Re: gEDA-user: anyone has had success with 0.2mm?
> What is the diameter of the drill helper? It's mindrill/2 so you can configure it through the DRC menu. What you really need is some formula or table that gives drill-specific diameters, since each drill is a different shape. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
DJ Delorie escreveu: > > That's what the drill helper *does*. > > But the copper is only 0.7 mil thick (1/2 oz) so a pin produces a much > deeper starter spot. What is the diameter of the drill helper? if it is too small, it will not help much. For what I know the drill has a flat region in the midle (the bigger ones have) I tested many helper diameters, if it is too small it will not help much, if it is too big the hole may start off center and cannot be corrected. Alain ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
DJ Delorie wrote: >> The hardest part is the 0.3mm vias in a drill press with no >> alignment aids. >> > > http://www.delorie.com/pcb/dremel-stand/ > > although the dremel shaft itself has about 6 mil of play in it. I've > tweaked the drill helper checkbox of the PS exporter to be more > suitable for this particular use; in addition, using a pushpin or > other sharp metal object, you can pre-poke the right spot and the > dremel will wander into it when you drill. > > I can reliably drill 13.5 mil vias with a 9 mil annulus. > > http://www.rejon.co.uk/manix_md1h.html Is the little guy I use. The 12K RPM is a bit low for 0.3mm but it is nice in terms of runout/wobble. I want to build my own spindle/BLDC one day when I have time so I can spin the bits and an appropriate speed. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
> I used another trick (some... time ago): make your copper with a > hole, That's what the drill helper *does*. But the copper is only 0.7 mil thick (1/2 oz) so a pin produces a much deeper starter spot. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
DJ Delorie escreveu: >> The hardest part is the 0.3mm vias in a drill press with no >> alignment aids. > > http://www.delorie.com/pcb/dremel-stand/ > > although the dremel shaft itself has about 6 mil of play in it. I've > tweaked the drill helper checkbox of the PS exporter to be more > suitable for this particular use; in addition, using a pushpin or > other sharp metal object, you can pre-poke the right spot and the > dremel will wander into it when you drill. > > I can reliably drill 13.5 mil vias with a 9 mil annulus. I used another trick (some... time ago): make your copper with a hole, that is, so thet the pad or via is a ring and it will "guide" the drill to the center automaticaly. It is like having a "pre-poke" !!! At the time I remember that the best results were achieved with the hole in the center of the pad half the size of the drill. I could accuratly use a 0.7mm drill with a shaft that had a few milimiters play in it! Alain ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
> The hardest part is the 0.3mm vias in a drill press with no > alignment aids. http://www.delorie.com/pcb/dremel-stand/ although the dremel shaft itself has about 6 mil of play in it. I've tweaked the drill helper checkbox of the PS exporter to be more suitable for this particular use; in addition, using a pushpin or other sharp metal object, you can pre-poke the right spot and the dremel will wander into it when you drill. I can reliably drill 13.5 mil vias with a 9 mil annulus. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
> Lope De Vega wrote: > > > I'm trying to build a circuit with a cp2102, which has > 0.5 mm between pins' center (actually 0.2mm between > pins). It is a qfn-28 package. > > I wanted to ask if anyone has had success with > something similiar? my workflow would be printing the > schematics as given by pcb in hq paper, and then > transferring them with the iron onto the pcb, as I > have't got any sort of specialized equipment, I'm just > a novice. > > Regards, > Not toner transfer but Kinsten brand thin substrate photo boards http://www.thehacktory.com/Simple-IR-RX-Prototype-V1p4-Top.jpg 0.45mm pitch 28pin QFN package with a exposed paddle. So it is quite doable at home. The hardest part is the 0.3mm vias in a drill press with no alignment aids. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
On Mon, Dec 03, 2007 at 11:24:36AM -0800, Dave N6NZ wrote: > > Randall Nortman wrote: > > The cheapest I've seen for 1 or 2 copies of a board with mask and > silkscreen is batchpcb.com, by the SparkFun guys. I've used them before. The board quality is top notch. If you need many of a small design or a very short run, they're good. $2.50/sq in becomes extremely expensive compared to the competition if your board gets too big, though. > if you back off to 8/8 > trace/space and 10 mil screen you will have lots of options for > prototyping services. The other thing to watch out for is min drill size. If you design for someone with a 15mil min drill and then have to adapt it to a fab with something larger (eg custompcb was 24mil, last I checked) you could be in big trouble. -- Ben Jackson AD7GD <[EMAIL PROTECTED]> http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
On Monday 03 December 2007 19:19:29 DJ Delorie wrote: > Is it time for another run of challenge boards? ;-) Maybe a home fab challenge. :) Peter -- Peter Brett Electronic Systems Engineer Integral Informatics Ltd signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
