G
Greg Neff
- Jan 1, 1970
- 0
No one in my experience (especially me) ever seems to get PCBs of any
complexity designed correctly straight off, there's always at least one
error on the prototype. They are usually OK the second time round, of
course. How general is this observation?
I've got a feeling that thorough checking of the prototype PCB design
probably costs more ultimately than just getting it made and fixing any
problems subsequently.
Leon
These days our PCBs tend to be on the complex side. We do
double-sided SMD, BGAs, fast signals, 16-layer construction, >800
components, etc. We usually have to spin the board a second time.
Occasionally a third time, but not too often (if we get bit at this
point it's usually due to a signal integrity or ESD/EMI issue). We
get close because we carefully control the design process:
1) We have a library of verified footprints. If we need a new
footprint then it is made and checked against a mechanical sample
prior to it being used in a design.
2) Our schematic libraries include every part number in our part
database. Each part in a library includes the part value,
manufacturer, manufacturer's part number, our part number, and
footprint. Yes, this means that we have a library part for each value
and size of resistor we use. The generation of the parts in the
schematic libraries is where most of our mistakes are made.
3) A schematic is entered that includes only mechanically critical
components. A PCB is designed with these parts placed as per the
specification. A copper-clad piece of FR4 is drilled and routed by
our PCB house. The mechanically critical parts are soldered and/or
glued to this board. This mechanical sample PCB allows verification
of form and fit in the target equipment. It also allows the
mechanical guys to work on the enclosure and wiring harness design.
4) A complete schematic is entered and run through DRC. The schematic
is peer-reviewed. A human-readable netlist (wirelist) is generated.
You would be surprised how many errors can be detected by reviewing
this wirelist.
5) A PCB netlist is generated. The netlist is imported into the PCB
tool.
6) The PCB layout is done, with several reviews along the way by the
design engineer. Any changes required at this stage are carefully
forward or back annotated as required.
7) A BOM is generated from the schematic, and a kit of parts is pulled
to allow building of two or three prototypes.
8) We build the prototype, and then the fun begins...
Breadboarding is a thing of the past for digital designs. It simply
won't work. The last wire-wrap prototype that we did was about 15
years ago.
================================
Greg Neff
VP Engineering
*Microsym* Computers Inc.
[email protected]