name box. Note Shielding attributes are read-only for E-Nets in Constraint Browser for eCADSTAR PCB Editor.	E-Net class, Net class, Net group, E-Net, Net.
Track Width Stack	Shield Track Width Stack	This attribute allows you to specify a Track Width Stack from the Rule library. These are created in the Rule Editor Dialog: Tracks Tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	E-Net class, Net class, E-Net, Net.
Gap	Shield Gap	Allows you to specify the clearance between the shield pattern and the track.	E-Net class, Net class, Net group, E-Net, Net.
Mode	Shield Mode	This attribute allows you to select from the following shield pattern modes: OFF: shielding is not added around the relevant track. If shielding is set for an E-Net, this setting allows you to turn it off for a constituent net. Same Layer: shielding is added on the same layer around the track. Same/Adjacent Layers: shielding is added on the same layer and on adjacent layers around the track. Adjacent Layers: shielding is only added on adjacent layers around the track.	E-Net class, Net class, Net group, E-Net, Net.
Signal	Signal	Allows you to display the signal that is associated with the items selected in the Signals tree in the Constraint Browser: Signals section, Signals Tab.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair.
Topology Template	Topology Template	Allows you to assign a compatible topology template to the E-Net or differential pair that you select in the Signals tree. This can be done using the Assign Topology Template dialog, or by specifying its name in the Topology Template cell. This attribute is only available in a High Speed environment. Click in this cell to display the Assign Topology Template dialog. You can also copy and paste an existing value in this cell. If you attempt to specify an incompatible value, then a warning message is shown, and the value is not updated. An incompatible value may have a topology structure which does not match the selected E-Net or differential pair. For example, it may comprise a different number of ICs or passive components. When you enter a compatible topology template, it is automatically checked. If the topological structure of the relevant signal does not follow the assigned topology template, then the value in this cell is shown in red. The topology template is also checked whenever the following actions are performed. Constraint Browser is launched. The routing pattern is updated while Constraint Browser is displayed. The Update values command is executed in Constraint Browser. The Undo, Redo or Delete command is executed when the Topology Template field is displayed. When the topological structure of the signal matches the assigned topology template, the value in this cell is immediately shown in black.	Differential Pair, E-Net.
Total Length	Total Length	The total routing length is displayed for a selected E-Net or net. This is displayed when you click Update Values in the Constraint Browser: Signals section, Signals Tab. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net, Net.
Max.	Total Length Max.	Allows you to specify a maximum value for the total length of all nets in a selected E-Net that is displayed in the Routing tab, Total Length column, in the Constraint Browser: Signals section, Signals Tab. If the value in the Total Length cell is greater than the value specified in the Total Length Max. cell, then it is displayed in red.	E-Net class, Net class, E-Net, Net.
Min.	Total Length Min.	Allows you to specify a minimum value for the total length of all nets in a selected E-Net that is displayed in the Routing tab, Total Length column, in the Constraint Browser: Signals section, Signals Tab. If the value in the Total Length cell is less than the value specified in the Total Length Min. cell, then it is displayed in red.	E-Net class, Net class, E-Net, Net.
Track Width Stack	Track Width Stack	For E-Nets and nets that you select in the Signals tree, in the Constraint Browser: Signals section, Signals Tab, this attribute allows you to specify a Track Width Stack from the Rule library. These are created in the Tracks tab in the Rule Editor dialog. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	E-Net class, Net class, E-Net, Net Pin Pair.
Unrouted Net Count	Unc. Count	Displays the number of unrouted nets for a selected signal. This value is displayed in the Signals tab and Classes/Groups tab in Constraint Browser when you click Update Values. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Net.
Via Count	Via Count	Displays the calculated number of vias for a selected item. If this exceeds the Max. Via Count value, then it is displayed in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net Pin Pair.
Voltage (V)	Voltage (V)	For E-Nets and nets, this attribute allows you to specify the voltage that is used for simulation purposes.	E-Net class, Net class, E-Net, Net.
Violated Length	Width Violation Length Actual	For a selected E-Net or net, this attribute allows you to display the length of track whose width is outside the values defined in the specified track width stack. This is selected in the Track Width Stack cell. Click Update Values to display the Violated Length value. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair, E-Net, Net, Pin Pair.

