Searching \ for '[ot]: eagle board editor question' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: massmind.org/techref/pcbs.htm?key=eagle
Search entire site for: 'eagle board editor question'.

Exact match. Not showing close matches.
PICList Thread
'[ot]: eagle board editor question'
2002\02\07@220747 by rad0

picon face
Using the hobby freeware version gives you a board of
100 by 80 mm

Why is the corner of the outline of the board not exactly on
the zero - zero crosshair?

Does this matter?

I see how you change this outline using the wire command
in the dimension layer.

But I'm asking the question because I wonder if it matters to
a board house??

So far I've only used pcb express, and they have their own little board
editor

And I want to use this eagle project generator with another board house
next time.

So I'm asking about the crosshair thing, but I'd also like to know
what a board house needs from you to make a board, what
do you send them??

Thanks

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\02\08@083747 by Edson Brusque

face
flavicon
face
Hello Rad0,

> Using the hobby freeware version gives you a board of
> 100 by 80 mm

   ok.

> Why is the corner of the outline of the board not exactly on
> the zero - zero crosshair?

   Don't have an idea.

> Does this matter?

   no.

> I see how you change this outline using the wire command
> in the dimension layer.

   Yes, simply delete and create a new rectangle on the dimension layer.

> But I'm asking the question because I wonder if it matters to
> a board house??

   No, doesn't matters.

> So far I've only used pcb express, and they have their own little board
> editor
>
> And I want to use this eagle project generator with another board house
> next time.

   Ok, no problemo.

> So I'm asking about the crosshair thing, but I'd also like to know
> what a board house needs from you to make a board, what
> do you send them??

   it depends on the board house. The board house I ever deal (Digicart, on
Brazil's south) initially asked for Tango or Gerber files. So I've sent a
freeware copy of Eagle and tell then how to use it. Now I only send the
Eagle's .BRD file.

   Best regards,

   Brusque

-----------------------------------
Edson Brusque
Research and Development
C.I.Tronics Lighting Designers Ltda
Blumenau  -  SC  -  Brazil
http://www.citronics.com.br
Say NO to HTML mail
-----------------------------------

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\02\08@094450 by rad0

picon face
> > So I'm asking about the crosshair thing, but I'd also like to know
> > what a board house needs from you to make a board, what
> > do you send them??
>
>     it depends on the board house. The board house I ever deal (Digicart,
on
> Brazil's south) initially asked for Tango or Gerber files. So I've sent a
> freeware copy of Eagle and tell then how to use it. Now I only send the
> Eagle's .BRD file.
>
>     Best regards,
>
>     Brusque
>
> -----------------------------------
OK, so just find out what the board house wants and give it to them, fine.

If you're still around, how does a gerber file orient itself?  I mean, if
you
have made a board in eagle somewhere off the origin, then produced a
gerber file for your board,

what's the gist of how a gerber file orients all the parts together on the
board??

Thanks again.

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\02\08@120439 by Edson Brusque

face
flavicon
face
Hello rad0,

> If you're still around, how does a gerber file orient itself?  I mean, if
> you
> have made a board in eagle somewhere off the origin, then produced a
> gerber file for your board,
> what's the gist of how a gerber file orients all the parts together on the
> board??

   please, download ViewMate (http://www.lavenir.com) it's a free Gerber file
viewer and will thought some things. Also, it's very usefull when you're
trying to make gerber output files with Eagle.

   Best regards,

   Brusque

-----------------------------------
Edson Brusque
Research and Development
C.I.Tronics Lighting Designers Ltda
Blumenau  -  SC  -  Brazil
http://www.citronics.com.br
Say NO to HTML mail
-----------------------------------

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\02\08@123625 by Rick Sherman

flavicon
face
>
> Why is the corner of the outline of the board not exactly on
> the zero - zero crosshair?
>
> Does this matter?


> > So I'm asking about the crosshair thing, but I'd also like to know
> what a board house needs from you to make a board, what
> do you send them??
>
> Thanks
>

Talk to the board house(s) before you start on the board if possible.
Most will be glad to send you a list of their requirements and
capabilities. Most  probably won't care too much where the 0,0
point is as long as it is plainly visible on the gerbers/mechanical
drawings.  It can save a lot of work (time & money)  if you know
the details in advance.

Rick

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\02\08@124402 by rad0

picon face
thanks gents...

