Better Gerber Review Tools

Question

As part of my current workflow producing a PCB layout I open my gerber files using gerbv. This allows me to switch on and off layers and check things are as they should be.

However I need to present the layout to some others in my team, preferably without needing gerbv. Currently I do this by offsetting all of the layers so they can be seen individually and then print to PDF.

This is pretty tedious and I cant help thinking there is a better way, so are there any gerber viewers that support the following.

• View a stack of layers from each side of the board (Would be great if this was something like the graphical view OSH park creates - example)
• Display each layer separately, without manual offset adjustment
• Output to PDF

Answer 1

For checking gerbers, I use GC-Prevue, but it's not much different from gerbv.

If you want to generate presentable images and your CAD tool does not offer that, try looking at some 3D gerber viewer tools:

• 3D Gerber Viewer is an online tool and does a decent job, similar to your example.
• ZozfPCB is a desktop application and seems to have quite a few features. It was a bit fiddly to use last time I tried it, though.

Answer 2

It's a very late answer and I'm sure the original poster no longer needs this, but the problem is common enough and still exists.

One way to achieve this is to use gerbv to make the various layers, then Image Magick's montage and convert programs to create the file you want.

The basic idea is to use gerbv on the command line to generate intermediate images; the rest is ordinary graphics not specific to gerber.

gerbv gerberfile.gbr -xpng -o tempfile.png

In Linux or similar shell, scripting that is pretty straightforward.

Here are parts of an image showing stacks on the left (just copper and solder mask, red=top, blue=bottom) and the silkscreen of those layers.

Script:

#!/bin/sh

# gerber2pdf
# convert gerber files to review pdf
# jonathanjo/2020-06-01

set -e

if [ $# -ne 1 ]; then
    echo "Usage: `basename $0` filenamebase" >&2
    exit 1
fi

fn="$1"

tcopper='#ff0000'
bcopper='#0000ff'
mask='#ffffff40'
silk='#ffffffff'
outline='#ffff00'
pcb='#004000'
dpi=1000

tmp=/tmp/$$
for x in COPPER-TOP SOLDERMASK-TOP SILKSCREEN-TOP \
    COPPER-BOTTOM SOLDERMASK-BOTTOM SILKSCREEN-BOTTOM \
    OUTLINES; do
    f="${fn}_${x}.gbr"
    if [ ! -f "$f" ]; then
        echo "`basename $0`: $f: no such file" >&2
        exit 1
    fi
done

gerbv -D $dpi -B0 \
    -b$pcb \
    -f$mask ${fn}_SOLDERMASK-TOP.gbr \
    -f$tcopper ${fn}_COPPER-TOP.gbr \
    -f$outline ${fn}_OUTLINES.gbr \
    -xpng -o $tmp.topc.png
gerbv -D $dpi -B0 \
    -b$pcb \
    -f$mask ${fn}_SOLDERMASK-BOTTOM.gbr \
    -f$bcopper ${fn}_COPPER-BOTTOM.gbr \
    -f$outline ${fn}_OUTLINES.gbr \
    -xpng -o $tmp.botc.png
gerbv -D $dpi -B0 \
    -b$pcb \
    -f$silk ${fn}_SILKSCREEN-TOP.gbr \
    -f$outline ${fn}_OUTLINES.gbr \
    -xpng -o $tmp.tops.png
gerbv -D $dpi -B0 \
    -b$pcb \
    -f$silk ${fn}_SILKSCREEN-BOTTOM.gbr \
    -f$outline ${fn}_OUTLINES.gbr \
    -xpng -o $tmp.bots.png

# many variants of the following also sensible
montage -geometry +10+10 -label '%f' \
    $tmp.topc.png $tmp.tops.png \
    $tmp.botc.png $tmp.bots.png \
    ${fn}.png
convert ${fn}.png ${fn}.pdf

rm -f $tmp.*

# end

Answer 3

To view your gerber files, I use an free, online Gerber Viewer to check my board size, hole and track sizes and clearances of the various PCB objects.Easy to use, just drag and drop your Gerber files here Or upload it here: https://gerber-viewer.easyeda.com/

It's no need any download or installation, works in modern web browsers on Windows, Mac, Linux. Easy to see all the detail of PCB parameters before making PCB to production.