PlaceParameterSet

Created: July 27, 2015 | Updated: April 11, 2017 | Applies to versions: 15.1, 16.0, 16.1, 17.0 and 17.1

The following pre-packaged resources, derived from this base command, are available:

Applied Parameters: None

Summary

This command is used to place a default Parameter Set object onto the active document. A Parameter Set is a design directive. It is essentially a container for one or more parameters, which can be associated to a net object within a schematic design.

For detailed information about this object type, see Parameter Set.

Access

This command can be accessed from the Schematic Editor by:

Choosing the Place » Directives » Parameter Set command from the main menus.
Right-clicking in the main design workspace and choosing the Place » Directives » Parameter Set command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter design directive placement mode.

Position the cursor over a wire or other net object and click, or press Enter, to effect placement.
Continue placing further directives or right-click, or press Esc, to exit placement mode.

Additional actions that can be performed during placement – while the parameter set is still floating on the cursor – are:

Press the Tab key to access the Parameters dialog, from where properties for the parameter set can be changed on-the-fly.
Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
Press the Spacebar to rotate the parameter set anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.

Tips

A default Parameter Set directive is devoid of parameters. Once placed, add the relevant parameter(s) to it through the Parameters dialog.
While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Place PCB Layout Directive

Applied Parameters: ParameterSet=PCBLayout

Summary

This command is used to place a PCB Layout directive onto the active document. This is essentially a pre-configured Parameter Set object, which is a container for one or more parameters, and which can be associated to a net object within a schematic design. Place a PCB Layout directive on a wire, bus, or signal harness, to define one or more design constraints targeting the associated net(s). When a PCB is created from the schematic, the information in the PCB layout directive is used to create relevant PCB design rules. The information specified by a PCB Layout directive is applied only to the net (or set of nets) to which it is connected.

For detailed information about this object type, see Parameter Set.

Access

This command can be accessed from the Schematic Editor by:

Choosing the Place » Directives » PCB Layout command from the main menus.
Right-clicking in the main design workspace and choosing the Place » Directives » PCB Layout command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter design directive placement mode.

Position the cursor over a wire or other net object and click, or press Enter, to effect placement.
Continue placing further directives or right-click, or press Esc, to exit placement mode.

Additional actions that can be performed during placement – while the parameter set is still floating on the cursor – are:

Press the Tab key to access the Parameters dialog, from where properties for the parameter set can be changed on-the-fly.
Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
Press the Spacebar to rotate the parameter set anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.

Tips

The parameters defined in this type of directive must be rule-based parameters. A default rule parameter with undefined value is present in a newly-placed PCB Layout directive.
When a PCB design rule is created from a PCB Layout directive, the word Schematic is used in the name for the rule, to distinguish the source of that rule.
A PCB Layout directive attached to a wire will generate a design rule with a rule scope of Net (e.g. InNet('LCD_LIGHT')). If the directive is attached to a bus, the generated design rule will have a rule scope of NetClass (e.g. InNetClass(LEDS[7..0])).
Attach a PCB Layout directive to a Blanket object, to have its rule parameters applied to each individual net covered by that blanket. If a Net Class directive is also attached to that blanket, the PCB Layout directive's rule parameters will target that net class, rather than each individual net. When importing the changes into the PCB document, this results in a single design rule being created (per parameter), with a scope set to target the net class.
Synchronization between a rule directive and its corresponding PCB rule is maintained through use of Unique IDs. When adding design rule parameters to objects on a schematic, a unique ID is given to each. The same IDs are given to the corresponding design rules that are created in the PCB. With this Unique ID, the constraints of a rule can be edited on either the schematic or PCB side and the changes pushed through upon synchronization.
While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Place Net Class Directive

Applied Parameters: ParameterSet=NetClass

Summary

This command is used to place a Net Class directive onto the active document. This is essentially a pre-configured Parameter Set object, which is a container for one or more parameters, and which can be associated to a net object within a schematic design. Net Class directives enable you to create user-defined net classes on the schematic. When a PCB is created from the schematic, the information in a Net Class directive is used to create the corresponding Net Class on the PCB. To make a net a member of a net class, attach a Net Class directive to the relevant wire, bus, or signal harness, and set the directive's ClassName parameter to the name of the desired class.

