I will comment on a few of Mr. Bitanga's questions....

At 08:58 AM 11/10/98 +0000, Jay Bitanga wrote:
>2.  I am a quite confused with the use of the grid system...  Is
>there a general grid system for THT (100 mils ?!?) and
>SMT components ???  I use a general grid of 20 mils for pure THT
>designs (component placement and routing)... is that correct ???

Lots of design is done without any rigid grid system. With these designs, a
grid is chosen simply on the basis of convenience. It used to be that if a
board was going to be autoplaced, it was important for components to be
on-grid. I don't think that present equipment has any kind of requirement
like this. But certain kinds of automated test devices may require or
prefer that test points be on, say, a .100 grid. I have not done much
design for automated test, so I won't say more about that.

Now, as to placement. If one has components whose pads are on .100 centers,
and these components can be packed edge-to-edge, such as resistors, then it
makes sense to place them on .100 centers, or perhaps on some submultiple,
like .05 or .025. 0.020 is indeed a submultiple, but a more difficult one
to work with. I usually place components on .100 centers, then nudge some
of them to a .050 grid.

Now, if all component pads on a board are on a .100 grid, and for the sake
of example I will say that they are all 60 mil pads with 35 mil holes,
which might be typical for I.C.s and resistors, through-hole, an immediate
advantage for manual routing appears. One can swing a trace clear across
the board in a single segment and miss all the pads.

This is a powerful argument for having all of one's holes on a .100 grid.
When manually routing a through-hole board, I tend to put even small vias
on a .100 grid, reserving "off-grid" vias for places where they are needed.

But I do not route on a .100 grid, it is too limiting. The actual grid I
used depends on the density and technology of the board, which drive the
track width and air gap specifications. So for a old-style through-hole
board with one trace between pads, I would use a 12 mil traces, 12 mil air
gap minimum on a 25 mil grid, and for diagonal traces in tight places, I
would go down to a 12.5 mil grid, just where needed. Note that 12 + 12 =
24, not 25. The extra mil ends up as extra space between tracks.

If that same board has two traces between pins, I would use 8 mil track, 8
mil air gap. Note, however, that such traces, in between the IC pins I
described, are not on a regular grid. From pad center to pad edge is 30
mils, add 8 mils air gap and one-half a trace to the trace center, thats 42
mils. Then add another 16 mils to the center of the next trace, and that is
58 mils. and then there are another 42 mils to the next pad.

In Tango PCB for DOS, my old companion who seems to be teetering on the
edge of retirement, one of the grid options was "8.3". Since the Tango
database was a 1 mil database, this was not really an 8.3 grid; rather, the
actual place positions were rounded off. But the result was that one could
put those 8 mil traces right on 42 mils and 58 mils, add some multiple of
100 mils. Once again, a powerful argument for having pads on grid.

Now I'm using Protel 98. I wish that they would have a grid command that
was a true fractional grid with round-off. It would be stated as grids per
inch; what I want is 120 grids per inch. I could use an 8.333 mil grid, but
this would produce design rule violations unless I pull down the track
size, the air gap, or the pad size.

But there are other grid systems that work. A 20 mil grid allows one to
place traces, in the above scenario, at 40 mils and 60 mils. These traces
can be 10 mil traces. But the I.C. pads have to come down to 50 mils. I
don't like that; I'd rather have a larger annular ring, so I don't use
those parameters. In fact, some connectors will need 40 mil holes. It's
already a bit thin with a 60 mil pad, not to mention a 50 mil one.

But on a dense board, I might be using 15 mil holes with 25 or 30 mil via
pads anyway....

One possibility is routing on a 5 mil grid. Because most SMT components in
the libraries that I use have pads on a 5 mil grid and likewise the pads
are in multiples of 10 mils in dimension, a 5 mil routing grid works well.
And if the traces are taken down to 7 mils, one can maintain an 8 mil air
gap with the traces being on 15 mil centers. And two of these traces will
pass between two 57 mil pads on .100 centers. They would be at 40 and 55 or
at 45 and 60. If one wants to keep the pads at 60, one can go to a 2.5 mil
grid.

For purely manual routing, however, the smaller the grid the more tedious
the work.

But the more recent tools, like Protel 98, actually make it possible to
route with no grid (though a 1 mil grid is probably still a good idea, and
"no grid" really means -- for Protel -- a .001 mil grid). They do this by
providing immediate DRC and/or automatic obstacle avoidance, So one can
route a track hard up against the clearance specifications without the kind
of tedious work that previously would have been necessary.

But autorouters, mostly, even when they are supposedly "gridless," function
better with the component pads on a grid, and the coarser the grid, the
better, until it is the normal separation of pads, i.e., .100 or .050 for SMT.

>I havent started with SMT design coz' Im confused about using the
>routing grid for components... Can you give me a sample (very plain)
>of how to place then route the wires from the components...

I think I have explained that. I'd put most SMT components on a 50 mil
grid. I might do quite a bit of routing on a 25 mil grid and then pop down
to 5 mils for detail work. The 25 mil grid makes it easy to run traces
between SMT pads without any fuss, because the 8 mil traces will be either
on the pad or directly in between them....

>3.  Is the rigid board gonna be obsolete ?!? Just curious because of
>the technology rapidly growing...

No. Flexible circuits have a particular and fairly narrow application. For
most applications it is preferable that the board (or most of it, anyway)
be rigid. Sometimes we make boards thicker to gain even more rigidity.

>4.  Is the term single-sided PCB with 2 layers the same as
>double-sided ???

