AVR-Chat

On 11/8/2010 11:30 AM, Chuck Hackett wrote:
>> -----Original Message-----
>> From: Geo
>>
>> I have had a quick look - might be easier to post the actual board files
>> as I could not switch off layers in the pdf to see things more clearly.
>
> Yup, It would be lots easier to see some stuff with some of the layers off.  I
> figured that anyone could see the PDF version but next time I'll put up PDF and
> Eagle versions.

Print each layer to a separate page pdf separately (as well as a page 
with all layers on).  Makes it easier for those without Eagle to view.

>> - There's a topside trace under IC5's tab.  It is too easy for that to short
>> to the tab
>
> I assume you mean the thin one under the two "legs"?  Yea, I'll have to watch that
> one (another Autorouter thing).  If you mean the thicker one coming from the right,
> that's GND which connects to the GND pour on the large tab of the 7805.

Another place to use Eagles restrict layers.  There is a layer to mark 
areas where vias should not be placed, one to mark where component side 
copper traces should not be routed and one to mark where solder side 
copper should not be routed.  More notes on autorouting later.

>>     - Consider adding power and ground planes.  It frees up your
>> available routing space considerably.  Also keeps supply impedances low.
>>    That will likely mean not using milling but in my experience milling
>> PCBs is overrated.
>
> How do power and GND planes prevent using isolation routing (I use pcb-gcode)?

Well, you could glue boards together after routing them to produce a 
four layer board.  I know it can be done but I've never been tempted to 
try. The usual technique, I understand, is to route the inner planes 
(usually power and ground) first on a double sided board and then route 
the signal layers on single sided boards before glueing the whole thing 
together.  I don't recall how connections were made to the inner layers.

Me, I let a board house take care of it, they have proper plating 
equipment to plate the vias to connect to the inner layers.

Proper power and ground planes do help routing a lot.  Since power 
traces are never very long, just long enough to drop a via to the plane, 
your signals never need to crawl all over the place to weave in amongst 
power and ground traces.

I really recommend you at least try routing with separate power and 
ground planes (IE a four layer board) and see how it frees things up for 
you.

> After doing some fine tuning on my mill I have found 10 mill traces/separation not a
> problem.
>
> In many cases I have increased the actual amount of copper that I remove (space
> between traces shown by Eagle) so that soldering is easier since there is no solder
> mask to prevent bridges (I wish I had steadier hands!)
>
>>     - Use Eagles via restrict layer to keep layers from underneath
>> connectors and chips.  Especially valuable when hand populating since it
>> considerably reduces the chances of a short and since vias are now
>> accessible the are available for adding test points or patches.  You may
>> have to accept some vias in unfortunate places but I'd at least try to
>> remove the issue. Auto-routers will relieve you of tedious work but they
>> need a lot of guidance to work well.
>
> Thanks for that ...
>
> Anywhere you know of to get more detailed info on the Autorouter?

Years ago on Eagle's support forums there was a few comments from one of 
Eagle's developers.  Mostly commenting on an autorouter control file 
submitted by a user that produced better results.  I still have that 
around and use variations on it since I'm using the oder version.  It 
might be worth tracking that commentary down but I don't remember there 
being a lot of meat to sink your teeth into.

A few suggestions for making optimal use of the autorouter.  Eagle's is 
not state of the art but it is useful for those of us who can't route 
1000 signal an hour on a 10,000 signal board.

    - First use it to help optimize part placement. By rough placing 
parts and doing an autoroute some changes to placement that would be 
easier to route become obvious that are not obvious when everything is 
obscured by the ratsnest.  Sometimes a couple of cycles of autoroute, 
ripup, move can make quite a difference.

    - Second hand route critical traces. Those that you want just so. 
Sometimes you can get a reasonable first pass on those by autorouting 
just the critical signals and then hand optimizing.  Save this as an 
intermediate file so you can use it as a base for further autorouting. 
Rather than ripping up the whole board, or tediously selecting what to 
rip-up yo simply start with a previously saved version that has what you 
want to keep constant as you work on other routing.

    - Make use of keep outs and restricts.  One useful technique when 
routing a number of parallel lines is rather than rely on the autorouter 
to get is correct when considering everything is to create a routing 
channel with restrict areas to hem in the traces.  Then route just the 
signals that are running parallel.

