[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, Dan Andersson [EMAIL PROTECTED] wrote: On Thursday 24 April 2008 20:26:28 sadkra wrote: Hello Everyone, I just finished my first sch-pcb project in Kicad. I tried to output the pcb in Postscript format. When I looked carefully at the Postscript file, I found that some of the pads are missing /or some pads are only half drawn in bottom-copper layer while bottom-copper mask shows the complete pad-mask. I may add that gerber output of the same pcb is fine without any problems. It will be of great help if someone throws any light on this. regards, sam_des The postscript output is NOT for PCB making!!! If you need Postscript for PCB making, use a Gerber Viewer and make a Postscript output from it. You can't trust anything but the Gerber file. //Dan, M0DFI No question, Gerber is mandatory when getting PCBs professionally manufactured. However, if you only want to hand make some prototypes or even for us hobbyists, PS output to a reasonable laser printer is useful. It gives an easy option of using toner-transfer products such as press-n-peel which is perfectly reasonable for simple layouts. FWIW, I also noticed the PS rendering problem with the RCA connector footprint here: http://www.cfdev.fr/KicadContrib/Foot/RCA.emp.zip because it has 'oval' pads (this is a parameter/setting in the library component editor BTW). In my case I had 4 of these parts in my design and only one printed correctly (the 'last' one placed). Chris.
[kicad-users] Re: Postscript Output
Hello, Just today I finally decided to forward my layout to my PCB manufacturer. I went to him personally to see what he has to say about oblong holes(or slots) in my layout. He checked my drill file with the software he uses with his CNC machine oblong holes all came correctly, atleast on PC. He didn't tell me what software he uses for his cnc or even which cnc he uses. Don't know why !! Let's see what I get on board, that's about 12 days. BTW, I also ran Pulsonix demo yesterday and it's Gerber output shows the holes(actual size or just a tiny dot). Can't we get such gerber with kicad ? For hand-drilling low quntity boards, it is useful to have these marks to easily locate center of the pad. Hope to see this thing implemeneted in kicad. I also wanted to add the I tried Pulsonix, Zuken in last couple of weeks I must say I am glad to stay with Kicad. thanks, sam_des
[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, Rick Collins [EMAIL PROTECTED] wrote: I'm not sure what you are asking about. I have never seen oblong holes in a board. Are you talking about a routed slot? When you produce gerber files, how are the oblong holes defined? Regular holes are defined in a drill file typically in the Excellon format. In what output file are your oblong holes defined? Hello, Some components do have non-circular leads such as Power Relays, Fuse Holders, Fuses etc. You can check the Gerber section in Kicad help, there is topic about rectangular holes. Also you can check Pad properties of any pad in kicad. BTW, these holes are defined in drill file only. Here is what my drill file drill report file says, -drl.rpt - T2 0.032 0.81mm (19 holes) T3 0.035 0.90mm (426 holes) (with 8 oblongs) T4 0.039 1.00mm (14 holes) .drl --- T3 X1.050Y-5.250G85X1.050Y-5.050 G05 X1.050Y-4.857G85X1.050Y-4.656 G05 X1.300Y-5.250G85X1.300Y-5.050 G05 X1.300Y-4.857G85X1.300Y-4.656 G05 X1.800Y-5.250G85X1.800Y-5.050 G05 X1.800Y-4.857G85X1.800Y-4.656 G05 X1.550Y-5.250G85X1.550Y-5.050 G05 X1.550Y-4.857G85X1.550Y-4.656 G05 T4 Well, I loaded the file in GerbView 6 all I can see a single hole. That was the reason I tried Postscript output. My ancient BoardMaker for DOS also supports such rectangular holes as standard pad type. But most modern layout softs doesnot allow this !? I have circumvented this problem(Eagle) by placing overlapping holes on a single pad thus creating rectangular hole. Since kicad does not allow this it does supports the non-circular holes I tried it. I just wanted to cross-check the output! regards, sam_des
Re: [kicad-users] Re: Postscript Output
Well, I loaded the file in GerbView 6 all I can see a single hole. That was the reason I tried Postscript output. My ancient BoardMaker for DOS also supports such rectangular holes as standard pad type. But most modern layout softs doesnot allow this !? I have circumvented this problem(Eagle) by placing overlapping holes on a single pad thus creating rectangular hole. Since kicad does not allow this it does supports the non-circular holes I tried it. I just wanted to cross-check the output! regards, sam_des Rectangular holes are no holes as such - they are milled squares. The softwares supporting milled areas can be used to define these structures but it's slightly unusual. Regarding square pads. The traditional Gerber plotters had only round apertures and could subsequently not do squares... The corners of the smallest structure had always the radius of the smallest apertures. Keep in mind that most PCB cad softwares must carry this heritage but KiCad is one of the better I've seen lately. //Dan
[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, sadkra [EMAIL PROTECTED] wrote: --- In kicad-users@yahoogroups.com, Rick Collins gnuarm.2006@ wrote: I'm not sure what you are asking about. I have never seen oblong holes in a board. Are you talking about a routed slot? When you produce gerber files, how are the oblong holes defined? Regular holes are defined in a drill file typically in the Excellon format. In what output file are your oblong holes defined? Hello, Some components do have non-circular leads such as Power Relays, Fuse Holders, Fuses etc. You can check the Gerber section in Kicad help, there is topic about rectangular holes. Also you can check Pad properties of any pad in kicad. BTW, these holes are defined in drill file only. Here is what my drill file drill report file says, -drl.rpt - T2 0.032 0.81mm (19 holes) T3 0.035 0.90mm (426 holes) (with 8 oblongs) T4 0.039 1.00mm (14 holes) .drl --- T3 X1.050Y-5.250G85X1.050Y-5.050 G05 X1.050Y-4.857G85X1.050Y-4.656 G05 X1.300Y-5.250G85X1.300Y-5.050 G05 X1.300Y-4.857G85X1.300Y-4.656 G05 X1.800Y-5.250G85X1.800Y-5.050 G05 X1.800Y-4.857G85X1.800Y-4.656 G05 X1.550Y-5.250G85X1.550Y-5.050 G05 X1.550Y-4.857G85X1.550Y-4.656 G05 T4 Well, I loaded the file in GerbView 6 all I can see a single hole. That was the reason I tried Postscript output. My ancient BoardMaker for DOS also supports such rectangular holes as standard pad type. But most modern layout softs doesnot allow this !? I have circumvented this problem(Eagle) by placing overlapping holes on a single pad thus creating rectangular hole. Since kicad does not allow this it does supports the non-circular holes I tried it. I just wanted to cross-check the output! regards, sam_des This may be a nit, but the drill file excerpt shown above is for routs, not drilled holes. The command is describing a hole that is dragged from the first point to the second. This will create a hole (also called a slot) that is as wide as the specified hole and as long as the path plus the hole size. The ends of the hole are rounded. So technically this is not a rectangular hole. These holes are not made by drills, they are routed. I believe you are asking for holes that are 0.035 x 0.200 inches. For rectangular pins, I often just drill a hole the max size of the pin. But 0.200 inches would be a bit large and would be very hard to solder. Using multiple drill holes to create a rectangular hole will likely be rejected by the board maker. A drill can't be used right next to a hole. The bit will slip sideways into the existing hole, possibly breaking the bit. That is why they rout slots. Because routing before plating is an extra step, board makers typically charge extra for slots.
