kicad-developers team mailing list archive

[Lorenzo Marcantonio <l.marcantonio@xxxxxxxxxxxx>]

On Sat, Nov 26, 2011 at 04:01:46AM -0700, Brian F. G. Bidulock wrote:

Read the notes document. Interesting stuff I think that some of them belong to the CAM world more than to the CAD; but maybe our manufacturing reality are different: for example here there is no plot-to-go for more than 2 layers, even a plain 4 layer is fabricator revised!

My comments: the NSMD technology is useful not only for BGA (which I don't
use:P) but for power SMD FETs too (these use pads that border on a zone
fill:D). I think that's our background is most different: you work on high
speed, I work on high power (50A per track and metal cores are not unusual
here...)

Teardrops an T-joins could be useful directly in the CAD, too, since they are
not process dependant. Track chamfering and mitering could be useful in
controlled impedance routing too (I have little experience with that, sorry,
our idea of *funny* tracks are 180um thick, 20mm wide ones --- there are
fabricators which do 6mm thick copper :D).

Unsupported and non-functional pad removal was one of the reason for which I
called for a copper mask for vias and pads (along with other DRC which you
righly requested).

Regarding complex pad shapes: aperture macros could be actually useful; the
problem is identifying the common subset: I never used DPF but, maybe, there
are some gerber features not available elsewhere and so on. In fact one of our
fabricator simply reject a gerber using AM for drawing thermals! Maybe their
CAM didn't support them correctly, I don't know. Anyway using multiple pads for
representing the drain of, say, a DirectFET drain is a PITA (you need to
connect all of them with bonding tracks *avoiding* cooling vias to satisfy
pcbnew DRC). BTW I have no idea of what the moire pattern could be used for
except for thermals:P

For this I think that the module format *must* be changed... if it's backward
compatible in reading I see no problem with that. Just add two new elements for
the 'aperture macro' and 'macro pad' and you're set, the euristics about
joining the same numbered pads IMHO are too complex and there's risk of d-code
number explosion; explicitly declaring a macro usage also would make easier to
maintain the module.

Comment about drill mark plotting (similar to the avoidance of AM for
thermals): some fabricators don't accept composite layers; you need a negative
subimage for drill marks and that would be rejected. At least I think everybody
now accepts polygonal fills, so we can junk the raster filled zones, at least.

Fiducial marks: in your country maybe you use SMEMA marks, our board marks are
different: circular 1mm pad, 2mm square mask *and* solder paste on the pad.
Don't ask me why, here in italy it seems to be the standard! I treat board
fiducials as modules, and local fiducials (when needed) as pads; a flag in the
pad structure could be useful maybe ("this is a fiducial"). BTW how are bad
fiducial used? they scratch them when a board is bad? bad boards in our panel
are simply marked with a blob of paint:P

Some feature requested, especially paneling, are clearly *not* belonging to a
CAD system... these are too dependant on the fabrication process. In fact, when
you have multiple board fabricator, you don't even enlarge solder mask, because
each of them has its rules concerning clearance and registration! Maybe
fabricators for ultrahighspeed boards are more specific in their specifications
but usually we're lucky if the copper deposit thickness is right:P:P Anyway I
concur that for board simulation you'll need to handle the track profile. Good
luck in finding the etchin parameters. Etch compensation IMHO pertain to a CAM
system, not to kicad. I'm a supporter of the unix philosophy: one program for
one thing; design with kicad, postprocess for fabrication with something else.
Otherwise we risk a bloaty beast. 

Isolation traces: I don't know about high speed design but I've been taught
that 'dead copper is bad'. When I do them I connect them to the appropriate
'shield potential'. It's not strange to have four or five different 'ground
potentials' on a board (and joining them is tricky). Anyway just handle them as
connected to some special net i.e. the disconnected net. And of course the same
is for isolation zones; question: could be some unrelated isolation so near to
be confused and so joined together? maybe just one isolation net is not enough.

Arced tracks and neck downs: useful, I agree (never had the need for an arced
track, beside).

Push-pull track: woot, the wondrous push/shove router:D:D Me want it:D

Solder dams, mask ganging and so one are strictly a CAM issue and shouldn't
belong to kicad. 

Embedded resistors: these could be used for thick film surface resistors, too!
Not laminated but dispensed, anyway the process is similar. No idea about the
computation, tough.

Venting/thieving: let them to the fabricator. An indication on where
vent/thieve can be useful (to avoid risking your precious ground shield:P).

Coupons: strictly fabrication features. Don't below to kicad since they depends
on *both* the fabricator and the assembler.

I read about your 'one tool to bind them all' section. Sorry, this industry
just don't work this way. You *have* to work with fabricators and assemblers.
One times we had to move a fiducials due to constraints in the pick and place
optics. Even if you send them enlarged masks they junk it and redo them (or at
least reject the production). As a board designer do your work, and let them do
their. Do you think you could know *all* of the quirks of their equipment? If
you need some specific guarantee (i.e. pressing tolerances) put them in written
on the fabrication layer and then send back the boards as defective if they
don't match. Design conservatively (i.e. try to absorb manufacturing tolerances)
If you have multiple suppliers of course it's even more difficult than that.

> The Eco, Comment and Drawing layers are simply as before.  Comment layer

I mean, not the layer name, but the layer *behaviour*. They all are simply
artwork layers. Same class different instance. 

> 258X expects the layer classes as laid out (except Eco and Comment).
> I didn't invent them.

Sorry, I don't know about 258X

> Another example, SolderPaste is not just a "pad-master", it is the solder
> paste stencil apertures, complete with stencil thickness considerations,
> bow-ties, D-shapes or homeplates; consideration for TFN and CGBA; paste
> in hole, etc.

Good luck on this, stencil are cut in a myriad of ways and every fabricator has its own rules. *They* need to fix stencil, you only need to tell them where the paste has to be put and how much of it. Laser cut, electroerosion or even paste dispensing... it's even different if paste is hand applied or machine applied, these are differences the designer can't cope with (because simply doesn't know)

> Contacts is for edge fingers, carbon contacts, tie bars for plating lines,
> etc.  These have additional rules so that they can be dipped or carbon
> deposit masks generated.

These also are manufacturing rules. Do you know the specifics of your manufacturer process?

> I already did Lavenir Format 2 (IPC-D-356) Lavenir Format 4 (IPC-D-356
> with NTD), IPC-D-356A and IPC-D-356B.  Also Barco DPF with netlist,
> Gencad, Gencam (IPC-2511A), GenCAM-XML (IPC-2411B) and 258X (IPC-2851).

I missed 356B... what's new regarding 356A?

> I also provided several classes of layer-sets.  Layersets are groups
> of substrate and copper in a buildup.  Layer set classes include:
> 
>   Laminate:- press cycle buildups.
>   Pth:- plate through holes (not necessarily through entire board, but
> 	through sub-lamminate).
>   Dcd:- Depth controlled drilling of outer layers of sublaminate.
>   HoleFill:- Hole filling from outer layers of sublaminate.
>   Laser:- Laser drilling from outer layers of sublaminate.
>   Backdrill:- Backdrilling of Pth for sublaminate.
>   Npth:- Non-plate-through holes in sublaminate.
>   Route:- edges, slots, wells, cutouts in sublaminate.

As before some of these are manufacturer dependant and don't belong to the cad: what about if the manufacturers prefer to laser drill (say) the 0,3 mm holes which you tought were mechanically drilled? just ask for the holes (finished hole *and* inner plating if needed), let them do their work and adjust for their process.

-- 
Lorenzo Marcantonio
Logos Srl