Re: gEDA-user: Board fabrication
> Wow, it's already there! The circles seem small -- is starting with > a small drill , then using a large one the recommended way to use > this pcb feature? The theory is that drill runout is a fixed amount, so larger drills wouldn't need a physical helper, just a visual target, because presumably they'd have more copper around them so precision isn't as neccessary. Smaller holes are more critical about placement, and then the target is closer to the drill tip size. The helper should guide the tip, but you shouldn't need to use multiple sizes. Twist drill bits should come to some sort of a point. For larger holes, brad point drills have a small point that works well with the helpers. I'm open to suggestions though. > I had to use export to ps to see it... That's what I always do. I use gv to preview them, and select which pages to print. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication
Wow, it's already there! The circles seem small -- is starting with a small drill , then using a large one the recommended way to use this pcb feature? I had to use export to ps to see it... When I used print layout as the pcb manual suggests, there was no to-file option, (lesstif compile), and when sent to a pdf converter (CUPS) the result was a very short pdf file -- See below: John G == DJ Delorie wrote: a concentric circle of copper to aim the drill bit in and keep it from walking away from the center of the larger via or mounting hole would be helpful. Have you tried the "drill helper" option? = %PDF-1.4 %Çì¢ 4 0 obj <> >> endobj 3 0 obj << /Type /Pages /Kids [ 4 0 R ] /Count 1 >> endobj 1 0 obj <> endobj 2 0 obj <>endobj xref 0 5 00 65535 f 000172 0 n 000220 0 n 000113 0 n 15 0 n trailer << /Size 5 /Root 1 0 R /Info 2 0 R /ID [(¡F¡\r9\n\\í"áç)(¡F¡\r9\n\\í"áç)] >> startxref 331 %%EOF ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication
Wojciech Kazubski wrote: Current "dril helper" option is not usefull since a black dot in the center creates a bump which will drive a drill bit off the pad/via center. It is a small circle in the current lesstif version of PCB... Very small -- did you zoom in? John G ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication
> Current "dril helper" option is not usefull since a black dot in the > center creates a bump which will drive a drill bit off the pad/via > center. The current drill helper leaves a ring, not a dot. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication
> > What if we made a via shape for ease of non-automated drilling, (for > > prototyping)? I think a concentric circle of copper to aim the > > drill bit in and keep it from walking away from the center of the > > larger via or mounting hole would be helpful. > > Have you tried the "drill helper" option? > If I remember well, in PCB gerber output had vias and pads filled, while PS output had full size holes "printed" in white inside vias and pads, just to see how the finished board will look like. Some people however have problem with gerber interpreters or make masks at printing shops that have no gerber interpreters, so having the option to produce postscript without holes would be good for them. For manual drilling (and homebrew laser print transfer technology) etched holes in pads may work as helpers for drilling. In such case it is best to have all drills reduced to some 10-20mils, just enough to put the drill bit in. Current "dril helper" option is not usefull since a black dot in the center creates a bump which will drive a drill bit off the pad/via center. Better option woud be a control over the drill size on printout. Small white circle will create a pit which is good guide for drilling. Implementing this should be relatively easy, simply ignore the real drill size read from internal data and replace it with 0 or a specified value (15mils?) when converting the board into ps. Wojciech Kazubski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication
> What if we made a via shape for ease of non-automated drilling, (for > prototyping)? I think a concentric circle of copper to aim the > drill bit in and keep it from walking away from the center of the > larger via or mounting hole would be helpful. Have you tried the "drill helper" option? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication
John Griessen wrote: What if we made a via shape for ease of non-automated drilling, (for prototyping)? I think a concentric circle of copper to aim the drill bit in and keep it from walking away from the center of the larger via or mounting hole would be helpful. I've used small vias w/ blown-up pads to center drill holes. you have to drill some copper, but using hs drills it doesn't seems to be a problem. Luciani has an approach to this and a lot of his parts have a cross for drill alignment of bigger holes. I have worked on some old electronics that were hand-built and it's clear that they center punched on crosses to get drills lined up. Nice as it sounds, I don't think pcb will let you put a via inside a via and still generate output. phil ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Board fabrication
What if we made a via shape for ease of non-automated drilling, (for prototyping)? I think a concentric circle of copper to aim the drill bit in and keep it from walking away from the center of the larger via or mounting hole would be helpful. Anyone else? The concept is just a smaller via on top of a larger one, and with no drc impact and no pin number -- best handled directly by pcb code...as one object rather than stacking two on each other though... John G ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication -- outline
