Florian Finsterbusch wrote:

>Hi Brian,
>we want to mill the whole PCB (drills + traces).
>Our mechanics uses an ISEL milling machine for mechanic prototypes.
>We want to use this machine also to manufacture our prototype PCBs.
>Therefore we need a converter-software from Gerber- to HPGL- or DXF-Files.
>(It has to convert the traces and pads to outlines for the milling-machine)

I have done something similar in protel. A year or so ago we looked at getting one of 
those t-tech machines. After looking at demo of the isolation software and the 
machine, I thought we could do this in protel with minimal effort.  The prototypes we 
did were not perfect, but were usable, and may depend on the complexity of the board. 
We used an excellon xl-5 driller/router which has some limitations (see below). 

What I used were two polygons with "no hatching" to get the isolation path for the top 
and bottom. Make the track width on the polygons about the same width as your router 
bit. I used 10mils for this. The bit we used has a "V" shape and varying the routing 
depth, you can vary the  isolation path width. These polygons were assigned to two 
nets that I created called "iso-top" and "iso-bottom". I created a net class called 
"isolation", and then a clearance rule of 1mil between this netclass and the board. 
You will also have to adjust the setting for the polygons to make sure you have a good 
isolation path.

After I got the isolation paths polygons, I copied these to another blank pcb (being 
careful to not rebuild them). All I had to do after that was make the gerbers from the 
polygons. we are using an xl-5 driller/router to make these protos, so i wrote a small 
program to convert the gerber files into a excellon route program.  

Some things from my setup that are different from yours is that the controller for our 
driller/router can't do arcs unless they are in 90 degree increments, so I had to use 
polygons with hexagons instead of arcs.

If you need a dxf file you can load the gerbers up into camtastic and export them out. 
I am not sure about getting an hpgl file.  When generating the gerbers for the 
isolation paths, it may help to check "sorted" in the cam manager gerber setup, this 
will help with optimizing the paths for the milling machine.

You will also need to mirror the bottom isolation polygon, so that when you flip the 
panel over to route the bottom, it lines up with the other side. It took me a few trys 
to get that sorted out :)

Its been a while since I did that, so I may have missed some steps.

Hope this gives you some ideas.

Christopher Brand
Ludlum Measurements, Inc.
PO Box 810
501 Oak Street
Sweetwater, TX 79556 USA
(915) 235-4947 phone
(915) 235-4672 fax

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to