1mm BGA virgin

So, having had one of those SMD-friendly infra-red oven heaters bought
for me as a birthday present, I'm trying to get my first ever BGA pcb
made, and I'm finding it more difficult than I'd expected. It's been
pretty easy to get PCBs manufactured before, so I'm wondering if I'm
doing something fundamentally wrong...

There's an image of the prototype board (it's basically a pin-header
mount for an ADV212 part so I can easily test out my connectivity) at
http://www.gornall.net/misc/adv212.gif. Each of the balls is 1mm
apart, and there's an array of them 11x11. I need to run vias in-
between the balls to other layers in order for it to route correctly,
and those vias have therefore to be rather small (6mil seems to fit
nicely between the balls).

My problem is finding somewhere that can drill such small vias
(pcbpool's DRU file prevents this, as does SunStone's, as does
custompcb.com, as does pcbzip.com, as does silvercircuits.com, as
does ... you get the picture). So, with no-one being able to
manufacture it, and this being my first ever BGA, I assume I'm doing
something wrong.


So:
  o Is there a PCB manufacturer who can drill tiny vias like this ?
  o Am I doing this wrong ?  Better: How am I going wrong ? :)
  o What SMT pads / via sizes would you use for a 1mm BGA part ?


Ideally I'd like to use a PCB manufacturer who takes Eagle BRD files -
I think I failed dismally at making the Gerber 274X files for
pcbfabexpress.com, though their customer service hasn't been wonderful
so far, so I'm not sure...

Anyone any ideas ?

Any help gratefully received :)

Simon

On Oct 16, 12:43 pm, Simon <goo...@gornall.net> wrote:
>
> So:
>   o Is there a PCB manufacturer who can drill tiny vias like this ?

Yes, but they are not cheap.  Last time I checked, 6 mil was quite do-
able.

>   o Am I doing this wrong ?  Better: How am I going wrong ? :)

Looking at your board, you are routing power and ground, and not very
well at that.  I would recommend using power planes; they don't add
that much cost to the boards, especially now that you can't use the
cheap-o houses.  Failing that, do it as a grid/flood, and don't use 2-
inch traces to avoid a via.

Also consider 'via in pad' construction.  Modern plating/soldering
techniques allow this (previously, the problem was flux entrapment,
that can be overcome.)

>   o What SMT pads / via sizes would you use for a 1mm BGA part ?

19 mil (0.47mm) is a typical pad size for fine-line BGAs.  Vias can be
the same size as the pads.  (19mil pads on a 1mm grid with vias
centered gets 9mil clearance.  >6 is acceptable.)

>

Look for Altera's AN114.  It has a bunch of good info about using this
size part.

If you're going to try and position/solder a fine-line BGA by hand in
a toaster oven, you're braver than me.  Good luck.

Alex.

"Simon" <google@gornall.net> wrote in message
news:ce3443d3-ccc9-4efa-833c-060060ac582b@i24g2000prf.googlegroups.com...
> So:
>   o Is there a PCB manufacturer who can drill tiny vias like this ?
>   o Am I doing this wrong ?  Better: How am I going wrong ? :)
>   o What SMT pads / via sizes would you use for a 1mm BGA part ?

Any "normal" PCB manufacturer can do this. But.... why such tiny holes? For
small vias, I define a pad size of 0.5mm/20 mil and a drill of 0.3mm/12 mil.

Meindert

On Oct 17, 12:16=A0am, "Meindert Sprang"
<m...@NOJUNKcustomORSPAMware.nl> wrote:
> "Simon" <goo...@gornall.net> wrote in message
>
> news:ce3443d3-ccc9-4efa-833c-060060ac582b@i24g2000prf.googlegroups.com...
>
> > So:
> > =A0 o Is there a PCB manufacturer who can drill tiny vias like this ?
> > =A0 o Am I doing this wrong ? =A0Better: How am I going wrong ? :)
> > =A0 o What SMT pads / via sizes would you use for a 1mm BGA part ?
>
> Any "normal" PCB manufacturer can do this. But.... why such tiny holes? F=
or
> small vias, I define a pad size of 0.5mm/20 mil and a drill of 0.3mm/12 m=
il.
>
> Meindert

Lack of experience :)

When you create a via in Eagle, it defaults to a pretty large one -
they don't fit between the BGA pads. Trying to work backwards made me
go too small, I think.

