Post by thread:[TECH] Board house questions...

On Tue, Mar 27, 2012 at 10:22 AM, John Gardner <spam_OUTgoflo3TakeThisOuTgmail.com> wrote: > I'm new to the business of having PCBs made. > > Autotrax 1.61 -> CadCentric -> 274X Gerbers, which look OK > in a Gerber viewer (http://www.gerber-viewer.com/default.aspx.) > > Has anyone else done this, or similar, or have a better scheme? > Autotrax is incredibly old, but if that's what you want to use it should work. Anything will work as long as you verify that your resulting Gerber files are correct. I would recommend Cadsoft Eagle or a free software program that I can't remember at the moment. For viewing Gerber files I recommend "GerbV": http://gerbv.sourceforge.net/ -- Martin K

On Tue, March 27, 2012 11:27 am, M.L. wrote: {Quote hidden}> On Tue, Mar 27, 2012 at 10:22 AM, John Gardner <.....goflo3KILLspam@spam@gmail.com> wrote: >> I'm new to the business of having PCBs made. >> >> Autotrax 1.61 -> CadCentric -> 274X Gerbers, which look OK >> in a Gerber viewer (http://www.gerber-viewer.com/default.aspx.) >> >> Has anyone else done this, or similar, or have a better scheme? >> > > > Autotrax is incredibly old, but if that's what you want to use it should > work. > > Anything will work as long as you verify that your resulting Gerber > files are correct. > > I would recommend Cadsoft Eagle or a free software program that I > can't remember at the moment. > > For viewing Gerber files I recommend "GerbV": > http://gerbv.sourceforge.net/ Honestly, I've found that looking at the Gerbers themselves haven't done anything for me in the last few designs I've done (including some rather large designs upwards of 6"x10", 4 layer). Maybe I trust in Eagle too much, but I think the only thing I could see in a Gerber is a rather gross error, and my experience has been that the Gerbers that Eagle (and with less experience, Altium) put out are accurate to the layout program. Proper application of design rules and listening to the warnings that the layout program gives me (don't forget online DRCs too- they have value!) have turned out to be much more effective uses of my time. If I were to switch to a program I had less experience with, maybe I'd run them through a Gerber viewer. But in the past 10 years, I don't remember a single time that reviewing a Gerber would have given me something that I couldn't have picked up in the layout program. Of course, the above comments are with Gerbers that are 100% generated by the layout program. Hand edit them, and all bets are off. I frequently get customers to ask me to review layouts, and gahh... I hate it when someone sends me just a Gerber, since the Gerber doesn't have any information about the net embedded- I feel like it is doing a code review of a .hex file. Sure, it can be done, but with a lot of effort, and my review is much more effective with the source files. Of course, a Gerber is better than nothing, but constructive comments on a complex design (with just Gerbers) are pretty difficult. Matt Bennett Just outside of Austin, TX 30.51,-97.91 The views I express are my own, not that of my employer, a large multinational corporation that you are familiar with

I used an external gerber viewer for a bit, then stopped... trusting my layout package to get it right. Soon after, a bug in Altium Designer's gerber export (which was quickly fixed afterward) messed up the direction on arcs in certain situations. I got a shipment of PCBs where incorrect arcs on pad thermals shorted almost everything on the board together. These were supposedly electrically tested, too. While they were technically correct productions from the given gerbers it must have raised some eyebrows. Lesson learned. I now check every single set of gerbers with an external viewer. Darron Black Houston, TX On 03/27/2012 01:43 PM, Matt Bennett wrote: {Quote hidden}> On Tue, March 27, 2012 11:27 am, M.L. wrote: >> On Tue, Mar 27, 2012 at 10:22 AM, John Gardner<goflo3KILLspamgmail.com> wrote: >>> I'm new to the business of having PCBs made. >>> >>> Autotrax 1.61 -> CadCentric -> 274X Gerbers, which look OK >>> in a Gerber viewer (http://www.gerber-viewer.com/default.aspx.) >>> >>> Has anyone else done this, or similar, or have a better scheme? >>> >> >> Autotrax is incredibly old, but if that's what you want to use it should >> work. >> >> Anything will work as long as you verify that your resulting Gerber >> files are correct. >> >> I would recommend Cadsoft Eagle or a free software program that I >> can't remember at the moment. >> >> For viewing Gerber files I recommend "GerbV": >> http://gerbv.sourceforge.net/ > Honestly, I've found that looking at the Gerbers themselves haven't done > anything for me in the last few designs I've done (including some rather > large designs upwards of 6"x10", 4 layer). Maybe I trust in Eagle too > much, but I think the only thing I could see in a Gerber is a rather gross > error, and my experience has been that the Gerbers that Eagle (and with > less experience, Altium) put out are accurate to the layout program. > > Proper application of design rules and listening to the warnings that the > layout program gives me (don't forget online DRCs too- they have value!) > have turned out to be much more effective uses of my time. If I were to > switch to a program I had less experience with, maybe I'd run them through > a Gerber viewer. But in the past 10 years, I don't remember a single time > that reviewing a Gerber would have given me something that I couldn't have > picked up in the layout program. > > Of course, the above comments are with Gerbers that are 100% generated by > the layout program. Hand edit them, and all bets are off. > > I frequently get customers to ask me to review layouts, and gahh... I hate > it when someone sends me just a Gerber, since the Gerber doesn't have any > information about the net embedded- I feel like it is doing a code review > of a .hex file. Sure, it can be done, but with a lot of effort, and my > review is much more effective with the source files. Of course, a Gerber > is better than nothing, but constructive comments on a complex design > (with just Gerbers) are pretty difficult. > > Matt Bennett > Just outside of Austin, TX > 30.51,-97.91 > > The views I express are my own, not that of my employer, a large > multinational corporation that you are familiar with.

