USING TANGO PCB TO DESIGN FOR MANUFACTURE

TWENTY-FOUR STEPS: USING TANGO PCB TO DESIGN FOR MANUFACTURE

by DANIEL LOMAX
(c) 1992 ALL RIGHTS RESERVED

CONTENTS:

INTRODUCTION.........................................................................2
1. GET ALL COMPONENT INFORMATION............................3
2. GET THE SCHEMATIC...........................................................4
3. ESTIMATE DENSITY..............................................................4
4. FLAG SPECIAL REQUIREMENTS.........................................4
5. SET PRELIMINARY DESIGN RULES....................................4
6. PREPARE NET LIST................................................................5
7. BUILD LIBRARY PARTS........................................................5
8. MAKE BOARD OUTLINE......................................................6
9. ADD MOUNTING HOLES......................................................6
10. LOAD NET LIST....................................................................6
11. MAKE PRELIMINARY PLACEMENT.................................7
12. ROUTE POWER.....................................................................7
13. FIRST-PASS AUTOROUTER................................................7
14. FINAL PLACEMENT.............................................................7
15. ROUTE....................................................................................7
16. RUN DESIGN RULE CHECK (OR NETS VERIFY)..............8
17. CORRECT DEVIATIONS.......................................................8
18. FABRICATION AND ASSEMBLY DRAWINGS..................8
19. INSPECTION..........................................................................9
20. CREATE AND ASSIGN APERTURES...................................9
21. CHECK APERTURE ASSIGNMENTS..................................10
22. SET UP AND CREATE PLOT FILES....................................10
23. ARCHIVE AND TRANSMIT PLOT FILES...........................10
24. ARCHIVE AND SAVE ALL RELEVANT FILES..................11
HOW TO GENERATE AN EXTERNAL GROUND PLANE......11


TWENTY-FOUR STEPS: USING TANGO PCB --2


INTRODUCTION.

There is no substitute for experience.
Having said that, I will add that we can, indeed, learn
from the experience of others. It is my hope today that you
will be able to benefit from my seventeen years of experience
as a printed circuit designer.
I started out completely on my own in Arizona, with no
books and no experienced designers to tell me how to proceed.
I had been a printer, and brought to PC design some of the
tricks of that trade, such as register pins and multilayer
mylar artwork. Then, twelve years ago, I went to work for a
moderately large company on the East Coast and really learned
how not to do design. My associates were quite certain that
they had little or nothing to learn, so certain that when the
work was slow it was time to catch up on the latest novel.
Free time, for me, was time to walk over to the assembly
line and ask how our designs were doing. Were they getting
solder bridges? Were there any insertion problems?
The assemblers were amazed. It seemed that no one from
the engineering department ever asked them such questions. It
turned out that there were lots of problems, and they would
file reports, which apparently never got to the design staff.
I also organized a tour of our principal PCB fabricator
and a discussion of design rules, with them and with all of
our designers, and wrote a design specification detailing
design process, trace widths, air gap, annular ring, etc. I
don't know if it helped anyone else, but I learned a lot.
I left that company to come out to California. I
understand that some of those designers are still there,
complaining about pay raises that don't match inflation.
But enough my personal story: I just want to make the
point that study pays off.
Study can start with books. Here are some in my library
(not necessarily the latest editions):
Preben Lund, Generation of Precision Artwork for Printed
Circuit Boards, John Wiley & Sons, New York, 1978.
I don't know if this is still available. It is the most
thorough book on the subject I have ever read, even if the
design standards it proposes are out of date.
Darryl Lindsey, The Design and Drafting of Printed
Circuits, Revised Edition, Bishop Graphics, Westlake Village,
California, 1984.
Bishop Graphics was THE place to buy tape-up
supplies. A good reference, but stodgy about design methods. I
still use the tables in the back.
Gerald L. Ginsberg, Printed Circuits Design, McGraw-Hill,
Inc., 1991. This is the book to read for today's PC design.
But by the nature of this field, books are out of date
before the ink is dry. Anyone designing circuit boards should
at least occasionally talk with those who fabricate and
assemble them. Most fabrication and assembly houses will
gladly arrange tours and discussions of design rules. After
all, knowledgeable designers make their life easier.



TWENTY-FOUR STEPS: USING TANGO PCB --3


Other valuable sources of information are manufacturers'
and distributors' catalogs. The best single catalog, which
includes mechanical information for most components, is from
Digikey, 1-800-344-4539.
If you are working in this field, there are several trade
magazines which will be happy to add you as subscribers
without charge:

Printed Circuit Design. (415) 905-2350.
Printed Circuit Fabrication (415) 905-2349.
Surface Mount Technology (708) 362-8711.

