Google Groups no longer supports new Usenet posts or subscriptions. Historical content remains viewable.
Dismiss

PCB Layout for BGAs

127 views
Skip to first unread message

gnuarm.del...@gmail.com

unread,
Jan 7, 2023, 12:49:27 PM1/7/23
to
A small board with a 100QFP is being redesigned for a new FPGA due to obsolescence. Gowin makes a 100QFP device that would be a good fit, but my customer has said "no" to the 100% Chinese brand... US government customers, ya know!

So now I'm looking at a BGA. I don't want to get into fine PCB design rules, so 1.0 mm ball pitch is my preference. The only devices I can find that fit on the board have 196 or 256 pins. But the real problem is availability.

Digikey has a few of the XC7S15-1FTGB196I and more a scheduled for delivery in April. Add in the various speed and temperature flavors trickling in (mostly in April) and I should be ok for the initial delivery in August... if I can get my hands on those. I don't know if Digikey factors in the backlog orders in these counts.

Mouser shows great inventory of Efinix parts, particularly the T13 and T20 in a 0.8 mm 256 pin BGA, 10s of thousands in stock. But I'd rather work with a 1.0 mm BGA. Oddly enough, LCSC shows part numbers, but zero inventory.

Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use? Did this impact the PWB cost?

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209

David Brown

unread,
Jan 8, 2023, 7:52:02 AM1/8/23
to
It's difficult to know the impact without knowing details of the board
you have at the moment. It is also somewhat dependent on the layout of
the balls on the part - some BGA's have missing balls, or their central
balls all connected to ground to make layout easier.

In general, 0.8 mm pitch should be doable in four layers, but you might
need finer tracks and clearances than you used before. In a recent
board we did, the 0.8 mm pitch BGA was fine with four layers and normal
vias. We did not need to switch to 6 layers with advanced vias until we
moved to the 0.65 mm version.

gnuarm.del...@gmail.com

unread,
Jan 8, 2023, 2:01:32 PM1/8/23
to
What are "normal" vias and track/space widths? All of the BGAs I'm looking at are solid arrays. I'd give you identifiers of the packages, but I've never found standard terms. Everyone has unique identifiers and more than one! Packaging is insane! I especially love how TI adds it to their data sheets with the reel packing and boxing data ahead of the package mechanical data. I'm sure that stuff is important to someone, but they could have a separate data sheet with all that. Some companies do that with the package mechanical data. Gotta love diversity... or not.

My board is already 6 layers because of the high density and narrow width, 23 mm x 115 mm. One layer is pretty much nothing but lengthwise routing and it's still very congested. Surface layers are hard to route on. Between the parts and the vias, there's no room left. In the new layout, a couple of larger chips are going bye bye, so maybe that will improve things a bit. But they are asking for some new features that will add some chips, so it may be an even swap.

--

Rick C.

+ Get 1,000 miles of free Supercharging
+ Tesla referral code - https://ts.la/richard11209

David Brown

unread,
Jan 9, 2023, 4:02:43 AM1/9/23
to
By "normal" vias I mean through-hole, without plugging or tenting - the
cheap ones. And by "normal" track widths and spacing, I mean the
perhaps 6 mil - cheap sizes that any pcb manufacturer can make without
extra charge. Basically, at 0.8 mm BGA we didn't need to do anything
special or consider it an especially high-density card. It was still an
effort to route, as there are a lot of connections in a small area. But
it didn't need extra cost for the pcb.

If you are already congested at 6 layers on the board, then you will
might have to go for beyond that. The first step is to talk to your pcb
and board manufacturers about via-in-pad, using tented or plugged vias.
If you can put the vias on the pads themselves, without causing voids
or blowouts during soldering, you can save a /lot/ of space. Next step
beyond that is microvias from outer layers to layers 2 and 5. We had to
do that for the 0.65 mm package BGA.

gnuarm.del...@gmail.com

unread,
Jan 9, 2023, 5:42:34 AM1/9/23
to
So you don't know what size ball pad, via pad/drill and trace/space you actually used? I'm finding it a bit harder than I expected to figure out dimensions that work. I'd love to use the Xilinx 196 ball, 1.0 mm pitch part, but they are still pretty hard to get. Efinix has nothing but smaller pitch BGAs. 256 ball, 0.8 mm pitch, or 169 ball, 0.65 mm pitch. 0.65 mm pitch just won't work for me.


> If you are already congested at 6 layers on the board, then you will
> might have to go for beyond that. The first step is to talk to your pcb
> and board manufacturers about via-in-pad, using tented or plugged vias.
> If you can put the vias on the pads themselves, without causing voids
> or blowouts during soldering, you can save a /lot/ of space. Next step
> beyond that is microvias from outer layers to layers 2 and 5. We had to
> do that for the 0.65 mm package BGA.

Absolutely not interested in 0.65 mm pitch, or any of the high density techniques like via in pad.

I can get away with nearly no vias, if I can route two traces between pins. That works at 1.0 mm, but at 0.8 mm, the trace/space has to be pretty small.

JLCPCB lists 0.2 mm drill (8 mil) and 0.45 mm via pads (18 mil). Assuming BGA lands of 0.4 mm means you can route 2 traces between pads only with 0.08 mm (3.2 mil) trace/space. Routing between the via holes is also tight, with trace/space of 0.08 mm (3.2 mil) and 0.13 mm (5.1 mil) (according to Xilinx). I've read elsewhere that the space to the via drill should be 0.2 mm (8 mil) minimum for lower cost boards, so this doesn't sound good for routing two traces. With that restriction, I could only route two rows of pins without vias. Adding vias to escape the BGA makes the entire section of the board a difficult for routing.

Yeah, I'd much prefer to go with a 1.0 mm part like the Xilinx 196 ball Spartan 7 parts. I just don't know if I'll be able to get them.

--

Rick C.

-- Get 1,000 miles of free Supercharging
-- Tesla referral code - https://ts.la/richard11209

David Brown

unread,
Jan 9, 2023, 7:42:20 AM1/9/23
to
I'm afraid I don't remember the sizes used - I was not directly involved
in the layout and routing. (I've done fine-pitched BGA layout, but it's
probably 15 years since I did a pcb design myself.)

Is it the routing you see as a problem for 0.65 mm pitch, or the cost of
boards with high density features, or the production of them? We have
found that while the 0.65 mm pitch parts were harder for the layout and
a little more expensive for the boards, parts in these packages can be a
lot easier to get hold of. The choice of 0.65 mm or 0.8 mm was forced
by component availability, rather than as a preference by our layout
folk. (Our production people have no qualms about mounting small pitch
BGAs.)

>
>> If you are already congested at 6 layers on the board, then you
>> will might have to go for beyond that. The first step is to talk to
>> your pcb and board manufacturers about via-in-pad, using tented or
>> plugged vias. If you can put the vias on the pads themselves,
>> without causing voids or blowouts during soldering, you can save a
>> /lot/ of space. Next step beyond that is microvias from outer
>> layers to layers 2 and 5. We had to do that for the 0.65 mm package
>> BGA.
>
> Absolutely not interested in 0.65 mm pitch, or any of the high
> density techniques like via in pad.
>
> I can get away with nearly no vias, if I can route two traces between
> pins. That works at 1.0 mm, but at 0.8 mm, the trace/space has to be
> pretty small.
>
> JLCPCB lists 0.2 mm drill (8 mil) and 0.45 mm via pads (18 mil).
> Assuming BGA lands of 0.4 mm means you can route 2 traces between
> pads only with 0.08 mm (3.2 mil) trace/space. Routing between the
> via holes is also tight, with trace/space of 0.08 mm (3.2 mil) and
> 0.13 mm (5.1 mil) (according to Xilinx). I've read elsewhere that
> the space to the via drill should be 0.2 mm (8 mil) minimum for lower
> cost boards, so this doesn't sound good for routing two traces. With
> that restriction, I could only route two rows of pins without vias.
> Adding vias to escape the BGA makes the entire section of the board a
> difficult for routing.
>

Mechanical drilling has a lot bigger tolerances than laser drilling, so
you do need to have extra space between the via hole and tracks on the
internal layers to account for the inaccuracies. Some manufacturers
will give you tighter specifications - in particular, some use lasers
for 0.2 mm holes. (And some, on the other hand, use mechanical drills
and charge extra for 0.2 mm holes due to extra breakage of the small
drill bits.)

> Yeah, I'd much prefer to go with a 1.0 mm part like the Xilinx 196
> ball Spartan 7 parts. I just don't know if I'll be able to get
> them.
>

That's always the big problem these days. I'm afraid I can't give much
advice there (at least, nothing that you won't already have thought of
yourself) - we are all in the same boat.


