EasyPC Gerber "Dimensions" File Problem

I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits
( http://www.4pcb.com ), and was told that the "dimensions" file
contained improper information ("only two small dashes"). This
resulted in my pcb design being put on "CAM Hold", which delayed its
processing.

I ended up having to create a PDF for them, with a drawing showing a
marked reference point and the dimensions to each side of the PCB
outline from the reference point, so they could make a Gerber
dimensions/outline file, for me, from that.

This was the first time that I had had someone else make boards for
me. This was for a 2-sided board, 9.75" x 2.9375". I did use
4pcb.com's very nice "FreeDFM" check, first, which showed NO errors.
And all of the PDF drawings of the copper layers, silkscreen, and
soldermask layers, which their FreeDFM automatically creates from
uploaded Gerber files and emails back, looked fine.

Using Windows Notepad, I looked in the Gerber "dimensions" file that
EasyPC had created. Here is the whole thing:

%FSLAX23Y23*%
%MOIN*%
G04 EasyPC Gerber Version 8.0.8 Build 2014 *
%ADD10C,0.00100*%
X0Y0D02*
D02*
D10*
X8076Y1105D02*
X9543Y2528*
X9886Y2813*
X9907Y2851*
X9916Y2764*
X9943Y2558*
Y2579D01*
Y2622D02*
Y2696*
X0Y0*
M02*

I'd never seen the inside of a Gerber file, before this, and don't
have a Gerber file viewer (YET). So I don't know if this looks
reasonable, or not. But apparently it's not, or else there was a
problem while transmitting it.

I'm also wondering if maybe there is some setting, within EasyPC, that
I need to change. If not, what could be the problem and what could I
do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.

Thanks.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

-

 

[Paul Burke]

tomg@fullnet.com wrote:

I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits
( http://www.4pcb.com ), and was told that the "dimensions" file
contained improper information ("only two small dashes"). This
resulted in my pcb design being put on "CAM Hold", which delayed its
processing.

The Gerber file you posted is just a stripe 0.57mm long and 0.026mm wide
according to GCPrevue (http://www.graphicode.com/). This is worth
downloading and using to check out your Gerbers before sending.

Where did the "dimensions" Gerber come from? It's not part of the usual
set, and there's an option in PCB plot to include the board outline in
the plot.

I did use
4pcb.com's very nice "FreeDFM" check, first, which showed NO errors.
And all of the PDF drawings of the copper layers, silkscreen, and
soldermask layers, which their FreeDFM automatically creates from
uploaded Gerber files and emails back, looked fine.

The Gerber is valid- it's just nonsense as a manufacturing file.

I'm also wondering if maybe there is some setting, within EasyPC, that
I need to change. If not, what could be the problem and what could I
do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.

Version 8 was just fine. So is version 10. I can't remember when they
introduced it, but the big thing for a while has been 3D view, which I
don't use being a sad git. The copper pour has also got a lot more reliable.

Paul Burke

 

I'm sorry of two of these are posted. It looks like my first attempt
has vanished.

On Mar 16, 4:42 am, Paul Burke <p...@scazon.com> wrote:

t...@fullnet.com wrote:
I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits
(http://www.4pcb.com), and was told that the "dimensions" file
contained improper information ("only two small dashes"). This
resulted in my pcb design being put on "CAM Hold", which delayed its
processing.

The Gerber file you posted is just a stripe 0.57mm long and 0.026mm wide
according to GCPrevue (http://www.graphicode.com/). This is worth
downloading and using to check out your Gerbers before sending.

Thanks, Paul! I have downloaded it.

Where did the "dimensions" Gerber come from? It's not part of the usual
set, and there's an option in PCB plot to include the board outline in
the plot.

The "dimensions" file was produced by EasyPC, with no special action
on my part. (It does appear to be part of the standard set of
Gerbers, in my EasyPC setup.)

Oddly, maybe, when I highlight the "Dimensions" plot name and click on
the "Layers" tab, the "Board Outline" line has its "Selected" column
set to "No", by default. (But there is a "Dimensions" line that has
"Selected" set to "Yes", by default.) Next time, I'll try also
setting "Board Outline" to "Yes", for the Dimensions file, since the
board outline is what the "CAM Hold" guys seemed to be wanting, from
that file. I must have been too sleep-deprived to think to check
that, at the time.

I also don't know if a separate Dimensions file would have been
required, if I'd simply included the board outline on some or all of
the other plots. But I had just used the default settings that EasyPC
had, which didn't include the board outline on ANY of the other plots,
and did include the Dimensions plot.

