Part Editor Panel: Detail Tab

The Detail tab in the Part Editor panel allows you to configure a selected part. You can specify its type and class, and its associated footprint, symbol and pin assignment. It is displayed by selecting a part in the eCADSTAR Library Editor and clicking Home > Edit > Part on the ribbon. In the Part Editor panel, select the Detail tab.

When opening the Part Editor panel, the pin assignment lock is automatically obtained. This ensures that only one user at a time can edit shared pin assignment information in parts. If you cannot obtain a pin assignment lock, then changes are not allowed that affect the pin assignment of a part, and a warning message is displayed. This shows the relevant user and machine name, but not the part name that holds the lock. The message is also shown if you open two instances of Part Editor that have different parts using the same pin assignment. The lock is removed when the Part Editor is closed.

Note

Pin assignment locks.

The Parts table in the Library Editor Panel: Parts Tab is not considered when obtaining a pin assignment lock. As some parts, such as new parts, do not have pin assignments, it is not always possible to create a pin assignment lock.
If a pin assignment lock is not obtained when the Part Editor is launched, then data for pin assignments is not saved for the relevant user. The following items are made unavailable in the Part Editor panel.

Item		Description
Detail tab		Footprint table
		Symbols table and Gate Count box
		Pin Assignment table and Pin Count box
Gate+Pin Equivalents tab		Gate + Pin Equivalents tree
Properties tab		System Part Attributes: Passive Connectivity
SPICE tab		SPICE Pin Mapping grid: SPICE Pin column
Ribbon tools and context menus	Rows	Append
		Insert
		Delete
	Assign	Pins
	Equivalents	Equivalent
		Create Sub Element
		Delete
		Delete All

Part Information

Item		Description
Type of part		Specify the Part Type as General, Jumper , Star Point or Etched.
	General	If selected, the part is considered a packaged part such as an FPGA device.
	Jumper	If selected, then the part is defined as a jumper. This allows it to have the same signal name on each pin. It also allows it to be inserted into a design without it being in the associated schematic.
	Star Point	If selected, then the part is defined as a star point. Star points can be used to connect multiple signals. They can have coincident pads without causing a DRC error. See Creating a Star Point.
	Etched	If selected, then the part is defined as a etched part. Etched can be used to create etched or printed parts. These are parts that are created out of copper. The “etched” definition allows users to modify in -component items (vias and copper figures) within eCADSTAR PCB Editor or to match the electrical configuration needed for the component. See Creating an Etched Part.
Reference Designator Prefix		Allows you to specify the prefix used in the reference designator for the part; for example, 'R' for resistors, 'C' for capacitors and 'D' for diodes. Either select the displayed value which currently exists in the library, or type a new value. If you define a new value, it can then be selected in the Reference Designator Prefix column in the Library Editor panel, Parts tab. Delete a selected value by right-clicking it and selecting Delete on the assist menu. The part is deleted from the library.
Part Class		Specify the part class for the part. Either select a displayed value which currently exists in the library, or type a new value. If you define a new value, it can then be selected in the Part Class column in the Library Editor panel, Parts tab. Delete a selected value by right-clicking it and selecting Delete on the assist menu. The part is deleted from the library.
Description		Displays the description that is in the library for the selected part. If you change the displayed value, the new value is shown in the Description column in the Library Editor panel, Parts tab.

Footprint

Item	Description
Name	Displays the name of the footprint that is associated with the selected part. Rename the footprint by clicking in this cell and defining a new name, or change the footprint that is associated with the part as follows: Point to the value in the Name column. The button is displayed. Click . The Library Searcher dialog is displayed. In the Library Searcher dialog, Footprint Name table, double-click the footprint that you want to associate with the part. The footprint is added to the Name column. If a footprint is not displayed in the Name box, you can create a new footprint to associate with the part by clicking Home > Footprint > New in Part Editor, and specifying the details in the New Footprint dialog. Alternatively, right-click in the Name box and select New Footprint on the assist menu.
Alternate	Allows you to associate a footprint alternate with the part (optional). If a footprint alternate is associated with the part, it is displayed. To change the footprint alternate, point to the Alternate box and select from the values that are listed.
Pin Count	Displays the number of pins for the footprint. This is a read-only value.