The first term does not exist. A single-sided board has copper on one side
only. Yes, the *board* has two sides. Haven't seen any moebius strips in
fiberglass and copper! "Single-side board is short for "single-side-copper
board." So, before one goes to what is called "multi-layer," there are two
kinds of boards: single-sided and double-sided. And most double-side
boards, except when they are made in someone's garage, are plated through,
that is, the hole walls have been plated to effect connections from one
side of the board to the other. There can be some exceptions, where it was
desired to save money by not plating through the board but the extra
strength of having pads on both sides of the board was desired. Such boards
require special design considerations....

> Is there a single sided board with an inner
>layer (ground or power) and is it different from double-sided ???

One never sees such an animal, because to make it would be just as
expensive as to make a true multilayer (4 layer) board. There are various
ways of making multilayer boards, but the minimal method is basically to
make 2 pc boards and laminate them together, then do the final drilling and
plating. I suppose that one could make a double-sided board and laminate it
to a single-sided board; it would cost almost as much as having two
double-sided boards. Consider that the fourth layer is free. Since it is
free, most designers would choose to use it.

I had a design recently which called for a multilayer board and where it
would have been very useful to have blind vias. But blind vias would have
raised the production cost too high. I suggested making this into,
effectively, a 3-layer board, that is a fully completed 2-layer board which
would then be partially glued to a one-sided board. This one-sided board
had no components on it, just a pattern which was a capacitative sensor.
Problem was that the sensor was large and severely restricted where vias
could be placed; this would have solved that problem. The customer did not
like the idea, so we made the usual four-layer board and I managed to get
it routed anyway.

>5.  I dont know how to calculate for the RF leakage,EMI. that sort of
>things ...Can you brief me on this...Pls. give a sample...

This is a *very* complex subject. There are fantastically expensive
programs which *might* do such a thing. Otherwise, one needs to learn the
basic rules. Perhaps someone else would be patient enough to explain them;
and there are some web sites with tips.

>6.  If I follow the IPC standards,  what is the reliability of my
>design ???

Better than if you don't, probably. Unless you really know what you are doing.

>7.  Isnt it that in IPC-D-275,  there are different routing
>techniques for analog and digital areas... Analog " power and ground
>traces placed last "  Digital " power and ground planes first "...
>Must that be followed always...  And how can I consider that this
>area is now the digital or analog area...  Does it also mean that I
>have  to separate, have different terminals, for the power and ground
>connections for analog and digital ???

See number 5....

I don't have a copy of D-275, but I can make a few comments about power and
ground. "digital" components are components which switch, often very
rapidly, between two discrete states. These two states represent "digits,"
usually 0 and 1, which explains the name. Such components are *relatively*
immune to noise, but they generate a lot of it. And they are not *totally*
immune to noise, one still needs to be careful about certain things.

"Analog" circuitry is circuitry where the level of a signal is important.
Consider a CMOS digital circuit; typically "0" would be 0 volts or ground,
and "1" would be 5 volts or VCC, power. In the digital circuit, 1 or maybe
2 volts would be, for the purposes of the circuit, the same as 0 volts.
Thus you can see why digital circuits are relatively noise immune. But in
an analog circuit with a 5 volt normal swing, a 1 volt noise level would
probably make the circuit completely useless. It you have a microphone,
going to an amplifier that merely makes the voltage swing produced by the
amplifier greater or gives it more drive current, and then a speaker
attached to the amplifier, this would be an example of an analog circuit.
And a little bit of noise could be quite annoying.

So in designing a board which has mixed analog and digital circuitry, one
places them on different areas of the board. I don't know about doing one
first or the other first, the sequence is not so important and might vary
depending on the design. But you do not want these two kinds of components
to share any space on the board, and you do not want to surround one kind
with the other.

Depending on the application, yes, you might need two separate power
"terminals," though it is common to have a single-point ground, that is,
one power supply, positive and ground, that serves both parts of the board,
and they connect to each other only at one point, typically next to the
main power bypass capacitor.

So if it is a multilayer board, one will split the planes and also not
allow digital copper to be coplanar (that is, parallel to) with analog
copper. So this means that both power and ground planes will be split, and
the splits will be reproduced on both planes. Except that for reasons of RF
noise, one will pull the power plane in some distance....

>8.  Is air gap and Trace spacing same ???

Well, trace-spacing equals air gap plus trace width, that is, this would be
center-to-center spacing. The space *between* the traces is the trace
air-gap. But air gap also refers to the space between any two conductive
objects on the board, such as trace-to-pad.

>I saw that for air gap
>measure is taken from end of trace to end of another trace... while
>in trace spacing, measure is taken from center to center of a trace,
>its like measuring its pitch...am I correct ???

Yes. Center-to-center trace spacing is the pitch.

>WHat will I follow ?

There is no substitute for knowing the capabilities of the fabrication
facility that will make the boards....

>9.  Are footprints for all PCB softwares the same (standardized) ???

No. But there are IPC standards which some people follow.

[log in to unmask]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433

################################################################
DesignerCouncil E-Mail Forum provided as a free service by IPC using LISTSERV 1.8c
################################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
To subscribe:   SUBSCRIBE DesignerCouncil <your full name>
To unsubscribe:   SIGNOFF DesignerCouncil 
################################################################
Please visit IPC's web site (http://www.ipc.org) "On-Line Services" section for additional information.
For technical support contact Hugo Scaramuzza at [log in to unmask] or 847-509-9700 ext.312
################################################################