pcb, gerber&drill files problem

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.

Should I send the files like this and why were those options unmarked ?

*sigh...

oh boy.. long night ahead

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

On 05/04/2013 10:39 AM, Chuck Huber wrote:

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"

This is especially important if you have the "Standard" or "Light"

versions and are trying to cram lots of parts in the license-defined

(160x100mm or 100x80mm) component placement area. The license permits

you to make the board itself larger than the component placement area,

and you can route traces through the larger area, but this results in

negative coordinates. Because of the license limitations you can't shift

the components to prevent this. Checking the "Pos. Coord." will cause

the Gerber layers to shift out of alignment unless you place some sort

of mark on every layer at a common Quadrant III point, an error-prone

requirement.

Unless your board house just can't deal with negative coordinates, let

them deal with it.

Am 04.05.2013 16:39, schrieb Chuck Huber:

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

shifted different distances.

Does EAGLE REALLY do this (I NEVER use the CAM processor, so I just

don't know)? If yes, this seems a very bad thing to me, which should

DEFINITELY be considered an error and be fixed.

If "Positive coordinates" is active, THE WHOLE BOARD should be shifted

by the minimum amount necessary to make ALL coordinates positive,

INDEPENDENT of the current output layers. Only this way the same Gerber

coordinates mean the same positions.

Andreas Weidner

On 5/3/2013 7:44 PM, Jim Raynor wrote:

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

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/75600#75600

 

Hi Jim,

The key here is the pos. coords option needs to be set the same across

all of the gerber tabs and drill job. Either have them all set or have

them unset but you can't have a mix. You don't have to make any changes

to the board design for this to work.

If pos. coords is checked across all of the tabs then all of the design

files will have the same offset added to them so everything will line up

nicely.

hth,

Jorge Garcia

Cadsoft Support

Am 07.05.2013 21:14, schrieb Jorge Garcia:

The key here is the pos. coords option needs to be set the same across

all of the gerber tabs and drill job. Either have them all set or have

them unset but you can't have a mix.

Fine to see that there is a possibility to make this work properly in EAGLE.

BUT since this is not obvious, why leave the user in the dark about it?

If "pos. coords" should be either on or off in ALL the CAM tabs, why not

  1. either make this option GLOBAL for the whole job (so as not to give

     the user the chance to screw things up),

  2. or leave it as it is, but, in case the user checked the option in

     SOME tabs, but not in others, display a warning that this MIGHT

     cause problems with the Gerber output?

If a software gives the user vital information on how NOT to do things,

or prevents him from doing these wrong things, that's MUCH better than

letting him run against the wall...

Andreas Weidner

On 05/08/2013 04:31 AM, Andreas Weidner wrote:

Am 07.05.2013 21:14, schrieb Jorge Garcia:

The key here is the pos. coords option needs to be set the same across

all of the gerber tabs and drill job. Either have them all set or have

them unset but you can't have a mix.

Good morning, Jorge,

Thanks for this bit of information.  I knew everything lined up with

pos. coords turned off.  I don't believe I've ever tried it with all of

them on.

I never use this anyway, and in the default (empty) CAM job they're on.

I have yet to run across a board fab house that can't handle negative

coordinates.  However, I can see where it'd be handy to have if you're

cutting your own boards.

 

Fine to see that there is a possibility to make this work properly in

EAGLE.

 

BUT since this is not obvious, why leave the user in the dark about

it? If "pos. coords" should be either on or off in ALL the CAM tabs,

why not

1. either make this option GLOBAL for the whole job (so as not to give

    the user the chance to screw things up),

Andreas makes a good point here.  Perhaps Pos Coord should be associated

with the job, and not each section.  The X and Y offset would also be

good candidates for the same treatment.

Enjoy,

    - Chuck

On 5/8/2013 4:31 AM, Andreas Weidner wrote:

Am 07.05.2013 21:14, schrieb Jorge Garcia:

The key here is the pos. coords option needs to be set the same across

all of the gerber tabs and drill job. Either have them all set or have

them unset but you can't have a mix.

 

Fine to see that there is a possibility to make this work properly in

EAGLE.

 

BUT since this is not obvious, why leave the user in the dark about it?

If "pos. coords" should be either on or off in ALL the CAM tabs, why not

  1. either make this option GLOBAL for the whole job (so as not to give

     the user the chance to screw things up),

  2. or leave it as it is, but, in case the user checked the option in

     SOME tabs, but not in others, display a warning that this MIGHT

     cause problems with the Gerber output?

Hi Andreas,

I like number 2, I'll file an enhancement report on this. I don't think

it would be difficult to implement so thanks for the idea.

Best Regards,

Jorge Garcia

If a software gives the user vital information on how NOT to do things,

or prevents him from doing these wrong things, that's MUCH better than

letting him run against the wall...

 

Andreas Weidner