Having pointed you in a direction for further
information, I am now going to go over my basic PC design
process.

1. GET ALL COMPONENT INFORMATION.

Get or make a parts list. (See more about this under
Prepare Net List).
I don't know how many times I've seen an engineer trying
to plug a 24-pin skinny DIP (.3" wide) into a pattern made for
a normal 24-pin DIP (.6" wide). I've learned to ask for
clarification if there is the least shadow of a doubt about
the mechanical dimensions of a component. It can be very time-
consuming to redo a layout; better to do it right the first
time.
What I need for each component is the outline and pin
sizes, locations, and designators. It is best, if possible, to
work from manufacturer's drawings, including tolerances, but
this is not always possible or practical. A sample component
can help.
Naturally, I don't need re-supply of all this information
every time I design with standard components; it is only
necessary for anything unusual.
I once designed in a relay from a catalog which showed a
picture of the top of the relay, on which was printed a
diagram of the pins. Naturally, by Murphy's law, the diagram,
although printed on the TOP, was a BOTTOM view, resulting in
full employment for the technicians who do cuts and jumps.
Make sure it is clear whether a view is from the top or
bottom.
It is amazing how many component drawings, in
manufacturers' catalogs, do not include the basic necessary
design information. It helps to have a fax, for somewhere that
manufacturer has a real drawing used to fabricate.
Also, before beginning, I need to know the finished board
mechanical considerations: dimensions, mounting holes, or any
other special concerns. Sometimes certain components must be
in pre-defined locations.


TWENTY-FOUR STEPS: USING TANGO PCB --4


2. GET THE SCHEMATIC.

If it is has been prepared in Tango-Schematic or another
compatible program, great. You will be able to generate a net
list (including parts information) without further ado.
Otherwise, you can either make up a net list using a word
processor, following the Tango net list format, or design the
board without a net list. More about this later.

3. ESTIMATE DENSITY.

When I have a complete list of all the components, I do a
density study. Using a spreadsheet program, I add up the
footprint area taken up by each component (the area that each
would use if packed as close as possible, maintaining air gap
between the pads: for a 16-pin IC, this is about .4"x.9", or
.36 square inch) and divide the total by the available board
area. For two-sided board design, my rule of thumb is below
50% is easy; above 60% is difficult. For 4-layer, the numbers
are below 60%, easy, above 70%, difficult. At this point, I
advise my customer about the design difficulty (which
translates to time and cost) and we work out whether or not
there are to be any changes to board specifications.

4. FLAG SPECIAL REQUIREMENTS.

Are there any signals which require wide traces for
reasons of high current or low impedance?
Does the board require a ground plane or other low-
impedance planes?
Are any circuit paths required to be of a fixed
impedance? What trace width is required to maintain that
impedance, given the board material thickness?
Are there any special noise requirements? Which signals
are noise-sensitive? Which are likely noise sources?
Do any components have fixed or restricted positions?

5. SET PRELIMINARY DESIGN RULES.

Generally, I start out with these design rules as a
default: 12 mil traces (signal), 50 mil traces (power). Air
gap 13 mils. 25 mil grid. Vias 50 mil with 28 mil hole.
Preferred component pad 60 mil with 35 mil hole. Minimum
annular ring (hole wall to pad outline) 10 mil.
This allows one trace between pads on 100 mil centers,
and one trace per grid. It is very easy to design to these
rules. Smaller grids and traces are more time-consuming.
Most of my boards do not need to deviate from this. But
if they do, I prefer to keep the deviations to a minimum. If,
for example, I allow 8 mil traces, I will only use them where
necessary. This improves the manufacturability of the board.
A few 8 mil traces may be greatly preferable to adding an
extra layer pair.


TWENTY-FOUR STEPS: USING TANGO PCB --5


As to fine-line designs, the smallest I have had to go is
8 mil traces, 8-mil air gap, vias 25 mil with 15 mil hole, for
a dense, surface-mount, six-layer design. I have never had to
use 8 layers, in seventeen years and about one hundred
different customers.
You can always tighten up the spacings later if you get
in a tight spot, and a few tight clearances won't materially
impact the board's producibility. But beware of fabricators'
saying "no problem" to 8 mil or smaller trace and air gap.
Fabricators have an interest in presenting themselves as
capable, and they all can, indeed, produce 8 mil trace and air
gap, or even smaller. But with what yield? How reliable will
those boards be?