Attribute type: Net

Display label	Attribute label	Description	Associated Attribute Types
Allow Ring	Allow Ring	Allows you to specify nets which are exempt from the Ring Removal function when manual routing. Set Ring Removal to ON in the Add Route command to activate this function. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Net.
Max. (Ω)	Characteristic Impedance Max. (Ω)	For the E-Net, net or pin pair that you select in the Signals tree in the Signals tab and Classes/Groups tab in Constraint Browser, this attribute allows you to specify the required maximum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	E-Net class, Net class, E-Net, Pin Pair.
Min. (Ω)	Characteristic Impedance Min. (Ω)	For the E-Net, net or pin pair that you select in the Signals tree in the Signals tab and Classes/Groups tab in Constraint Browser, this attribute allows you to specify the required minimum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	E-Net class, Net class, E-Net, Pin Pair.
Clearance Class	Clearance Class	For the signals that you select in the Signals tree, this attribute allows you to specify a clearance class that you created in the Clearance Class Manager dialog. This dialog is displayed by clicking Utility > Clearance Class Manager in the Constraint Browser menu.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Color	Color	For a selected signal, this attribute allows you to specify a color in the displayed Select color dialog. All items with the selected signal are displayed in the color that you specify.	Differential pair class, E-Net class, Net class, Component, Differential Pair, E-Net, Net.
Comment	Comment	Displays the comment that you associate with the selected item.	Component, Pin, Net.
Hole/Area Design Rule Stack	Hole/Area Design Rule Stack	For the signals that you select in the Signals tree, this attribute allows you to specify a Hole/Area Design Rule Stack from the Rule library. This defines the minimum clearances between holes and layout areas, and conductor types. These are created in the Rule Editor dialog, Conductor Clearance tab, Hole/Area sub tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button. Hole/Area Design Rule Stacks are defined in the Rule Editor dialog, Conductor Clearance tab, Hole/Area sub tab.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Actual	Length Difference in Pin Pair Actual	The maximum difference between the lengths of two pins in a pin pair that is calculated when you click Update Values. If this value is greater than the Max. value that you specify, then it is shown in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net, Skew Group.
Max.	Length Difference in Pin Pair Max.	Allows you to specify the maximum difference between the lengths of two pins in a pin pair. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net, Skew Group.
Max. Via Count	Max. Via Count	Allows you to specify a maximum number of vias for a selected item. This attribute is only available in a High Speed environment. You can specify a value for the following items: E-Nets E-Net classes Nets Net classes	E-Net class, Net class, E-Net, Net.
Net Class	Net Class	Using the Net class dialog, this attribute allows you to specify a net class that you created in the Net Class Manager dialog. This is accessed by clicking Edit > Net Class Manager in the Constraint Browser dialog.	Net.
Net Layer	Net Layer	For a selected net, this attribute allows you to specify the conductor layers on which it can be routed on using the Autorouter. Select the required conductor layers in the displayed Net Layer dialog. Display this dialog by pointing the cursor at this cell and then clicking the button. You can set a value for this column in the Routing tab in either the Signals tab or Classes/Groups tab in Constraint Browser. The value is automatically set in both locations when you enter it. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Net class, Net.
Net Type	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. This attribute is not available in Constraint Browser for eCADSTAR PCB Editor.	Net.
No. of required Testpoints	No. of required Testpoints	Shows the number of testpoints for a selected net, and allows you to specify a value. You can set a value for this column in the Routing tab in either the Signals tab or Classes/Groups tab in Constraint Browser. The value is automatically set in both locations when you enter it. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Net.
