nivek@rover.ri.cmu.edu (Kevin Dowling) (09/25/89)
We've been using McCadd, a schematic entry program, routing and layout package for the Macintosh. For output it can print on the Laserwriter (Postscript) so we can preview mask layouts. Reprographics places that generate artwork for PCB production usually use 'Gerber' formats however. McCadd does supply a Gerber translator for their product as do other PC layout programs on the market. From what I understand the Gerber format was first done by a PCB company that established this standard to communicate with these NC controlled X/Y tables that moves a little aperture wheel around and blinks a light on and off while tracing lines and pads out on a photo-sensitive surface. This has caused some headaches for us. We'd like to just ship a McCadd file off and forget about the rest but there are not great numbers of photoplot houses with all the right tools. "Just send us Gerber formats, or some HP format" is the usual response. With some work we can generate the Gerber formats and the drill tape... My questions are: Have there been proposed new formats for describing PC board layouts? Could postscript or PICT or some subset of these be used to generate layouts? Is Gerber good enough for the forseeable future? Since masks for PC production are just dark and light areas you can just 'paint' a board using a single small aperature and lots of time, but are there printers of high-resolution that can plot 1:1 masks on mylar directly? How about a system that could write on boards directly? (A PCB printer!) There has been a proliferation of PCB generation programs, there are several for the PC, a couple for the Mac, and other workstation based. Do all these generate Gerber formats? nivek Aka : Kevin Dowling Bell: (412) 268-8830 Arpa: nivek@rover.ri.cmu.edu Mail: Robotics Institute Carnegie Mellon University Pgh, PA 15213-3890
phil@ingr.com (Phil Johnson) (09/25/89)
In article <6261@pt.cs.cmu.edu> nivek@rover.ri.cmu.edu (Kevin Dowling) writes: > >(Postscript) so we can preview mask layouts. Reprographics places that >generate artwork for PCB production usually use 'Gerber' formats however. >McCadd does supply a Gerber translator for their product as do other PC >layout programs on the market. > You will find that all of the PC houses use the Gerber Photoplot format. The Gerber format is the industry accepted standard for photoplotting. It was originally developed by Gerber Scientic, who produced the first photoplotters for PCB generation. The format defines a specific aperature wheel, aperature, coordinates, and flash. The output of the photoplotter is the slicks for each signal, plane, drill, solder mask, silkscreen layers, and any other user defined layers. Any printed circuit board layout software that does not provide the ability to produce a Gerber tape is at best a "toy" system (toy system: a drawing package the claims to provide PCB layout capabilities). > >My questions are: Have there been proposed new formats for describing PC >board layouts? Could postscript or PICT or some subset of these be used to >generate layouts? Is Gerber good enough for the forseeable future? > The IPC-D-350B exchange file format that has been defined by the industry association for transfering PCB definition, You are fairly safe with the Gerber format. The PC houses are still in the transition phase of implementing the IPC-D-350B standard. If your software does not support the Gerber format and can not give you an availablity date for IPC-D-350B, then I recommend you find a real PCB layout package. "NO ONE" would want to pay the cost for photoplotting in postscript and PICT has limited platform support and is inferior to Gerber or 350B. >Since masks for PC production are just dark and light areas you can just >'paint' a board using a single small aperature and lots of time, but are An aperature wheel contains more than various sizes of "dots". An aperature wheel contains various size dots for plotting traces and areas. Also, there are aperatures for pads, vias, and other special symbols as define by the user. Rather than "painting the fill area between the inner circle and the outer circle of a pad" as you purpose the correct pad aperature is flashed. Your method compared to the aperature method is about a factor of 10 to 20 time slower. Multiply that by the number of pads, holes, and vias that you have on a normal board and you could end up plotting a board for days. >there printers of high-resolution that can plot 1:1 masks on mylar directly? >How about a system that could write on boards directly? (A PCB printer!) > The resolution needed is determined by the density of the PC layout. If you are laying out a PCB using a 0.1 inch grid then a 300 dpi laser printer should be sufficient for your needs. If you are using a finer grid and doing layouts such as multiple traces between pads you will need a 1200 or 2400 dpi laser printer. Most PCB houses should take your slicks for use in producing the PCBs, but NOT guarantee the boards. This is because they do not have control over the quality and registration of the slicks. I have seen a board prototyping system the "routers" the board. Routering actually uses a router bit to remove copper plate form the board. I don't remember the name of the company who sells it though. >There has been a proliferation of PCB generation programs, there are several >for the PC, a couple for the Mac, and other workstation based. Do all these >generate Gerber formats? Every "REAL" (real is defined as production quality) PCB layout package that I have seen provides a Gerber format output. I appologize if I sound somewhat condesending, but I have dealt with this same situation many times as an Application Analysis for electronic design at Intergraph Corp. I have seen many users buy a "CAD" system that "provides" PCB layout capabilities. In reality, layout is only one facet of PCB design. If your package does not output industry accepted or standard formats it is difficult to produce the board and a picture on a computer screen IS NOT a printed circuit board. -- Philip E. Johnson UUCP: usenet!ingr!b3!sys_7a!phil MY words, VOICE: (205) 772-2497 MY opinion!
henry@utzoo.uucp (Henry Spencer) (09/26/89)
In article <6564@ingr.com> phil@ingr.UUCP (Phil Johnson) writes: >You will find that all of the PC houses use the Gerber Photoplot format. The >Gerber format is the industry accepted standard for photoplotting... Out of curiosity, is the Gerber format *documented* anywhere, or is it one of these "well, you know what I mean" formats where it is assumed that everyone with any interest already knows how it works? -- "Where is D.D. Harriman now, | Henry Spencer at U of Toronto Zoology when we really *need* him?" | uunet!attcan!utzoo!henry henry@zoo.toronto.edu
phil@ingr.com (Phil Johnson) (09/28/89)
In article <1989Sep26.154248.15220@utzoo.uucp> henry@utzoo.uucp (Henry Spencer) writes: >Out of curiosity, is the Gerber format *documented* anywhere, or is it one >of these "well, you know what I mean" formats where it is assumed that >everyone with any interest already knows how it works? I have checked since my posting and found that the Gerber Photoplotting File Format is specified in the MIL-SPEC-RS274 document. You should be able to get a copy from a local photoplotter sales office, such as Optronics or Scitec. The Gerber photoplotters were based on flash tube type technology. The trend has moved toward the laser-based technology, so that photoplot time and quality can be more predicted (You don't have to continually calculate the remaining useful life of the flash tube). The technology doesn't matter, in that the Gerber format is considered THE PCB photoplotting format. Each photoplotter manufacturer will probably add extensions that take advantage of special features of their models, but you should be very safe with the vanilla Gerber format. To paraphrase Julia Childs: " Bon Aperature" -- Philip E. Johnson UUCP: usenet!ingr!b3!sys_7a!phil MY words, VOICE: (205) 772-2497 MY opinion!