6. PREPARE NET LIST.

If you are using a schematic capture program, such as
Tango Schematic, it should provide a net list for you, but if
you do not have such a program, it may pay to manually make up
such a list from the schematic. Look in the PCB manual for a
description of the net list format.
First, the parts section. I usually put this together
using a database program (Microsoft Works), because I can sort
it various ways and use other tools (like the spreadsheet for
estimating density). Then I convert it to Tango format using
the word processor. Doing this forces me to be clear about all
the components before I actually start designing.
Then, the nets section. Sometimes I work from hand-drawn
schematics. I only make up a CAD schematic if my customer is
willing to pay for it, which most are not. So, if I am going
to use the nets section of the net list, I make up a name for
each net, usually based on the name of the first pin I am
entering for that net. (Like NETR1-1 for a net including R1-
1.) Naturally, every pin must have a unique name. For two-pin
non-polarized components, I assign pin 1 just according to how
the component is drawn on the schematic: pin 1 is top or left.
For boards which include a lot of bussed signals, like
memory arrays, it is much faster to simply design the board
directly and then generate the net list from the board,
checking it off against the schematic.
If I make a net list from a hand-drawn schematic, I will
usually provide it to my customer at this point for
verification. Sometimes we just check it here.

7. BUILD LIBRARY PARTS

When I am making up the part section of the net list, I
note which parts are standard or otherwise already part of my
library(s). I give those parts the already-used pattern names.
If the net list is coming from Tango-Schematic, and my
customer is using the correct pattern names, I will be able to
skip this. (It is also possible to set up Orcad so that the
net list includes the proper patterns.)


TWENTY-FOUR STEPS: USING TANGO PCB --6


For each part which is not already in the library, I give
it a new name, and keep a record of this name.
Then I go into PCB and build these parts, adding them to
the library under the new names I've assigned. If I change any
of these names, I go back and change the net list.
This entire step may be postponed until after the
already-defined components have been placed. This has the
advantage that, at that time, it will be easy to see what pad
shapes and holes are already in use, and the new components
should be built using those shapes and holes if practical.
When building parts, remember the following points:
(a) Holes should be 8 to 20 mils larger than the pin
diameter. For square pins, the hole may be tightened a bit. We
typically use a 40 mil hole for 25 mil square pins (which are
35 mils on the diagonal).
(b) The more different hole sizes, in general, the more
difficulty for the fabricator, who will try to combine hole
sizes to reduce the number of different drills required.
Better that you, the designer, control this process, for only
you know the actual sizes of the pins that will be going into
those holes. We do a lot of boards with the following holes:
28, 35, 40, 52, 125, and perhaps one or two other holes.
(c) The pads you use should allow for a minimum annular
ring, ordinarily, of 10 mils. Better, if possible, give 12
mils or more. For single-side boards, the more annular ring
the better (like 20 mils or even more for heavy components)
for the only thing keeping that pad from lifting off the board
is the glue under the annular ring. The more area, the less
chance it will pull off under stress.

8. MAKE BOARD OUTLINE.

I draw the board outline. That's what the Board layer is
for.... I also add the board title, revision level, my
customer's name, and my company's name on that layer. These
will then appear on all films (since I enable the board layer
on all films).

9. ADD MOUNTING HOLES.

This is easy to overlook, but most boards require holes
for mounting, even if they haven't been specified. Don't wait
until the board is full of dense circuitry.

10. LOAD NET LIST

As I am writing this, I don't recall whether the entry
level Tango PCB has autoplacement. If not, you will have to
wait to load the net list until after you have placed all the
components. Otherwise, now is the time to load the net list.
(Even if you have no net section to the net list, load the
part section to help you with placement. You will need to have
something in the net section, or Tango won't accept the list.)


TWENTY-FOUR STEPS: USING TANGO PCB --7


Note also that the Nets Load routine will ask you for
power and ground plane nets. If you are not designing a
multilayer board (with power and ground planes), do not assign
net names to power and ground.
Autoplace the components. Tango PCB Plus will place
everything that has an existing library part assigned to it.
You could then complete step 6 at this time, and place the
rest of the components.

11. MAKE PRELIMINARY PLACEMENT.

Using the rat's nest display, force vectors, or whatever
tools are available to you, place the components on the board,
leaving space between them as necessary to leave pathways for
routing. Here is where experience will play the greatest part.
The density study information will help you here, for you
should have some idea from that how close you must place
components.

12. ROUTE POWER.

For two-sided design, unless the board is such that power
routing is not critical, I do not autoroute power. The routers
just don't understand power routing principles.
Basically, I minimize the trace length between bypass
capacitors and the chips they bypass. If the design is TTL,
there is some advantage to keeping the ground trace shorter
vs. the power trace, due to the tighter noise margin on the
ground side.
It is also preferable to route power and ground traces
independently back to the main bypass capacitor rather than
having one power or ground trace that snakes through the
design. If there is room, power may be gridded; that is, there
may be multiple power traces, cross-connected. It is better to
avoid large loops, however.

