Problem with gerber file names

[[email protected]]

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...
The Gerber file produced by my CAD are:
myproj.TOP
myproj.BOT
myproj.SMT
myproj.SMB
myproj.SST
myproj.DRD
myproj.DTS
myproj.GTD
thruhole.TAP

but none of them concerns the board outline.....
Anybody knows how to produce this missing Gerber file?

I have realized that the gerber extentions produced by the post-
processor of OrCAD Layout are different from that ones produced by
Protel and EAGLE, for istance.
GKO is a Gerber extention used by these two CADs and I wish two know
the corresponding extention (if exists) in OrCAD.

Regards,
Alex

 

[John Larkin]

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...
The Gerber file produced by my CAD are:
myproj.TOP
myproj.BOT
myproj.SMT
myproj.SMB
myproj.SST
myproj.DRD
myproj.DTS
myproj.GTD
thruhole.TAP

but none of them concerns the board outline.....
Anybody knows how to produce this missing Gerber file?

It's usually submitted as a fab drawing, not a gerber. It has the
outline plus materials, stackup, color, and tolerance notes.

John

 

[www.china-powerseller.com]

Dear friend :
It is my fortunate writing to you . you will discover this is a wealth
accumulation place.
The website of our company is http://www.china-powerseller.com
We are a big agent for Laptop
Mobile Phone\Digital Camera\CDJ\DJM\Apple Ipod\PSP\VEDEO GAMES
\Television\GPS\Telescope in CHINA .
All of our commodities is the most advanced quality but lowest price.
we also have the

safest and most
convenient transaction way to guarante the transaction arries on
normally .
looking forward to your coorporation and cause all of us both to
profit.
you can contact us by Email:china.seller#hotmail.com
MSN: china.seller#hotmail.com
best wishes!
your sincerely

http://www.china-powerseller.com
MSN/Email: [email protected]

 

[TT_Man]

Dear friend :
It is my fortunate writing to you . you will discover this is a wealth
accumulation place.
The website of our company is http://www.china-powerseller.com
We are a big agent for Laptop
Mobile Phone\Digital Camera\CDJ\DJM\Apple Ipod\PSP\VEDEO GAMES
\Television\GPS\Telescope in CHINA .
All of our commodities is the most advanced quality but lowest price.
we also have the

safest and most
convenient transaction way to guarante the transaction arries on
normally .
looking forward to your coorporation and cause all of us both to
profit.
you can contact us by Email:china.seller#hotmail.com
MSN: china.seller#hotmail.com
best wishes!
your sincerely

WTF has that got to do with Gerbers? Western Union payment as well I
presume?

 

[Didi]

Here is a typical text file I send out with my boards.
Last time I had to convert my Gerbers to extended-Gerber,
which cost me some work but OTOH elliminates a potential
source of error (D-codes are embedded in the x-Gerber).

Here is the file (just inserted as it is, hopefully it is
of some use):

-------
25 - 59.8 mil (1.52 mm) circle,
27 - 63 mil (1.6 mm) circle.

Drilling tools:
1 - 0.3 mm (about 0.2 after plating), 0.2 drilling is also OK,
2 - 1.0 mm,
3 - 1.0 mm,
4 - 1.0 mm,
5 - 1.3 mm,
6 - 3.1 mm,
7 - 2.0 mm.

The board must be cut by the contour of one of the inner layers
(e.g. layer 2, ipnl2.gbr) as if the cutting tool has zero width
and moves through the middle of the countour line.

The stackup is as following:
ipnl1.gbr
ipnl2.gbr
ipnl3.gbr


ipnl4.gbr
ipnl2.gbr
ipnl5.gbr

Total board thikness apr. 1.5 mm or so (perhaps 1.6 is popular
nowadays).

The spacing between ipnl2.gbr (the GND layer) and its neighbour
layers, both in the top and bottom 3 sets, must be something
like 6 mil or so (so the impedance of the top and bottom
signal layers referenced to the neighbour GND layer is about
50 ohm). All this assumes FR4 material.

The signal layers have been routed with 5 mil gaps and traces in mind,
with 4 mil spaces when passing close to vias/BGA pads. The Gerber
files have been verified to pass a 4 mil gap check.

For any questions please contact Dimiter Popoff <[email protected]>,
or Skype didi_tgi (or call ++359/2/9923340 )

 

[Didi]

Oops, part of the file was lost, here I go again:

Here is a typical text file I send out with my boards.
Last time I had to convert my Gerbers to extended-Gerber,
which cost me some work but OTOH elliminates a potential
source of error (D-codes are embedded in the x-Gerber).

