High Density Interconnect (HDI) techniques are increasing in the PCB domain. HDI provides the ability to place components on both sides of the board and helps reduce the PCB layer stack. Allegro PCB Router started evolving in this direction from the SPB16.2 version with drill holes and microvias. In the SPB16.3 release, constraints for blind and buried vias, and stacked via enhancements, were provided.
With the SPB16.5 release, SPECCTRA provides ability to use inset/tangency and stagger via patterns.
Read on for more details …
A tangent via pattern consists of two vias connected to each other through tangency of their pads: Side View of Tangent pattern:
Superposition of Tangent patterns:
Notice the changes in the clearance descriptor syntax, especially the tangency and inset rules at bottom:
For details, please refer to command reference manual.
Translating tangency from PCB Editor / SPIF changes
The bbvia tangency configuration in Allegro PCB Designer is recognized like a bbvia to bbvia samenet clearance value specified to 0. The rule is accounted in via configuration creation; even if samenet DRC checker is turned off, both core bbvia and microvia types are affected. SPIF will translate the “tangency” keyword as a legal value instead of 0 clearance on all hierarchy levels.
Example:The following class tangency allows tangency between bbvia and bbvia.rule class RF_SP (clearance tangency (type bbvia_bbvia))The following command allows tangency on net ADDR5 between bbvia and microviarule net ADDR5 (clearance tangency (type microvia_bbvia))The following command allows tangency in BGA region between microvia and microviarule region BGA_U383_1_4 (clearance tangency (type microvia_ microvia))
You can now highlight the tangent and inset vias by using the highlight command in SPECCTRA -
highlight via_tangency on
This will highlight the tangent vias as shown below:
highlight via_tangency offThis will remove the highlight of via_tangency.Please share your experiences using this new capability.
Jerry "GenPart" Grzenia