Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..

2010-08-28 Thread Andy Eskelson
One other thing I've just realised:

The IC is a surface mount device Usually the module is designed for the
tracks to be on the COMPONENT side of the PCB. If you intend to produce
the PCB in the conventional way with the components on the top, and the
tracks on the other side, then you may have a problem. Check the
orientation of the IC very carefully, as you will need to fit it to the
underside (copper) side of the PCB, and that will usually mean that you
have to flip the module. 


Andy




On Sat, 28 Aug 2010 01:10:59 +0200
Fabio Varesano fabio.vares...@gmail.com 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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! Groups 
 Links
 
 
 


Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..

2010-08-27 Thread Andy Eskelson

Personally I don't like lots of filled zones unless that really are
necessary, but that's a fairly minor point.

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. 

How are you going to mount the board? Some hardware mounting holes
might be useful. 

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.

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'm not going to comment on the actual circuit as I've never used this
device.

Regards
Andy






On Fri, 27 Aug 2010 21:18:29 +0200
Fabio Varesano fabio.vares...@gmail.com wrote:

 Hi guys,
 
 I just finished working on my first pcb design and I did it with Kicad.
 
 I'm a computer science master student so I'm pretty confident with
 computers and I know my stuff in the software side of things .. but we
 don't have courses on pcb designs nor on electronics (a part from some
 phisics which covers circuits and electro-magnetism.. but nothing
 deep), so that's been quite a challenge to get were I'm right now.
 
 I'm working on my final thesis project and we are working with
 different kind of sensors (accelerometers, magnetometers, gyros and
 more) to develop nice kind of user-computer interactions such as body
 movement recognition, tangible in objects UIs, etc..
 
 Until now we used pre-made boards (Arduino and some breakout boards)
 with some soldering or bread boarding.. but I'm now feeling quite
 limited by this so I'm trying to move on and pass to the next step:
 developing my own circuits boards that fit my needs.
 
 So here I am. To make things simple I started creating something
 similar to something I already know: Sparkfun ADXL335 breakout board
 (http://www.sparkfun.com/commerce/product_info.php?products_id=9269#)
 
 I used this accelerometer in the past so I know how this works also on
 the electrical side of things.
 
 So, I designed using Kicad the schematics, the pcb layout and sorted
 out the libraries of kicad..
 
 So, I'd like you to have a look at my Kicad project and let me know
 what you think. As I said I'm a complete beginner so that's likely I
 missed lot of things there..
 
 Please note that the pcb design is going to be create with home made
 etching on a single side.
 
 This is the accelerometer I used:
 http://www.sparkfun.com/datasheets/Components/SMD/adxl335.pdf
 The schematic I wanted to copy:
 http://www.sparkfun.com/datasheets/Sensors/ADXL335_v10.pdf
 
 
 Here you find the project files
 http://www.varesano.net/temp/adxl335_breakout_board.tar.gz
 
 
 Thanks for your time,
 
 Fabio Varesano
 
 
 
 
 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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! Groups 
 Links
 
 
 


Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..

2010-08-27 Thread Fabio Varesano
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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! Groups 
Links

* To visit your group on the web, go to:
http://groups.yahoo.com/group/kicad-users/

* Your email settings:
Individual Email | Traditional

* To change settings online go to:
http://groups.yahoo.com/group/kicad-users/join
(Yahoo! ID required)

* To change settings via email:
kicad-users-dig...@yahoogroups.com 
kicad-users-fullfeatu...@yahoogroups.com

* To unsubscribe from this group, send an email to:
kicad-users-unsubscr...@yahoogroups.com

* Your use of Yahoo! Groups is subject to:
http://docs.yahoo.com/info/terms/



Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..

2010-08-27 Thread Andy Eskelson

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.


e.g.
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. 


Andy


On Sat, 28 Aug 2010 01:10:59 +0200
Fabio Varesano fabio.vares...@gmail.com 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 http://www.kicadlib.org 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 http://groups.yahoo.com/group/kicad-develYahoo! Groups 
 Links