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\02\08@130315 by Martin Peach

flavicon
face
GC-Prevue from Graphicode at http://www.graphicode.com/ works better for me.
It allows you to print any layer or combination of layers including the
drill holes so you could do a single board 'manually'.
/\/\/\/*=Martin

{Original Message removed}

2002\02\08@174402 by David P. Harris

picon face
How do you use this.  I can't even figure out how to do the CAM processing.
Can you outline the steps you take.  For example, which output device do I use -
my guess: Gerber_auto_23.
David

Martin Peach wrote:

> GC-Prevue from Graphicode at http://www.graphicode.com/ works better for me.
> It allows you to print any layer or combination of layers including the
> drill holes so you could do a single board 'manually'.
> /\/\/\/*=Martin
>
> {Original Message removed}

2002\02\08@175729 by Martin Peach

flavicon
face
You do File->Import and pick the folder with your gerbers in it. It took me
a few tries to get all the setup right because there are lots of options.
You can either print to a printer or do a Print Screen and paste into
Clipboard viewer and save as a bmp from there, then use GIMP or Photoshop to
scale the image...
/\/\/\/*=Martin

{Original Message removed}

2002\02\08@180349 by David P. Harris

picon face
OK, but I can't generate the Gerbers.  Asks for wheel files and all-sorts.  What
a newby I am!
David

Martin Peach wrote:

> You do File->Import and pick the folder with your gerbers in it. It took me
> a few tries to get all the setup right because there are lots of options.
> You can either print to a printer or do a Print Screen and paste into
> Clipboard viewer and save as a bmp from there, then use GIMP or Photoshop to
> scale the image...
> /\/\/\/*=Martin
>
> {Original Message removed}

2002\02\08@181233 by Martin Peach

flavicon
face
Well you need to have the gerbers ready before you start the viewer
application...the wheel file would be the aperture file. Usually there is a
file for each layer on the board plus an aperture file (sometimes the
apertures are defined in the gerber file so the aperture file is redundant)
and a drill file which is not a gerber file but Excellon or somesuch. I
don't know how or if Eagle can generate gerbers. I'm using CircuitMaker2000.
/\/\/\/*=Martin

{Original Message removed}

2002\02\08@185115 by Edson Brusque

face
flavicon
face
Hello David P.,

> How do you use this.  I can't even figure out how to do the CAM
processing.
> Can you outline the steps you take.  For example, which output device do I
use -
> my guess: Gerber_auto_23.

   it's a bit dificult but after you have it done it right once it appears
to be more logical.

   Are you using Eagle4.08r2? I think 3.55 does the same way, but can't
remember the details. Anyway, I hardly have to deal with the CAM processor,
because the board house does all these work for me.

   First, open the CAM Processor. You can do this choosing CAM Processor
from the file menu of schematics or board.

   Then, file\open\job\ and choose one of the predefined job files. To a
quick start, choose one of the "ger???.cam".

   You'll see various tabs on the top of the window workspace. Each tab is
a file that will be generated, like one .cmp file for the component side
solder mask (with top, pads and vias layers), one .plc file for the silk
screen mask (with dimension, tplace, tnames and tvalues layers) etc.

   In the bottom of the workspace you have buttoms to add and delete files.
You can do as many as you want. You can have top (component side) solder
mask, bottom solder mask, top silk, bottom silk, top stop mask, bottom stop
mask etc.

   For each tab (section), you can give section name (description), user
prompt (something it will ask to continue), offsets (live at 0), file
extension (the defaults are ok) etc.

   You have an option where you tell each section the device that will be
used (file output format).

   On the "Style" checkbox group you have various options for making the
file "upside-down", "mirrored" etc. Live the "optimize" and the "pos.coord"
checked. The defaults are usually ok.

   The drill file is a bit more complex. You have to create a drill rack
file. It's like a file where the size of the drills disponible at the PCB
plant. A file can contain something like:

           T01 0.012in
           T02 0.024in
           T03 0.032in
           T04 0.036in
           T05 0.040in
           T06 0.044in
           T07 0.080in
           T08 0.125in

   You can generate this file for your board using the "drillcfg.ulp" user
language program. Run it from the Board application. If you don't have many
drills disponible at the same time on the plant, you can reduce the number
of hole sizes editing the ???.drl file prior to generating your gerber
output:

           T01 0.012in
           T02 0.024in
           T03 0.036in
           T04 0.036in
           T05 0.044in
           T06 0.044in
           T07 0.080in
           T08 0.125in

   But then you'll have to play with the tolerance values.

   Hope this got you started. If not, ask. :)

   Best regards,

   Brusque

-----------------------------------
Edson Brusque
Research and Development
C.I.Tronics Lighting Designers Ltda
Blumenau  -  SC  -  Brazil
http://www.citronics.com.br
Say NO to HTML mail
-----------------------------------

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


More... (looser matching)
- Last day of these posts
- In 2002 , 2003 only
- Today
- New search...