schHiCreatePin
schHiCreatePin(
[ ?terminalName t_terminalName ]
[ ?direction t_direction ]
[ ?usage t_usage ]
[ ?interpret t_interpret ]
[ ?mode t_mode ]
[ ?netExpr t_netExpr ]
[ t_justify ]
[ t_fontStyle ]
[ n_fontHeight ]
)
=> t
Description
Creates a pin of a specified type in your schematic. Usable only when editing schematics.
Arguments
|
?terminalName t_terminalName
|
Terminal name of the pin to create; must be enclosed in quotation marks. To create more than one pin, use a space between names as a delimiter. Each pin is placed individually. If you did not specify t_terminalName or you specify it as nil, the Options form appears.
|
|
?direction t_direction
|
Direction of the pin; must be enclosed in quotation marks.
Valid Values: input, output, inputOutput, switch
|
|
?usage t_usage
|
Type of pin; must be enclosed in quotation marks.
Valid Values: schematic, offSheet
|
|
?interpret t_interpret
|
Interprets terminalName; must be enclosed in quotation marks. If you set t_interpret to member, a pin for each member name in t_terminalName is generated in the order presented in t_terminalName. For example, if you designate a multibit terminal name as addr<7:0>, the schematic editor places each member name, addr<7> through addr<0>, and each of these member name pins individually. If you set t_interpret to full, a pin for each space-delimited terminal name from t_terminalName is placed individually. Valid Values: full, member
Default: full
|
|
?mode t_mode
|
Mode you use to place the pins; must be enclosed in quotation marks. If you set t_mode to array (placement field), the schematic editor places the current pin as if in single mode. Then, if there are any remaining pins to place, it prompts you for a second point that sets the offset between the remaining pins. When a hierarchical pin exists in a sheet schematic, the schematic editor preserves the direction of the terminal when you create an offsheet connector for the same terminal with a different direction. In this case, the direction specified for the offsheet pin is used only to select its master.
Valid Values: single, array
Default: single
|
|
?netExpr t_netExpr
|
A string containing the net expression in NLP syntax; must be enclosed in quotation marks.
|
|
t_justify
|
Justification to give the label text with respect to its placement; must be enclosed in quotation marks.
Valid Values: upperLeft, upperCenter, upperRight, centerLeft, centerCenter, centerRight, lowerLeft, lowerCenter, lowerRight
|
|
t_fontStyle
|
Label font style; must be enclosed in quotation marks.
Valid Values: euroStyle, fixed, gothic, math, roman, script, stick, swedish, milSpec
|
|
n_fontHeight
|
Label height in user units.
Default: 0.0625
|
Value Returned
Examples
Creates a pin for an input offsheet pin. You can drag and place the pin using the mouse. The schematic editor designates the terminal name data1.
schHiCreatePin( ?terminalName "data1" ?direction "input" ?usage "offSheet" )
Adds a net expression to an inout offsheet pin.
schHiCreatePin( ?terminalName "data1" ?direction "input" ?usage "offSheet" ?netExpr "[@power:%:vdd!]" )
For each member name, addr<7> through addr<0>, you can drag and place a schematic input pin with a member name.
schHiCreatePin( ?terminalName "addr<7:0>" ?direction "input" ?usage "schematic" ?interpret "member" )
Places one schematic input pin for each space-delimited name addr<7:0>, data4, and data5.
schHiCreatePin( ?terminalName "addr<7:0> data4 data5" ?direction "input" ?usage "schematic" ?interpret "full" )
Places an array of schematic input pins.
schHiCreatePin( ?terminalName "addr<2:0>" ?direction "input" ?usage "schematic" ?interpret "member" ?mode "array" )
Related Topics
schPinMasters
The Syntax of an Inherited Net Expression
Return to top
