pcb-rnd knowledge pool

 

Index: using and creating footprints

Ifootprint by Tibor 'Igor2' Palinkas on 2017-12-25	Tags: index, footprint, library, lib, subcircuit
node source

 

Abstract: n/a

 

Using existing footprints

Using footprints has two main aspects: library (how/where to get the footprints) and importing from schematics .

Library sources, footprint types

Pcb-rnd has a modularized library support: differnet fp_ plugins access local and remote footprint libraries differenlty. At the end all footprints are accessible through a unified runtime library. Related nodes:

• pcblib - insight on how the lib shipped with pcb-rnd was designed
• fp_wget - tips on using remote footprint libs over HTTP
• parametric - introduction to parametric footprints
• library_t - insight on how deep the runtime library can get

Importing from schematics

When a raw netlist is imported, no footprints are placed, only the netlist is initialized. In an "import schematics", both netlist and footprint names are imported.

Footprint names are typically set as symbol attributes on the schematics.

How to design footprints

Technically

Drawing a footprint is creating a subcircuit . A subcircuit is a generic grouping mechanism that is also used as the footprint implementation in pcb-rnd. Related nodes:

• tutorial on building a subcircuit
• finished subcircuits are normally put in a local footprint library ; this is most often done by simply saving the file and copying it into a directory that is then added to the library search path in the preferences window
• once a subcircuit is placed in a board the subcircuit lock applies to its parts, keeping the subcircuit intact, but the the loose subc option allows editing it
• subcircuit files can be open by pcb-rnd directly, e.g. pcb-rnd footprint.lht and then pcb-rnd will be in a "footprint editor mode" where you can freely modify the footprint and save it as a footprint
• footprints typically need a refdes text

Details to consider

There are a lot of fine details to consider when designing a footprint:

• Origins of the subcircuit:
  • there's an origin by the subcircuit is grabbed when placed from the library, marked with a diamond (rhombus) sign on screen
  • by default that's also the pick-and-place origin in some cases; it can be overridden by manually specifying a pick-and-place origin point
• Terminal geometry: padstack design considerations (board density, soldering aspects)
• Terminal numbering ; terminals have to be numbered and this numbering has to match the schematic symbol's numbering (or there must be a device mapping layer in the workflow)
• documentation layers: what to draw on silk, what to draw on assembly or fab layers; best practice: do not overload the silk layer with drawings/doc that are not really useful when printed on the board
• keepout layers: both for documentation and getting the drc check for overlapping footprints

Terminals can be numbered by hand, using the {e t} keys over the terminal, or using scripts such as the termnum script, available from edakrill.

Padstack design

Terminals of a footprint is most commonly created using padstacks. Padstacks are constructed and broken up in a very similar way to subcircuits.

When designing a padstack, you should consider:

• board density: on dense boards, smaller pads are recommended (but that may be harder or more expensive to poppulate)
• copper geometry:
  • for manual soldering, you may want larger copper shape on the side facing the technicial so it is easier/faster to solder the pin
  • thru-hole pins and vias should normally have a copper ring on all copper layers
  • in case of smallish SMD parts, especially passives, the wrong copper pad size can lead to thombstoning
  • sometimes the first terminal of a footprint is marked by slightly different pad geometry (e.g. square instead of round for thru-hole); but this may interfere with board density or high-speed/high-freq requirements
• mask shape:
  • has to be drawn explicitly!
  • most pins and pads normally need a mask shape, else solder mask will cover the pad and the pin/lead can not be soldered
  • the mask normally needs to be a bit larger than the copper shape, to compensate for mask misalignment
  • it's usually a safe bet to generate the mask shape from copper shape using the derive button in the padstack editor
• paste shape:
  • typically used on SMD pads only
  • has to be drawn explicitly!
  • should be as big as, or smaller than the copper shape
  • it's usually a safe bet to generate the mask shape from copper shape using the derive button in the padstack editor
  • some pads, like the central pad of a qfn, may require a pattern of smaller paste blobbs; a padstack can create only a single paste shape per paste layer; a pattern should be drawn separately, e.g. as polygons on the paste layer (within the same subcircuit)
  • at certain sizes, it is best practice to use chamfed or round corner paste patterns so paste doesn't stick in the sharp corner
• hole or slot:
  • a thru-hole pin has either a hole or a slot in the padstack; hole is always circular (for a "pin" which is circular or square), slot can be of any shape, typically it's a round cap line (for a "tab")
  • a circular hole is created by specifying the diameter (in the padstack editor)
  • a slot is created by drawing the shape on a boundary or mech layer while constructing the padstack
  • the hole/slot for a metal pin/tab is almost always plated; plating is a single bit data you can toggle in the padstack editor
  • the hole/slot for a plastic/positioning pin or for a mounting hole is typically unplated; plating is a single bit data you can toggle in the padstack editor
  • values and geometry in pcb-rnd generally refers to finished values; that is, a plated hole with 0.8mm diameter means the diameter of the finished hole (the inner diameter of the copper pipe) is 0.8mm, and the fab had to use a larger drill to compensate for plating (the copper pipe's wall thickness)
  • in theory a footprint can contain padstacks with blind/burried holes, but that's not common in practice