> ..Last time I looked, Autotrax still works :) What O/S are you using it with. I paid realish $ for Autotrax long long long ago. Now available as a legitimate free download I understand. My recollection is that when I stopped using it some years ago as a quick circuit diagram drawing tool it was because it would no longer work under the Windows I was using - I could not even do a screen capture from it. If it has started working again with newer versions of Windows or if you have a version of Autrotrax that works with XP and newer it would be good to know. As a drawing tool it was fine enough for many things, a grand-master (which I'm not) could lay out most modern PCBs with it given enough time and the auto router even worked after a fashion. Russel

On Tue, Mar 27, 2012 at 2:43 PM, Matt Bennett <.....mattpiclistKILLspam.....hazmat.com> wrote: > Honestly, I've found that looking at the Gerbers themselves haven't done > anything for me in the last few designs I've done (including some rather > large designs upwards of 6"x10", 4 layer). Maybe I trust in Eagle too > much, but I think the only thing I could see in a Gerber is a rather gross > error, and my experience has been that the Gerbers that Eagle (and with > less experience, Altium) put out are accurate to the layout program. It only takes one really stupid error to make you want to look at the gerbers every single time. Boards aren't very cheap nor very quick to make, so it's not a bad idea to check out the end product. -- Martin K

.... What O/S are you using it with (?) Virtual PC 2007 / DOS 6.22. Works fine, other than no mouse support, courtesy Bill & Co. Not that big a deal with Autotrax. (Unimaginable to the short-pants crew, I know...) .... If it has started working again with newer versions of Windows or if .... you have a version of Autrotrax that works with XP and newer it would .... be good to know. As a drawing tool it was fine enough for many things, .... a grand-master (which I'm not) could lay out most modern PCBs with it .... given enough time and the auto router even worked after a fashion. Easytrax is also available free, & I understand runs under XP, W98, perhaps even ME, which I know you'll want to resurrect :), others, so presumably mouse-able. Look here - http://www.lupinesystems.com/easytrax/ and here - http://www.altium.com/community/downloads/en/downloads_home.cfm For Autotrax 1.61 274X Gerbers & other goodies see - http://www.lh1.org/AUTOTRAX/autotrax.html#CCC Jac

Jack, In a gerber viewer you should be able to verify that each layer of the pcb you have designed has plotted correctly. The plot tool (traxplot) produces one file for each layer. The layers being (for a double sided board): Top copper Top solder resist Top silk screen Bottom copper Bottom solder resist Bottom silk screen Keep out layer Mechanical layers Drill detail Drill master If you have smt components, you may also see top and bottom pad master layers. Apertures may or may not be embedded in the gerber files. If not, you need to create an aperture file. Drill files are text files that represent the drill size, and location of holes. A gerber file is usually created to verify the position of the holes, for visual verification. The manufacturer will use the text file of X Y locations for manufacture. I'm basing this on more recent Protel 99, but I have used Autotrax back in the day and seem to remember that the same files are generated. There is usually an option to include one or more of the mechanical layers on each gerber layer. What can you do with this information? Using the gerber viewer, you can turn on / off the layers of interest to verify the the gerber generator (traxplot) has generated correct files. You can check that solder resist mask is pulled back from pads by the amount you expect, that no silk screen is covering pads, that a smt pad does not have a hole in the middle of it, that drill sizes are correct. I always check the gerbers before sending to a fab. Single sided through to 12 layer BGA type technology. It's not unknown for aperatures to get messed up. I use camtastic, which came with Protel 99. When I have an errant hole, say it's 1.27mm dia, and I know that I don't use that profile, I can check the gerber to see exactly where it is. I don't know how to do that in Protel. Also, checking plated and non plated holes are where you expect them. In Protel 99, and I think that it's the same for Autotrax, you place the string .LEGEND on one of the drill layers. This gets rendered as a drill table on the gerber when you plot. Hope it helps. ....Andy On 28/03/2012 01:14, John Gardner wrote: > If anyone would stoop to answer my question about what I should > see in a Gerber viewer I'd appreciate it. > > thanks, Jack