Max.	Pin Pair Length Max.	For the E-Net, net or pin pair that you select in the Signals tree, this attribute allows you to specify the required maximum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Min.	Pin Pair Length Min.	For the E-Net, net or pin pair that you select in the Signals tree, specify the required minimum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Same Net Design Rule Stack	Same Net Design Rule Stack	Allows you to specify a Same Net Design Rule Stack from the Rule library. This defines the clearance that is applied, by default, between conductors with the same net. These are created in the Rule Editor dialog, Conductor Clearance tab, Conductor sub tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button. Same Net Design Rule Stacks are defined in the Rule Editor dialog, Conductor Clearance tab, Conductor sub tab.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net.
Net name	Shield Net name	Using the Net selector dialog, this attribute allows you to specify the signal name of the shield pattern. You can narrow down the signals displayed in the dialog by selecting or clearing the GND, Power and Signals check boxes, and by filtering the displayed values using the Net name box.	E-Net class, Net class, Net group, E-Net, Net.
Track Width Stack	Shield Track Width Stack	This attribute allows you to specify a Track Width Stack from the Rule library. These are created in the Rule Editor Dialog: Tracks Tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	E-Net class, Net class, E-Net, Net.
Gap	Shield Gap	Allows you to specify the clearance between the shield pattern and the track.	E-Net class, Net class, Net group, E-Net, Net.
Mode	Shield Mode	This attribute allows you to select from the following shield pattern modes: OFF: shielding is not added around the relevant track. If shielding is set for an E-Net, this setting allows you to turn it off for a constituent net. Same Layer: shielding is added on the same layer around the track. Same/Adjacent Layers: shielding is added on the same layer and on adjacent layers around the track. Adjacent Layers: shielding is only added on adjacent layers around the track.	E-Net class, Net class, Net group, E-Net, Net.
Signal	Signal	Allows you to display the signal that is associated with the item that you select.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair.
Total Length	Total Length	The total routing length is displayed for a selected E-Net or net. This is displayed when you click Update Values in the Constraint Browser: Signals section, Signals Tab. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net, Net.
Max.	Total Length Max.	Allows you to specify a maximum value for the total length of all nets in a selected E-Net that is displayed in the Routing tab, Total Length column, in the Constraint Browser: Signals section, Signals Tab. If the value in the Total Length cell is greater than the value specified in the Total Length Max. cell, then it is displayed in red.	E-Net class, Net class, E-Net, Net.
Min.	Total Length Min.	Allows you to specify a minimum value for the total length of all nets in a selected E-Net that is displayed in the Routing tab, Total Length column, in the Constraint Browser: Signals section, Signals Tab. If the value in the Total Length cell is less than the value specified in the Total Length Min. cell, then it is displayed in red.	E-Net class, Net class, E-Net, Net.
Track width Stack	Track width Stack	For E-Nets and nets that you select in the Signals tree, in the Constraint Browser: Signals section, Signals Tab, this attribute allows you to specify a Track Width Stack from the Rule library. These are created in the Tracks tab in the Rule Editor dialog. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	E-Net class, Net class, E-Net, Net, Pin Pair.
Unrouted Net Count	Unc. Count	Displays the number of unrouted nets for a selected signal. This value is displayed in the Signals tab and Classes/Groups tab in Constraint Browser when you click Update Values. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Net.
Via Count	Via Count	Displays the calculated number of vias for a selected item. If this exceeds the Max. Via Count value, then it is displayed in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net, Pin Pair.
Voltage (V)	Voltage (V)	Specify the voltage that is used for simulation purposes. You can specify a value for E-Nets, E-Net classes, nets and net classes. The value is displayed in Voltage column in the Signals tab and Classes/Groups tab in Constraint Browser.	E-Net class, Net class, E-Net, Net.
Violated Length	Width Violation Length Actual	Allows you to display the length of track whose width is outside the values defined in the specified track width stack. This is selected in the Track Width Stack cell. Click Update values in Constraint Browser to display the Violated Length value. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair, E-Net, Net, Pin Pair.

