Eagle 6.5 Lite version: Board Prints OK, Export Image not correct.

As far as i can tell, the 'export - image' option exports exactly what you see on the screen, which also has the tracks run through the pads.

The printer output does some extra processing to clean the holes in the pads, as you have noticed.

One option would be to print to PDF, which is a standard print output option in eagle i think. Otherwise use something like imageprinter (http://code-industry.net/imageprinter.php) to 'print' to a jpeg or so.

Have fun,

Guido

Am 20.01.2014 00:54, schrieb Paul Bigwood:

Hi

 

I'm new to Eagle and have searched the forum archive but couldn't find

anything to help with this. Apologies if its been aired before.

I have created a schematic and board layout  for a simple single layer

board..

The board prints fine on my printer for etching,  but I want to export

the etch board design as an image so I can copy the image using paint or

similar programs to make multiple copies on a single etch board. (its an

Amateur radio Aerial project  that needs 10 copies of the board for the

project.), but when I export the image I get this, where the track

overlays the holes. If I  print the design on the printer it is

perfect.  I've tried all sorts of view combinations [ BOTTOM, PADS, VIA

etc ] with the export function but  always get this type of image where

the holes/ vias  are overlayed by  the tracks. You can see it clearly on

the I/O Power connections at the ends of the board.

 

I've obviously got a setting wrong somewhere as online tutorials show it

is possible!

 

Any help appreciated.

 

Paul

 

Hi Paul,

in 2006, I guess, there was a posting in one of the newsgroups dealing

with this subject.

A customer modified the Postscript definition in the CAM Processor's

configuration file so that the drill holes remained open. Let me simply

add the whole message:

<----- original post -

>

Several people have wanted to have drill-aid style functions available

when in the CAM process (drill-aid.ulp is a utility that fills in MOST

of the hold area of pads/etc so that the hole in the copper left by

photo or hobbyist plotting/etching techniques acts as a pilot hole for

drills, rather than matching the full size of the drill.)  This is very

handy for manual or non-CNC drilling.

However, this has not worked from the CAM processor; only via PRINTing,

which has assorted drawbacks if you're going to do further processing of

the output files. 

You CAN acheive drill-aid style processing via the CAM processor, at

least for postscript and embedded-postscript if you define a couple of

new output devices that constrain the size of the "holes" they print.

Use something like the following text added to eagle.def after you've

changed the "5000" to whatever you prefer for the shrunken hole size

(in 1/10000 mms, so 5000 = 0.5mm, etc)

The hole function is supposed to be for generic devices, but is only

currently implemented for postscript-like output.  A similar

redefinition should work for other devices  (I assume that gerber

doesn't actually support unfilled pads?  It's not the way gerber

works, right?)

Enjoy

BillW

-

@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)

<----- /original post -

>

BTW: The additional device definition belongs into eagle.def.

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

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

Hi Bill and Guido,

Thanks for the suggestions.

I'll try the pdf printing idea and also the CAM processing device definition.

I thought of printing it double size on my printer and then putting the printout on my scanner and importing the file into photoshop. I can then scale down to original size and

also duplicate the scan.

I'll put something on here as to how I do it in the end.

Best Regards

Paul

Hi Paul,

I have the same trouble. I created a thread some time ago, but nobody answered: PCB image export problem.

What I do to work around this is use the command Set->Misc->Display Mode. First, I set the display mode to "No Drills", and export an image like this, so I can generate the milling routing.

After that, I set the display mode to "Real", set also only the layers Dimension, Pads and Vias, and export another image, so I can generate the drill routing.

I think this is easier than printing and scanning it again.

Hope it helps,

Yuri

By the way, I made a script that makes all these setting and export the images for top and bottom layers.

I could not figure out a way to select the directory while the script is running, so I put a fixed location (desktop).

This is script is easy to understand, and you can adjust for your own use.

Here it goes:

BRD:

display = abcdefg @

set display_mode NODRILL

display none

display top -tplace -tstop

export image C:\Users\projetos5\Desktop\top.bmp monochrome 1000

display -top bottom -bplace -bstop

export image C:\Users\projetos5\Desktop\bot.bmp monochrome 1000

set display_mode REAL

display -bottom

export image C:\Users\projetos5\Desktop\top-drills.bmp monochrome 1000

display abcdefg

display = abcdefg;

The problem only occurs with version 6.5.

Using version 6.4 the problem is not present.

You can use the 6.4 version for export only immage

regards Adriano