I got some great advice from Bill at www.crimpcircuits-usa.com, and I
found http://www.ddiglobal.com/press/technical_bulletins/BGA_Guidelines.pdf
(Bill actually sent me the relevant diagram from that PDF :)

Part of the problem is that I had to make the package up in Eagle
myself, and I over-estimated the size of the SMT pad (naively using
the same size as the ball). That gave me 0.6mm pads on a 1mm grid,
where I really should be using ~0.5mm pads. Using 0.5mm will give me
the crucial amount of space for a via-with-restring-and-separation
without going to tiny drill/via sizes, I think - I'll try it out as
soon as I get a chance :).

As for Alex' comment about the power plane - I did originally have
layer-2 specified as one, but in desperation (to try and get it to
route) I removed it in case it was interfering with the vias. I'll put
it back in :)

Thanks for the help :)

Simon

On Oct 17, 10:16=A0am, "Meindert Sprang"
<m...@NOJUNKcustomORSPAMware.nl> wrote:
>
> Any "normal" PCB manufacturer can do this. But.... why such tiny holes? F=
or
> small vias, I define a pad size of 0.5mm/20 mil and a drill of 0.3mm/12 m=
il.
>

Normal manufcturers nowadays have no problem making 0.2mm holes
and 0.1mm trace/gap & annular ring (costs some more, of course).
On a 1.27mm BGA, this allows (given a hole in each pads centre,
which is my way) 3 traces between the pads on both top and bottom,
thus allowing to route all signals on the top an bottom layer;
the inner layers are just power and GND planes as necessary,
split as neeeded. Looking at the first board I made using
such technology its revision texts say the year has been 2000.
(feels like it was yesterday, it is about time someone would do
something about this mad flight of time...).

Didi

------------------------------------------------------
Dimiter Popoff               Transgalactic Instruments

http://www.tgi-sci.com
------------------------------------------------------
http://www.flickr.com/photos/didi_tgi/sets/72157600228621276/

Original message: http://groups.google.com/group/comp.arch.embedded/msg/de5=
a605d1a571949?dmode=3Dsource

Simon

Take a look at PCB train in the UK, a simillar service to PCB Pool
which you mentioned. I used them to make a 1mm BGA (SPARTAN 3E) pcb
which I then soldered using a toaster oven.
I was even able to put the power pour on the top layer by carefull use
of FPGA pins to get the power out.

I'm not at the right computer, so I don't have the dimensions to hand.

Colin

On Oct 20, 2:10=A0am, "colin_toog...@yahoo.com"
<colin_toog...@yahoo.com> wrote:
> Simon
>
> Take a look at PCB train in the UK, a simillar service to PCB Pool
> which you mentioned. I used them to make a 1mm BGA (SPARTAN 3E) pcb
> which I then soldered using a toaster oven.
> I was even able to put the power pour on the top layer by carefull use
> of FPGA pins to get the power out.
>
> I'm not at the right computer, so I don't have the dimensions to hand.
>
> Colin


Thanks Colin :)

I have managed to get the thing to route, with a partial (coudn't
quite manage the entire plane) ground plane and a complete power plane
- and it conforms to the dru-settings for SunStone (http://tinyurl.com/
5u5g5o), although it took 5 hours to route, and that's on a top-end
Mac Pro - I wish Eagle had a multithreaded autorouter.... I'll
probably be ordering it this afternoon. Since I'm in the US, shipping
costs would probably be quite high from the UK, not to mention that
the exchange-rate isn't exactly favourable right now :)

Good to know you got the toaster-oven thing to work. I'm going to ease
into it, some TSOP RAM chips, a QFP (video decoder), and then the BGA
(image compression)... Rather looking forward to breaking the new
ground with the whole SMT thing :)