Here is the file (just inserted as it is, hopefully it is
of some use):

-------
File description:
ipnl1.gbr - top signal layer (layer 1),
ipnl2.gbr - GND plane layer, goes as layer 2 and 5,
ipnl3.gbr - internal plane, layer 3,
ipnl4.gbr - internal plane, layer 4,
ipnl5.gbr - bottom signal layer (layer 6).

NOTE: ipnl2.gbr, ipnl3.gbr and ipnl4.gbr are plotted as NEGATIVES.
They are all copper planes except for the lines and pads plotted
on them.

ipnsm1.gbr - solder mask for top layer,
ipnsm2.gbr - solder mask for bottom layer.

D-codes:

11 - 4.3 mil (0.11 mm) circle,
12 - 6.3 mil (0.16 mm) circle,
14 - 9.8 mil (0.25 mm) square,
15 - 9.8 mil (0.25 mm) circle,
16 - 11.8 mil (0.30 mm) square,
19 - 17.3 mil (0.44 mm) circle,
21 - 20.1 mil (0.51 mm) circle,
22 - 50 mil (1.27mm) circle,
23 - 55.1 mil (1.40 mm) circle,
25 - 59.8 mil (1.52 mm) circle,
27 - 63 mil (1.6 mm) circle.

Drilling tools:
1 - 0.3 mm (about 0.2 after plating), 0.2 drilling is also OK,
2 - 1.0 mm,
3 - 1.0 mm,
4 - 1.0 mm,
5 - 1.3 mm,
6 - 3.1 mm,
7 - 2.0 mm.

The board must be cut by the contour of one of the inner layers
(e.g. layer 2, ipnl2.gbr) as if the cutting tool has zero width
and moves through the middle of the countour line.

The stackup is as following:
ipnl1.gbr
ipnl2.gbr
ipnl3.gbr


ipnl4.gbr
ipnl2.gbr
ipnl5.gbr

Total board thikness apr. 1.5 mm or so (perhaps 1.6 is popular
nowadays).

The spacing between ipnl2.gbr (the GND layer) and its neighbour
layers, both in the top and bottom 3 sets, must be something
like 6 mil or so (so the impedance of the top and bottom
signal layers referenced to the neighbour GND layer is about
50 ohm). All this assumes FR4 material.

The signal layers have been routed with 5 mil gaps and traces in mind,
with 4 mil spaces when passing close to vias/BGA pads. The Gerber
files have been verified to pass a 4 mil gap check.

For any questions please contact Dimiter Popoff <[email protected]>,
or Skype didi_tgi (or call ++359/2/9923340 )

-----

Dimiter

On Mar 7, 6:53 pm, [email protected] wrote:

- Hide quoted text -
- Show quoted text -

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...
The Gerber file produced by my CAD are:
myproj.TOP
myproj.BOT
myproj.SMT
myproj.SMB
myproj.SST
myproj.DRD
myproj.DTS
myproj.GTD
thruhole.TAP

 

[Richard Henry]

11 - 4.3 mil (0.11 mm) circle,
12 - 6.3 mil (0.16 mm) circle,
14 - 9.8 mil (0.25 mm) square,
15 - 9.8 mil (0.25 mm) circle,
16 - 11.8 mil (0.30 mm) square,
19 - 17.3 mil (0.44 mm) circle,
21 - 20.1 mil (0.51 mm) circle,
22 - 50 mil (1.27mm) circle,
23 - 55.1 mil (1.40 mm) circle,
25 - 59.8 mil (1.52 mm) circle,
27 - 63 mil (1.6 mm) circle.

Where can you get a square drill?

 

[Arlet]

Where can you get a square drill?

These do not refer to the drills. These are the "D-codes". These
shapes are used to draw the artwork.

See http://www.artwork.com/gerber/appl2.htm

 

[John B]

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...
The Gerber file produced by my CAD are:
myproj.TOP
myproj.BOT
myproj.SMT
myproj.SMB
myproj.SST
myproj.DRD
myproj.DTS
myproj.GTD
thruhole.TAP

but none of them concerns the board outline.....
Anybody knows how to produce this missing Gerber file?

I have realized that the gerber extentions produced by the post-
processor of OrCAD Layout are different from that ones produced by
Protel and EAGLE, for istance.
GKO is a Gerber extention used by these two CADs and I wish two know
the corresponding extention (if exists) in OrCAD.

Regards,
Alex

It's been a long time since I used OrCad, but I think you'll find the
board outline is in the '.DRD' file. You can also get it to include the
board outline in the copper layer files ('.TOP' & '.BOT').

 

[martin griffith]

On Mar 7, 9:46 am, "Didi" <[email protected]> wrote:

Where can you get a square drill?

http://upper.us.edu/faculty/smith/reuleaux.htm


martin

 

[Peter Bennett]

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...

In Protel, *.GKO would be the keep-out layer, which would rarely match
the board outline.