Attribute type: Component

Display label	Attribute label	Description	Associated Attribute Types
0	0	For a selected component, this attribute allows you to specify a permitted placement angle of 0 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
45	45	For a selected component, this attribute allows you to specify a permitted placement angle of 45 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
90	90	For a selected component, this attribute allows you to specify a permitted placement angle of 90 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
135	135	For a selected component, this attribute allows you to specify a permitted placement angle of 135 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
180	180	For a selected component, this attribute allows you to specify a permitted placement angle of 180 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
225	225	For a selected component, this attribute allows you to specify a permitted placement angle of 225 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
270	270	For a selected component, this attribute allows you to specify a permitted placement angle of 270 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
315	315	For a selected component, this attribute allows you to specify a permitted placement angle of 315 degrees. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
Color	Color	Allows you to specify the display color of the component area that is associated with the component selected in the Components tree. Specify a color in the Select color dialog and click OK. This dialog is displayed by pointing the cursor at the Color cell, and then clicking the displayed button. In 3D View mode, the component is displayed in the color that you specify. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair class, E-Net class, Net class, Component, Differential Pair, E-Net, Net.
Comment	Comment	Displays the comment that you associate with the selected item.	Component, Pin, Net.
Current Rating	Current Rating	The nominal current rating that is specified for a component.	Component.
Device Type	Device Type	Displays whether the part associated with a selected component is either active or passive. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
Dimensions	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.	Component.
Frequency	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.	E-Net class, Net class, E-Net, Net.
Gender	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).	Component.
Manufacturer	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.	Component.
Manufacturer Part Number	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.	Component.
Maximum Height	Maximum Height	For a selected part, this attribute allows you to display the distance between the top of the part and the board. This is specified in the Maximum Height (mm) column, in the Library Editor Panel: Parts tab. The value must be greater than the Standoff Height value. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
Maximum Operating Temperature	Maximum 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.	Component.
Minimum Operating Temperature	Minimum 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.	Component.
Mounting Type	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".	Component.
Number of Rows	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.	Component.
Package Type	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.	Component.
Part	Part	Displays the part name associated with the relevant component.	Component.
Part Number	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.	Component.
Passive Type	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: defines the selected part as 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.	Component.
Permitted Placement Side	Permitted Placement Side	For a selected component, this attribute allows you to specify its permitted placement side. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Component.
Pin Count	Pin Count	The number of pins is displayed for a selected part.	Component.
Placement Group Name	Placement Group Name	Allows you to specify a placement group. See Placing Proximity Components.	Component, Pin.
Standoff Height	Standoff Height	For a selected part, the distance is displayed between the bottom of the part and the board. This is specified in the Standoff Height (mm) column, in the Library Editor Panel: Parts tab. This attribute is not available in Constraint Browser foreCADSTAR Schematic Editor.	Component.
Terminal Pitch	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.	Component.
Tolerance	Tolerance	Displays the tolerance for the Value attribute. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Tolerance column.	Component.
Value	Value	Displays the value associated with the selected item.	Component.
Vendor Name	Vendor Name	Displays the Vendor Name that is associated with the component. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Vendor Name column.	Component.
Vendor Reference	Vendor Reference	Displays the Vendor Reference that is associated with the component. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Vendor Reference column.	Component.
Voltage Rating	Voltage Rating	Displays the voltage rating of the component. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Voltage Rating column.	Component.
Wattage	Wattage	Displays the electrical power of the component, expressed in watts. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Wattage column.	Component.

Attribute type: Pin

Display label

Attribute label

Description

Associated Attribute Types

Model Name

Displays the pin buffer model that is assigned to the relevant pin. This value is added when you create a new PCB design. It is also added to the Analysis tab in the Constraint Browser: Component/Parts Section, Components Tab. To ensure that the displayed information is current, perform a Simulation Library Reload. This is required if you:

add, delete or modify the Device Name value.
modify the pin model that is assigned to a device in Simulation Library Manager. This can be done by re-importing a device with different pin model assignments.

Note
If there are any failed pin assignments, these are listed when you execute the Simulation Library Reload command after selecting a model for the first time.

Pin.

Model Type

Displays the type of pin buffer model that is assigned to the relevant pin. The following types are supported in eCADSTAR.

Model Type	Description
Input	Input model
Output	Output model
Bidirect	Bidirectional model. Examples include DDR3 or DDR4 DQ data pins that can switch from driver to receiver. Bidirectional pins are associated with both input models and output models in the simulation library.
TriState	Tri-state (3-state) model. A tri-state output has three output states: high, low or high-impedance (off) and has models for both conditions. If you connect two or more outputs together, you rarely intend them to drive simultaneously. A tri-state device can be "switched off" to allow other devices to drive safely.
TLConnector	Connector model that is based on transmission lines.
LEConnector	Lumped element connector model.
Terminator	Terminator models may comprise resistors, or a combination of resistors, inductors and capacitors.
Circuit	Circuit model that comprises either a manually-entered passive circuit or an imported SPICE model.
Series	A manually-entered model that more accurately reflects parasitic effects within a passive component. For example, representing a capacitor by a capacitance value alone is too simplistic for high-speed design. This is because the parasitic effects of its packaging and materials become very significant.
InputAMI	Special input model that is suitable for IBIS AMI simulation. Such models can include signal processing hardware that cannot be simulated using standard buffer models.
OutputAMI	Special output model that is suitable for IBIS AMI simulation. Such models can include signal processing hardware that cannot be simulated using standard buffer models.
BidirectAMI	Special bidirectional model that is suitable for IBIS AMI simulation. Such models can include signal processing hardware that cannot be simulated using standard buffer models.
TriStateAMI	Special tri-state model that is suitable for IBIS AMI simulation. Such models can include signal processing hardware that cannot be simulated using standard buffer models.

