On Thu, Oct 14, 2004 at 10:04:39AM +0100, David SMITH wrote:
> On Thu, Oct 14, 2004 at 10:50:34AM +0200, Wojciech Kazubski wrote:
> > > It looks pretty good, but while enjoying the enclosed popcorn, I noticed
> > > that the TO-220 hole size seems a little small. 0.020" for a pin that is
> > > about 0.060" wide.
> >
> > This may come from old times and be done by someone drilling pcbs himself.
> > In this case it is convinent to have all drill holes reduced to 15-20mils to
> > act as a guide for manual drilling.
> >
> > Better idea would be an option to reduce drill to that value when creating
> > postscript printout. I think it should be easy to implement, just force the
> > drill size to specified value when parsing the file for postscript output.
> > I think that PCB should not forget about those who want to make simple boards
> > at home.
>
> Some (most) PCB packages have different parameters to specify the drill size
> and the centre hole. This way, the Excellon drill file has the correct
> sizes in, and the person drilling the hole can still have a small guide hole.
I send the manufacturer the Excellon file and tell them that the holes in
the files are the final required inner diameter of the hole.
It's their job to computer their plating constants into drill size ;-)
This is the accompanying README that is a part of twister.zip:
Printed circuit board manufacture request
=========================================
Name Ronja Twister version 20040408
Constr. class 4
Shape Rectangle, middle of the outline that is present in
all layers
Width 4080 mil (103.632 mm)
Height 3280 mil (83.312 mm)
Layer file format Gerber RS 274X
Drill data format Excellon
Drill data meaning Diameter of resulting hole (not diameter of the drill)
Layers Two-layer through-plated, 2x soldermask, 1x silkscreen
Material FR4
Material thickness 1.5mm
Copper thickness 18um
Chirality All layers are presented as if viewed from component
side.
Copper polaroty Positive. Dark places in file mean copper.
Soldermask polarity Negative. Clear spaces in file mean mask matter.
Silkscreen polarity Positive. Dark places in file mean paint
Through-plating All holes are through-plated
Gold-plating None
Surface treatment Hot Air Levelling
Edge treatment Shearing
Testing Optical
Note: Gerber RS274 format means "Gerber RS-274X Format", defined in the year
1998 by company Barco Graphics N.V., Gent, Belgium (Barco ETS, Tramstraat 69,
B-9052 Gent, [EMAIL PROTECTED]), see
http://nexp.cs.pdx.edu/twiki-gerber/pub/Gerber/GerberFiles/rs274xrevd_e.pdf
File meaning
============
twister.pcb.output_back.gbr solder side - copper
twister.pcb.output_backmask.gbr solder side - soldermask
twister.pcb.output_fab.gbr drilling checkplan
twister.pcb.output_front.gbr component side - copper
twister.pcb.output_frontmask.gbr component side - soldermask
twister.pcb.output_frontsilk.gbr component side - silkscreen
twister.pcb.output_plated-drill.cnc drill data - throughplated holes
Views
-----
Views are in PostScript format and have only informal meaning to check
that the data have been interpreted correctly. They are not intended for
being exposed on a film.
twister.pcb.output_back.ps solder side - copper
twister.pcb.output_backmask.ps solder side - soldermask
twister.pcb.output_fab.ps drilling checkplan
twister.pcb.output_front.ps component side - copper
twister.pcb.output_frontmask.ps component side - soldermask
twister.pcb.output_frontsilk.ps component side - silkscreen
Cl<
>
> I don't know whether PCB does this.
>
> Also, the PCB package I use (not PCB I'm afraid...) uses square pads for
> TO220s, so the pad can still be reasonably-sized, yet not have pad-pad DRC
> problems.
>
> --
> David Smith Work Email: [EMAIL PROTECTED]
> STMicroelectronics Home Email: [EMAIL PROTECTED]
> Bristol, England GPG Key: 0xF13192F2
