Zone filling does help with the etchant usage, but I don't tend to go
overboard with it. For example I would not have bothered to fill the
small area to the bottom left and bottom right  hand corner of the IC
(breakout board-back.pdf Also that long tail extending down between the
top right hand connection pin and the one below. It looks as if it should
be going to an IC pin, but it's part of the zone fill.

No reason to remove them, just my personal preference. You will find that
there is a lot of than in PCB work...

There are lots of 6 pin conectors. A simple 0.1 inch header can be used, 
SIL-6 is one, or Head_4x2 (8 pins) pin_aray_3x2 to name a few.

There are dozens of connectors, some will not be in the libs, you might
find them elsewhere, but a simple connector is good practice for drawing
up your own module give it a try. 

If you have not already done so, print out the module documentation from
CVpcb. ("display footprints list documentation) 3rd icon from right in my
version. It useful to have that by your side when choosing modules. You
can also find that document in : /usr/local/kicad/doc/help/footprints_doc
or under kicad in program files if using windows.

With mounting holes, so people just use a big pad and set the drill size
to what they want, while others draw it graphically. If you are going to
have the board made by a production house then you need to define it as
the correct size. For home production I just shove a normal pad down. The
hole when etched makes a good drill centre.

The tracks, yes you need them the correct size for the IC pin spacing, 
But you seem to have made that the thickest track you have used. When
hand soldering, thin tracks lift very easily. Likewise, give yourself
plenty of clearance to avoid solder bridges when building the units. You
will not have any solder mask on the board, so the extra clearance makes
it less likely for solder splashes to happen, and if they do they are
easier to clear.

The tracks from the other side of some of the connection pads look
thinner than the tracks from the IC, that could be a product of the
pdf...I will check... No the postscript looks much the same. 

For such a small board you have a lot of PCB area, so make use of it.

The links, yes spot on, treat them as component side wiring. If you had
any wire ended components in the design, they can also be used  be used to
bridge over tracks. 


On Sat, 28 Aug 2010 01:10:59 +0200
Fabio Varesano <> wrote:

> Hi Andy, thanks for having a look at this. Please read below..
> On 08/27/2010 11:38 PM, Andy Eskelson wrote:
> >  
> > 
> > 
> > Personally I don't like lots of filled zones unless that really are
> > necessary, but that's a fairly minor point.
> Well, I read that this is good practice as this make less use of
> etchant during the etching process. Isn't that true?
> > several other points:
> > 
> > Do try to put your connection pins on the edge of the board. It makes
> > wiring up much easier. You could also consider some form of connector.
> Yep, that's the best I've been able to come out with.. I do know that
> it will be painful to plug this. Do you have any suggestion for a 6
> pin connector? Somehow I didn't find something suitable in the library.
> > 
> > How are you going to mount the board? Some hardware mounting holes
> > might be useful.
> Yep, good point. How do you draw mounting holes with kicad?
> > 
> > The tracks to the pins look rather thin. Thin tracks tend to lift when
> > soldering, also a small speck of dust on the film can cause a
> > break in the track. Using a thicker track will help in both cases.
> You mean the tracks to the accelerometer IC? Well, they quite match
> the IC pins size. I don't think I could have made them bigger. Maybe
> you are suggesting making them thin below the IC and bigger on the
> rest of the board?
> > 
> > On single sided boards, don't be afraid to use a few links it makes life
> > MUCH easier.
> > 
> > An Easy way to do this is to treat the board as double sided, and use the
> > top tracks as wire links. Beef up the vias to a suitable size to take your
> > wire links. Obviously you need to manually route this.
> > 
> I understand. So you are using wires as bridges to pass over one or
> more track, right? Interesting..
> Thanks for your suggestions. Really helpful. You rock!
> FV
> ------------------------------------
> Please read the Kicad FAQ in the group files section before posting your 
> question.
> Please post your bug reports here. They will be picked up by the creator of 
> Kicad.
> Please visit for details of how to contribute your 
> symbols/modules to the kicad library.
> For building Kicad from source and other development questions visit the 
> kicad-devel group at! Groups 
> Links

Reply via email to