Randall Nortman wrote: > On Mon, Dec 03, 2007 at 10:07:23AM -0800, Lope De Vega wrote: >> I'm trying to build a circuit with a cp2102, which has >> 0.5 mm between pins' center (actually 0.2mm between >> pins). It is a qfn-28 package. > > I have never played with toner transfer schemes, Ditto for me... > had them professionally printed, > then I soldered the chips on by hand. I have done it both with a > toaster oven reflow process and with a plain old soldering iron. Same here. Toaster oven is great fun. For hand soldering, round up the *smallest* tip you can for your soldering iron. 1/64 diameter, for instance. Flux is your friend. > Having boards fabbed can be pretty cheap, especially if they're just > one or two layers, and especially if you don't want soldermask. It > was cheap enough that I skipped right past trying to etch boards > myself. Yes, having played in the soup many years ago, I'm perfectly happy not to do that part any more. I've use APCircuits, and PCBExpress.com (division of SunStone, not to be confused with expresspcb.com...) both with and without solder mask, and been very happy with the results. A friend swears by Olimex, I've never tried them. The cheapest I've seen for 1 or 2 copies of a board with mask and silkscreen is batchpcb.com, by the SparkFun guys. I currently have 4 designs sitting in "panelized" status, and I presume right now they are in the soup, or soon will be, someplace in China. I've never tried them before -- I'll post a report when they come back. Minimum order from batchpcb is one square inch -- your order costs $2.50 per square inch, plus $10 *order* set-up (not job set-up, so N designs in 1 order is still $10), plus shipping. You can only order *with* two sided mask and two sided silk. Anyway, at $2.50 per square inch, and a reasonable set-up charge, I can't get motivated to futz with toner transfer. PCBExpress will do 6/6 design rules in their prototype service, but if you back off to 8/8 trace/space and 10 mil screen you will have lots of options for prototyping services. Not to discourage you from trying toner transfer, of course :) I have to say, though, that I'd try it out on something less aggressive than a fine pitch part for the first go. -dave ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
> These days I do 4-layer boards mostly, so home etching is just not > an option anyway. Yes, it is: http://www.delorie.com/electronics/usb-gpio/ And yes, I think we've all agreed that I'm at least partly insane. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
On Mon, Dec 03, 2007 at 10:07:23AM -0800, Lope De Vega wrote: > I'm trying to build a circuit with a cp2102, which has > 0.5 mm between pins' center (actually 0.2mm between > pins). It is a qfn-28 package. Same spacing as QFP, which I've done successfully. I didn't try to toner-transfer it, though! I did have my soldermask ganged by the manufacturer but I was still able to put down a 208 pin QFP without bridges, just using lots of flux. I'm not sure how a home-etch board would fare. FT232R would be easier to put down, I think. -- Ben Jackson AD7GD <[EMAIL PROTECTED]> http://www.ben.com/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
> I wanted to ask if anyone has had success with something similiar? I've done 0.4mm pitch TQFP with toner transfer and a soldering iron. It takes some care, but it can be done. 0.5mm pitch is now "easy" for me. Note, however, that I use Pulsar's coated paper, which gives better results than plain paper, and a Metcal 0.02" conical tip in my iron. I also prefer to reflow SMT parts with a hotplate rather than hand iron them, although I've done it both ways. Is it time for another run of challenge boards? ;-) http://www.delorie.com/pcb/smd-challenge/ http://www.delorie.com/pcb/smd-challenge/old/proto-boards.html http://www.delorie.com/pcb/first.html ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: anyone has had success with 0.2mm?
On Mon, Dec 03, 2007 at 10:07:23AM -0800, Lope De Vega wrote: > > I'm trying to build a circuit with a cp2102, which has > 0.5 mm between pins' center (actually 0.2mm between > pins). It is a qfn-28 package. I have never played with toner transfer schemes, but I have done boards with 0.5mm pitch packages and had them professionally printed, then I soldered the chips on by hand. I have done it both with a toaster oven reflow process and with a plain old soldering iron. Each method has advantages and disadvantages, but it is doable. Whether or not you can do a toner transfer board with that kind of precision is another matter, and I'm sure DJ can say something about that. Having boards fabbed can be pretty cheap, especially if they're just one or two layers, and especially if you don't want soldermask. It was cheap enough that I skipped right past trying to etch boards myself. These days I do 4-layer boards mostly, so home etching is just not an option anyway. -- Randall ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: anyone has had success with 0.2mm?
Hello, I've been for a while using gschem and pcb though just for practice, I've never materialized anything with them, though now I'm willing to. I'm trying to build a circuit with a cp2102, which has 0.5 mm between pins' center (actually 0.2mm between pins). It is a qfn-28 package. I wanted to ask if anyone has had success with something similiar? my workflow would be printing the schematics as given by pcb in hq paper, and then transferring them with the iron onto the pcb, as I have't got any sort of specialized equipment, I'm just a novice. Regards, Get easy, one-click access to your favorites. Make Yahoo! your homepage. http://www.yahoo.com/r/hs ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