Cheers,
  Simon

On 20 Oct, 21:32, Simon <goo...@gornall.net> wrote:
> On Oct 20, 2:10=A0am, "colin_toog...@yahoo.com"
>
> <colin_toog...@yahoo.com> wrote:
> > Simon
>
> > Take a look at PCB train in the UK, a simillar service to PCB Pool
> > which you mentioned. I used them to make a 1mm BGA (SPARTAN 3E) pcb
> > which I then soldered using a toaster oven.
> > I was even able to put the power pour on the top layer by carefull use
> > of FPGA pins to get the power out.
>
> > I'm not at the right computer, so I don't have the dimensions to hand.
>
> > Colin
>
> Thanks Colin :)
>
> I have managed to get the thing to route, with a partial (coudn't
> quite manage the entire plane) ground plane and a complete power plane
> - and it conforms to the dru-settings for SunStone (http://tinyurl.com/
> 5u5g5o), although it took 5 hours to route, and that's on a top-end
> Mac Pro - I wish Eagle had a multithreaded autorouter.... I'll
> probably be ordering it this afternoon. Since I'm in the US, shipping
> costs would probably be quite high from the UK, not to mention that
> the exchange-rate isn't exactly favourable right now :)
>
> Good to know you got the toaster-oven thing to work. I'm going to ease
> into it, some TSOP RAM chips, a QFP (video decoder), and then the BGA
> (image compression)... Rather looking forward to breaking the new
> ground with the whole SMT thing :)
>
> Cheers,
> =A0 Simon

Simon

Two observations.

1) You only want to use the oven for the BGA, with flux as your friend
a soldering iron will make a better job of everything else. You will
find videos on youtube showing you how. Also you want to do the BGA
first so that you can look down between each row during inspection.

2) All autorouters are crap, allthough some are less crap than others
( and yes I have used SPECTRA). I guarantee that you could have got
better results doing it manually. Also, if you plan to do a lot of PCB
design you will find yourself making a much better job of placement if
you then have to route what you placed.

Email me if you want to chat about the oven some more.

Best of luck

colin

On 21 Oct, 08:24, "colin_toog...@yahoo.com" <colin_toog...@yahoo.com>
wrote:
> On 20 Oct, 21:32, Simon <goo...@gornall.net> wrote:
>
>
>
> > On Oct 20, 2:10=A0am, "colin_toog...@yahoo.com"
>
> > <colin_toog...@yahoo.com> wrote:
> > > Simon
>
> > > Take a look at PCB train in the UK, a simillar service to PCB Pool
> > > which you mentioned. I used them to make a 1mm BGA (SPARTAN 3E) pcb
> > > which I then soldered using a toaster oven.
> > > I was even able to put the power pour on the top layer by carefull us=
e
> > > of FPGA pins to get the power out.
>
> > > I'm not at the right computer, so I don't have the dimensions to hand=
.
>
> > > Colin
>
> > Thanks Colin :)
>
> > I have managed to get the thing to route, with a partial (coudn't
> > quite manage the entire plane) ground plane and a complete power plane
> > - and it conforms to the dru-settings for SunStone (http://tinyurl.com/
> > 5u5g5o), although it took 5 hours to route, and that's on a top-end
> > Mac Pro - I wish Eagle had a multithreaded autorouter.... I'll
> > probably be ordering it this afternoon. Since I'm in the US, shipping
> > costs would probably be quite high from the UK, not to mention that
> > the exchange-rate isn't exactly favourable right now :)
>
> > Good to know you got the toaster-oven thing to work. I'm going to ease
> > into it, some TSOP RAM chips, a QFP (video decoder), and then the BGA
> > (image compression)... Rather looking forward to breaking the new
> > ground with the whole SMT thing :)
>
> > Cheers,
> > =A0 Simon
>
> Simon
>
> Two observations.
>
> 1) You only want to use the oven for the BGA, with flux as your friend
> a soldering iron will make a better job of everything else. You will
> find videos on youtube showing you how. Also you want to do the BGA
> first so that you can look down between each row during inspection.
>
> 2) All autorouters are crap, allthough some are less crap than others
> ( and yes I have used SPECTRA). I guarantee that you could have got
> better results doing it manually. Also, if you plan to do a lot of PCB
> design you will find yourself making a much better job of placement if
> you then have to route what you placed.
>
> Email me if you want to chat about the oven some more.
>
> Best of luck
>
> colin

I have another question regarding power planes in a multilayer board
(6 Layers) for a 256 ball 0.8mm BGA.  From a emc point of view the
vias to the power planes should not have thermal relief, however from
a manufacturing point of view are no thermal reliefs liable to be a
problem with reflowing and joint reliability