genrate drill file from gerber and fab data

Jan 2, 2008

Hi,

I need to know whether it is possible to generate .drl file without
having PCB layout file?
I have all the other Gerber files and Fab drawing in .dwg (AUTOCAD)
format.Also I have got Aperture definition files in .gap fomat and
gerber files in .gbr format.But i dont have any file of .PCB format
containing any layout data.

How is it possible to hand generate the .drl file?
And how to verify it?

Please answer as soon as possible as my target date is tomorrow
itself.

-VK

TT_Man · Jan 2, 2008

<venu.mehta@gmail.com> wrote in message
news:536ed388-d522-4636-b541-4975eddf27c5@l6g2000prm.googlegroups.com...

No, you will have to get your pcb fabricator to make a drill file for
you...sounds expensive...

TT_Man · Jan 2, 2008

<venu.mehta@gmail.com> wrote in message
news:536ed388-d522-4636-b541-4975eddf27c5@l6g2000prm.googlegroups.com...

place vias over every pad/hole and make a drill file from that?

Christopher Ott · Jan 2, 2008

<venu.mehta@gmail.com> wrote in message
news:536ed388-d522-4636-b541-4975eddf27c5@l6g2000prm.googlegroups.com...

The depths to which I despise Autocad for PCB's knows no bounds. I still
occasionally run into people with .dxf or .dwg's, but it's becoming very
infrequent now. However, the short answer is yes you can generate a drill
file by hand. Import to Viewmate (freeware) to verify.

Below is a sample drill file from one of my small boards. Use the following
link to help interpret http://en.wikipedia.org/wiki/G-code

Notice that each line only shows the coordinates which changed. T1-T4 in the
beginning defines the drill diameters in inches. Not sure what the M72 & M48
commands are. Assuming M30 means stop...

Happy hunting!

Chris
--------

M72
M48
T1F00S00C0.0200
T2F00S00C0.0460
T3F00S00C0.0520
T4F00S00C0.1500
%
T01
X014100Y014750
Y018900
X017100Y018350
X019000
X018000Y031000
Y031500
X017500
X017000
X016500
X016000
Y031000
X016500
X017000
X017500
T02
X005300Y010000
X007300
X009300
X003300
X002250Y015500
Y017500
Y019500
X003300Y025000
X005300
X007300
X009300
T03
X023600Y015450
X026300
X026050Y029450
X022800Y029440
T04
X034900Y005000
X016500
X032800Y022100
M30

JeffM · Jan 2, 2008

venu.mehta@ gmail.com wrote:

This demonstrates why specialized tools exist
what a bad idea it is to use the wrong tool for the job.

Another element you are missing in your inappropriate tool:
http://www.google.com/search?q=cache:Fc9eFlq5PDAJ:en.wikipedia.org/wiki/Physical_verification+electrical.rule.check+Design.rule.check

RHRRC · Jan 2, 2008

On 2 Jan, 07:04, venu.me...@gmail.com wrote:

I do not know what you mean by "..all the other Gerber files..." -
other to what?
The Apertures file is a simple ascii file: as to why you have more
than one for your pcb I am bemused.
The Gerber files contain all the layout data for the pcb - thats why
Gerbers are used (so that the pcb house does not have to keep copies
of every single piece of drafting sotware yet invented).

If you do have the Gerbers (it will be a type 274D if it requires a
seperate apertures file) just dowload a free Gerber viewer -there are
many so try Viewmate, GC Prevue or whatever takes your fancy as they
will all help you - and you will be able to see the pcb.
Wade through the helpfile and learn what to do.
You will have to do some work such as identifying and / or sizing the
holes.

Many pcb design packages have a gerber import facility to allow you to
dothe same.

You are obviously not familiar with pcb design so please note that
there is no universal standard for the naming of file types in the pcb
world. A dot.pcb file is just the name chosen by that particular
software company - I know of three different formats/file types called
dot.pcb and I am sure there are others. Ditto with names used for
Gerbers but the gerber files themselves are in a universally standard
format/file type.

Good luck

Brad Velander · Jan 3, 2008

VK,
There is no easy or simple manner for anyone to describe to you how to
rebuild/regenerate a drill file for your files. It can be done, it can be
done fairly easily by someone that fully understands what they are doing and
have access to a suitable Gerber editing tool. The key there is a Gerber
tool that will do file editing, typically any of the freely available tools
on the internet are just Gerber viewers. If this was a medium
size/complexity board with mostly SMT components, a few mounting holes and a
bunch of vias, I don't see why I wouldn't be able to manually ressurrect the
drill data in an hour or two, but then I have been doing PCB design for
decades. However I could spend three - four times that amount of time just
trying to explain to you what you need to do and how to do it.