Theo

unread,
Jan 9, 2023, 9:50:52 AM1/9/23
to
gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
> Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use?
> Did this impact the PWB cost?

I've not done this for real, but I did a bit of playing around with PCB
routing such BGA FPGAs. I was trying to see if it was feasible to use them
on cheap PCB processes with basic soldering (I never actually made any
boards to test it). One of the limitations of cheap processes is the
tolerances can be quite slack: eg 6mil track width/spacing, which makes
doing the BGA escapes hard.

An interesting (to me) observation was that you may be able to make PCB
routing easier by choosing your pinout wisely - eg don't route signals from
inner or adjacent balls where you don't need them. That means it wasn't
such a headache to have more pins because you can ignore many of them. For
some of them, it was fine to short adjacent pins to (safe) power rails if it
wasn't possible to separate them.

Another observation was that it might be fine to have a net route through
unused pins if they're all high impedance in the FPGA config. I'd not do
this for fast signals, but maybe OK for slow/static ones.

Not ideal, but a couple of tricks where FPGAs offer a little bit more PCB
routing flexibility compared with off the shelf parts.

Theo

gnuarm.del...@gmail.com

unread,
Jan 9, 2023, 5:46:49 PM1/9/23
to
I'm trying to be as conservative as possible. I'd rather not use BGAs at all, but the only QFPs I can find that fit on the board are Gowin, which is not on the approved vendor list with my customer. They are too Chinese.

I'm concerned about adding cost for the boards, cost for the assembly and just an easy road forward. I spend the last two years building 8,000 units when the CODEC factory burnt down. The customer knows about this issue, but the previous CM turned flaky on me and all but stopped delivering product.

I have a new CM, but I don't want to go through production problems again.
JLCPCB does 0.2 mm holes without extra charge, along with 0.45 mm via pads. They charge a bit extra for 0.4 mm pads. I guess it makes for a smaller target. I look at various PCB maker's pages to see what they state they can do.


> > Yeah, I'd much prefer to go with a 1.0 mm part like the Xilinx 196
> > ball Spartan 7 parts. I just don't know if I'll be able to get
> > them.
> >
> That's always the big problem these days. I'm afraid I can't give much
> advice there (at least, nothing that you won't already have thought of
> yourself) - we are all in the same boat.

Yeah, I need to get in touch with a real distributor, rather than the web guys. Someone who has a sales person who will work with me. I remember in 1999, when I started working for myself, the sales people were dying to get their foot in the door. They quoted me great prices! Now, not so much.

--

Rick C.

-+ Get 1,000 miles of free Supercharging
-+ Tesla referral code - https://ts.la/richard11209

Stef

unread,
Jan 9, 2023, 7:30:34 PM1/9/23
to
On 2023-01-09 gnuarm.del...@gmail.com wrote in comp.arch.fpga:
>
> I'm trying to be as conservative as possible. I'd rather not use BGAs at all, but the only QFPs I can find that fit on the board are Gowin, which is not on the approved vendor list with my customer. They are too Chinese.
>

Digikey has a number of FPGAs in QFP100/144 in stock. Efinix,
Microchip, Lattice, Xilinx. Nothing that suits your needs?

--
Stef

Kinkler's First Law:
Responsibility always exceeds authority.

Kinkler's Second Law:
All the easy problems have been solved.

gnuarm.del...@gmail.com

unread,
Jan 9, 2023, 8:59:22 PM1/9/23
to
On Monday, January 9, 2023 at 7:30:34 PM UTC-5, Stef wrote:
> On 2023-01-09 gnuarm.del...@gmail.com wrote in comp.arch.fpga:
> >
> > I'm trying to be as conservative as possible. I'd rather not use BGAs at all, but the only QFPs I can find that fit on the board are Gowin, which is not on the approved vendor list with my customer. They are too Chinese.
> >
> Digikey has a number of FPGAs in QFP100/144 in stock. Efinix,
> Microchip, Lattice, Xilinx. Nothing that suits your needs?

The QFP144 is far too large. Efinix has no QFP100 parts. Lattice has no QFP100 parts that I've seen since the LFXP parts revision 2.0 of my board used. Xilinx has not had any in decades, unless you mean the very small, yet expensive CPLD thing they sell. Microchip might have some QFP100 parts in one of their older lines that I'm not so familiar with. I believe their logic cells can be either logic, or FFs, but not both. So you need roughly double the count, if not more. They are very expensive too. I've never been inclined to research such an old product, much like the Spartan 3. I get that in a QFP100, but how long will they continue to make Spartan 3 devices... which have also climbed significantly in price. It's what is called NRND. Gowin would have been perfect, but at one point they were put on a US list of CCMC (Communist Chinese Military Companies). Even though they were taken off, my customer sells a lot to the US government, so they don't like the "optics".

Did I miss any?

Trust me, I've been traveling this road for the last eight years from when Lattice first announced the end of the line for the LFXP parts. Surprisingly, I noticed the other day that Arrow, who invested heavily in the line when Lattice announced EOL, still has almost 30,000 of them. In theory, I could continue to use those, but I do expect to sell more than 30,000 over the next 10 years. In fact, I am going to turn this over to a CM, who will in turn, pay me a royalty for every unit shipped. Other than consulting, I will be out of the business, but still receive payments for everything sold. I won't be the guy worrying about where to find what part!

At this point, I'd be happy with the Xilinx XC7S15-1FTGB196I. Digikey has over 800 in stock which is more than half of what I need. They claim they will have the rest by April. I just don't know how to get on the list to receive them. I guess the fact that they have inventory, means no one is in line to get the April lot. I really need to talk to someone who can give me straight answers about the future availability though. It would not help to design in a part that let's me ship the first order, then not receive any parts for the next year!

--

Rick C.

+- Get 1,000 miles of free Supercharging
+- Tesla referral code - https://ts.la/richard11209

Stef

unread,
Jan 10, 2023, 3:52:54 AM1/10/23
to
On 2023-01-10 gnuarm.del...@gmail.com wrote in comp.arch.fpga:
> On Monday, January 9, 2023 at 7:30:34 PM UTC-5, Stef wrote:
>> On 2023-01-09 gnuarm.del...@gmail.com wrote in comp.arch.fpga:
>> >
>> > I'm trying to be as conservative as possible. I'd rather not use BGAs at all, but the only QFPs I can find that fit on the board are Gowin, which is not on the approved vendor list with my customer. They are too Chinese.
>> >
>> Digikey has a number of FPGAs in QFP100/144 in stock. Efinix,
>> Microchip, Lattice, Xilinx. Nothing that suits your needs?
>
> The QFP144 is far too large. Efinix has no QFP100 parts. Lattice has no QFP100 parts that I've seen since the LFXP parts revision 2.0 of my board used. Xilinx has not had any in decades, unless you mean the very small, yet expensive CPLD thing they sell. Microchip might have some QFP100 parts in one of their older lines that I'm not so familiar with. I believe their logic cells can be either logic, or FFs, but not both. So you need roughly double the count, if not more. They are very expensive too. I've never been inclined to research such an old product, much like the Spartan 3. I get that in a QFP100, but how long will they continue to make Spartan 3 devices... which have also climbed significantly in price. It's what is called NRND. Gowin would have been perfect, but at one point they were put on a US list of CCMC (Communist Chinese Military Companies). Even though they were taken off, my customer sells a lot to the US government, so they don't like the "optics".
>
> Did I miss any?

Okay, QFP144 is too large, that severily limits the QFP options, but
Lattice does have a QFP100: ICE40HX1K-VQ100. But this one may not have
enough logic for you, its the smallest in the series.

--
Stef

Rube Walker: "Hey, Yogi, what time is it?"
Yogi Berra: "You mean now?"

gnuarm.del...@gmail.com

unread,
Jan 10, 2023, 9:20:02 AM1/10/23
to
No, that is too small. They also have a QFN84, which unfortunately is two rows, requiring finer than 0.1 mm trace/space. Again, only supporting the 1K size, and oddly enough, no support for the PLL.

The current design is 3 kLUTs at 90% utilization. I was surprised it fit. I don't want to squeeze a new design so tightly, and I need to add some logic, so I'm shooting for at least a 5 kLUT part and prefer larger. The current design has uLaw and I'd like to be able to add Alaw, not that it's a lot of logic, but it's something more than a couple of LUTs. Then there's the multipliers... the current design uses one multiply, done using LUTs. I've been asked to provide gain controls, requiring two more multipliers, 16 x 8 minimum. This could be done by shift and add, so not horribly large. But built in multipliers would help with the size and the iCE40 line has none.

