Searching \ for '[EE] panelize with Eagle' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/pcbs.htm?key=eagle
Search entire site for: 'panelize with Eagle'.

Exact match. Not showing close matches.
PICList Thread
'[EE] panelize with Eagle'
2002\09\27@093813 by Stefano

flavicon
face
Hi guys,

I am running several different pcboards to try different RF solutions for
a PIC based wireless telecomunication system for toys.
Well, every different PCB has its own setup price, so to reduce the price
I would like to put all PCB in a signel BIG project so I pay only 1 setup
price.....

How can I panelize with Eagle (can I ???).
Shold I get some gerber editor (lavenir like) ?
Does something "cheap" exist around ?

THANKS,

Stefano Curtarolo

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email spam_OUTlistservTakeThisOuTspammitvma.mit.edu with SET PICList DIGEST in the body


2002\09\27@095429 by Wouter van Ooijen

face picon face
Olimex will do panalisation for you when you tell them how place the
different PCB files you provide them are to be arragenged.

Wouter van Ooijen

-- -------------------------------------------
Van Ooijen Technische Informatica: http://www.voti.nl
consultancy, development, PICmicro products

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email .....listservKILLspamspam@spam@mitvma.mit.edu with SET PICList DIGEST in the body


2002\09\27@095444 by Dale Botkin

flavicon
face
You can.  There's a ULP script to do it named panelize.ulp.  You wil have
to make a new PCB, then you can copy & paste the others into it.
Instructions are witht he ULP.

Dale
---
We are Dyslexia of Borg.
Fusistance is retile.
Your ass will be laminated.

On Fri, 27 Sep 2002, Stefano wrote:

> How can I panelize with Eagle (can I ???).

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email listservspamKILLspammitvma.mit.edu with SET PICList DIGEST in the body


2002\09\27@100926 by Wagner Lipnharski

flavicon
face
Stefano wrote:
> Hi guys,
>
> I am running several different pcboards to try different RF
solutions
{Quote hidden}

You can download the PANELIZE4.ULP from eagle website
(http://www.cadsoft.de), it should do it for you.

/_/_/_/_/_/_/_/_/_/_/_/_/_/_/_/_/_/_/
Wagner Lipnharski - UST Research Inc
Orlando FLorida - USA - http://www.ustr.net
/_/_/_/ Atmel AVR Consultant /_/_/_/

--
http://www.piclist.com#nomail Going offline? Don't AutoReply us!
email .....listservKILLspamspam.....mitvma.mit.edu with SET PICList DIGEST in the body


2002\09\27@101356 by Al Williams

flavicon
face
It is very easy to panelize your gerbers directly.

Here's a copy of a note I sent a different list:

If you are using Eagle for PCB layout here is a tip:

If you want to step and repeat your board, it is a pain since Eagle is
size-limited. Plus you have to break back annotation so it will let you
arbitrarily create new things on the PCB and is just a general pain.

Here's the trick. Create your gerber files like normal. Then open each
gerber layer and put the following in:

%SRX_Y_I_J_*%

Where the blanks are numbers:

X = Number of X repeats
Y = Number of Y repeats
I = Distance from start of one to start of next in X direction
J = Distance from start of one to start of next in Y direction

So... If you have a 3"x2" board and you want a 4x5 repeat with .25 inch
between each board you could write:

%SRX4Y5I3.25J2.25*%

If you don't produce a Gerber drill file, this might be a problem to fix
up the drills to match. With a gerber drill, it should be OK.

Haven't tried this with a real board, but works great in a Gerber viewer
like ViewMate.


###

So the question is, how do you do this same trick with an Excellon drill
file?

Al Williams
AWC
* Easy RS-232 Prototyping (New & Improved)
http://www.al-williams.com/awce/rs1.htm




> {Original Message removed}

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