So far I have only seen one suitable answer to your enquiry from other
posters, seems most of them don't know how to read your original post and
they are looking for a reason to rant about AutoCAD or the precise
formatting of the Gerbers you have obviously inheritted from someone else.
Don't worry, having a fabrication drawing done in AutoCAD is very common, I
have done it that way for decades because ECAD/PCB CAD tools typically suck
big-time as a general drawing or documentaion tool.

(Note: the original post said nothing other than he had a "fabrication
drawing" in AutoCAD format, not a PCB design, nor Gerbers generated from an
AutoCAD PCB design.)

There is one slight possiblity that could be your saving grace. Do you
have a Gerber viewer and have you loaded and viewed the Gerber files? Is
there a Gerber file that appears to be only the holes for the board? This
would be strictly circular flashes on a layer all by themselves, no traces
or other lines, except maybe a board outline, titleblock or drawing template
surrounding the board itself. These flashes are they sized appropriately for
the desired hole sizes (query them with your viewer tool and it should tell
you the aperture (flash) size, this should match to the drill sizes called
out in the fabrciation drawing if it contains the drill sizes). If you have
one of those layers in your Gerbers, almost any fabrciator can turn that
Gerber layer into a drill file in minutes and your problem is solved.

If you desire, you could send me the files in question and I could give
them a looking over your you and then be in a position better advise/assist
you.

bveland at shaw dot ca

--
Sincerely,
Brad Velander.

"TT_Man" <Someone@ntlworld.com> wrote in message
news:sSJej.1712$a61.1385@newsfe3-win.ntli.net...

David Wright · Jan 4, 2008

If you have the gerber files, you should be able to set a flag in the setup
routine in ORCAD to generate the drill file. There are some other tools
that can generate drill files from Gerber files that do not require PCB
layout. However, if you have a precision AUTOCAD file this might also work.
If all else fails, go back one revision and patch the PCB board or bypass
the revision and relayout the PCB.

Check one of the PCB board vendors for gerber file conversion tools.

<venu.mehta@gmail.com> wrote in message
news:536ed388-d522-4636-b541-4975eddf27c5@l6g2000prm.googlegroups.com...

Brad Velander · Jan 5, 2008

Hi David,
The OP hasn't posted since his first message. I believe from the manner
I read his post, he has the Gerber files and a fabrication drawing and
that's it. I don't believe he has any PCB files or a PCB CAD tool. Sounds
like he got these fabrication files dumped on him with nothing else and now
he is trying to get them fab'ed without even an original drill file (or
possibly he does have a drill file but doesn't recognize it or it's format).

I always try to pound into designers to do a simple readme text file to
be zipped up with their fab files. The readme lists all files, their
layer/stackup association, type (Gerber/drill/etc) and the particular
data/machine formats of each file. Then nobody ends up in these situations
or at least somebody had to do something intentionally stupid for them to
end up in this type of situation.

--
Sincerely,
Brad Velander.

"David Wright" <dwright2@mc.net> wrote in message
news:13nssd3soo9a5b9@corp.supernews.com...

sycochkn · Jan 17, 2008

<venu.mehta@gmail.com> wrote in message
news:536ed388-d522-4636-b541-4975eddf27c5@l6g2000prm.googlegroups.com...

It is possible that one of your gerber files contains images for locating
holes, but I would not depend on it.

Bob

sycochkn · Jan 17, 2008

"Christopher Ott" <spamtrap at ottelectronics dot com> wrote in message
news:EOidnQchB4Q6eubanZ2dnUVZ_qOknZ2d@giganews.com...

Autocad works fine for manual PCB layout. But each program that converts to
Gerber from dxf requires its own special format for the drawings. Going from
Gerber to dxf for a particular AutoCAD setup requires its own special format
out of the conversion program. Going from Autocad to other software also
requires its own special conversion software.

Bob

genrate drill file from gerber and fab data

Guest

TT_Man

Guest

TT_Man

Guest

Christopher Ott

Guest

JeffM

Guest

RHRRC

Guest

Brad Velander

Guest

David Wright

Guest

Brad Velander

Guest

sycochkn

Guest

sycochkn

Guest

Welcome to EDABoard.com

Sponsor

Online statistics

Forum statistics

genrate drill file from gerber and fab data

Guest

TT_Man

Guest

TT_Man

Guest

Christopher Ott

Guest

JeffM

Guest

RHRRC

Guest

Brad Velander

Guest

David Wright

Guest

Brad Velander

Guest

sycochkn

Guest

sycochkn

Guest

Log in

Welcome to EDABoard.com

Sponsor