Oddly enough, many of the Lattice lines (even relatively modern ones) have no multipliers. The entire XO3 line has no multipliers. The MachXO3D has a couple of parts in an QFN72 with enough I/Os (barely), but not much availability. Hmmm... this may have improved. The MachXO3D-9400 has enough inventory in various configurations to do the initial order. But the I/O count on the QFN72 probably won't be enough with the added features. Ignoring that, the current inventory might get me through the current order, but 53 weeks for any further inventory. Digikey tells you more are coming in April. When you enter a number, it's always available in April, even a million.

--

Rick C.

++ Get 1,000 miles of free Supercharging
++ Tesla referral code - https://ts.la/richard11209

jan Coombs

unread,
Jan 10, 2023, 12:33:54 PM1/10/23
to
On Tue, 10 Jan 2023 06:19:58 -0800 (PST)
"gnuarm.del...@gmail.com" <gnuarm.del...@gmail.com> wrote:

> But built in multipliers would help with the size and the iCE40 line has none.

Just four or eight multipliers, and many more on-chip goodies:

https://www.latticesemi.com/en/Products/FPGAandCPLD/iCE40UltraPlus

dev board
https://tinyvision.ai/collections/kits/products/upduino-v3-1

Jan Coombs
--


Michael Schwingen

unread,
Jan 10, 2023, 1:35:24 PM1/10/23
to
On 2023-01-09, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
>
> I'm concerned about adding cost for the boards, cost for the assembly and
> just an easy road forward. I spend the last two years building 8,000
> units when the CODEC factory burnt down. The customer knows about this
> issue, but the previous CM turned flaky on me and all but stopped
> delivering product.
>
> I have a new CM, but I don't want to go through production problems again.

0.8mm BGA should be no problem for any reputable CM - fine-pitch QFP is
usually more trouble.

> JLCPCB does 0.2 mm holes without extra charge, along with 0.45 mm via
> pads. They charge a bit extra for 0.4 mm pads. I guess it makes for a
> smaller target. I look at various PCB maker's pages to see what they
> state they can do.

That should be enough to fit a via between the 0.8mm-BGA pads - that's what
we do regulary. If you want blocking caps underneath the BGA, you will
probably require plugged/plated vias. You will have to look at the pinout
and do the fanout routing to see how many layers you need.

Talk to your PCB manufacturer about the details before doing the final
layout - there is some fine tuning (eg. drill size, annular ring, spacing)
where different PCB manufacturers have different preferences regarding which
rules will yield good results - when doing do, 0.8mm BGA should be possible
at modest PCB costs.

cu
Michael
--
Some people have no respect of age unless it is bottled.

Michael Schwingen

unread,
Jan 10, 2023, 1:39:43 PM1/10/23
to
On 2023-01-10, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
>
> The QFP144 is far too large. Efinix has no QFP100 parts. Lattice has no
> QFP100 parts that I've seen since the LFXP parts revision 2.0 of my board
> used.

We have used Lattice MachXO2 in TQFP100 in the past - not sure if these fit
your needs.

> At this point, I'd be happy with the Xilinx XC7S15-1FTGB196I.

Okay, this sounds like the MXO2 might be two sizes to small for you.

gnuarm.del...@gmail.com

unread,
Jan 10, 2023, 5:17:35 PM1/10/23
to
Yes, sorry, they do make a few multiplier chips with FPGA tiles. I was referring to parts that I might be able to use. They have a couple of 8 kLUT parts, only one in a package that I could use. I can pick between a 0.8 mm ball pitch, or 0.65 mm. Not really excited about either, even though there's a bit of inventory of the 256 ball, 0.8 mm part. But no insight into future deliveries.

This looking for usable parts gets old fast, and I've been doing it for over a year now. When I find the guy responsible for this shortage, I'm going to give him a piece of my mind!

--

Rick C.

--- Get 1,000 miles of free Supercharging
--- Tesla referral code - https://ts.la/richard11209

gnuarm.del...@gmail.com

unread,
Jan 10, 2023, 5:44:31 PM1/10/23
to
On Tuesday, January 10, 2023 at 1:35:24 PM UTC-5, Michael Schwingen wrote:
> On 2023-01-09, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
> >
> > I'm concerned about adding cost for the boards, cost for the assembly and
> > just an easy road forward. I spend the last two years building 8,000
> > units when the CODEC factory burnt down. The customer knows about this
> > issue, but the previous CM turned flaky on me and all but stopped
> > delivering product.
> >
> > I have a new CM, but I don't want to go through production problems again.
> 0.8mm BGA should be no problem for any reputable CM - fine-pitch QFP is
> usually more trouble.

Part of my problem is a lack of having designed with BGAs before. I can find footprint recommendations, but they are different for every manufacturer. It didn't occur to me that this might be because even though they have the same pitch and ball count, they may not have the same ball size.

The two primary choices right now are a 196 ball, 1.0 mm pitch and 256 ball, 0.8 mm pitch. Can you share the design rules you used for these parts?


> > JLCPCB does 0.2 mm holes without extra charge, along with 0.45 mm via
> > pads. They charge a bit extra for 0.4 mm pads. I guess it makes for a
> > smaller target. I look at various PCB maker's pages to see what they
> > state they can do.
> That should be enough to fit a via between the 0.8mm-BGA pads - that's what
> we do regulary. If you want blocking caps underneath the BGA, you will
> probably require plugged/plated vias. You will have to look at the pinout
> and do the fanout routing to see how many layers you need.
>
> Talk to your PCB manufacturer about the details before doing the final
> layout - there is some fine tuning (eg. drill size, annular ring, spacing)
> where different PCB manufacturers have different preferences regarding which
> rules will yield good results - when doing do, 0.8mm BGA should be possible
> at modest PCB costs.

You mean my CM who orders the PWBs? Yeah, I've tried asking before and they say they would need a design so they could get a quote. I know, that sounds lame, but I used four different CMs over the last decade and they have all said the same thing. They don't have design rules, that's for me to know.

--

Rick C.

--+ Get 1,000 miles of free Supercharging
--+ Tesla referral code - https://ts.la/richard11209

gnuarm.del...@gmail.com

unread,
Jan 10, 2023, 6:48:55 PM1/10/23
to
On Tuesday, January 10, 2023 at 1:39:43 PM UTC-5, Michael Schwingen wrote:
> On 2023-01-10, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
> >
> > The QFP144 is far too large. Efinix has no QFP100 parts. Lattice has no
> > QFP100 parts that I've seen since the LFXP parts revision 2.0 of my board
> > used.
> We have used Lattice MachXO2 in TQFP100 in the past - not sure if these fit
> your needs.
> > At this point, I'd be happy with the Xilinx XC7S15-1FTGB196I.
> Okay, this sounds like the MXO2 might be two sizes to small for you.

I have the Lattice selection guide, the Lattice package guide, Lattice data sheets and have marked all the packages I might use on all the parts I might use.

No, the MXO2 parts are pretty limited for this. The existing design is shoehorned into the 3 kLUT XP part. I was surprised it routed. I have to add some logic and I don't have the same confidence in routing, so I want plenty of room in this part. 5 kLUTs should do the job, but I'd like to have a bit more. The Xilinx part has 6000 LCs, but there is no such thing as a LC in a Xilinx part, that's a marketing term. The XC7S6 has 3,752 6LUTs and twice that many FFs, so it should be about like an 8 kLUT device, but who knows if the routing is up to it. The only one in stock is the XC7S15, so that's the one I would use, at least to start. But I need a better price than the $25, and some expectation of getting more parts.

Anyone see signs of the shortages easing?

--

Rick C.

-+- Get 1,000 miles of free Supercharging
-+- Tesla referral code - https://ts.la/richard11209

David Brown

unread,
Jan 11, 2023, 5:26:48 AM1/11/23
to
On 10/01/2023 23:17, gnuarm.del...@gmail.com wrote:
>
> Yes, sorry, they do make a few multiplier chips with FPGA tiles. I
> was referring to parts that I might be able to use. They have a
> couple of 8 kLUT parts, only one in a package that I could use. I
> can pick between a 0.8 mm ball pitch, or 0.65 mm. Not really excited
> about either, even though there's a bit of inventory of the 256 ball,
> 0.8 mm part. But no insight into future deliveries.
>
> This looking for usable parts gets old fast, and I've been doing it
> for over a year now. When I find the guy responsible for this
> shortage, I'm going to give him a piece of my mind!
>

The reason you can parts in high-density packages, but not low-density
packages, is that there are lots of people such as yourself who are so
reluctant to use the small pitch devices. (This is not criticism - you
have solid reasons for preferring larger pitch devices, as do many
others.) Big manufacturers often prefer smaller pitch and higher
density, as it can lead to lower overall costs for their products, even
if design is more costly and the pcbs are more expensive.

There have been component supply issues for several years now, with only
gradual improvement in many areas. But there is a general pattern of
somewhat higher availability in smaller pitch parts.

David Brown

unread,
Jan 11, 2023, 5:42:23 AM1/11/23
to
On 10/01/2023 23:44, gnuarm.del...@gmail.com wrote:
> On Tuesday, January 10, 2023 at 1:35:24 PM UTC-5, Michael Schwingen
> wrote:
>> On 2023-01-09, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com>
>> wrote:
>>>
>>> I'm concerned about adding cost for the boards, cost for the
>>> assembly and just an easy road forward. I spend the last two
>>> years building 8,000 units when the CODEC factory burnt down. The
>>> customer knows about this issue, but the previous CM turned flaky
>>> on me and all but stopped delivering product.
>>>
>>> I have a new CM, but I don't want to go through production
>>> problems again.
>> 0.8mm BGA should be no problem for any reputable CM - fine-pitch
>> QFP is usually more trouble.
>
> Part of my problem is a lack of having designed with BGAs before. I
> can find footprint recommendations, but they are different for every
> manufacturer. It didn't occur to me that this might be because even
> though they have the same pitch and ball count, they may not have the
> same ball size.
>
> The two primary choices right now are a 196 ball, 1.0 mm pitch and
> 256 ball, 0.8 mm pitch. Can you share the design rules you used for
> these parts?
>

The board stackup, routing and bypassing recommendations from FPGA
manufacturers are basically bollocks. I believe it is primarily a
matter of being able to fob off complaints and support requests by
saying "Did you follow our layout application notes, impossible though
they may be? If not, it's not /our/ fault that you have problems."

OK, that's a bit of an exaggeration, but you can ignore the suggestions
of 16 layers with 8 different power planes and a dozen different
capacitor sizes mounted directly below the device.


Yes, there are complications for BGA layouts. And I'm afraid you are
going to have to do some research, some learning, and some discussions
with both PCB manufacturers (or their proxies) and board builders.

For the same pitch of BGA, there can be different sized balls, and
different sized pads on the underside of the BGA device which will
affect the shape of the ball after soldering. Pad size on the pcb has
different options. You have a key decision between solder mask defined
and non-solder mask defined pads, which affects mechanical strength,
thermal stability, solder paste masks, routeability, and manufacturing
requirements. And BGA soldering has different requirements in
production than non-BGA devices.


I have no doubt that this is something you can master quite quickly -
it's not /that/ hard. But it's not something you can learn just by a
thread on a newsgroup.



gnuarm.del...@gmail.com

unread,
Jan 11, 2023, 7:42:44 AM1/11/23
to
The very fine pitch parts are used to save space on the board. Some applications, like cell phones, simply require it. Not sure it saves any money, really. If you save on board size, you pay that back for finer pitch and laser drilled holes.

--

Rick C.

-++ Get 1,000 miles of free Supercharging
-++ Tesla referral code - https://ts.la/richard11209

gnuarm.del...@gmail.com

unread,
Jan 11, 2023, 7:49:38 AM1/11/23
to
I see the opposite. When FPGA makers offer routing suggestions, they often provide one for routing of 100% of I/O pins, and another, using fewer layers, routing a portion of the I/O pins. So clearly they are trying to optimize cost of the boards for the user. No sign of CYA.


> Yes, there are complications for BGA layouts. And I'm afraid you are
> going to have to do some research, some learning, and some discussions
> with both PCB manufacturers (or their proxies) and board builders.
>
> For the same pitch of BGA, there can be different sized balls, and
> different sized pads on the underside of the BGA device which will
> affect the shape of the ball after soldering.

I haven't done a survey to check this yet. Do you know this for a fact?


> Pad size on the pcb has
> different options. You have a key decision between solder mask defined
> and non-solder mask defined pads, which affects mechanical strength,
> thermal stability, solder paste masks, routeability, and manufacturing
> requirements. And BGA soldering has different requirements in
> production than non-BGA devices.
>
>
> I have no doubt that this is something you can master quite quickly -
> it's not /that/ hard. But it's not something you can learn just by a
> thread on a newsgroup.

It's not "hard", it's "hard" to find the information for layout recommendations from each FPGA vendor. I'm going to need to put together a compendium of layout information, before I can compare vendors. The vendors may make it easy for me, based on availability and pricing. Xilinx is not in the running unless I can get someone there to give assurance of better supply in six months. Right now I'll have to buy every part in inventory of several combinations of speed and temperature, to build the order I have coming.

--

Rick C.

+-- Get 1,000 miles of free Supercharging
+-- Tesla referral code - https://ts.la/richard11209

Michael Schwingen

unread,
Jan 11, 2023, 12:06:01 PM1/11/23
to
> Part of my problem is a lack of having designed with BGAs before. I can
> find footprint recommendations, but they are different for every
> manufacturer. It didn't occur to me that this might be because even
> though they have the same pitch and ball count, they may not have the same
> ball size.

> The two primary choices right now are a 196 ball, 1.0 mm pitch and 256
> ball, 0.8 mm pitch. Can you share the design rules you used for these
> parts?

I have a 529 pin BGA with 0.8mm pitch. SMD pads for the BGA are 0.4mm, vias
are also 0.4mm with 0.2mm drill. Using these rules, a via fits nicely
between 4 BGA pads.

I have plugged/plated vias in order to put 0402/0201 capacitors underneath
the BGA, but if you can place the capacitors outside the BGA area, normal
vias should do.

>> Talk to your PCB manufacturer about the details before doing the final
>> layout - there is some fine tuning (eg. drill size, annular ring, spacing)
>> where different PCB manufacturers have different preferences regarding which
>> rules will yield good results - when doing do, 0.8mm BGA should be possible
>> at modest PCB costs.
>
> You mean my CM who orders the PWBs? Yeah, I've tried asking before and
> they say they would need a design so they could get a quote. I know, that
> sounds lame, but I used four different CMs over the last decade and they
> have all said the same thing. They don't have design rules, that's for me
> to know.

OK, if you do not order the PCBs yourself, you have to forward this through
your CM. You will probably have to prepare a sample design (just the BGA
area with fanout), produce gerbers, and have them ask for feedback. Same
about the layer stackup if you need controlled impedances.

gnuarm.del...@gmail.com

unread,
Jan 11, 2023, 10:30:01 PM1/11/23
to
On Wednesday, January 11, 2023 at 1:06:01 PM UTC-4, Michael Schwingen wrote:
> On 2023-01-10, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
> >
> > Part of my problem is a lack of having designed with BGAs before. I can
> > find footprint recommendations, but they are different for every
> > manufacturer. It didn't occur to me that this might be because even
> > though they have the same pitch and ball count, they may not have the same
> > ball size.
>
> > The two primary choices right now are a 196 ball, 1.0 mm pitch and 256
> > ball, 0.8 mm pitch. Can you share the design rules you used for these
> > parts?
> I have a 529 pin BGA with 0.8mm pitch. SMD pads for the BGA are 0.4mm, vias
> are also 0.4mm with 0.2mm drill. Using these rules, a via fits nicely
> between 4 BGA pads.

You would need to use 5 mil trace and space to get between the pads. That doesn't sound too bad. Via to pad is 6.5 mil, again good.

Where did you get your pad size numbers? Your via pad only gives you 4 mil annular ring. That sounds a bit tight. To make that a 5 mil annular ring would shorten the 6.5 mil via to pad space to 5.5 mil, still good. Why did you choose a 0.4 mm pad?


> I have plugged/plated vias in order to put 0402/0201 capacitors underneath
> the BGA, but if you can place the capacitors outside the BGA area, normal
> vias should do.
> >> Talk to your PCB manufacturer about the details before doing the final
> >> layout - there is some fine tuning (eg. drill size, annular ring, spacing)
> >> where different PCB manufacturers have different preferences regarding which
> >> rules will yield good results - when doing do, 0.8mm BGA should be possible
> >> at modest PCB costs.
> >
> > You mean my CM who orders the PWBs? Yeah, I've tried asking before and
> > they say they would need a design so they could get a quote. I know, that
> > sounds lame, but I used four different CMs over the last decade and they
> > have all said the same thing. They don't have design rules, that's for me
> > to know.
> OK, if you do not order the PCBs yourself, you have to forward this through
> your CM. You will probably have to prepare a sample design (just the BGA
> area with fanout), produce gerbers, and have them ask for feedback. Same
> about the layer stackup if you need controlled impedances.

I asked my CM the general question of their BGA assembly experience and an estimated cost increment for going from a 100QFP to the 196 ball, 1.0 mm pitch BGA and 256 ball, 0.8 mm BGA. We'll see what they come up with. If they can give me a dollar figure, they should be able to give me dimensions they are comfortable working with.

Thanks for discussing this with me.

--

Rick C.

+-+ Get 1,000 miles of free Supercharging
+-+ Tesla referral code - https://ts.la/richard11209

David Brown

unread,
Jan 12, 2023, 2:45:14 AM1/12/23
to
A great many boards are built into products. It's not just on cell
phones or other consumer gadgets that saving space is important. If the
device you are making can be smaller, then it uses less material
(plastic, aluminium, whatever), weighs less, can go in a smaller box,
costs less to deliver, smaller storage space, etc. For most people who
only see one part of a system, it can be surprising how these things add
up in the complete price of many products. Shave off a percent or two
of the price at each step, and it all adds up (actually, it all
/multiplies/ up!) to lower cost overall even if the board is more
expensive. Of course you have to be dealing with large quantities
(bigger numbers than anything we make) for these things to be important
- but it's the big buyers that buy most of the parts!

Even if we just stick to the pcb itself, pcbs cost per square
centimetre. Using smaller packages can mean higher cost per unit area,
but can also mean lower total area if the package size is the driving
factor (rather than mechanics, connectors, etc.). Reduced total area
can lead to more boards per panel for part placement and soldering, and
lower manufacturing costs.

David Brown

unread,
Jan 12, 2023, 6:42:10 AM1/12/23
to
Fair enough. Certainly you want to look at all the information you can
here - you just have to be aware that some of it will be conflicting,
and some of it will be overkill. I read somewhere (a long time ago, and
I've forgotten the details) of someone who initially made their design
following application notes for bypass capacitors. Then to save costs,
they depopulated about 90% of these capacitors, basically at random.
There were no measurable differences in signal integrity, EMC results,
or any functionality.

>
>> Yes, there are complications for BGA layouts. And I'm afraid you
>> are going to have to do some research, some learning, and some
>> discussions with both PCB manufacturers (or their proxies) and
>> board builders.
>>
>> For the same pitch of BGA, there can be different sized balls, and
>> different sized pads on the underside of the BGA device which will
>> affect the shape of the ball after soldering.
>
> I haven't done a survey to check this yet. Do you know this for a
> fact?

Yes.

BGA balls are attached to circular pads on the underside of the BGA
package, and the size of these pads can be different for different
packages with the same pitch. In general, you get the mechanically
strongest bond when the pads on the pcb (or the opening in the solder
mask, for solder mask defined pads) is the same size. But that does not
mean you /always/ want them to be the same as there are other factors in
the trade-offs, and it's quite rare that mechanical strength is
critical. (If you are gluing on a large heatsink, without screws, and
then mounting the board upside down in a high vibration environment,
you'll have different requirements from a "normal" usage.)

>
>
>> Pad size on the pcb has different options. You have a key decision
>> between solder mask defined and non-solder mask defined pads, which
>> affects mechanical strength, thermal stability, solder paste masks,
>> routeability, and manufacturing requirements. And BGA soldering has
>> different requirements in production than non-BGA devices.
>>
>>
>> I have no doubt that this is something you can master quite quickly
>> - it's not /that/ hard. But it's not something you can learn just
>> by a thread on a newsgroup.
>
> It's not "hard", it's "hard" to find the information for layout
> recommendations from each FPGA vendor. I'm going to need to put
> together a compendium of layout information, before I can compare
> vendors. The vendors may make it easy for me, based on availability
> and pricing. Xilinx is not in the running unless I can get someone
> there to give assurance of better supply in six months. Right now
> I'll have to buy every part in inventory of several combinations of
> speed and temperature, to build the order I have coming.
>

That's the unfortunate reality these days. Find out what you can get
hold of, check if it looks good enough, then buy the stock. There's no
point in finding out that vendor X has good layout and manufacturing
information, or vendor Y has good toolchains, if you can only get parts
from vendor Z. (This is not news to you, of course - I'm just
sympathising.)

Michael Schwingen

unread,
Jan 12, 2023, 8:36:39 AM1/12/23
to
On 2023-01-12, gnuarm.del...@gmail.com <gnuarm.del...@gmail.com> wrote:
>> I have a 529 pin BGA with 0.8mm pitch. SMD pads for the BGA are 0.4mm, vias
>> are also 0.4mm with 0.2mm drill. Using these rules, a via fits nicely
>> between 4 BGA pads.
>
> You would need to use 5 mil trace and space to get between the pads. That
> doesn't sound too bad. Via to pad is 6.5 mil, again good.

Trace width in the BGA area is 0.11mm (for data lines).

> Where did you get your pad size numbers? Your via pad only gives you 4
> mil annular ring. That sounds a bit tight.
> To make that a 5 mil annular
> ring would shorten the 6.5 mil via to pad space to 5.5 mil, still good.
> Why did you choose a 0.4 mm pad?

That is the minimum given by our PCB manufacturer - small via pads allow for
bigger traces where needed (power traces, despite using a 8-layer PCB).

That is the area where you can fine tune after discussion with your PCB
manufacturer. Some may like a bigger annular ring, some may prefer smaller
ring and more pad-to-trace clearance.

https://www.nxp.com/docs/en/package-information/PBGAPRES.pdf

has some information about the BGA pad design. Our BGA has 0.45mm pads on
the BGA side, so the 0.4mm pads are on the lower end of the recommended
range.

> I asked my CM the general question of their BGA assembly experience and an
> estimated cost increment for going from a 100QFP to the 196 ball, 1.0 mm
> pitch BGA and 256 ball, 0.8 mm BGA. We'll see what they come up with. If
> they can give me a dollar figure, they should be able to give me
> dimensions they are comfortable working with.

I would expect pick & place to be easier for the 0.8mm BGA than the TQFP.
Cost increase will probably happen at the PCB level (small annular ring, or
more expensive surface finish - TQFP may work with HASL, BGA needs a flatter
finish. However, ENIG is not that expensive nowadays.)

David Brown

unread,
Jan 12, 2023, 10:06:43 AM1/12/23
to
Yes, BGAs can often be easier to place than TQFP's - you have a bigger
pitch, and they "float" to the correct place even if there is a slight
placement error.

On the other hand, you need better control of the soldering parameters,
and they are harder if you have a board that has awkward heat flow -
many high components nearby, or big thermal masses. And it is harder to
check connectivity and good quality soldering.

A good production facility will have tools to help here. They will do
the first boards with temperature probes between the balls, and X-Ray to
check the quality of the soldering. Make sure you have a production
house that is not scared to give you feedback - many far eastern places
will just do their best with what you give them, and never tell you how
to improve your layout.

Re-work is, obviously, far more difficult with BGAs.


John Larkin

unread,
Jan 13, 2023, 11:39:49 PM1/13/23
to
On Sat, 7 Jan 2023 09:49:24 -0800 (PST), "gnuarm.del...@gmail.com"
<gnuarm.del...@gmail.com> wrote:

>A small board with a 100QFP is being redesigned for a new FPGA due to obsolescence. Gowin makes a 100QFP device that would be a good fit, but my customer has said "no" to the 100% Chinese brand... US government customers, ya know!
>
>So now I'm looking at a BGA. I don't want to get into fine PCB design rules, so 1.0 mm ball pitch is my preference. The only devices I can find that fit on the board have 196 or 256 pins. But the real problem is availability.
>
>Digikey has a few of the XC7S15-1FTGB196I and more a scheduled for delivery in April. Add in the various speed and temperature flavors trickling in (mostly in April) and I should be ok for the initial delivery in August... if I can get my hands on those. I don't know if Digikey factors in the backlog orders in these counts.
>
>Mouser shows great inventory of Efinix parts, particularly the T13 and T20 in a 0.8 mm 256 pin BGA, 10s of thousands in stock. But I'd rather work with a 1.0 mm BGA. Oddly enough, LCSC shows part numbers, but zero inventory.
>
>Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use? Did this impact the PWB cost?

The 0.8 mm 256-ball T20 isn't bad...

https://www.dropbox.com/s/xjqgj2pz9mdhtma/P941_FPGA.jpg?raw=1

The BGA pads are 16 mils. 8 mil drills on the BGA vias. 6 mil traces
mostly, except for the 50 ohm monsters. No big deal these days. Works
great.

We considered a T8 for a simpler application, but its 0.5 mm ball
pitch looked nasty.

The efinix tool chain looks like it was developed in someone's garage,
which is actually praise. It's free and simple and just works without
200 gbyte downloads and doing battle with FlexLM.


gnuarm.del...@gmail.com

unread,
Jan 14, 2023, 12:20:55 AM1/14/23
to
On Saturday, January 14, 2023 at 12:39:49 AM UTC-4, John Larkin wrote:
> On Sat, 7 Jan 2023 09:49:24 -0800 (PST), "gnuarm.del...@gmail.com"
> <gnuarm.del...@gmail.com> wrote:
>
> >A small board with a 100QFP is being redesigned for a new FPGA due to obsolescence. Gowin makes a 100QFP device that would be a good fit, but my customer has said "no" to the 100% Chinese brand... US government customers, ya know!
> >
> >So now I'm looking at a BGA. I don't want to get into fine PCB design rules, so 1.0 mm ball pitch is my preference. The only devices I can find that fit on the board have 196 or 256 pins. But the real problem is availability.
> >
> >Digikey has a few of the XC7S15-1FTGB196I and more a scheduled for delivery in April. Add in the various speed and temperature flavors trickling in (mostly in April) and I should be ok for the initial delivery in August... if I can get my hands on those. I don't know if Digikey factors in the backlog orders in these counts.
> >
> >Mouser shows great inventory of Efinix parts, particularly the T13 and T20 in a 0.8 mm 256 pin BGA, 10s of thousands in stock. But I'd rather work with a 1.0 mm BGA. Oddly enough, LCSC shows part numbers, but zero inventory.
> >
> >Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use? Did this impact the PWB cost?
> The 0.8 mm 256-ball T20 isn't bad...
>
> https://www.dropbox.com/s/xjqgj2pz9mdhtma/P941_FPGA.jpg?raw=1

I can't really see much detail. It looks like there are virtually no pads on the vias under the BGA. What size are they?


> The BGA pads are 16 mils. 8 mil drills on the BGA vias. 6 mil traces
> mostly, except for the 50 ohm monsters. No big deal these days. Works
> great.

Yeah, 0.8 mm pad centers are doable, but I don't know where the line is for higher pricing on the PWB. The via pads seem to be pushing the technology line at JLCPCB. Not that I'm using them, but if they can do it, pretty much anyone should be able to do it. They build 0.45 mm via pads and 0.2 mm drills (5 mil annular ring and 8 mil drill), but charge extra for a 0.4 mm via pads (4 mil annular ring).


> We considered a T8 for a simpler application, but its 0.5 mm ball
> pitch looked nasty.

I didn't price the T8, because they use the logic cells for routing in a way they don't explain, so no way to factor it in. The T12 would be gravy for my design I expect, but it's only $1 more for the T20, so why not? If it saves a day of work, it's a break even for 1,000 units. If it enables a future expansion, it's worth much more than that! Both parts seem to have the same pin out, including I/O counts, so switching between them should only be a recompile.


> The efinix tool chain looks like it was developed in someone's garage,
> which is actually praise. It's free and simple and just works without
> 200 gbyte downloads and doing battle with FlexLM.

The large downloads are from the support for the many, many products the big three FPGA companies sell. Don't expect Efinix tools to continue to be small... and they aren't really free. You have to buy a board. That's more than I've paid for tools from FPGA vendors.

I'd really like to use the Gowin parts (LQFP100). But the customer is hinky about parts from a Chinese company. They sell stuff to the US Government.

--

Rick C.

++- Get 1,000 miles of free Supercharging
++- Tesla referral code - https://ts.la/richard11209

John Larkin

unread,
Jan 14, 2023, 11:08:03 AM1/14/23
to
On Fri, 13 Jan 2023 21:20:50 -0800 (PST), "gnuarm.del...@gmail.com"
<gnuarm.del...@gmail.com> wrote:

>On Saturday, January 14, 2023 at 12:39:49 AM UTC-4, John Larkin wrote:
>> On Sat, 7 Jan 2023 09:49:24 -0800 (PST), "gnuarm.del...@gmail.com"
>> <gnuarm.del...@gmail.com> wrote:
>>
>> >A small board with a 100QFP is being redesigned for a new FPGA due to obsolescence. Gowin makes a 100QFP device that would be a good fit, but my customer has said "no" to the 100% Chinese brand... US government customers, ya know!
>> >
>> >So now I'm looking at a BGA. I don't want to get into fine PCB design rules, so 1.0 mm ball pitch is my preference. The only devices I can find that fit on the board have 196 or 256 pins. But the real problem is availability.
>> >
>> >Digikey has a few of the XC7S15-1FTGB196I and more a scheduled for delivery in April. Add in the various speed and temperature flavors trickling in (mostly in April) and I should be ok for the initial delivery in August... if I can get my hands on those. I don't know if Digikey factors in the backlog orders in these counts.
>> >
>> >Mouser shows great inventory of Efinix parts, particularly the T13 and T20 in a 0.8 mm 256 pin BGA, 10s of thousands in stock. But I'd rather work with a 1.0 mm BGA. Oddly enough, LCSC shows part numbers, but zero inventory.
>> >
>> >Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use? Did this impact the PWB cost?
>> The 0.8 mm 256-ball T20 isn't bad...
>>
>> https://www.dropbox.com/s/xjqgj2pz9mdhtma/P941_FPGA.jpg?raw=1
>
>I can't really see much detail. It looks like there are virtually no pads on the vias under the BGA. What size are they?

The BGAVIAs are 12.5 mil OD with 8 mil drills. The other vias on the
board STANDARDVIA and POWERVIA are bigger.

I have seen vias with no annullar ring, just a trace falling into a
hole, but the PCB houses don't like that.

Filled via-in-pad would be cool but that's complex and expensive. As
is buried vias.

>
>
>> The BGA pads are 16 mils. 8 mil drills on the BGA vias. 6 mil traces
>> mostly, except for the 50 ohm monsters. No big deal these days. Works
>> great.
>
>Yeah, 0.8 mm pad centers are doable, but I don't know where the line is for higher pricing on the PWB. The via pads seem to be pushing the technology line at JLCPCB. Not that I'm using them, but if they can do it, pretty much anyone should be able to do it. They build 0.45 mm via pads and 0.2 mm drills (5 mil annular ring and 8 mil drill), but charge extra for a 0.4 mm via pads (4 mil annular ring).

We use US suppliers for production boards, and they seem to think this
6-layer board is within the normal range. One advantage to using a big
FPGA (256 balls in this case) is that you don't have to go deep to hit
enough balls, so may save a PCB layer or two. The T20-256 is a nice
part and Digikey has 29,000 in stock.

Another project used a 484 ball Zynq and we used almost every ball.
Lots of different power pours too. That took 10 layers. Another recent
board has a 400-ball ZYNQ with a few unused PS pins and fits on 8
layers.

The ZYNQ has analog inputs but, crazily, they are all differential so
they make you ground a perfectly good i/o pin for every analog input
that you want.

>
>
>> We considered a T8 for a simpler application, but its 0.5 mm ball
>> pitch looked nasty.
>
>I didn't price the T8, because they use the logic cells for routing in a way they don't explain, so no way to factor it in. The T12 would be gravy for my design I expect, but it's only $1 more for the T20, so why not? If it saves a day of work, it's a break even for 1,000 units. If it enables a future expansion, it's worth much more than that! Both parts seem to have the same pin out, including I/O counts, so switching between them should only be a recompile.
>
>
>> The efinix tool chain looks like it was developed in someone's garage,
>> which is actually praise. It's free and simple and just works without
>> 200 gbyte downloads and doing battle with FlexLM.
>
>The large downloads are from the support for the many, many products the big three FPGA companies sell. Don't expect Efinix tools to continue to be small... and they aren't really free. You have to buy a board. That's more than I've paid for tools from FPGA vendors.

$150! That's in the noise, and an eval board is good anyhow.


>
>I'd really like to use the Gowin parts (LQFP100). But the customer is hinky about parts from a Chinese company. They sell stuff to the US Government.

Yeah, we have a lot of aerospace customers and avoid Chinese parts.

gnuarm.del...@gmail.com

unread,
Jan 14, 2023, 1:05:36 PM1/14/23
to
On Saturday, January 14, 2023 at 12:08:03 PM UTC-4, John Larkin wrote:
> On Fri, 13 Jan 2023 21:20:50 -0800 (PST), "gnuarm.del...@gmail.com"
> <gnuarm.del...@gmail.com> wrote:
>
> >On Saturday, January 14, 2023 at 12:39:49 AM UTC-4, John Larkin wrote:
> >> On Sat, 7 Jan 2023 09:49:24 -0800 (PST), "gnuarm.del...@gmail.com"
> >> <gnuarm.del...@gmail.com> wrote:
> >>
> >> >A small board with a 100QFP is being redesigned for a new FPGA due to obsolescence. Gowin makes a 100QFP device that would be a good fit, but my customer has said "no" to the 100% Chinese brand... US government customers, ya know!
> >> >
> >> >So now I'm looking at a BGA. I don't want to get into fine PCB design rules, so 1.0 mm ball pitch is my preference. The only devices I can find that fit on the board have 196 or 256 pins. But the real problem is availability.
> >> >
> >> >Digikey has a few of the XC7S15-1FTGB196I and more a scheduled for delivery in April. Add in the various speed and temperature flavors trickling in (mostly in April) and I should be ok for the initial delivery in August... if I can get my hands on those. I don't know if Digikey factors in the backlog orders in these counts.
> >> >
> >> >Mouser shows great inventory of Efinix parts, particularly the T13 and T20 in a 0.8 mm 256 pin BGA, 10s of thousands in stock. But I'd rather work with a 1.0 mm BGA. Oddly enough, LCSC shows part numbers, but zero inventory.
> >> >
> >> >Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use? Did this impact the PWB cost?
> >> The 0.8 mm 256-ball T20 isn't bad...
> >>
> >> https://www.dropbox.com/s/xjqgj2pz9mdhtma/P941_FPGA.jpg?raw=1
> >
> >I can't really see much detail. It looks like there are virtually no pads on the vias under the BGA. What size are they?
> The BGAVIAs are 12.5 mil OD with 8 mil drills. The other vias on the
> board STANDARDVIA and POWERVIA are bigger.

2.25 mil (0.057 mm) is a pretty narrow via ring. Why not have a larger via pad? You have just over 0.2 mm (8 mil) clearance between via pad and BGA pads. Is this narrow annular ring buying you something? You could use a 0.4 mm (16 mil) via pad for an annular ring of 0.1 mm (4 mil) and still have 0.165 mm (6.5 mil) clearance between ball pads and via pads. Do you feel that's not enough?


> I have seen vias with no annullar ring, just a trace falling into a
> hole, but the PCB houses don't like that.

No, and they don't like small annular rings, because that's a small target to drill. I run into boards that the PCB fab house made badly at the vias and they are disasters. The tiny cracks that develop are hard to find and don't repair well.

Efinix recommends 0.46 mm (18.1 mil) ball pad, 0.5 mm (20 mil) via pad and a 0.25 mm (10 mil) drill, with 0.1 mm (4 mil) trace/space and 0.085 mm (3.3 mil) clearance between ball pad and via pad. The trace/space seems fine, but I'd like more clearance between via and ball pads. The question is, where to shave it from? Shaving 2 mil from the via pad leaves 4 mil annular ring and 4.3 mil clearance. Shaving from the ball pad seems like a bad idea. But if it works...

This is something that should have a spreadsheet, with a diagram that adjusts the image to show the details. All the tradeoffs become apparent very quickly. lol


> Filled via-in-pad would be cool but that's complex and expensive. As
> is buried vias.
> >
> >
> >> The BGA pads are 16 mils. 8 mil drills on the BGA vias. 6 mil traces
> >> mostly, except for the 50 ohm monsters. No big deal these days. Works
> >> great.
> >
> >Yeah, 0.8 mm pad centers are doable, but I don't know where the line is for higher pricing on the PWB. The via pads seem to be pushing the technology line at JLCPCB. Not that I'm using them, but if they can do it, pretty much anyone should be able to do it. They build 0.45 mm via pads and 0.2 mm drills (5 mil annular ring and 8 mil drill), but charge extra for a 0.4 mm via pads (4 mil annular ring).
> We use US suppliers for production boards, and they seem to think this
> 6-layer board is within the normal range. One advantage to using a big
> FPGA (256 balls in this case) is that you don't have to go deep to hit
> enough balls, so may save a PCB layer or two. The T20-256 is a nice
> part and Digikey has 29,000 in stock.

I don't follow that exactly. If I could get a 100 ball BGA on 1.0 mm centers, I would have zero trouble with routing and breakout. That could be routed 100% on a double sided board. One side gets the two outer rings of pads leaving 6x6. The other layer routes the remainder. But FPGA companies don't like small packages. They have much more demand at the larger I/O counts. Xilinx has a 196 ball, 1.0 mm package, but not much inventory and lead time is the standard 52 weeks.

The real problem is having to use the packages that are in stock. Everything other than Efinix is 52 week lead time, which is not a real forecast, rather just the point where they stop counting.


> Another project used a 484 ball Zynq and we used almost every ball.
> Lots of different power pours too. That took 10 layers. Another recent
> board has a 400-ball ZYNQ with a few unused PS pins and fits on 8
> layers.

Yeah, when you have that many I/Os, it's tough to keep the layer count down.


> The ZYNQ has analog inputs but, crazily, they are all differential so
> they make you ground a perfectly good i/o pin for every analog input
> that you want.
> >
> >
> >> We considered a T8 for a simpler application, but its 0.5 mm ball
> >> pitch looked nasty.
> >
> >I didn't price the T8, because they use the logic cells for routing in a way they don't explain, so no way to factor it in. The T12 would be gravy for my design I expect, but it's only $1 more for the T20, so why not? If it saves a day of work, it's a break even for 1,000 units. If it enables a future expansion, it's worth much more than that! Both parts seem to have the same pin out, including I/O counts, so switching between them should only be a recompile.
> >
> >
> >> The efinix tool chain looks like it was developed in someone's garage,
> >> which is actually praise. It's free and simple and just works without
> >> 200 gbyte downloads and doing battle with FlexLM.
> >
> >The large downloads are from the support for the many, many products the big three FPGA companies sell. Don't expect Efinix tools to continue to be small... and they aren't really free. You have to buy a board. That's more than I've paid for tools from FPGA vendors.
> $150! That's in the noise, and an eval board is good anyhow.
> >
> >I'd really like to use the Gowin parts (LQFP100). But the customer is hinky about parts from a Chinese company. They sell stuff to the US Government.
> Yeah, we have a lot of aerospace customers and avoid Chinese parts.

Where exactly are Efinix parts made? Their parts say China on them.

--

Rick C.

+++ Get 1,000 miles of free Supercharging
+++ Tesla referral code - https://ts.la/richard11209

John Larkin

unread,
Jan 14, 2023, 2:17:24 PM1/14/23
to
On Sat, 14 Jan 2023 10:05:33 -0800 (PST), "gnuarm.del...@gmail.com"
<gnuarm.del...@gmail.com> wrote:

>On Saturday, January 14, 2023 at 12:08:03 PM UTC-4, John Larkin wrote:
>> On Fri, 13 Jan 2023 21:20:50 -0800 (PST), "gnuarm.del...@gmail.com"
>> <gnuarm.del...@gmail.com> wrote:
>>
>> >On Saturday, January 14, 2023 at 12:39:49 AM UTC-4, John Larkin wrote:
>> >> On Sat, 7 Jan 2023 09:49:24 -0800 (PST), "gnuarm.del...@gmail.com"
>> >> <gnuarm.del...@gmail.com> wrote:
>> >>
>> >> >A small board with a 100QFP is being redesigned for a new FPGA due to obsolescence. Gowin makes a 100QFP device that would be a good fit, but my customer has said "no" to the 100% Chinese brand... US government customers, ya know!
>> >> >
>> >> >So now I'm looking at a BGA. I don't want to get into fine PCB design rules, so 1.0 mm ball pitch is my preference. The only devices I can find that fit on the board have 196 or 256 pins. But the real problem is availability.
>> >> >
>> >> >Digikey has a few of the XC7S15-1FTGB196I and more a scheduled for delivery in April. Add in the various speed and temperature flavors trickling in (mostly in April) and I should be ok for the initial delivery in August... if I can get my hands on those. I don't know if Digikey factors in the backlog orders in these counts.
>> >> >
>> >> >Mouser shows great inventory of Efinix parts, particularly the T13 and T20 in a 0.8 mm 256 pin BGA, 10s of thousands in stock. But I'd rather work with a 1.0 mm BGA. Oddly enough, LCSC shows part numbers, but zero inventory.
>> >> >
>> >> >Anyone work with 0.8 mm BGAs? What PWB feature dimensions did you use? Did this impact the PWB cost?
>> >> The 0.8 mm 256-ball T20 isn't bad...
>> >>
>> >> https://www.dropbox.com/s/xjqgj2pz9mdhtma/P941_FPGA.jpg?raw=1
>> >
>> >I can't really see much detail. It looks like there are virtually no pads on the vias under the BGA. What size are they?
>> The BGAVIAs are 12.5 mil OD with 8 mil drills. The other vias on the
>> board STANDARDVIA and POWERVIA are bigger.
>
>2.25 mil (0.057 mm) is a pretty narrow via ring. Why not have a larger via pad?