While Net Classes can be created fairly easily from within the PCB editor, the logical function or grouping of Nets is usually much clearer in the Schematic, and so it makes more sense to drive the process from there.

For detailed information about this object type, see Parameter Set.

Access

This command can be accessed from the Schematic Editor by:

Choosing the Place » Directives » Net Class command from the main menus.
Right-clicking in the main design workspace and choosing the Place » Directives » Net Class command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter design directive placement mode.

Position the cursor over a wire or other net object and click, or press Enter, to effect placement.
Continue placing further directives or right-click, or press Esc, to exit placement mode.

Additional actions that can be performed during placement – while the parameter set is still floating on the cursor – are:

Press the Tab key to access the Parameters dialog, from where properties for the parameter set can be changed on-the-fly.
Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
Press the Spacebar to rotate the parameter set anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.

Tips

A newly-placed Net Class directive contains a default parameter with name ClassName, and undefined value. Simply edit this parameter's value to define the name for the net class.
Attach a Net Class directive to a Blanket object, to create a net class whose members are the individual nets covered by that blanket. If a PCB Layout directive is also attached to that blanket, the PCB Layout directive's rule parameters will target that net class, rather than each individual net. When importing the changes into the PCB document, this results in a single design rule being created (per parameter), with a scope set to target the net class.
To ensure Schematic defined Net Classes are propagated to the PCB, the following options must be set in the Options for PCB Project dialog:
1. Enable the Generate Net Classes option located in the User-Defined Classes region of the dialog's Class Generation tab.
2. On the dialog's Comparator tab, set the Differences Associated with Nets » Extra Net Classes checking mode to Find Differences.
While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Place Stimulus Directive

Applied Parameters: ParameterSet=Stimulus

Summary

This command is used to place a Stimulus directive onto the active document. This is essentially a pre-configured Parameter Set object, which is a container for one or more parameters, and which can be associated to a net object within a schematic design. A Stimulus directive is used to identify a node or net to be stimulated when a digital simulation is run. This directive is only used during netlist generation. It holds no significance for any schematic processes.

For detailed information about this object type, see Parameter Set.

Access

This command can be accessed from the Schematic Editor by:

Choosing the Place » Directives » Stimulus command from the main menus.
Right-clicking in the main design workspace and choosing the Place » Directives » Stimulus command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter design directive placement mode.

Position the cursor over a wire or other net object and click, or press Enter, to effect placement.
Continue placing further directives or right-click, or press Esc, to exit placement mode.

Additional actions that can be performed during placement – while the parameter set is still floating on the cursor – are:

Press the Tab key to access the Parameters dialog, from where properties for the parameter set can be changed on-the-fly.
Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
Press the Spacebar to rotate the parameter set anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.

Tips

While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Place Test Vector Index Directive

Applied Parameters: ParameterSet=TestVectorIndex

Summary

This command is used to place a Test Vector Index directive onto the active document. This is essentially a pre-configured Parameter Set object, which is a container for one or more parameters, and which can be associated to a net object within a schematic design. Test vector directives are used to identify a node with a simulation test vector. The test vectors are referred to by a column number, which indicates the column of the test vector file to use when the simulation is run. This directive is only used during netlist generation. It holds no significance for any schematic processes.

Access

This command can be accessed from the Schematic Editor by:

Choosing the Place » Directives » Test Vector Index command from the main menus.
Right-clicking in the main design workspace and choosing the Place » Directives » Test Vector Index command from the context menu.

Use

After launching the command, the cursor will change to a cross-hair and you will enter design directive placement mode.

Position the cursor over a wire or other net object and click, or press Enter, to effect placement.
Continue placing further directives or right-click, or press Esc, to exit placement mode.

Additional actions that can be performed during placement – while the parameter set is still floating on the cursor – are:

Press the Tab key to access the Parameters dialog, from where properties for the parameter set can be changed on-the-fly.
Press the Alt key to constrain the direction of movement to the horizontal or vertical axis, depending on the initial direction of movement.
Press the Spacebar to rotate the parameter set anti-clockwise or Shift+Spacebar for clockwise rotation. Rotation is in steps of 90°.

Tips

While attributes can be modified during placement (Tab to bring up associated properties dialog), bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.