After having worked for several years with various version of
Protel, Protel 99
is the 32bit version with very few bugs. The 99 version is really useful.
Protel3.0 was still 16bit though announced as Protel95.
Protel98 was a bit crappy, it had too many bugs.
It is best run on a fast Pentium (III) with lots of RAM.
A Pentium 166 with 64MB is the lower limit.
A screen with 1600x1200 in truecolor is about the one to have.
The OS of choice is WinNT4.0
Whereas previous version had the schematic and PCB layout and other packages
separate, Protel99 is an All-in-One package.
Some ideas have changed. After working for several month with Protel 99,
a useful setup is slowly crystalizing out.
- 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
- 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
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
More special strings are listed on page 68 of the manual.
.. to be continued
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.
The various special strings are listed on page 495 of the manual.
The most important ones are : .PCB_FILE_NAME_NO_PATH, .LAYER_NAME,
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.
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
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.
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
min trackwidth 10mil
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.
Unfortunately there is no real newsgroup, just a place to subscribe
"subscribe proteledausers". A very unfortunate solution as every message
is broadcasted and fills the mailbox. Can be 50++ mails per day.
last updated: 16.jan.00
Copyright (99,2000) Ing.Büro R.Tschaggelar