kicad-developers team mailing list archive

[Alex G <mr.nuke.me@xxxxxxxxx>]

-----BEGIN PGP SIGNED MESSAGE-----
Hash: SHA1

On 08/30/2010 07:39 PM, Lorenzo Marcantonio wrote:
> On Mon, 30 Aug 2010, Alex G wrote:
> 
>> Thanks again. It's a pretty handy tool, I must admit.
>>
>> Ok, so for an M3 washer it yields:
>> 7.3mm pad for 3.1mm hole (tight fit) with 7.6mm courtyard
>> 7.7mm pad for 3.5mm hole (loose fit) with 8.0mm courtyard
>> Interpolating, I guess it should be
>> 7.4mm pad for 3.2mm hole with 7.7mm courtyard
>>
>> Courtyard is defined as:
>>> The area that provides an electrical and mechanical clearance around
>>> the component body and land pattern boundaries.
>>
>> So I'm assuming this means "don't put any tracks in that zone". I'm not
>> sure, but I think kicad allows setting pad clearances that are different
>> than the net values.
> 
> No, it's keep that area free of exposed stuff. Tracks under solder mask
> can go there, exposed track or mechanical stuff don't. Also the
> courtyard is strictly rectangular. The underlying idea is that courtyard
> is needed for tooling (hot air nozzles, BGA reworkers and so on).
> 
But, we may take the size of the courtyard and draw a circle on the
silkscreen. This would help with positioning footprints such as mounting
holes. Not exactly standard-ish, but should help kicad users understand
not to put anything else there.

> Since you're not tooling a single hole, just disregard the courtyard.
> Electrical clearance isn't stated by IPC but depends on your process
> *and* on the voltages running on the pad (look around the net for
> creepage and insulation for details, for SELV work it doesn't apply
> anyway).
> 
Well of course, if the net clearance is larger than the clearance of the
pad, then kicad should take the larger clearance.

(NOTE TO CODE-WRITERS: if this is not the case, it must be.)

So if you have a 700V line, you will most likely put it in a net class
with huge clearance, and kicad will take care of you (at least it _should_).

>> While the tool allows for calculating land patterns for screw heads and
>> washers, there's no option for nuts (no pun intended).
> 
> Nuts are like washers since you need the space for the wrench:D At
> least, that's my theory. More than one time I had to change the layout
> because the board couldn't be fixed (typical issue: a big capacitor in
> the wrench travel area and no other way to turn it).
> 
Back in the days when I was using 1PIN as mounting holes, I had a
nut-shaped spacer (no pun intended) short out an LED I placed too close,
so I know what you mean.

>> Going back to our DSUB connectors with 3.2 mm mounting holes, I guess
>> this means a 7.4mm pad with a minimum clearance of 0.15mm.
>> Lorenzo, I'm expecting a confirmation or a "you got it totally wrong you
>> idiot!!!" . :-p
> 
> Your clearance is for a 6mil process (the default for the IPC
> calculator); nothing esoteric but if I can I prefer an 8mil process
> (0,2mm) since it's cheaper for mass production; also 6mil isn't done by
> some 'hobby' manufacturer... I don't know your library standard, just
> try to be consistent.
> 
Personally, it's 0.25mm clearance, and the smallest track I ever did was
0.4mm. This with a 1200dpi printer, UV LED's for exposure, and Bungard
pre-sensitized boards. I don't know what process Oyvind had in mind when
designing the footprints, but this is definitely an interesting point to
consider. So for an 8mil, it should be a 7.4mm pad with 0.2mm clearance,
right?

