Protel 99

Useful setup

• Have an own directory for your projects, eg c:\protel99\myprojects
• Have an own .ddb for your personal libraries, eg mylibs.ddb
  with MySch.lib, MyPCB.lib, MySMD.lib, RF_Comp.lib, RF_foot.lib
  as libraries
• Name special schematic components and its footprint identical,
  as the footprint does not allow to have a comment.
• don't have too many open design's as they're loaded at startup.
• I have all schematic components drawn myself, as I don't like the
  predrawn libraries.

hints

Schematic hints

• Startup - special strings

  Setting the document options, (size, title, ...) is not sufficient.
  Place the text '.TITLE' into the sheet at the title location makes the
  defined document title appear there. Without this string the field stays
  empty.
  More special strings are listed on page 68 of the manual.
  
  

PCB hints

• Startup

  The minimal and maximal track width defaults to 10mil. Change that to
  whatever appropriate. ->Menu, Design Rules
  
  

• GND plane version

  The normal PCB has a clearance of 10mil, the version with GND planes
  has a clearance of 20mil. This is a file generated afterwards with a
  different name. I use *.pcb and *_WP.pcb respectively.
  
  Octagons around pads are prefered. Arcs tend to invert on a printout,
  at least on my HL1050, I have to kind of reload the printer(for each
  layer) to prevent the arcs being the other way around.
  
  

• special strings

  The various special strings are listed on page 495 of the manual.
  The most important ones are : .PCB_FILE_NAME_NO_PATH, .LAYER_NAME,
  .LEGEND
  
  

• Mirroring footprints at odd locations

  Footprints of connectors may be at odd location, meaning outside a snap.
  When they are selected, the cursor is at pin 1 (I have them this way).
  It is mirrored with X or Y, then the location is not preserved, and there
  is no snap. The solution is to place pad at the location where pin 1 will be
  after the mirroring, eg pin 2 or pin 20 or whatever. The pad will snap there,
  and the mirrored footprint snaps to the pad again.
  
  

• special components

  I have a component named '001_Origin' which is a 10mil track cross which is
  placed at the origin (0,0). It gives the SMD placer a hint where the origin
  of the coordinate system is. When etching myself, it helps align the films.
  
  Another component is the '001_Writing', consisting of the special strings :
  .LAYER, .PCB_FILE_NAME_NO_PATH, .PRINT_DATE, .PRINT_TIME on each layer.
  Mirror if appropriate. It helps getting the right side of the films correctly
  aligned.
  
  An important component when self etching is the alignment cross. I have 4 of
  them in the corners. They are on top and bottom layer with a width of 10 and
  100 mils in diameter.
  
  Having those components also on the schematic, simplyfies working with them,
  as they might get deleted if not remembered.
  
  

• self etching

  I usually have two files : fileXY.pcb and fileXY_WP.pcb, the first one is
  the one routed with clearance 15 mil, the second one is a copy after the routing
  Then the GND planes are a applied after increasing the clearance to 20 or 25 mil.
  Should a change occur to the layout it is applied to the first file, then
  it has to be copied again to the second and the GND planes are applied.
  
  The top and bottom layers are printed onto paper first, and after careful
  inspection onto a polyester film. The top layer is mirrored, while the bottom
  layer is printed straight. Don't forget to tick 'show holes' in the printer menu,
  It helps drilling the holes.
  
  When etching the pcb's yourself, these are some values based on experience
  with a 600 dpi Laser printer using 90 um polyester films FOLAPROOF 0970.4.440
  from FOLEX.
  min trackwidth 10mil
  clearance 10mil
  via 28/52
  
  Though the etching technology would allow smaller values, the films have some
  thermally induced distortions. And then there is the alignment of top and bottom
  layer which may change a fraction when the pcb board is inserted between the two.
  The critical point is that the via's holes may not meet the via anymore.
  
  hints are welcome
  
  I found the minimal holesize to be 0.7mm = 28mil. Though smaller drills are
  available, they just break too often, at 7$ each.

Links