Exact match. Not showing close matches.
'[TECH] Board house questions...'
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?
Is it enough for Seeed, for instance, to fab a board?
On Tue, Mar 27, 2012 at 10:22 AM, John Gardner <gmail.com> wrote: goflo3
> 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":
-- Martin K
|On Tue, March 27, 2012 11:27 am, M.L. 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.
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.
Just outside of Austin, TX
The views I express are my own, not that of my employer, a large
multinational corporation that you are familiar with
Thanks, Martin -
....Autotrax is incredibly old, but if that's what you want to use it
I'm incredibly old - Last time I looked, Autotrax still works :)
I spent Sunday afternoon with the Eagle demo - Cryptic is fair,
I think, & I have a blind, unreasoning prejudice against buying
software that the authors don't think is worth documenting.
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.
On 03/27/2012 01:43 PM, Matt Bennett wrote:
> multinational corporation that you are familiar with.
I'm not sure about what I should be seeing with a Gerber viewer.
The GBL file for a two-layer board I laid out in Autotrax indeed
shows the bottom layer, but the GTL file shows both - Seems
Do I need to save each layer independently & produce just the
applicable gerber ( *.gtl, *.gbl, & so on...) for that *.pcb ?
> ..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.
On Tue, Mar 27, 2012 at 2:43 PM, Matt Bennett <hazmat.com> wrote: mattpiclist
> 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
On Tue, Mar 27, 2012 at 2:49 PM, John Gardner <gmail.com> wrote: goflo3
> Thanks, Martin -
> ...Autotrax is incredibly old, but if that's what you want to use it
> should work.
> I'm incredibly old - Â Last time I looked, Autotrax still works :)
> I spent Sunday afternoon with the Eagle demo - Cryptic is fair,
> I think, & I have a blind, unreasoning prejudice against buying
> software that the authors don't think is worth documenting.
> Â Jack
It's well documented, there's also quite a long tutorial on using
Eagle. Available via searching google or the Cadsoft website.
|.... 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 -
Thanks, Martin - I'll look more. I found Sparkfun's tutorial
Sunday, but it's 4 versions ago, & was'nt much use - The
Devil's in the details, getting started..
If anyone would stoop to answer my question about what I should
see in a Gerber viewer I'd appreciate it.
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 solder resist
Top silk screen
Bottom solder resist
Bottom silk screen
Keep out layer
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.
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
I should add that Cadcentric has other capabilities
which I'm not yet able to evaluate - Interesting stuff...
More... (looser matching)
- Last day of these posts
- In 2012
, 2013 only
- New search...