[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, Dick Hollenbeck [EMAIL PROTECTED] wrote: Jean Pierre said oblong pads, not oblong holes. Pad being copper area around the hole. Yes, but Jean Pierre is not the only other person in this conversation. The OP Sadkra said, BTW, non-circular(oblong) holes are also shown incorrectly on PS output. And can't check that with gerber. Rick
[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, jean-pierre charras [EMAIL PROTECTED] wrote: sadkra a écrit : Hello Everyone, I just finished my first sch-pcb project in Kicad. I tried to output the pcb in Postscript format. When I looked carefully at the Postscript file, I found that some of the pads are missing /or some pads are only half drawn in bottom-copper layer while bottom-copper mask shows the complete pad-mask. I may add that gerber output of the same pcb is fine without any problems. It will be of great help if someone throws any light on this. Postscript output has a bug: after drawing oblong pads, some next drawings can be incorrectly drawn (bad size) This old bug is now solved (Postscript output will be Ok in next release, coming soon) Can you confirm you have oblong pads on your board ? Jean-Pierre CHARRAS Maître de conférences Directeur d'études 2ieme année. Génie Electrique et Informatique Industrielle 2 Institut Universitaire de Technologie 1 de Grenoble BP 67, 38402 St Martin d'Heres Cedex Recherche : GIPSA-LIS - INPG 46, Avenue Félix Viallet 38031 Grenoble cedex Thanks everyone ! Yes, my PCB do have oblong pads. But they are quite long way away from pads that are missing or half drawn. These missing pads are Circular. BTW, non-circular(oblong) holes are also shown incorrectly on PS output. And can't check that with gerber. I as glad to see the support for non-circular holes (can't find that in many commercial packages), but I want to check before committing my design to PCB manufacturer. Can we output the gerber with actual or small holes ? That's why I tried Postscript. regards, sam_des
[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, sadkra [EMAIL PROTECTED] wrote: Thanks everyone ! Yes, my PCB do have oblong pads. But they are quite long way away from pads that are missing or half drawn. These missing pads are Circular. BTW, non-circular(oblong) holes are also shown incorrectly on PS output. And can't check that with gerber. I as glad to see the support for non-circular holes (can't find that in many commercial packages), but I want to check before committing my design to PCB manufacturer. Can we output the gerber with actual or small holes ? That's why I tried Postscript. regards, sam_des I'm not sure what you are asking about. I have never seen oblong holes in a board. Are you talking about a routed slot? When you produce gerber files, how are the oblong holes defined? Regular holes are defined in a drill file typically in the Excellon format. In what output file are your oblong holes defined?
[kicad-users] Re: Postscript Output
--- In kicad-users@yahoogroups.com, Dan Andersson [EMAIL PROTECTED] wrote: On Thursday 24 April 2008 20:26:28 sadkra wrote: Hello Everyone, I just finished my first sch-pcb project in Kicad. I tried to output the pcb in Postscript format. When I looked carefully at the Postscript file, I found that some of the pads are missing /or some pads are only half drawn in bottom-copper layer while bottom-copper mask shows the complete pad-mask. I may add that gerber output of the same pcb is fine without any problems. It will be of great help if someone throws any light on this. regards, sam_des The postscript output is NOT for PCB making!!! If you need Postscript for PCB making, use a Gerber Viewer and make a Postscript output from it. You can't trust anything but the Gerber file. //Dan, M0DFI I don't think anyone was planning to make PCBs from the PS output. But I assume the OP was using it as a check plot. If it is not intended to be accurate, why is it there?
Re: [kicad-users] Re: Postscript Output
I don't think anyone was planning to make PCBs from the PS output. But I assume the OP was using it as a check plot. If it is not intended to be accurate, why is it there? AS an owner of a postscript printer I'd say I like the PS option of KiCad but frankly, the output is rather rubbish... The other alternative is HP Plotter format - Yikes... So the PS output is not a bad choice for anything but pcb production purpose. I do prefer the Gerber file but I use the Geda Gerber viewer instead a it's more integrated in the Linux environment than KiCad's Gerber viewer. //Dan
