Gerber output vias and pads are filled

On 01/17/2011 11:59 AM, tstbeyaz wrote:

 

After creating top layer gerber data, I viewed the result with a gerber

viewer program. I notice that the pads haso no drills, they are fully

filled. Is it the way pcbs are produced?. The Holes of the vias are

drilled after photoengraving by drill bit, SO the holes of the vias are

not photoengraved?

 

The check: pads filled is always check, by the cam processor.

 

Which method is better, photoengraving the copper and then drilling it,

or the copper of the hole is not etched and the via/pad is produced only

by drilling.

 

tstbeyaz.

 

>

Take a look messages with drill-aid.ulp mentioned in the body.

Paul R.

This is the way that gerbers work.  The drilling machine is completely separate from the photoplotter (and drillings usually happens first, so that the holes can be plated through.)  drill-aid.ulp will provide "pilot holes" in printed output (suitable for toner transfer or home photoplotting), and there's a change to eagle-def to provide similar capability for Postscript and EPS output from the CAM processor (by me!), but as far as I know, the very idea of "holes" in an output object is entirely foreign to the gerber format...

On 18.01.2011 06:06, WestfW wrote:

This is the way that gerbers work.  The drilling machine is completely separate from the photoplotter (and drillings usually happens first, so that the holes can be plated through.)  drill-aid.ulp will provide "pilot holes" in printed output (suitable for toner transfer or home photoplotting), and there's a change to eagle-def to provide similar capability for Postscript and EPS output from the CAM processor (by me!), but as far as I know, the very idea of "holes" in an output object is entirely foreign to the gerber format...

 

The PCB will be produced by a pcb manufactorer, But sometimes there are

cheap alternative suppliers for prototypes who IMHO dont have cnc drill

machine but drill by hand. If I ensure that they also use my excellon

file (have a drill machine) the gerber data in this filled (no holes)

should be ok.

How is this change to Eagle-def if I need the pilot holes in the gerber

file?

thanks.

tstbeyaz.

On Tue, 18 Jan 2011, tstbeyaz wrote to us saying :

>The PCB will be produced by a pcb manufactorer, But sometimes there are

>cheap alternative suppliers for prototypes who IMHO dont have cnc drill

>machine but drill by hand.

To be honest, I would avoid any such "cheap alternative suppliers".

There are places out there that will do properly manufactured PCBs

complete with solder mask and silk screen off professional grade tooling

for the same price as the so-called cheap alternatives. And definitely

avoid any place that can't cope with the Gerbers generated by Eagle's

CAM processor (or even anywhere that queries them).

But YMMV.

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

The contents of     | All power corrupts, but we need electricity.

this message are    |

purely my opinion.  |

Don't believe a     |

word.               |

"tstbeyaz" <ferhatincal@gmail.com> wrote in message

news:ih1shn$fb1$1@cheetah.cadsoft.de...

 

After creating top layer gerber data, I viewed the result with a gerber

viewer program. I notice that the pads haso no drills, they are fully

filled. Is it the way pcbs are produced?. The Holes of the vias are

drilled after photoengraving by drill bit, SO the holes of the vias are

not photoengraved?

 

The check: pads filled is always check, by the cam processor.

 

Which method is better, photoengraving the copper and then drilling it, or

the copper of the hole is not etched and the via/pad is produced only by

drilling.

 

tstbeyaz.

 

>

Tstbeyaz,

There are software packages that will leave the pads (drill holes) open

where the holes will be drilled.  This is old technology and created for the

days when hand drilling was the standard practice.  This is long since gone

and it is preferred to have filled (solid) pads in order to ensure plated

through holes.

Terri

Am 18.01.2011 08:09, schrieb tstbeyaz:

On 18.01.2011 06:06, WestfW wrote:

>> This is the way that gerbers work.  The drilling machine is completely

>> separate from the photoplotter (and drillings usually happens first,

>> so that the holes can be plated through.)  drill-aid.ulp will provide

>> "pilot holes" in printed output (suitable for toner transfer or home

>> photoplotting), and there's a change to eagle-def to provide similar

>> capability for Postscript and EPS output from the CAM processor (by

>> me!), but as far as I know, the very idea of "holes" in an output

>> object is entirely foreign to the gerber format...

>>

 

The PCB will be produced by a pcb manufactorer, But sometimes there are

cheap alternative suppliers for prototypes who IMHO dont have cnc drill

machine but drill by hand. If I ensure that they also use my excellon

file (have a drill machine) the gerber data in this filled (no holes)

should be ok.

 

How is this change to Eagle-def if I need the pilot holes in the gerber

file?

 

thanks.

tstbeyaz.

There is a possibility to use Postscript output with the CAM Processor

and have the drill holes visible, and you can use drill-aid.ulp before.

This device definition was posted some time ago in this newsgroup.

I just add it here:

EPS-Drillaid]

@EPS

Long     = "Postscript with max hole size in pads/etc, ala drill-aid.ulp"

Header3  = "%% redefine our /h function with a fixed diameter\n"\

           "/h {  %% draw a hole\n"\

           "   /d  exch def\n  %% Still need to pop diam off stack\n"\

           "   d 5000 gt {\n"\

           "      /d  5000 def\n  %% But override it to 0.5mm\n"\

           "   } if\n"\

           "   /y  exch def\n"\

           "   /x  exch def\n"\

           "   d 0 gt {\n"\

           "     newpath\n"\

           "     x EU y EU d 2 div EU 0 360 arc\n"\

           "     currentgray dup\n"\

           "     1 exch sub setgray\n"\

           "     fill\n"\

           "     setgray\n"\

           "     } if\n"\

           "   } def\n"\

           "%% The drawing\n"

@PS

Long     = "Postscript (printable) with max hold size ala Drill-aid.ulp"

Header2  = "%% redefine our /h function with a fixed diameter\n"\

           "/h {  %% draw a hole\n"\

           "   /d  exch def\n  %% Still need to pop diam off stack\n"\

           "   d 5000 gt {\n"\

           "      /d  5000 def\n  %% But override it to 0.5mm\n"\

           "   } if\n"\

           "   /y  exch def\n"\

           "   /x  exch def\n"\

           "   d 0 gt {\n"\

           "     newpath\n"\

           "     x EU y EU d 2 div EU 0 360 arc\n"\

           "     currentgray dup\n"\

           "     1 exch sub setgray\n"\

           "     fill\n"\

           "     setgray\n"\

           "     } if\n"\

           "   } def\n"\

           "%% Remainder of Header2 copied from define for PS device\n"\

           "%% the real drawing size:\n"\

           "\n"\

           "/MinDrawX %6d EU def\n"\

           "/MinDrawY %6d EU def\n"\

           "/MaxDrawX %6d EU def\n"\

           "/MaxDrawY %6d EU def\n"\

           "\n"\

           "%% the usable page size:\n"\

           "\n"\

           "/LeftMargin 0.25 inch def  %% change these if drawing gets

clipped!\n"\

           "/BotMargin  0.25 inch def\n"\

           "/PageWidth  %7.4f inch def\n"\

           "/PageHeight %7.4f inch def\n"\

           "\n"\

           "%% are we going to rotate?:\n"\

           "\n"\

           "/RotateDrawing %d 0 ne def\n"\

           "\n"

           ;(x1, y1, x2, y2, Width, Height, DoRotate)

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

FAQ: http://www.cadsoft.de/faq.htm