Defining Net Classes by Area on a Schematic

Old Content - visit altium.com/documentation
Modified by Jason Howie on Oct 12, 2015
Related Video

Blankets in Schematic 

Contents

Altium Designer already allows you to create user-defined net classes on the schematic side using Net Class directives attached to each 'member' wire, bus or harness. When a PCB is created from the schematic source documents, the information in a Net Class directive is used to create the corresponding net class on the PCB. Assignment of nets to the required classes using this method is, however, time-consuming, prone to error and also creates unnecessary clutter in the schematic source documents. The Summer 09 release of Altium Designer delivers a streamlined, time-efficient and visually-tidy new method of net class definition, using the new Blanket directive.

Creating a Net Class from a Blanket Directive

Accessed from the Place»Directives sub-menu, the Blanket directive (shortcut P, V, L) is placed in the same intuitive way as a Compile Mask directive. Simply place the Blanket around the required nets – which you want to group together into the same net class when taken over to the PCB – then attach and define a Net Class directive to the blanket's perimeter. The Net Class directive will be applied to all nets that fall within the area defined by the blanket.
 

To generate the PCB Net Class from a perimeter Net Class directive attached to the Blanket directive, ensure that the Generate Net Classes option is enabled in the User-Defined Classes region, on the Class Generation tab of the Options for PCB Project dialog (Project»Project Options).


Quickly create a PCB net class, whose member nets are defined on the schematic using a Blanket directive.

To apply the perimeter Net Class directive to a net under a Blanket directive, an object associated to that net – a pin, a port, a net label, a power port, a wire/bus/harness segment (including both ends) – must fall within the bounds of the blanket. Note that for net identifiers, such as net labels, the hotspot must be within the blanket. If member nets do not come across into the PCB net class as expected, try adjusting the area of the blanket accordingly.

 

You can also copy a perimeter Net Class directive and attach it to another Blanket directive or even individual wires, busses or harnesses – the result will be to add all additional nets associated with the same Net Class directive, to the same generated PCB Net Class.

Highlighting Nets Covered by a Blanket Directive

To get a graphical indication of which nets are 'covered' by a Blanket directive, you can use the Schematic Editor's highlighting pen feature. Simply click on the button at the bottom-right of the main design window, then click on the perimeter of the required Blanket directive.
 

Press Spacebar to change the color of the highlighting pen. To clear all highlighting on the active sheet, click on the Clear button at the bottom right of the main design window.


Use the highlighting pen feature to visually get a better idea of which nets are affected by a Blanket directive.

Highlighting is applied to all wire and bus segments associated to nets covered by the Blanket directive. Nets formed through direct pin-to-pin connection of components (e.g. two series resistors), or through direct component pin-to-power port connections (e.g. capacitor to GND), will not be highlighted.

Selecting Net Objects covered by a Blanket Directive

To quickly select all objects associated to nets 'covered' by a Blanket directive, you can use the Edit»Select»Connection command. Simply launch this command and click on the perimeter of the required Blanket directive. All wire segments, bus segments, harness segments, pins and power ports associated to nets falling under the Blanket's coverage will be highlighted and selected, as well as the Blanket directive itself.

Quickly select all objects associated to nets affected by a Blanket directive.

The selected objects will be highlighted in the selection color defined in the Selections field, on the Schematic – Graphical Editing page of the Preferences dialog (DXP»Preferences).

Additional uses of the Blanket Directive

Use of the Blanket directive does not rest solely with the definition of net classes on the schematic. In fact, any schematic design directive that is based on the Parameter Set feature can be attached to the perimeter of a Blanket directive, and the corresponding parameter(s) applied to each of the nets therein.

Applying a PCB Layout Directive (to Individual Nets)

The following image shows use of a Blanket directive to apply a PCB Layout directive, with a defined Width rule, to each of the individual nets within.

Quickly create design rules targeting nets captured within the confines of a Blanket directive.

Applying a PCB Layout Directive (to Net Class)

Typically, when creating a Net Class using a Blanket directive, you might also define PCB layout information to apply to those member nets within. A PCB Layout directive attached to the perimeter of a Blanket directive – to which a Net Class directive is also attached – will be applied to 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, with a scope set to target the net class.

Add design rules targeting the net class created using a Blanket directive.

When specifying PCB design rules to target the generated net class, you can either add PCB Layout directive(s) to the perimeter of the Blanket directive, or add the rules directly as parameters contained within the Net Class directive.

Applying a Differential Pair Directive

Note - the following functionality is not working correctly in versions of the software since Summer 09, but will be fully functional again in Altium Designer 16, and later.

By attaching a Differential Pair directive to the perimeter of a Blanket directive, you can quickly create differential pair objects based on differential nets within the blanket.

Quickly create differential pairs based on the differential nets captured within the confines of a Blanket directive.

Printing Schematics containing Blanket Directives

When generating output from source schematic documents, you have the option to include (or exclude) Blanket directive objects from that output. The location of the control to do this, depends on the output being generated:

  • Smart PDF – enable/disable the Blankets option as required, in the Schematics region, on the Additional PDF Settings page of the Smart PDF Wizard.
     

    Controlling display of Blankets when generating a Smart PDF.


     

  • Schematic prints from an OutJob file – enable/disable the Blankets option as required, in the Drawings region of the Schematic Print Properties dialog, when configuring the associated output generator.
     

    Controlling display of Blankets when generating schematic prints from an Output Job Configuration file.


     

  • Schematic prints direct from the Schematic Editor – enable/disable the Blankets option as required, in the Drawings region of the Schematic Print Properties dialog, when configuring from the Preview dialog (File»Print Preview)
     

    Controlling display of Blankets when generating schematic prints directly from the Schematic Editor.
You are reporting an issue with the following selected text and/or image within the active document: