BUILD_PCS MACRO

The BUILD_PCS MACRO Creates a Named PHYSICAL_CONSTRAINT_SET (PCS) which can be applied to matching NetNames or referenced by an Electrical Constraint Set (ECS)

Physical Constraint Sets

A Physical Constraint Set is use to constrain the PHYSICAL attributes of signals on each routing  layer. 

The dal Stackup tool creates named PCS for each impedance rule extracted from the stackup spreadsheet.

If more impedance rules are needed, the BUILD_PCS macro can be used to easily define them in a few rows

BUILD_PCS can define impedance width and spacing rules for each layer as well as the minimum width required for matching power nets.

It can also create rules to exclude routing layers for target nets

BUILD_PCS  

This Line tells dal constraints to create a new named PCS 

syntax: 

BUILD_PCS  | NAME=> | NAME_FOR_PCS

the TYPE=> Attribute  tells dal constraints what type of PCS the user wants to create

Valid options are: DIFF_IMPEDANCE, SINGLE_ENDED_IMPEDANCE and POWER

UNITS

The UNITS=>Attribute tells dal constraints what units to use for the PCS 

Valid options are: MILS and MM

ON_LAYERS

the ON_LAYERS=> attribute lets the user exclude certain routing layers for the target nets

The ON_LAYERS attribute is converted to AllegroPCB ALLOW_ETCH contraints 

All nets default to ALLOW_ETCH =1 for every layer.

The ON_LAYERS lets us turn off the ALLOW_ETCH for specific layers

Syntax:

ON_LAYERS=>-12,-15 

this command says that the target nets are allowed on every layer except  Layers 12 and 15

TRACE_WIDTH_PARAMETERS

the TRACE_WIDTH_PARAMETERS attribute provides a list of routing widths and spacing for each routing layer (using the UNITS attribute)

example syntax for TYPE=>DIFF_IMPEDANCE  

TRACE_WIDTH_PARAMETERS=> L1,L24=10/7.5:L4,L5,L8,L9,L16,L17,L20,L21=3.7/5

This specifies that target diff_pair nets  on Layers 1 and 24  should be routed at 10 mils and 7.5 mil edge to edge spacing. On layers 4,5,6,7,8,9,16,17 and 21 target diff_pairs should be routed at 3.75 mils and 5  mil spacing

example syntax for TYPE=>SINGLE_ENDED_IMPEDANCE 

TRACE_WIDTH_PARAMETERS=> L1,L24=12:L4,L5,L8,L9,L16,L17,L20,L21=6

This specifies that target single_ended nets  on Layers 1 and 24  should be routed at 12 mils, On layers 4,5,6,7,8,9,16,17 and 21 target single_ended nets should be routed at 6 mils

example syntax for TYPE=>POWER

MEMBERS

The MEMBERS=> Attribute tells dal constraints what nets to apply the new PCS to. 

This is an optional attribute when you are creating a PCS that will be assigned from an ECS.

The syntax is MEMBERS=>net_match1,net_match2.... net_matchN

like

MEMBERS=>P48V,P48V_RTN

This tells dal constraints to assign this PCS to any net containing 'P48V' or 'P48V_RTN'

in this case the net_match is a simple text pattern 

The MEMBERS net_matches are treated as regular expressions by dal constraints and are quite powerful.

To see more information on regular expression entry see  Regular Expressions In CadEnhance Tools

NOT_MATCHING

The NOT_MATCHING=>Attribute is optional and works together with the MEMBERS attribute to fully define the set of target nets

The NOT_MATCHING is a  comma separated list of patterns that will be used to exclude nets from the set of nets that match the MEMBER patterns

Together the 2 attributes make very simple to define a large set of nets without having to create a very large list of specific matches