The Model Type value is added when you create a new PCB design. It is also added to the Analysis tab in the Constraint Browser: Component/Parts Section, Components Tab. To ensure that the displayed information is current, perform a Simulation Library Reload. This is required if you:

add, delete or modify the Device Name value.
modify the pin model that is assigned to a device in Simulation Library Manager. This can be done by re-importing a device with different pin model assignments.

Note
If there are any failed pin assignments, these are listed when you execute the Simulation Library Reload command after selecting a model for the first time.

Pin.

Net

Displays the net that is associated with the selected item.

Pin.

Pin Circuit Label

When implied power is specified for a part in eCADSTAR Library Editor, the embedded signal is displayed that is associated with the relevant pin. This attribute is not available in Constraint Browser for eCADSTAR PCB Editor.

Pin.

Pin Name

Displays the names of the pins that are associated with a signal. These are defined in the Part Editor in eCADSTAR Library Editor.

Pin.

Pin Number

Displays the pin number for a selected pin. This is defined in the Part Editor in eCADSTAR Library Editor.

Pin.

Pin Type

Displays the pin type of the selected item. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor. The following values may be displayed.

INPUT: indicates that the selected item is an input pin.

OUTPUT: indicates that the selected item is an output pin.

BIDIRECT: indicates that the selected item is a bidirectional pin.

POWER: indicates that the selected item is a power pin.

GROUND: indicates that the selected item is a ground pin.

NC: indicates that the selected pin is not connected.

Pin.

Placement Group Name

Allows you to specify a placement group. See Placing Proximity Components.

Component, Pin.

Signal

Displays the signal is that is associated with the selected pin.

Differential pair class, E-Net class, Net-class, Differential Pair, E-Net, Net, Pin Pair.

Attribute type: Pin Pair

Display label	Attribute label	Description	Associated Attribute Types
Match Ratio (%)	Characteristic Impedance Match Ratio	For the total length of the E-Net or net that you select in the Signals tree, the percentage is displayed which is within the minimum and maximum impedance values that you specify. When you click Update values, characteristic impedance is calculated using the layer stack and material values in the design. The match ratio is not displayed if the minimum and maximum values of the characteristic impedance are not set. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Pin Pair.
Max. (Ω)	Characteristic Impedance Max. (Ω)	For the E-Net or net that you select in the Signals tree, specify the maximum characteristic impedance. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net-class, E-Net, Pin Pair.
Min. (Ω)	Characteristic Impedance Min. (Ω)	For the E-Net or net that you select in the Signals tree, specify the minimum characteristic impedance. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net-class, E-Net, Pin Pair.
Max. (Ω)	Differential Impedance Max. (Ω)	Specify the maximum differential impedance value that is permitted for the differential pair.	Differential pair class, Differential Pair, Pin Pair.
Min. (Ω)	Differential Impedance Min. (Ω)	Specify the minimum differential impedance value that is permitted for the differential pair.	Differential pair class, Differential Pair, Pin Pair.
Differential Pair Rule Stack	Differential Pair Rule Stack	For a differential pair, specify a differential pair rule stack from the Rule library. These are created in the Rule Editor Dialog: Differential Pairs Tab. Select a value in the Rule Stack dialog. This dialog displayed by pointing the cursor in this cell, and then clicking the displayed button.	Differential pair class, Differential Pair.
Actual	Length Difference between Positive/Negative Actual	This attribute shows the maximum difference in length between the positive and negative tracks of a differential pair. This is displayed when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair class, Differential Pair.
Actual	Pin Pair Delay Actual	For a pin pair that you select in the Signals tree, the calculated propagation delay is displayed when you click Update values in Constraint Browser. This value is calculated based on the pin pair lengths in the design. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor. See Creating Multiple Pin Pairs.	Pin Pair.
Max.	Pin Pair Delay Max.	For the E-Net that you select in the Signals tree, specify the maximum delay that is permitted between the pin pairs.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Min.	Pin Pair Delay Min.	For the E-Net that you select in the Signals tree, specify the minimum delay that is permitted between the pin pairs.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Actual	Pin Pair Length Actual.	If you select a pin pair in the Signals tree, then its length in the design is displayed when you click Update values in Constraint Browser. If the displayed value is outside of the minimum or maximum values that you specify for the relevant E-Net, net or pin pair, then it is displayed in red. See Creating Multiple Pin Pairs. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor. Note The actual routed length of the pin pair is shown, rather than the manhattan length.	Pin Pair.
Max.	Pin Pair Length Max.	For the E-Net, net or pin pair that you select in the Signals tree, this attribute allows you to specify the required maximum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Pin Pair Length Max. Actual	Pin Pair Length Max. Actual	This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Min.	Pin Pair Length Min.	For the E-Net, net or pin pair that you select in the Signals tree, this attribute allows you to specify the required minimum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, E-Net, Net, Pin Pair, Skew Group.
Pin Pair Length Min. Actual	Pin Pair Length Min. Actual	This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Track Width Stack	Track Width Stack	For E-Nets and nets that you select in the Signals tree, this attribute allows you to specify a Track Width Stack from the Rule library. These are created in the Tracks tab in the Rule Editor dialog. In Constraint Browser for eCADSTAR PCB Editor, select a value in the displayed Track Width Stack dialog. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor. Note If the Minimum copper width is defined by Track width stack check box is selected in the PCB Editor: Application Settings, Area fill section, then the specified Track Width Stack value defines the minimum copper width of the area fills that you create on the canvas in eCADSTAR PCB Editor. This value overrides the setting in the Rule Editor Dialog: Tracks Tab, Default track width stack box. If the Minimum copper width is defined by Track width stack check box is not selected in the PCB Editor: Application Settings, Area fill section, then this value and the Default track width stack value in the Rule Editor Dialog: Tracks Tab are ignored.	E-Net class, Net class, E-Net, Net, Pin Pair.
Via Count	Via Count	Displays the calculated number of vias for a selected item. If this exceeds the Max. Via Count value, then it is displayed in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net, Pin Pair.
Violated Length	Width Violation Length Actual	Allows you to display the length of track whose width is outside the values defined in the specified track width stack. This is selected in the Track Width Stack cell. Click Update values in Constraint Browser to display the Violated Length value. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Differential Pair, E-Net, Net, Pin Pair.

Mode: Class/Group

Attribute type: Net class

See: Net.

Attribute type: E-Net class

See: E-Net.

Attribute type: Differential pair class

See: Differential Pair.

Attribute type: Net group

Display label	Attribute label	Description	Associated Attribute Types
Net name	Shield Net name	Using the Net selector dialog, this attribute allows you to specify the signal name of the shield pattern. You can narrow down the signals displayed in the dialog by selecting or clearing the Ground, Power and Signals check boxes, and by filtering the displayed values using the Net name box.	E-Net class, Net class, Net group, E-Net, Net.
Gap	Shield Gap	Allows you to specify the clearance between the shield pattern and the track.	E-Net class, Net class, Net group, E-Net, Net.
Mode	Shield Mode	This attribute allows you to select from the following shield pattern modes: OFF: shielding is not added around the relevant track. If shielding is set for an E-Net, this setting allows you to turn it off for a constituent net. Same Layer: shielding is added on the same layer around the track. Same/Adjacent Layers: shielding is added on the same layer and on adjacent layers around the track. Adjacent Layers: shielding is only added on adjacent layers around the track.	E-Net class, Net class, Net group, E-Net, Net.

Attribute type: Differential Pair

See: Differential Pair.

Attribute type: E-Net

See: E-Net.

Attribute type: Net

See: Net.

