[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]
Re: gEDA-user: new footprint guidelines
At 03:56 PM 9/30/2010, you wrote:
Rick Collins wrote:
This is just a 3 page list of the land pattern naming conventions.
This is not really the standard at all.
[snip]
I can send you this doc if you would like.
Yes, please
Ok, I'll send the attachment separately.
All PCB CAD systems I've seen display a layout with the positive
X to the left and positive Y to the top.
Till now I thought for 'pcb' X+ is to the right and Y+ is down -
and I still do.
This is/was the convention for scan-line oriented 2D graphics
display systems.
(0, 0) is in top left, X is right, Y is down.
If you have the positive Y axis down, your rotations will be
reversed from the standard... I think. Actually I have no idea how
to consider this. That may be a standard used for a "display
system", but nothing to do with PCB layout. As you say, go into
your CAD program and move the cursor around. I am pretty confident
it will give coordinates with the positive X to the right and
positive Y up. That is how all the Gerber file viewing programs do
it as well as the PCB layout packages I have seen. Are you telling
me PCB does it differently?
Will it really give you a Y coordinate for a part that increases as
the part is moved to the bottom of the screen?
It's dawning on me, that we are talking of different things:
the Gerber export probably (didn't check) has X+ -> right, Y+ -> top
as you say -
I was talking about the internal and screen coordinate sytem of "our" pcb.
Yeah, that wouldn't matter at all. It is just the position it
reports which should be indicated on the screen somewhere and you
select or move a part, no?
Of course. You have to give them assembly information to show how
to orient the board. Even then the XYRS file is not enough for them.
They have to figure out how to rotate the part from the feeder to
match your orientation. They don't trust standards. I'm sure that
is from experience.
An assembly house with some experience with a customer can mentally split
this rotation into two operations:
a) rotate from the feeder to a (house internal) standard orientation
This would actually be a machine reference.
b) rotate from the standard orientation to board placement
Yes, this requires they somehow relate your XYRS file and the board
position to the machine reference.
Where I want to get us, is being a consistent customer, for whom they
no longer need to think about step b).
From what I can tell, they don't bother with the two steps. The
machine picks the part from the feeder and before placing it, the
operator verifies it is oriented correctly. Done once for a given
feeder and a given side of your board, the rest of the parts from
that feeder should be good. This is 100% reliable and not really a
lot of time on their part. Even if they do the steps you are talking
about, they will do the step I have outlined. They aren't engineers
and they don't think like engineers. They don't want to figure out
what things don't work, they just want to make them work. Their way
is much easier in the long run I am sure.
Because you made me think twice, I just tested what pcb does with
some cursor movements,
looking at the coordinate counters. That's what makes the axes
obvious for me.
So what does PCB do?
See above / please check yourself.
I don't have PCB, so I can't check.
The parts are all designed to be soldered on a board, so they don't
have complete freedom to be "tumbled" unless you aren't planning to
assemble them. The fab house will know the top of the board is the
side you tell them on the assembly or fabrication drawing. Usually
it is not one of the long skinny sides, e.g. 0.062" wide. Are you
over-thinking this part?
Yes and No. The number of practical orientations a board and part
can have are very limited,
but to check them, until now a human will be involved. True
automation readines requires
that you can feed the file into the machine, the machine knows,
where it's fixtures are
and therefore will correctly transform design positions to machine
positions without
manual intervention. The operator just has to follow the rule,
that the (0, 0) marking
on the board (to be invented) "has to be at the fixture with the red dot".
Trouble is that the machine doesn't know how the parts are oriented
in the feeders. Rather than trust that the "system" works if they
get each piece right, they manually run through an sample of each
component type to make sure it is placed on the board right. That
is all they care about and you only do this once for a given
board. They call this "setup" and charge a couple of hundred
dollars for it. Not enough of a charge to worry about and it gives
them a warm fuzzy feeling that they aren't screwing up.
The assembly house I'm talking to, offers to provide standard parts.
I imagine,
they use a combination of machine vision and having resolved step a) from
above "once and forever" with their part suppliers.
When you say "parts", do you mean footprint data for the CAD
packages? They may use machine vision to eliminate the user for
some of this, but there is no "forever" in this industry. Parts can
come in tape reels, trays, tube and loose. The same part can be
available in three of these. Equivalent parts from different
suppliers can be supplied with different orientations.
The bottom line is, ask your assembler what they want. Don't assume
anything.
To help everyone involved, I include 'TOP' and 'BOT' in my
copyright notices, written
in copper. My current board isn't square, but then I could state,
that the baseline
of the copyright is parallel to X-axis in the XYRS file.
I'm sure they can use all the help they can get. Don't you provide
assembly drawings with TOP and BOTTOM in them? I've never had an
assembler not ask for a good drawing. As long as they know which
side is top and if the component locations are shown on a good
drawing, they can handle everything else the way they are
accustomed to doing it. I ask them what they want, not try to
figure out what they need. That is what I was doing when I got so
frustrated with the goofy standards.
Tbh, this is the first time I ever talked to an assemby house. I
want to provide them
data as good and consistent as I can, right from the start. To show them the
compoent locations I will provide the silk, solder-stop and
component layer as gerbers
accompanied by the XYRS file for placement, the paste-mask as starter
for their own. Do you think that's enough / too much?
What I have been asked for is an assembly drawing, clearly showing
pin 1 on each and every part, with the emphasis on "clearly". I've
had assemblers want to know how to orient right angle connectors even
though it is clear that they must point to the edge of the
board. (They were really trying to tell me I had pin 1 wrong because
the connector supplier put a pin 1 on their drawings and I used a
different pin 1.) If you give them a clear diagram for pin 1 of each
non-reversible part, I expect they will be very happy.
They also want a reference of the XYRS to partnumbers&sources, so they can
provide an offer with their own components (ev. cheaper because tape&reel
instead of cut tape) and need it anyway, if they use my provided material.
So I have to merge my part list (open office calc) with the xy-file from pcb.
That's why I think a "part" attribute known to gschem and pcb makes sense.
I am trying to get TinyCAD and FreePCB to pass all part data I choose
through the system so the XYRS and BOM files are produced at the end
when the Gerbers are produced. I'm getting push back about the size
of the netlist, etc. Right now it is a multi step process requiring
manual entry (re-entry actually) of data to make it all work and is
error prone.
About the .xy-file I'll have to read, how the footprint coordinates
and placement in the board influence the actual values. I think it
will be a bit tricky to check the footprints, since pcb doesn't show
the true coordinates but computes an offset on the fly to make all
screen coordinates positive - this is a bad idea for working on .fp-files.
That doesn't make a lot of sense to me, but I'm not sure why it is
bad. I use 0,0 as the lower left corner of the board and my fab
drawing gives coordinates of the fiducial marks on the board along
with major drill holes (like mounting points). So all coordinates on
the board are positive. Why would you want it different? I don't
know what a .fp file is.
BTW, all part coordinates should be wrt the centroid of the part, not
pin 1. Some CAD packages used to use pin 1, but it is standard
practice to use the package centroid now.
What sort of checking of the footprints do you want to do? You
should use a Gerber viewer to verify the Gerber files. Nothing
inside the CAD system matters if the Gerber files aren't right. What
would be great is a viewer that understands the part shapes and
positions the parts according to the XYRS file on top of the Gerber
file images so you can verify alignment and orientation.
Good luck!
Rick
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user