    - after everything is routed, review the result for obvious 
optimizations to do by hand.

All of this is more work than just letting the autorouter do whatever it 
wants but less than doing everything by hand.  The results are likewise 
intermediate.  Generally, however, only a few areas are critical enough 
to require hand attention.

Myself I find Eagle's biggest lack not the old autorouter but the fact 
it doesn't have hierarchical schematics.



>
>>     - I'd be worried about the size of the heat sink on the regulator.
>> You won't need much of a voltage drop or current draw to overwhelm it.
>> Consider more copper on multiple layers with thermal vias.
>
> I don't think I'll be taxing the regulator at the moment but I'll watch that.
>
> I also ran into a problem with the Autorouter where, without a GND pour it would
> route the board 100% but with a GND pour (polygon covering the whole board) it would
> not route 100% (the polygon fell apart in places).  Ideas?

Yep, only flood fill after routing.  It's another reason to use power 
and ground planes instead of flood fill.

>
>>     - I don't trust crystals to sockets, I'd solder it to the board.
>
> At the moment I wanted to use a socket because I was not absolutely positive that I
> would stick with the 14.xxx Mhz Xtal, but, since customers will be handling these in
> the field, I think I agree that it might be a good idea to solder them to protect
> against one vibrating loose.

Unless you expect the customers to replace the crystal I wouldn't even 
consider socketing it for an embedded device.

>>     - Add a silkscreen rectangle (or several) for notes in marker such as
>> stuff date, version etc...
>>     - I normally put PCB part number and rev in copper (the stuffed board
>> gets a part number and rev written by marker on silkscreen rectangles)
>
> In the lower-left corner I have a Part number (BC002) and version date (2010-10-18)
> in the silkscreen (top side).  Hadn't considered another additional info on the
> copper side.  After all, they are usually together :-)

I use the copper for PCB part and rev info and a write on silkscreen 
section for the stuffed board part number and rev.  On occasion there's 
not enough room in the copper to put board info and I have to move it to 
the silkscreen.

A also usually put a layer indicator in each copper layer so I might 
have one copper layer labelled Component, one labelled solder, one 
labelled Power and one labelled Ground.  I've also seen them labelled 0, 
1, 2, 3.  Mostly a holdover from manual tape and photo days but still 
occaisionally useful, if nothing else it's a nice paranoid double check. 
  There's that word again. :)

>
>>     - Samtec has a nice sealed connector with a pigtail to a board
>> mounted socket that might work for your application, I can look up the
>> part number if you like.
>
> Always looking for a better way - fire away ...

Take a look at the SCP/SCR series.   I used the SCP2/SCR2 series on a 
recent project.  A nice sealed plug at the case and a simple dual header 
style plug on the PCB with a prewired connection between them.  ANd from 
Samtec you can get them in small quantities for a reasonable price

http://www.samtec.com/Search/Search.aspx?q=scp#Results

>
>>     - Don't be afraid to put components on the back of the board,
>> particularly passives.  That can free up considerable room if you are
>> using surface mount and if you are hand stuffing it's not usually harder
>> to handle.
>
> The only negative I can think of is that, having SMDs on the back side rules out
> "hot plate" soldering for one side.  I do have a hot air "pencil iron" size
> soldering iron (~1/16" air discharge) that I use for individual parts - I'm a
> beginner at this SMD stuff :-)

You can leave them until you've done all the fine pitch components with 
the fancy gear.  Standard 0805 and larger passives are straightforward 
to do with an ordinary iron.

>> Robert has a good point about REV number etc on the PCB. This way you will
>> know at a glance which version this is, if you happen to make a few modified
>> versions over time.
>
> Changes?  Why would I do that?  :-)

Nah, never happen. :) I forgot to mention another use for those 
silkscreen rectangles is as a place to write a S/N

Enjoy

Robert

-- 
http://www.aeolusdevelopment.com/

  From the Divided by a Common Language File (Edited to protect the guilty)
ME - "I'd like to get Price and delivery for connector Part # XXXXX"
Dist./Rep - "$X.XX Lead time 37 days"
ME - "Anything we can do about lead time?  37 days seems a bit high."
Dist./Rep - "that is the lead time given because our stock is live....
we currently have stock."