Mode: Skew Group

Attribute type: Skew Group

Display label	Attribute label	Description	Associated Attribute Types
Actual	Delay Difference in Pin Pair Actual	The calculated maximum propagation time between two pins in a pin pair. This value is displayed in Constraint Browser for eCADSTAR PCB Editor when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Skew Group.
Actual	Length Difference in Pin Pair Actual.	Displays the maximum difference between the lengths in a Skew Group that is calculated when you click Update values in Constraint Browser. If this value is greater than the Max. value that you specify, then it is shown in red. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	E-Net class, Net class, E-Net, Net, Skew Group.
Max.	Length Difference in Pin Pair Max.	Allows you to specify the maximum difference between the lengths of pin pairs in a selected Skew Group.	E-Net class, Net class, E-Net, Net, Skew Group.
Max.	Pin Pair Delay Max.	For the E-Net that you select in the Signals tree, this attribute allows you to specify the maximum delay that is permitted between the pin pairs.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Min.	Pin Pair Delay Min.	For the E-Net that you select in the Signals tree, this attribute allows you to specify the minimum delay that is permitted between the pin pairs.	Differential pair class, E-Net class, Differential Pair, E-Net, Pin Pair, Skew Group.
Max.	Pin Pair Length Max.	For the E-Net, net or pin pair that you select in the Signals tree, this attribute allows you to specify the required maximum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, Differential Pair, E-Net, Net, Pin Pair, Skew Group.
Min.	Pin Pair Length Min.	For the E-Net, net or pin pair that you select in the Signals tree, specify the required minimum distance between the pin pairs. Specify a value that is greater than 0, and less than or equal to 20000mm.	Differential pair class, E-Net class, Net class, E-Net, Net, Pin Pair, Skew Group.
Max.	Relative Delay Difference Max.	For a selected Skew Group, specify the maximum propagation time for the Skew Group, relative to the specified base signal.	Skew Group.
Actual	Relative Delay Difference Max. Actual	The calculated maximum propagation time for the Skew Group, relative to the specified base signal. This value is displayed in Constraint Browser for eCADSTAR PCB Editor when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Skew Group.
Min.	Relative Delay Difference Min.	For a selected Skew Group, specify the minimum propagation time for the Skew Group, relative to the specified base signal.	Skew Group.
Actual	Relative Delay Difference Min. Actual	The calculated minimum propagation time for the Skew Group, relative to the specified base signal. This value is displayed in Constraint Browser for eCADSTAR PCB Editor when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Skew Group.
Max.	Relative Length Difference Max.	For a selected Skew Group, specify the maximum difference between the lengths in the Skew Group and the length of the base signal.	Skew Group.
Actual	Relative Length Difference Max. Actual	The calculated maximum difference between the lengths in the Skew Group and the length of the base signal. This value is displayed in Constraint Browser for eCADSTAR PCB Editor when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Skew Group.
Min.	Relative Length Difference Min.	For a selected Skew Group, specify the minimum difference between the lengths in the Skew Group and the length of the base signal.	Skew Group.
Actual	Relative Length Difference Min. Actual	The calculated minimum difference between the lengths in the Skew Group and the length of the base signal. This value is displayed in Constraint Browser for eCADSTAR PCB Editor when you click Update values in Constraint Browser. This attribute is not available in Constraint Browser for eCADSTAR Schematic Editor.	Skew Group.

Attribute type: Pin Pair

See: Pin pair.

Mode: Component

This mode is not available in Constraint Browser for eCADSTAR Schematic Editor.

Attribute type: Component

See: Component.

Attribute type: Pin

See: Pin.

Mode: Part

This mode is not available in Constraint Browser for eCADSTAR Schematic Editor.

Attribute type: Part

The following attributes that are displayed are read-only.