Item

Description

Name

Displays the name of the footprint that is associated with the selected part. Rename the footprint by clicking in this cell and defining a new name, or change the footprint that is associated with the part as follows:

Point to the value in the Name column. The button is displayed.
Click . The Library Searcher dialog is displayed.
In the Library Searcher dialog, Footprint Name table, double-click the footprint that you want to associate with the part. The footprint is added to the Name column.

If a footprint is not displayed in the Name box, you can create a new footprint to associate with the part by clicking Home > Footprint > New in Part Editor, and specifying the details in the New Footprint dialog. Alternatively, right-click in the Name box and select New Footprint on the assist menu.

Alternate

Allows you to associate a footprint alternate with the part (optional). If a footprint alternate is associated with the part, it is displayed. To change the footprint alternate, point to the Alternate box and select from the values that are listed.

Pin Count

Displays the number of pins for the footprint. This is a read-only value.

Symbols

Item		Description
Gate Count		Specify the number of gates in the selected part. A corresponding number of rows is added to the Symbols table.
Symbols table		Allows you to specify a symbol and alternate for each gate that you add using the Gate Count box. Read-only values are displayed for Gate and Pin Count.
	<Filter>	Allows you to enter a value to filter the relevant column. See: Filtering Displayed Values in eCADSTAR Tables.
	Gate	The gate number. This read-only value is automatically assigned when you specify the number of gates.
	Name	Displays the name of the symbol that is associated with each gate. Change the symbol that is associated with a gate as follows. Point to a cell in the Name column for the relevant gate. The button is displayed. Click . The Library Searcher dialog is displayed. In the Library Searcher dialog, double-click a symbol in the Symbol Name column. The symbol is added to the Name column in the Symbols table.
	Alternate	If a symbol alternate is associated with the selected symbol, point to the Alternate box and select it from the values that are displayed.
	Pin Count	Displays the number of pins associated with each symbol. This is a read-only value.

Pin Assignment

The Pin Assignment table allows you to define the mapping of footprint pins to symbol pins. You can type values in each cell, or copy and paste values using the assist menu.