One thing that I did change, after my first "freeDFM" check, was to
select "Hardware Fill" and "Hardware Arcs", in the "Output" tab's
"Device Setup" dialog, under "RS-274-X (Extended Gerber)", because
without "Hardware Fill", the poured copper areas were filled using
_lines_, which, only in certain cases, caused freeDFM to complain
about lots of very thin tracks. I could actually see them, too, on
the PDFs of the artwork that were emailed back to me (at least at
magnifications above something like 1200X). The Gerber files were
also significantly larger, without "Hardware Fill". Using "Hardware
Arcs" is apparently a good idea, too, since, otherwise, arcs are
rendered using multiple line segments.

I did use
4pcb.com's very nice "FreeDFM" check, first, which showed NO errors.
And all of the PDF drawings of the copper layers, silkscreen, and
soldermask layers, which their FreeDFM automatically creates from
uploaded Gerber files and emails back, looked fine.

The Gerber is valid- it's just nonsense as a manufacturing file.

You should try their free FreeDFM service! ( http://www.freedfm.com ,
or, http://www.4pcb.com ) It's not just a Gerber syntax checker. It
checks (apparently) ALL sizes and clearances, etc etc, and also
automatically "thickens" all silkscreen artwork to meet their minimum
line-thickness requirement. Then, usually within a few minutes, it
emails back a fairly-well-detailed report, which includes a nice price
quote with both prototype and production pricing, PDFs of the artwork
for each layer (a free on-line Gerber viewer, in essence), and, an
Error Summary, with the number (quantity) of each type of error found,
and five samples of each type of error it found. Each error-sample
includes three zoom views of artwork showing the error, with a text
description giving the error margin/measurement and its coordinates,
plus a description of the relevant manufacturing requirement that was
not met. It seems like it probably saves their CAM engineers and
their customers a ton of time and aggravation, at least for
inexperienced customers like me. (But apparently they need to start
also checking the Dimensions file, if it's used.)

Aside: I didn't take advantage of any of their pricing "specials".
But my prototypes' pricing seemed pretty good, although maybe a bit
weird: They wanted $54 each for qty 5 ($270), but $30 each for qty 10
($300), for a three-day turnaround. I took the 10! But now I'm
kicking myself for not checking the price for 20. (In the emailed
price quote that's included with the freeDFM report, you can simply
change a quantity and click to update the list of quotes versus turn-
times, and can click on any unit-price to place an order.) Those
prices, for 2.94" x 9.75" 2-sided .031" FR4, included lead-free
solder plating, green solder mask on both sides, white silkscreen on
top, board dimensions cut within .01", and other stuff. They must use
lasers to do the drilling, because I didn't see anything at all about
pricing versus number of drill sizes, or anything like that. And I
also had some non-standard hole sizes, which were never mentioned.
All-in-all, it was a relatively-painless first-timer experience (and,
probably largely thanks to their freeDFM check, would have been almost-
completely uneventful, had it not been for my Dimension file
problem). I also liked being able to go to their website to track the
progress of the boards' processing. (This is starting to sound like
an advertisement. But no, I am not affiliated with Advanced Circuits
or their people in any way. I just enjoyed their nicely-automated
setup, and their very-attentive service.)

I'm also wondering if maybe there is some setting, within EasyPC, that
I need to change. If not, what could be the problem and what could I
do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.

Version 8 was just fine. So is version 10. I can't remember when they
introduced it, but the big thing for a while has been 3D view, which I
don't use being a sad git. The copper pour has also got a lot more reliable.

Yes, I love EasyPC v8. The 3D and better-rendering stuff was just
starting to be hinted-at, in my v8, but was only in a few of the
examples, as far as I could tell, not being too interested at the
time, as I was first learning it. I would actually like to have 3D,
now, so I could more-easily check component clearances, etc. But I
don't know if it could do what I need, since I'd like to be able to
see the clearances between components on two boards that are at a
right angle to each other. If they could provide that, I'd upgrade
tomorrow, even though that would mean paying more, to also raise my
pin limit above 1000, since one of the six boards I'd like to simulate
in 3D together, at the moment, has something like 975 pins. I'll
email them and try to find out more about the 3D capabilities.

I'm REALLY glad to hear that the copper pouring is more reliable, in
v10! That's one of the (few) main things in v8 that is fairly-often
quite aggravating.