13. FIRST-PASS AUTOROUTER

I don't have the autorouter, but I use the RoutePro demo
package here to see how the board will route. I can see
problem areas pretty quickly; it isn't necessary to run the
router to completion at this point.

14. FINAL PLACEMENT.

Nothing is final. But, more or less, after this point we
stick with routing and not with moving components around.
Sections which were easily handled by the autorouter might be
compressed a little, congested areas spread out.

15. ROUTE.

If you are fortunate enough to have an autorouter, now is
the time to let it shine. I send boards off to a friend on the



TWENTY-FOUR STEPS: USING TANGO PCB --8


East Coast who runs RoutePro on them for 35 cents a pin. I've
gotten boards back in about two hours....
If I'm manually routing the board, I route critical
traces first.
Sometimes, I change the design sequence and place and
route sections of a board, and then put the sections together.
For very high density design, this might be the only way to
go. Each section is designed for maximum density.

16. RUN DESIGN RULE CHECK (OR NETS VERIFY)

If you have PCB Plus, run the DRC. If not, you will have
to be content with Nets Verify. Better, get PCB Plus, which
has the DRC. For just two or three jobs, the difference in
price is well worth it.
If you don't have DRC, you can edit all features on the
board to make them larger in each dimension by half the
clearance, and then re-run Nets Verify. If any nets short, you
may have clearance problems. (For 13 mil clearance, add 12
mils to pad and via diameters and line widths. This won't work
with square pad corners and polygons. Like I said, better to
get PCB Plus.)
Also print the unconnected pins report and verify that,
indeed, all those pins are supposed to be unconnected. Ninety
percent of all net list errors will show up here. (I learned
this from an engineer who would register the tape-ups for all
layers of a board and look for pins with no trace.)
If you have designed the board without the net section of
the net list, run Nets Generate. This will create a net list.
This net list can then be checked against the schematic, and
used as a basis for further changes.

17. CORRECT DEVIATIONS.

For each error reported on the DRC (or Nets Verify), I
correct either the board or the net list.
If I correct the net list, I make sure that the change
gets incorporated into the schematic.
I correct the net list using a utility I wrote called
UPDATE which takes a list of corrections and incorporates them
into the net list. This forces me to document all net list
changes.
Examples of net list changes would be gate swapping or
allowed connector reassignments. Often, too, with CAD
schematics, we find power supply problems, and we correct
them. (If a part has a hidden pin 'VSS', and VSS and GND
haven't been defined as equivalent, the VSS pins will be
isolated.)

18. FABRICATION AND ASSEMBLY DRAWINGS.

I don't normally prepare formal fabrication and assembly
drawings. The drill film serves for fabrication and the silk-
screen(s) for assembly. Particularly useful can be a print of



TWENTY-FOUR STEPS: USING TANGO PCB --9


the top side silk-screen together with thru-hole and top-side
pads. (And likewise with the bottom, if there are components
on the bottom.)
What I do for a drill guide is basically what Accel
recommends: we place appropriate pads outside the board
outline and add text to the drill layer describing the holes
and their quantities (using a statistics report as a guide,
remembering to deduct one from the quantities if the extra
drill pads have already been placed).

19. INSPECTION

This I leave to my customers, usually. The design should
be inspected carefully for mechanical and functional problems.
I provide them with the .PCB file or with a set of check-
plots, depending on their requirements. Most of my customers
have the PCB demo and can view my designs or print out their
own check-plots. This is the superior way of dealing with
inspection. I post the .PCB file on my BBS and they call up
and down-load it.
Alternatively, I have a Postscript fax, which translates
Postscript check-plot files from PCB Plus to fax TIFF files
and sends them to my customer's fax. The quality is very good,
almost as good as with a laser printer.
Another customer insists on color check-plots, which I
mail to him.
Potential mechanical problems:
(a) Components interfere, placed to close together.
(b) Hole sizes too small or too large.
(c) Components not in correct locations.
Functional problems:
(a) Routing of critical nets likely to cause noise
problems.
(b) Improper net list changes.
(c) Other schematic errors noticed at this point.
If problems are found, we either go back to step 14,
moving components or rerouting the board, or just fix the
problems and go on without further inspection, depending on
the extent of the problems found.