I put the board outline on a "mechanical" layer, then ask the Gerber
output routine to include that layer on all copper layers. I can then
instruct the board shop to trim the boards to the outline - seems to
work fine for me.

In any case, you have to tell the shop the board outline somehow -
either by including it on the copper layer, or by providing a separate
file.

The readme file I send with my Gerbers looks like:

=================================

Job: 0983 TRIUMF Octal DAC
PC Board P-13190 rev 0

The following files are required for this job:
p13190.GTL Component side copper photoplot file
p13190.GP1 Internal Ground Plane
p13190.GP2 Internal Power Plane
p13190.GBL Solder side copper photoplot file
p13190.GTO Top Component layout silkscreen
p13190.GBO Bottom Component layout silkscreen
p13190.GBS Bottom Solder Mask
p13190.GTS Top Solder Mask
p13190.TXT Drill file
readme.txt This file


Note: the Gerber files include embedded aperture data.

Tool Hole Size Hole Count Plated Tool Travel
---------------------------------------------------------------------------
T1 16mil (0.4064mm) 343 112.54 Inch (858.64 mm)
T2 25mil (0.635mm) 9 36.08 Inch (916.40 mm)
T3 35mil (0.889mm) 172 77.13 Inch (1959.06 mm)
T4 40mil (1.016mm) 10 5.77 Inch (146.46 mm)
T5 50mil (1.27mm) 12 16.87 Inch (428.41 mm)
T6 55mil (1.397mm) 6 3.68 Inch (93.48 mm)
T7 110mil (2.794mm) 10 27.68 Inch (703.05 mm)
T8 141mil (3.5814mm) 4 11.60 Inch (294.54 mm)
---------------------------------------------------------------------------
Totals 566 291.34 Inch (7400.04
mm)


The board is 7.20" x 11.95", +/- .010", four layer,
..0625" nominal thickness, FR-4 material
1 oz or greater copper
Standard through-hole plating, standard white tin plating on exposed
copper.
Standard gold plating on edge connector

Solder mask both sides (different masks)
Component Ident silkscreen on both sides

Trim boards to outline on component side artwork

--
Peter Bennett, VE7CEI Vancouver BC, Canada
peterbb4 (at) interchange.ubc.ca
new newsgroup users info : http://vancouver-webpages.com/nnq
GPS and NMEA info: http://vancouver-webpages.com/peter
Vancouver Power Squadron: http://vancouver.powersquadron.ca

 

[nospam]

I put the board outline on a "mechanical" layer, then ask the Gerber
output routine to include that layer on all copper layers. I can then
instruct the board shop to trim the boards to the outline - seems to
work fine for me.

Bet they hate you making them strip the outline from every gerber layer
before they plot it.

Give them an outline on a separate layer, they will either just look at it
or use it as a guide for creating a route.

I always give a paper (well PDF) copy of that layer including basic
dimensions and showing holes one of which is dimensioned so there can be no
confusion about alignment between gerbers and drill files.
--

 

[Eeyore]

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...

If they can't use the files that OrCad produces do you really want to use them ?

Doesn't bode well for their competence !

Graham

 

[Brian]

Hi everybody,
I'm trying to prototyping a board with an on-
line sevice found on the web. They ask me some gerber files that don't
match with mine produced with OrCAD Layout.
Notably they ask me a .GKO file - the gerber file associated with
board outline-, but OrCAD doesn't produce any gerber file with this
features...
The Gerber file produced by my CAD are:
myproj.TOP
myproj.BOT
myproj.SMT
myproj.SMB
myproj.SST
myproj.DRD
myproj.DTS
myproj.GTD
thruhole.TAP

but none of them concerns the board outline.....
Anybody knows how to produce this missing Gerber file?

I have realized that the gerber extentions produced by the post-
processor of OrCAD Layout are different from that ones produced by
Protel and EAGLE, for istance.
GKO is a Gerber extention used by these two CADs and I wish two know
the corresponding extention (if exists) in OrCAD.

Regards,
Alex

Gerber isn't an intelligent format. You could put the outline on any
layer (I have gotten in some pathetic gerber files at times). But the
proper place for the board out line is eiter on your drill drawing or
on a seperate mechanical layer you make. You will have to go into your
gerber set-up and add the outline layer to your drill drawing gerber
output if it is not already putting it their (or create a new one
called Mechanical). I haven't used Orcad in 15 years, can't help much
on the details of the process.

Its probably NOT that the company can't use Orcad Gerber, its simply
that the outline layer is not in any gerber file. How can they figure
the outline if it is undefined in the files? Or, I could be wrong and
they are incompetent. If you email me the gerbers (if nothing top
secret), I would be happy to take a peek.

Brian