Parameter Set

Parent Page: Objects

A Prameter Set.

Summary

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.

Availability

Parameter sets are available for placement in the Schematic Editor only. Both default (empty) and specific (Test Vector Index, Stimulus, PCB Layout, Net Class, Differential Pair) parameter set directives are available. Access the corresponding commands from the main Place menu as follows:

• choose Place » Directives » Parameter Set [P, V, M]
• choose Place » Directives » Test Vector Index [P, V, T]
• choose Place » Directives » Stimulus [P, V, S]
• choose Place » Directives » PCB Layout [P, V, P]
• choose Place » Directives » Net Class [P, V, C]
• choose Place » Directives » Differential Pair [P, V, F].

Placement

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

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

Additional Placement Actions

• Press the Spacebar while in placement mode to rotate the directive. Rotation is anti-clockwise and in steps of 90°.
• Press the X or Y keys while in placement mode to flip the directive along the X-axis or Y-axis respectively.

Non-Graphical Editing

The following three methods of non-graphical editing are available:

...via an associated properties dialog

This method of editing uses the following dialog to modify the properties of a parameter set directive.

The Parameters dialog.
The Parameters dialog can be accessed prior to entering placement mode, from the Schematic - Default Primitives page of the Preferences dialog (Tools » Schematic Preferences). This allows you to change the default properties for the parameter set directive, which will be applied when placing subsequent parameter set directives.
During placement, the Parameters dialog can be accessed by pressing the Tab key.
After placement, the Parameters dialog can be accessed in one of the following ways:

• double-clicking on the placed parameter set directive
• selecting the parameter set directive and choosing Properties from the right-click pop-up menu
• choosing the Change command from the Edit menu and then clicking once over the placed parameter set directive.
  The parameter set directive's member parameters can be added, edited or removed from within the Parameters dialog. The properties of a parameter are available to view/modify in the Parameter Properties dialog.
  
  The Parameter Properties dialog.
  When a parameter is added as a rule, the parameter name (Rule) is locked and cannot be changed.
  The parameters of a parameter set directive can be edited independently of the parent set directive. As such, the Parameter Properties dialog can be accessed using the three methods described previously (replacing parameter set directive with the relevant parameter object whose properties you wish to view/modify).

...via the SCH Inspector panel

The SCH Inspector panel enables you to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering, the panel can be used to make changes to multiple objects of the same kind, from one convenient location.

...via the SCH List panel

The SCH List panel allows you to display design objects from one or more documents in tabular format, enabling you to quickly inspect and modify object attributes. When used in conjunction with the SCH Filter panel, it enables you to display just those objects falling under the scope of the active filter - allowing you to target and edit multiple design objects with greater accuracy and efficiency.

Graphical editing

This method of editing allows you to select a placed parameter set directive directly in the workspace and change its location or orientation graphically.
When a parameter set directive is selected in the workspace, a dashed box will appear around the directive. The box encloses the area occupied by the directive only. For each visibility-enabled member parameter of the set a dashed line will be visible, connecting the text field of the parameter to the body of the directive, thereby affirming association:

A placed PCB Rule Parameter Set.

• Click anywhere inside the dashed box and drag to reposition the parameter set directive as required. The directive can be rotated or flipped while dragging.

The parameter set directive's parameter text fields, which can be graphically edited independently of the parent directive, can only be adjusted with respect to their size by changing the size of the font used (accessed through the relevant Parameter Properties dialog). As such, editing handles are not available when any of these objects are selected:

• Click anywhere inside the dashed box and drag to reposition the text object as required. The object can be rotated or flipped while dragging:

If the Enable In-Place Editing option is enabled on the Schematic - General page of the Preferences dialog (Tools » Schematic Preferences), you will be able to edit the value for a parameter directly in the workspace (with the exception of parameters that have been added as rules). Select the text object and then click once to invoke the feature. Type the new value as required and then click away from the text object or press Enter to effect the change.

Notes

1. When placing a default parameter set directive there will be no existing parameters.
2. A PCB Layout directive allows you to assign PCB layout information to a net in the schematic. 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 to which it is connected.
3. 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 or bus and set the directive's ClassName parameter to the name of the desired class.
   The Generate Net Classes option (for User-Defined Classes) must be enabled, on the Class Generation tab of the Options for Project dialog, to make use of this feature.
4. A Differential Pair directive allows you to define a differential pair object on the schematic. Attach a directive of this type to both the positive and negative nets of the intended pair. The nets themselves must be named with the suffixes of _P and _N respectively. Both parameter set objects will contain a single parameter entry, with Name: DifferentialPair and Value: True.
   
   Each pair of directives (one for the positive net, one for the negative) of this type will yield a differential pair object when transferred to the PCB during the synchronization process. Each of these differential pair objects will be added to the default Differential Pair class: All Differential Pairs.
   The name of a generated differential pair object will be the root name for the net pair on the schematic. For example directives added to RX0_N and RX0_P on the schematic will generate a differential pair object on the PCB with the name RX0. You can rename differential pair objects on the PCB side only.
5. 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.
6. 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.