20. CREATE AND ASSIGN APERTURES.

Because almost every new board has a different mix of
components, and thus of primitives (the basic shapes that make
up the board design), almost every design requires a unique
set of photoplot apertures. If one is using a standard set of
apertures, the special apertures required for a particular
design must be created before making the plot files, or it
will be necessary to draw those features, using the draw
aperture.
I prefer to avoid drawing primitives, because it greatly
increases the size of the plot files. (For the same reason, I
generally avoid polygons.) But I do allow Tango to draw drill



TWENTY-FOUR STEPS: USING TANGO PCB --10


symbols and thermal reliefs. Those are simple enough not to be
a problem.
I have written a program called PLOTPREP which will
create and assign apertures as needed. It is available from
Trace Engineering. The report-only version, which flags any
errors in aperture assignments (but doesn't create or assign
apertures), is free.
In general, do not create apertures with holes. They are
not necessary for board production, and can actually be
harmful. If you must use holes in apertures, make them
substantially smaller than the hole which will be drilled.

21. CHECK APERTURE ASSIGNMENTS.

Tango is weak in this area. There is no easy way to check
aperture assignments, and an incorrect assignment may lead to
bad film. The Aperture Report is not organized to make this
easy. Call Trace Engineering for information about how to get
a free copy of PLOTPREP to automate this process.

22. SET UP AND CREATE PLOT FILES

Most of my jobs use the same plot file definitions, so
this is pretty easy.
I enable the Board layer for all plots.
Wherever you have a choice, do not enable Pad/Via holes
for plots intended for actual board production. Even if your
apertures don't have holes, Tango will retract the traces
enough to keep the holes clear, and in some cases this can
create problems. If the apertures have full-size holes, or if
the pad is drawn with a hole, any fabrication misregister
could result in incomplete contact between the hole wall and
the pad.
I run the drill film first. Making sure that I have saved
all changes to the board, I then delete a block containing the
drill pads (those extra pads outside the board outline
mentioned above), and run all the other films. I can then undo
the block delete, just to be sure I don't accidentally save
the file without the drill block.
I also run an Aperture Report at this time.
You may wish to preview the files using File Load
Photoplots, or one of the other viewing programs (Graphicode
Prevue is free).

23. ARCHIVE AND TRANSMIT PLOT FILES.

I archive, using PKZIP, all the plot files, together with
the Aperture Report, and send the archive by modem to my
photoplotters. At this point I am pretty confident about the
films; they generally go directly to the fabricators from the
photoplotters. But for a large run, it might be prudent to
look over the films first....


TWENTY-FOUR STEPS: USING TANGO PCB --11


24. ARCHIVE AND SAVE ALL RELEVANT FILES.

Beside the files which went to the photoplotters, I also
keep, as a separate archive, the following files:
(a) the Net List
(b) Schematic files, if any
(c) the .PCB file, of course
(d) PCB.INI and PCB.DFN
The last ones are often overlooked, but PCB.DFN is
especially important, for it contains all the aperture
definitions used to make the plot files, as well as the plot
file definitions. PCB.INI refers to the libraries used for
component placement, and also contains the display setup.

HOW TO GENERATE AN EXTERNAL GROUND PLANE.

There are several utilities which will do this for you,
available through Trace Engineering. But I am going to
describe how to do it without the utilities.
I am going to assume that the plane is a top side plane,
and that there are other non-ground traces also on the top
side.
Route the ground as you would any other signal. I use a
24-mil trace, and I try to cross over the pad rather than
terminating the trace at the pad. This trace will later
provide the actual connections to the ground plane. It is
better for the solderability of the pads if there are two ties
for each pad at 135 or 180 degrees from each other.
You may then run DRC on the board, as if it had no ground
plane.
When you are all done with the design, and have made the
regular plots, including the top side MYBOARD.TOP, save the
board file. Then run Nets Hilite on the ground net, then
Delete Hilite. You may save the resulting file, calling it
BLOWOUT.PCB. Make a photoplot file of the top side; presumably
it will be called BLOWOUT.TOP.
Assuming you want 15 mil clearance on the ground plane,
instruct the photoplotter to plot BLOWOUT.TOP as a negative,
with apertures 30 mils larger in X and Y dimensions than those
for the other files; and then to merge it with MYBOARD.TOP as
a positive.
The result will be a perfect ground plane with no
isolated sections. All pads and traces other than the ground
trace will be relieved from the plane by 15 mils. The grounded
pads will be tied to the plane by the ground trace. Any vias
in the ground net will be solidly connected to the ground
plane, with no thermal relief, which is fine for vias. The
only problem with this procedure is that there may be pieces
of unconnected plane here and there, a problem in RF designs.
There are ways to make planes so that the results may be
previewed and edited before plotting. Ask about our utilities
which support this.
This procedure can also be used to produce split internal
planes.