If you have opened pcbnew (the board editor) from a KiCad project it doesn’t let you append a board (an artificial limitation IMO). You can try to open pcbnew as a standalone program, open the actual board, then append the other board, save, open again as a project. Save a backup first!
hehe
backup is allready saved now i’m so close to done 
so what i did was use gerbview to open the drill file and then save it as a new board with the front adhesion layer
then i did as @eelik suggested and i was able to append the drill board to my working one
of course all the holes for the components covers the purple dots for the holes… BUT not the via and that was the most important thing, ie i want to check that i got all the via’s
so i spend some hours to get the last few connections done and fine adjusted placements of via’s
for some reason the board has 2 ic’s on it but its not to be found on any schematic
i found what they are in a spare parts catalogue and i think i can manage to make the few connections in the schematic by looking at the board
but i have found something very frustrating… it’s the 74ls02 symbol that comes with kicad. it has the power pins hidden and i need them visible as a seperate unit. i managed to make them visible.
but dont want the symbol that shows up on unit a-d
i did google again and got no where.
a few screen captures: https://imgur.com/a/AuE4T
if i remove the checkmark for common in unit A it stays in unit A but goes away in all the others.
My aim is to remove the symbol shape only in last unit (E)
last pic on imgur is showing my problem more clear. Unit A and E are as i want them, But the rest is missing the symbol chape
figured that
it says 1 unconnected but i cant see any white lines anywhere, can kicad zoom in to where it thinks this unconnected is so i can fix it?
This thread may help
I’m unsure how KiCad DRC manages a trace that passes ‘clean over’ a pad (ie no trace corner inside pad), given your creation method, you might have one of those ?
i found it… between 2 pads on a big ic
turend out that on schematic i have by mistake placed the same wire label on the pad next to the right one
deleted the label and all was good again, but i only found out as i turned off all layers
I have fine adjusted most of the tracks on the top layer
is it possible to do octogon shaped pads in kicad? i have googled a bit but nothing comes to mind
No. In kicad v5 you will be able to use rounded rectangles or complex shapes via polygon pads.
have a strange issue
as you can see at one pad the copper flood does connect to the pad but not the other, i have checked that both pad settings are set to solid
what could be wrong here, i’m open to user mistake but i cant figure what
copper zones have an offset to the edge cuts layer.
Is there a specific reason you are using edge cuts drawings for oval “drills” instead of defining them as oval in the pad settings?
ahh will try and see if i can fix that
i used edge cut as a milling option that these holes need
EDIT: Fixed, thanks once again. It’s getting close where i should mention Kicad forum somewhere on the copper
one of the last things before i can go and fine polish every small track
i have a track that just ends blind on the board and i have routed it from the blind end
are there a way i can tell kicad what net name a track belongs to? or do i have to rip the tracks and route from the pad it connects to?
a pic says more than 1000 words: https://imgur.com/a/q6NAP
I don’t think there is a way to set the net name directly from the GUI, but a couple of possibilities;
-
Turn off DRC, connect the track to the pad you want. Then re-import the netlist. I find this causes tracks to be reassociated with the pads they are overlapping on the board, even if they weren’t drawn that way originally.
-
(For advanced users) Close the pcb, make a backup! Edit the kicad_pcb file in a text editor (but not a word processor). Find the segments with no net name and manually add the net name to them, e.g.
(segment (start 71.8656 80.9263) (end 83.9067 92.9674) (width 0.25) (layer B.Cu) (net 35))
(segment (start 85.2187 94.2794) (end 83.9067 92.9674) (width 0.25) (layer F.Cu) (net 35))
(segment (start 85.2187 95.27) (end 85.2187 94.2794) (width 0.25) (layer F.Cu) (net 35))
There is a table near the start of the kicad_pcb file giving the number for each net name.
In v5 the net can be set in track’s Properties dialog. I don’t know about v4, if it’s not there, maybe you have to try what bobc suggested.
Trying this in 5.0.0-rc2-dev-44-gde6b32d23 shows a few rules
- If the pin has a net-name, a free trace vertex routed or moved anywhere within the PAD circle, automatically gets the net name applied to the polygon.
- A free trace, (no vertex within any pins), can be tagged to any NET in the net list (but cannot be given a new net name)
- An un-named pad, can be tagged to any net in the list, but cannot be given a new net name
- Move of a free but named trace so any vertex is then within an un-named pad, loses the trace net name, but if any other vertex is anchored (vertex inside a named pad), it will keep the net name.
Not sure if there is a way to disable that last feature ?
Applying those rules, it depends on if your pad is named, and if it needs a new net name.
Best idea is to connect a net name to the pin, in the schematic, and it should automatically name the trace polygon (using the first rule).
i use 4.0.7 and yes there are only one “simple” way to do it… connect from the pad on the chip and work from there
next “problem”:
i have spent a lot of time to make the edgecut lines connect, but i have found out that the userport and cassette ports are not quite right
can i move things in blocks in a precise way? i move one outer edge and the 2 arcs as a single block say 0.6mm?
Looks like group select, and move-exact is what you need.
Select items all move grouped, & non selected item stay, so you will need to add/subtract the gaps to close the polygon.
yep… i was just about to say that i selected the parts individual and used the move exact command
another odd one…
in 3d view the pads for the userport and cassette are grey, but you can just get a glimpse that they are yellow under it
arround the lower edge and to the left plus a few spots i have added a zone that removes the solder mask
and i did the same on the pads in the upper left of the board but they still come out grey for some reason
pic from 3d view: https://imgur.com/a/7OZAG
what could it be?