pcb, gerber&drill files problem

Question

Hi there,

I'm ready to send my first board to a pcb manufacturer. I've generated the GBL,GTL,GBS,GTS,GBO,GTO and the drill TXT file using the manufacturer's cam.

Now the problem is that when I open those files with two separate gerber viewers (GERBV 2.6 and Viewplot) I get the same result.. the holes are where they're supposed to, but everything else is placed +0.409 mm from the origin, on both axes.

It took me a while to understand what's wrong, and after that I placed everything in Eagle's Board Editor 0.409 mm right from and 0.409 mm above the origin. After that I generated a new set of gerber/drill files and the problem seemed to be solved. I mean I get the same exact (positive) results in two different gerber viewers.

My questions is why is that happening, if it's normal (like an alignment of the board from 0.409,0.409 and not from 0,0) and if should send it like that.

Can I trust these software viewer that the board would look exactly like that when finished ?

what's bother me the most is that in the second scenario the holes are still at the same coordinates and only the other layers were repositioned (although I selected and moved everything in eagle).

thanks in advance

dukepro · Answer

On 05/03/2013 08:03 PM, Jim Raynor wrote:

I just made some progress !?

In the manufacturer's CAM everything but the drill file has "Pos.
Coord." and "Optimize" checked.
I've enabled these two options for the drill file, repositioned the
board at 0,0 (lower left corner) and remade the gerber+drill files.
Now everything looks in place, but I still wonder why.

To fix this, your best bet is to leave the "Pos. Coord." option OFF

(unchecked) on all sections of your CAM job. Everything will line up

properly.

This has come up several times in the past. See my post in

eagle.support.eng dated 26-Mar-2013. Search for "Gerber files and Pick

and place file"

The "Pos. Coord." options causes Eagle to move the entire layer such

that no part of any object is in any quadrant other than the first.

That is, everything has positive coordinates. For example, if your

board has the bottom and left edges along the X and Y axes, and you run

a 10-mil wire around the board, then half of this line is below the X

axis, and to the left of the Y axis. Eagle will shift the layer 5 mils

right and 5 mils up so that the entire wire is X>=0 and Y>= 0.

Eagle does this on a layer-by-layer basis, so different layers may get

shifted different distances. Your drill file already had everything in

Quadrant 1, thus no shift occurred. In the past, I have had the copper

layers shifted one distance, and the tNames shifted a different

distance, and the bNames shifted yet another distance.

If your board house can't handle negative coordinates, they will shift

the entire design (not just one layer at a time) as they see fit.

Besides, they will generally add your design to a much larger panel (48"

x 48" comes to mind) consisting of multiple designs from different

customers. They process the entire panel and cut it up after the entire

panel is fabricated. Many times, they will place multiple copies of

your design on a single panel to more efficiently utilize the panel.

Larger designs are placed first, and smaller designs fill in the edges.

To find out what's causing the shift you observed, turn on all layers

with the "display all;" command. You'll probably see something you

don't care about (like component values) hanging to the left of the

Y-axis, or below the X-axis.

HTH,

- Chuck