Em Ter 10 Out 2006 09:52, John Luciani escreveu: > On 10/10/06, Stefan Salewski <[EMAIL PROTECTED]> wrote: > > My questions: > > What is the right way to generate the outline for the board > > producer? My vendor asks for a 10 mils line around the board. IN THEORY he cuts the board exactly in the inner edge of that line, so the line does not appear on the board when it is ready, but he never do it. So, it is important to never touch any lines or pins or anything else that can made a short circuit. > > Should I rename the gerber files? (I think name of > > board.group0.gbr should be board.front.gbr, this name was used > > in pcb documentation) Yes, to my vendor it is only important to make the name clear. Fortunatelly pcb 20050830 still names the layers as bottom and top, so I dont have to change any names, except for the plated holes because my vendor does not know what a unplatted hole are :) > > Should I send all .gbr and .cnc files to board fabricator? Send him the files that are necessary, like bottom, top, frontsilk, frontmask, bottommask, etc. > > Is it necessary to send more informations to board fabricator? I allways to say how much important is to have that board on time, or as soon as possible (sometimes I have to implore with knees, when that doesnt work, I offer to pay double...) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication -- outline
Stefan, A quick way to get results is to manually "draw" the board outline on an empty layer you rename "outline": This is inelegant, but quick error-free. It requires absolutely no programming. If "outline" doesn't sound like a good name to your vendor, you can easily change it. Layer(7 "outline") ( Line[10 30 10 10 1000 2000 0x0004] Line[40 10 40 30 1000 2000 0x0004] Line[40 30 10 30 1000 2000 0x0004] Line[10 10 40 10 1000 2000 0x0004] ) In Gerbv, you'll be able to load a layer with just these four lines. It's probably good if the corners hit exactly the same point so as not to confuse your board-house's software. phil ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication -- outline
Outlines should be drawn with lines on their own "outline"[*] layer. It should be in its own layer group. Most fabs want 10 mil lines, but they all seem to use the centerline of the lines as the actual outline. The CVS version of pcb has a patch that omits the pins and vias from the gerber and postscript files for that layer, as long as the layer is named "outline"[*] and it's the only layer in its group. The exported file for that layer will be called "outline" instead of being named as if it's a copper group. [*] It can be named "outline" or "route" but IMHO route is more confusing, especially when you're running the autorouter ;-) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Board fabrication -- outline
On 10/10/06, Stefan Salewski <[EMAIL PROTECTED]> wrote: My questions: What is the right way to generate the outline for the board producer? This depends on the manufacturer. I use PCB Express and they request a 1mil copper line on the top layer. I usually add this line after I complete the layout. Should I rename the gerber files? (I think name of board.group0.gbr should be board.front.gbr, this name was used in pcb documentation) I have a script that renames the files for the PCB Express conventions which are --- # File extensions # Layer #1 = .top # Layer #2 = .l2(or .bot if only 2 layers) # Layer #3 = .l3 # Layer #4 = .l4(or .bot if only 4 layers) # Layer #5 = .l5 # Layer #6 = .bot # Topside Silkscreen = .slk # Bottom Silkscreen = .bsk # Top Soldermask= .smt # Bottom Soldermask = .smb # NC Drill File = .dri (combined plated and unplated holes) Should I send all .gbr and .cnc files to board fabricator? One gerber file for each copper layer, top and bottom mask file, top and bottom silkscreen file and the drill file (or files) Is it necessary to send more informations to board fabricator? It depends on the manufacturer. You may need to specifiy board thickness, ounces of copper, etc. For the low price vendors these are usually part of the package price. (* jcl *) -- http://www.luciani.org ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Board fabrication -- outline
Hello, I have finished my first board using gEDA and will now sent gerber files to my board manufacturer. I will send data to www.bilex-lp.com, because they are cheap and accepting gerber files. (They seem to have only a homepage in german language) The last two steps i have to do is to create a correct outline of my board and choose filesnames in a way people at www.bilex-lp.com will understand. I have two small boards (b1.pcb and b2.pcb) which i put together using "File->Load layout data to paste buffer" to file board.pcb. To get the outline, I added a new layer to this file called "outline" and draw the outline rectangle in this layer. I was not sure if I have to use a separate layer group for this outline layer. If i do not use a separate group, then the outline rectangle is drawn with copper. So I tried a separate group, but then gerber export produces an additional file ( board.group2.gbr) which contains not only the outline but other elements too. Here is the filelist generated by gerber export (pcb version 20060822): b1.pcb b2.pcb board.backmask.gbr board.fab.gbr board.frontmask.gbr board.frontpaste.gbr board.frontsilk.gbr board.group0.gbr board.group1.gbr board.group2.gbr board.pcb board.plated-drill.cnc board.unplated-drill.cnc These files are available at http://www.ssalewski.de/board.tar.gz My questions: What is the right way to generate the outline for the board producer? Should I rename the gerber files? (I think name of board.group0.gbr should be board.front.gbr, this name was used in pcb documentation) Should I send all .gbr and .cnc files to board fabricator? Is it necessary to send more informations to board fabricator? Thanks Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