Display label	Attribute label	Description	Associated Attribute Types
0	0	For a selected part, this attribute allows you to specify a permitted placement angle of 0 degrees.	Component.
45	45	For a selected part, this attribute allows you to specify a permitted placement angle of 45 degrees.	Component.
90	90	For a selected part, this attribute allows you to specify a permitted placement angle of 90 degrees.	Component.
135	135	For a selected part, this attribute allows you to specify a permitted placement angle of 135 degrees.	Component.
180	180	For a selected part, this attribute allows you to specify a permitted placement angle of 180 degrees.	Component.
225	225	For a selected part, this attribute allows you to specify a permitted placement angle of 225 degrees.	Component.
270	270	For a selected part, this attribute allows you to specify a permitted placement angle of 270 degrees.	Component.
315	315	For a selected part, this attribute allows you to specify a permitted placement angle of 315 degrees.	Component.
Comment	Comment	Displays the comment that you associate with the selected item.	Component, Pin, Net.
Current Rating	Current Rating	The nominal current rating that is specified for a part.	Component.
Decap	Decoupling Capacitor	If selected, then the relevant part is specified as a decoupling capacitor (decap). The icon for the part in the Parts tree is updated to indicate that it is a decoupling capacitor. You can add decoupling capacitors to the library using theComponent Settings Dialog. In order to use them in a design, you must add them from the library. This is done by clickingImport Design Rule Library (Partial)orImport (Design Rule Library)in theRule Editor Dialog, in. Any two-pin device can be set as a	Component.
Device Type	Device Type	Displays whether the part associated with a selected component is either active or passive.	Component.
Dimensions	Dimensions	Displays the dimensions of the part that are specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Dimensions column.	Component.
Frequency	Frequency	Displays the frequency of the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Frequency column.	E-Net class, Net class, E-Net, Net.
Gender	Gender	Displays the gender of the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Gender column. The gender of a part can be specified as "male" (plug) or "female" (socket).	Component.
Jumper	Jumper	If selected, then the relevant part is specified as a jumper. The icon for the part in the Parts tree is updated to indicate that it is a jumper. You can add a jumper to the library using the Component Settings Dialog. You must then set it as jumper in the Part Editor Panel: Detail Tab, Part Information section. In order to use them in a design, you must add them from the library. This is done by clicking Import Design Rule Library (Partial) or Import (Design Rule Library) in the Rule Editor Dialog, in eCADSTAR PCB Editor.	Component.
Manufacturer	Manufacturer	Displays the Manufacturer for the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Manufacturer column.	Component.
Manufacturer Part Number	Manufacturer Part Number	Displays the Manufacturer Part Number for the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Manufacturer Part Number column.	Component.
Maximum Height	Maximum Height	For a selected part, this attribute allows you to display the distance between the top of the part and the board. This is specified in the Maximum Height (mm) column, in the Library Editor Panel: Parts tab. The value must be greater than the Standoff Height value.	Component.
Maximum Operating Temperature	Maximum Operating Temperature	Displays the maximum operating temperature of the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Maximum Operating Temperature column.	Component.
Minimum Operating Temperature	Minimum Operating Temperature	Displays the minimum operating temperature of the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Minimum Operating Temperature column.	Component.
Mounting Type	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 part might include "through-hole" or "surface mount".	Component.
Number of Rows	Number of Rows	Displays the number of rows of pins on the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Number of Rows column.	Component.
Package Type	Package Type	Displays the type of package for the part 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.	Component.
Part Number	Part Number	Displays the part number of the part that is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Part Number column.	Component.
Passive Type	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: defines the selected part as 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.	Component.
Permitted Placement Side	Permitted Placement Side	For a selected part , this attribute allows you to specify its permitted placement side.	Component.
Pin Count	Pin Count	The number of pins is displayed for a selected part.	Component.
Standoff Height	Standoff Height	For a selected part, the distance is displayed between the bottom of the part and the board. This is specified in the Standoff Height (mm) column, in the Library Editor Panel: Parts tab.	Component.
Terminal Pitch	Terminal Pitch	Displays the distance between the pins on the part that are specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tabTerminal Pitch column.	Component.
Tolerance	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.	Component.
Value	Value	Displays the value associated with the selected item.	Component.
Vendor Name	Vendor Name	Displays the Vendor Name that is associated with the part. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Vendor Name column.	Component.
Vendor Reference	Vendor Reference	Displays the Vendor Reference that is associated with the part. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Vendor Reference column.	Component.
Voltage Rating	Voltage Rating	Displays the voltage rating of the part. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Voltage Rating column.	Component.
Wattage	Wattage	Displays the electrical power of the part, expressed in watts. This is specified in the Library Editor Panel: Parts tab, or the Part Editor Panel: Properties tab, Wattage column.	Component.

Attribute type: Part pin

Display label	Attribute label	Description	Attribute type
Pin Name	Pin Name	Displays the names of the pins that are associated with a signal.	Pin.
Pin Type	Pin Type	Displays the pin type of the selected item. The following values may be displayed: INPUT: indicates that the selected item is an input pin. OUTPUT: indicates that the selected item is an output pin. BIDIRECT: indicates that the selected item is a bidirectional pin. POWER: indicates that the selected item is a power pin. GROUND: indicates that the selected item is a ground pin. NC: indicates that the selected pin is not connected.	Pin.

Display label

Attribute label

Description

Attribute type

Pin Name

Displays the names of the pins that are associated with a signal.

Pin.

Pin Type

Displays the pin type of the selected item.
The following values may be displayed:

INPUT: indicates that the selected item is an input pin.

OUTPUT: indicates that the selected item is an output pin.

BIDIRECT: indicates that the selected item is a bidirectional pin.

POWER: indicates that the selected item is a power pin.

GROUND: indicates that the selected item is a ground pin.

NC: indicates that the selected pin is not connected.

Pin.

Related Topics
Constraint Browser
Customize Table Configuration Dialog
Attributes Dialog
Library Editor Panel: Parts Tab
Part Editor Panel: Detail Tab
Part Editor Panel: Gate+Pin Equivalents Tab
Part Editor Panel: Properties Tab
Properties Panel
Reference Dialog
Filtering Displayed Values in eCADSTAR Tables