Item		Description
Pin Count		Displays the number of pins in the footprint. This value corresponds with the number of rows in the Pin Assignment table. Specify the number of rows in the Pin Assignment table by entering a value in the Pin Count box. Alternatively, right-click in the Pin Assignment table and select Add Row, Insert Row or Delete Row on the assist menu. When you assign a footprint to the part, this value is automatically updated to match the pin count of the footprint. If the Pin Count value is decreased, rows are removed from the Pin Assignment table in descending alphanumeric order.
Pin Assignment table		The Pin Assignment table allows you to define the pin assignment for a selected part by entering a value in each column. You can save the specified settings before completing the pin assignment. These settings are displayed in the Part Editor Panel: SPICE Tab, SPICE Pin Mapping table. This table allows you to assign a pin in a SPICE model to a pin on the part. Note If you make a change in the Pin Assignment table, then the SPICE Pin value in the Part Editor Panel: SPICE Tab may become invalid as it is not automatically updated. When updating the existing footprint, or specifying a new footprint or alternate that has the same pin naming pattern: If the number of pins is increased: the Pin Assignment table and Pin Count values are updated to match the new footprint pin count. Extra rows are added to the table, with relevant pin numbers. If the number of pins is decreased: the Pin Count value is displayed in red to indicate that extra footprint pin rows are defined in the Pin Assignment table. The rows that no longer match the pin names within the footprint are displayed in red. Edit the table to remove or correct the highlighted rows. When updating the existing footprint or setting a new footprint or alternate, with a different pin naming pattern: The Pin Count value is displayed in red to indicate that extra footprint pin rows are defined in the pin assignment table. Edit the table to remove or correct the rows that are shown in red.
	<Filter>	Allows you to enter a value to filter the relevant column. See: Filtering Displayed Values in eCADSTAR Tables.
	Footprint Pin	When you assign a footprint to the part, the pin numbers or names that are assigned to the footprint are automatically displayed in this column, but can still be edited. If a part has no footprint assigned, you must add the required values to this column. This value is displayed in the Part Editor Panel: SPICE Tab, Footprint Pin column.
	Label	Enter a unique label for each pin assignment. This value is displayed in the Part Editor Panel: SPICE Tab, Label column. Note If a part is defined with only a single gate, then this value is used for labeling the pins in both eCADSTAR Schematic Editor and eCADSTAR PCB Editor. If a part is defined with multiple gates, then this value is used for labeling the footprint pins in eCADSTAR PCB Editor, and the Gate Label value is used to label the symbol pins for the gates in eCADSTAR Schematic Editor. This is because the pin label must be unique in eCADSTAR PCB Editor, but the pin gate label can be duplicated per gate. For example, each instance of the same gate can have a duplicated label. However, each instance of the pin label must be unique.
	Circuit Label	If required, enter a label for each pin assignment. Duplicate circuit labels are permitted. For each pin, you can specify that a circuit label is displayed instead of a label. This value is displayed in the Part Editor Panel: SPICE Tab, Circuit Label column.
	Type	Specify the type of each pin by selecting a value from the following options. UNDEFINED: the pin type is undefined. This is the default pin type. INPUT: sets the pin type as "Input". OUTPUT: sets the pin type as "Output". BIDIRECT: sets the pin type as "Bidirectional". POWER: sets the pin type as "Power". GROUND sets the pin type as "Ground". NC: the pin is not connected. For a part with multiple gates: if you change the value in the Type column, the same value is set for the identical gates. This value is displayed in the Part Editor Panel: SPICE Tab, Type column.
	Gate	Specify the gate number using the value that are displayed in the Gate column in the Symbols group.
	Symbol Pin	Specify the number of the symbol pin. This must be less than or equal to the Pin Count value for the relevant gate in the Symbols group. To assign pins using a semi-automatic process, select a relevant row in the Symbol Pin column and select Home > Pins > Assign on the ribbon. Alternatively, right-click the selected row and select Assign on the assist menu. The Assign Pins dialog is displayed. Select multiple rows using the Ctrl or Shift keys. This value is displayed in the Part Editor Panel: SPICE Tab, Symbol Pin column.
	Gate Label	Specify the gate label using a value that is unique per gate. This value is displayed in the Part Editor Panel: SPICE Tab, Gate Label column. Note If a part is defined with only a single gate, then the Label value is used for labelling the pins in both eCADSTAR Schematic Editor and eCADSTAR PCB Editor. If a part is defined with multiple gates, then the Label value is used for labeling the footprint pins in eCADSTAR PCB Editor, and the Gate Label value is used to label the symbol pins for the gates in eCADSTAR Schematic Editor. This is because the pin label must be unique in eCADSTAR PCB Editor, but the pin gate label can be duplicated per gate. For example, each instance of the same gate can have a duplicated label. However, each instance of the pin label must be unique. This column is only made available when values are added in both the Gate and Symbol Pin columns. If this is the first time the Gate and Symbol Pin values are assigned, the Gate Label column is populated with the Symbol Pin value. This column is made unavailable unless more than one gate is specified (excluding the power box). If the number of specified gates is reduced to one (excluding the power box), all values in the Gate Label column are deleted and this column is made unavailable. If you delete the Gate Label value, the Symbol Pin value is displayed instead. If both Gate Label and Symbol Pin values exist in a row, and the Symbol Pin value is deleted, the Gate Label value is deleted and the column is made unavailable. If both Gate and Symbol Pin values exist in a row, and the Gate value is deleted, the Gate Label value is deleted and the column is made unavailable. For a part with multiple gates: if you change the Gate Label value for a pin, the corresponding Gate Label values are updated on the pins of the identical gates. If you choose a symbol with a Component Type of Power Box, then a gate row is considered as a power box. Otherwise, it is considered as a gate. Refer to the following guide to using power boxes:
	Signal	If Ground or Power is selected in the Type column, then you can specify the signal that is carried on the associated pin, if required.
	Pin Length	Sets the track length in package for part pins. If you set Pin Length for a component pin in eCADSTAR PCB Editor, the component pin setting is given priority and referenced.

Note

For non-gated parts, the value in the Label column is used for the symbol pin in eCADSTAR Schematic Editor and for the footprint pin in Footprint Editor. This is illustrated below.
For gated parts, the value in the Gate Label column is used for the symbol pin in eCADSTAR Schematic Editor. However, the value in the Label column is used for the footprint pin in Footprint Editor. This is illustrated below.
If there are unsaved changes in the Detail tab, then the "*" character is displayed next to the Part Editor tab.