> In our experience with an 8mil process and 0,4mm vias you can do most
> stuff included 0,5 pitch TQFP and some VQFN. For BGA work I'd require
> 6mil (or 4mil, depending on how much pin you need to fan out:D). IIRC
> 4mil is the limit for 'standard' processing (at a premium rate,
> anyway!).
> 
Jurgen Bungard (the big boss of Bungard) told me in an email that their
pre-sensitized boards can go down to 1 mil. I don't know if any
manufacturer actually supports this. For me the problem is the artwork.
I daren't go below 0.25mm tracks of fear that imperfections will eat
away the track.
Anyway, back to the point, for a component such as a DSUB connector, it
makes sense to consider an 8mil process, while for other finer-pitch
components, we have no choice but to go lower than that.

> 3.2mm is the correct hole for a M3 screw and 7,4mm seems fine for
> a washer pad (the washer itself is 7mm, BTW). So yes, I agree with your
> data.
> 
Thank you!
Oyvind, we might want to increase the pad size of the DSUB connectors to
7.4mm.

> As a bonus here is a production tested HDE15 female, right angle dsub
> (done from Tyco specs IIRC). Since it's a snapon boardlock, so no special
> handling for fixing screws, only a hole.
> 
> $MODULE HDE15-F-RA
> Po 11811 49213 0 15 4BD826B3 4BD826BF ~~
> Li HDE15-F-RA
> Cd High-Density D-Sub, 15-poles, Right Angle
> Sc 4BD826BF
> AR Op 0 0 0
> T0 0 0 394 394 0 39 N V 21 N"HDE15-F-RA"
> T1 0 0 394 394 0 39 N I 21 N"HDE15-F-RA"
> DS -5866 0 -5866 2362 60 21
> DS -5866 2362 -3976 2362 60 21
> DS -3976 2362 -3976 0 60 21
> DS 3996 0 3996 2362 60 21
> DS 3996 2362 5866 2362 60 21
> DS 5866 0 5866 2362 60 21
> DS 6142 0 -6142 0 60 21
> DS -6142 0 -6142 -6417 60 21
> DS -6142 -6417 6142 -6417 60 21
> DS 6142 -6417 6142 0 60 21
> DS 3248 2362 3248 0 60 21
> DS -3248 2362 -3248 0 60 21
> DS 3248 2362 -3248 2362 60 21
> $PAD
> Sh "" C 1260 1260 0 0 0
> Dr 1260 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 4921 -3504
> $EndPAD
> $PAD
> Sh "" C 1260 1260 0 0 0
> Dr 1260 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -4921 -3504
> $EndPAD
> $PAD
> Sh "6" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 2150 -3504
> $EndPAD
> $PAD
> Sh "7" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 1248 -3504
> $EndPAD
> $PAD
> Sh "8" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 346 -3504
> $EndPAD
> $PAD
> Sh "9" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -555 -3504
> $EndPAD
> $PAD
> Sh "10" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -1457 -3504
> $EndPAD
> $PAD
> Sh "1" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 1697 -4504
> $EndPAD
> $PAD
> Sh "2" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 799 -4504
> $EndPAD
> $PAD
> Sh "3" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -102 -4504
> $EndPAD
> $PAD
> Sh "4" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -1004 -4504
> $EndPAD
> $PAD
> Sh "5" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -1906 -4504
> $EndPAD
> $PAD
> Sh "11" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 1701 -2504
> $EndPAD
> $PAD
> Sh "12" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po 799 -2504
> $EndPAD
> $PAD
> Sh "13" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -102 -2504
> $EndPAD
> $PAD
> Sh "14" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -1004 -2504
> $EndPAD
> $PAD
> Sh "15" C 709 709 0 0 0
> Dr 472 0 0
> At STD N 00E0FFFF
> Ne 0 ""
> Po -1906 -2504
> $EndPAD
> $EndMODULE  HDE15-F-RA
> 
Time to try my skills at cut'n'pastin' components into libraries.

Alex

-----BEGIN PGP SIGNATURE-----
Version: GnuPG v1.4.10 (GNU/Linux)
Comment: Using GnuPG with Fedora - http://enigmail.mozdev.org/
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=s0uZ
-----END PGP SIGNATURE-----