I did just go to http://www.numberone.com , and looked at a list of
some of the improvements in v10. One that caught my eye was something
about showing clearances on-the-fly, while editing tracks. I'd
probably have given them my car, for that, a while back. I'm
definitely going to upgrade, now.

Thanks, Paul!

Paul Burke

Tom Gootee

http://www.fullnet.com/~tomg/index.html

-

 

[RHRRC]

On 16 Mar, 09:42, Paul Burke <p...@scazon.com> wrote:

t...@fullnet.com wrote:
I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits
(http://www.4pcb.com), and was told that the "dimensions" file
contained improper information ("only two small dashes"). This
resulted in my pcb design being put on "CAM Hold", which delayed its
processing.

The Gerber file you posted is just a stripe 0.57mm long and 0.026mm wide
according to GCPrevue (http://www.graphicode.com/). This is worth
downloading and using to check out your Gerbers before sending.

Where did the "dimensions" Gerber come from? It's not part of the usual
set, and there's an option in PCB plot to include the board outline in
the plot.

I did use
4pcb.com's very nice "FreeDFM" check, first, which showed NO errors.
And all of the PDF drawings of the copper layers, silkscreen, and
soldermask layers, which their FreeDFM automatically creates from
uploaded Gerber files and emails back, looked fine.

The Gerber is valid- it's just nonsense as a manufacturing file.



I'm also wondering if maybe there is some setting, within EasyPC, that
I need to change. If not, what could be the problem and what could I
do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.

Version 8 was just fine. So is version 10. I can't remember when they
introduced it, but the big thing for a while has been 3D view, which I
don't use being a sad git. The copper pour has also got a lot more reliable.

Paul Burke

I suspect there is a 'glitch' with this particular installation of
easypc since this is- and has been for a very long time - a well
known, capable, and respected pcb layout package.

from the sample gerber given - it ain't all there!!

I suspect that the 'dimensions' the pcb house was asking for is the
aperture dimensions file - generally just referred to as the apertures
file - in days of old, but not so oftennow, it was called the D codes
sizing file (or similar).
Normally easypc (and just about every other pcb package) produces 274X
gerbers - they do not have a seperate apertures file. If the output is
set to 274D gerbers then there must be a seperate aperture file.
Since the pcb house could make no sense of the gerber file provided I
guess they may have asked for the aperture dimensions file to see if
that was the problem since this is the only other 'gerber' file there
is.
On the other hand it could be nothing to do with it.

 

On Mar 15, 3:03 pm, t...@fullnet.com wrote:

I sent a set of Gerber files from EasyPC v8.0.8 to Advanced Circuits
(http://www.4pcb.com), and was told that the "dimensions" file
contained improper information ("only two small dashes"). This
resulted in my pcb design being put on "CAM Hold", which delayed its
processing.

I ended up having to create a PDF for them, with a drawing showing a
marked reference point and the dimensions to each side of the PCB
outline from the reference point, so they could make a Gerber
dimensions/outline file, for me, from that.

This was the first time that I had had someone else make boards for
me. This was for a 2-sided board, 9.75" x 2.9375". I did use
4pcb.com's very nice "FreeDFM" check, first, which showed NO errors.
And all of the PDF drawings of the copper layers, silkscreen, and
soldermask layers, which their FreeDFM automatically creates from
uploaded Gerber files and emails back, looked fine.

Using Windows Notepad, I looked in the Gerber "dimensions" file that
EasyPC had created. Here is the whole thing:

%FSLAX23Y23*%
%MOIN*%
G04 EasyPC Gerber Version 8.0.8 Build 2014 *
%ADD10C,0.00100*%
X0Y0D02*
D02*
D10*
X8076Y1105D02*
X9543Y2528*
X9886Y2813*
X9907Y2851*
X9916Y2764*
X9943Y2558*
Y2579D01*
Y2622D02*
Y2696*
X0Y0*
M02*

I'd never seen the inside of a Gerber file, before this, and don't
have a Gerber file viewer (YET). So I don't know if this looks
reasonable, or not. But apparently it's not, or else there was a
problem while transmitting it.

I'm also wondering if maybe there is some setting, within EasyPC, that
I need to change. If not, what could be the problem and what could I
do about it? Anyone? Or maybe it's time to upgrade to EasyPC v10.

Thanks.

- TomGootee

http://www.fullnet.com/~tomg/index.html

-

Just for completeness' sake: The solution was to select the Dimensions
plot and then select Layers and make sure that Board Outline was
selected.

No more "Cam Hold" delays.

- Tom Gootee

http://www.fullnet.com/~tomg/index.html

-