I don't know. My PCB guy decides stuff like that. I'd guess that he
wanted it to pass some design rule check, or maybe he started metric.
The board houses haven't complained as far as I know.

You should do your own thing and check with whoever will make your
boards.




gnuarm.del...@gmail.com

unread,
Jan 14, 2023, 7:20:56 PM1/14/23
to
Sounds good, but I've never been able to get a board house to even discuss these issues. They always take the approach that they will work with what I give them, which means, if it gives poor results, it's my problem.

There are a number of board companies with published capabilities, but they all vary, enough that there seems to be no consensus. Just like your via pad size. I've never seen a board house that says that would be a standard board. I was just looking at one company who wants 10 mil annular ring on inner layers and 7 mil annular ring on surface layers. That's a huge difference from 2.25 mil. On the other hand, they will print 2.5 mil trace/space!

I guess that's why we make prototypes.

--

Rick C.

---- Get 1,000 miles of free Supercharging
---- Tesla referral code - https://ts.la/richard11209

Richard Damon

unread,
Jan 14, 2023, 7:39:59 PM1/14/23
to
IF you contact a "Good" board shop, they should be able to give you
their specification to make the board.

They may have several levels (of cost) with different requirements.


If you board shop is NOT giving you a promise that the boards theya have
built will be "successful", then I would not touch them.

Yes, capabilities do vary a lot, so I always like to talk with my CMs
about what shops they use for the sort of class board we are working on,
and check with the shop on their requirements.

We also keep a general idea of capabilities, so if one shop is a bit
better on one spec, we might try not fully using that so other shops are
likely able to handle it.

John Larkin

unread,
Jan 14, 2023, 8:34:09 PM1/14/23
to
On Sat, 14 Jan 2023 16:20:53 -0800 (PST), "gnuarm.del...@gmail.com"
We always specify bare-board testing and warpage and tolerances, so we
don't get bad boards. What we can get is expensive boards.


>
>There are a number of board companies with published capabilities, but they all vary, enough that there seems to be no consensus. Just like your via pad size. I've never seen a board house that says that would be a standard board. I was just looking at one company who wants 10 mil annular ring on inner layers and 7 mil annular ring on surface layers. That's a huge difference from 2.25 mil. On the other hand, they will print 2.5 mil trace/space!

Zero annular ring seems to be OK on inners. That reduces capacitance.
5 or even 4 mil traces are usually standard price. I don't know why my
guy used 6 on the board that I posted.

We do email our board houses and often they answer!

>
>I guess that's why we make prototypes.

We don't prototype actual products; just go for it.

gnuarm.del...@gmail.com

unread,
Jan 14, 2023, 8:44:49 PM1/14/23
to
On Saturday, January 14, 2023 at 8:39:59 PM UTC-4, Richard Damon wrote:
> On 1/14/23 7:20 PM, gnuarm.del...@gmail.com wrote:
> > On Saturday, January 14, 2023 at 3:17:24 PM UTC-4, John Larkin wrote:
>
> >> You should do your own thing and check with whoever will make your
> >> boards.
> >
> > Sounds good, but I've never been able to get a board house to even discuss these issues. They always take the approach that they will work with what I give them, which means, if it gives poor results, it's my problem.
> >
> > There are a number of board companies with published capabilities, but they all vary, enough that there seems to be no consensus. Just like your via pad size. I've never seen a board house that says that would be a standard board. I was just looking at one company who wants 10 mil annular ring on inner layers and 7 mil annular ring on surface layers. That's a huge difference from 2.25 mil. On the other hand, they will print 2.5 mil trace/space!
> >
> > I guess that's why we make prototypes.
> >
> IF you contact a "Good" board shop, they should be able to give you
> their specification to make the board.

Ok, which are the "good" ones? I assume you mean a place that makes the bare boards. A CM typically buys bare boards and assembles the parts. Like I said, they work with what you give them and will do their best. They expect the designers to do the design work.


> They may have several levels (of cost) with different requirements.
>
>
> If you board shop is NOT giving you a promise that the boards theya have
> built will be "successful", then I would not touch them.

They don't charge for boards that don't work, of course. But the parts that get thrown out are mine. I was a bit surprised to find out they actually expect to see 20% fall out because of parts not properly picked up. They get pulled off the tape, but if they are not aligned well enough, they get flung into space. One of the parts on my previous build had a $200 part on it. We lost some 40 or so, I don't recall the exact number. They recovered a few of them from various nooks and crannies. I've always been told about losses, but I thought that was mostly the tiny passives that don't matter. This was a pretty small, TSSOP-20.


> Yes, capabilities do vary a lot, so I always like to talk with my CMs
> about what shops they use for the sort of class board we are working on,
> and check with the shop on their requirements.
>
> We also keep a general idea of capabilities, so if one shop is a bit
> better on one spec, we might try not fully using that so other shops are
> likely able to handle it.

I got the "Award Letter" the other day and with the onerous conditions, I may not be able to accept the order. Two years ago, we went through this via a third party CM who did their integration. It took months to resolve the issues. They want prototypes in May. Ain't gonna happen.

They want me to guarantee all manner of things that I can't guarantee, such as being able to manufacture the boards for 10 years. They want indemnifications for all manner of things. They even claim ownership of any "unpatented knowledge or information" that is disclosed to them is considered to be "part of the consideration for this Agreement". I believe this is what is called "trade secrets".

This is far more onerous than what had been negotiated previously though their CM. Now, I have to start all over again.

--

Rick C.

---+ Get 1,000 miles of free Supercharging
---+ Tesla referral code - https://ts.la/richard11209

gnuarm.del...@gmail.com

unread,
Jan 14, 2023, 8:52:48 PM1/14/23
to
You aren't paying attention. I don't use a PWB fabricator, I use a Contract Assembly house to assemble my boards. They are a middle man between me and the PWB fabricator. Once, no twice I've had to get on the phone with the actual PWB fabricator to convince him that he should not clip my silk screen. The use such a large clip radius that they made half the refdes illegible. That really makes the board hard to debug.


> >I guess that's why we make prototypes.
> We don't prototype actual products; just go for it.

I don't have a choice, the customer wants 16 early protos, then 146 protos, then 100 pieces for pilot and 1100 FRS. So there is no "go for it". I'm sure I'll munge something up. Replacing the two main parts on the board and moving the connectors to the other side, means it's a complete redesign, at least for the artwork, if not the schematic.

--

Rick C.

--+- Get 1,000 miles of free Supercharging
--+- Tesla referral code - https://ts.la/richard11209

Richard Damon

unread,
Jan 14, 2023, 9:31:38 PM1/14/23
to
On 1/14/23 8:44 PM, gnuarm.del...@gmail.com wrote:
> On Saturday, January 14, 2023 at 8:39:59 PM UTC-4, Richard Damon wrote:
>> On 1/14/23 7:20 PM, gnuarm.del...@gmail.com wrote:
>>> On Saturday, January 14, 2023 at 3:17:24 PM UTC-4, John Larkin wrote:
>>
>>>> You should do your own thing and check with whoever will make your
>>>> boards.
>>>
>>> Sounds good, but I've never been able to get a board house to even discuss these issues. They always take the approach that they will work with what I give them, which means, if it gives poor results, it's my problem.
>>>
>>> There are a number of board companies with published capabilities, but they all vary, enough that there seems to be no consensus. Just like your via pad size. I've never seen a board house that says that would be a standard board. I was just looking at one company who wants 10 mil annular ring on inner layers and 7 mil annular ring on surface layers. That's a huge difference from 2.25 mil. On the other hand, they will print 2.5 mil trace/space!
>>>
>>> I guess that's why we make prototypes.
>>>
>> IF you contact a "Good" board shop, they should be able to give you
>> their specification to make the board.
>
> Ok, which are the "good" ones? I assume you mean a place that makes the bare boards. A CM typically buys bare boards and assembles the parts. Like I said, they work with what you give them and will do their best. They expect the designers to do the design work.
>
>

There are a number of them, As I said, If you are using a CM, you will
need to talk with them and find who they use and talk to them about
their requirements.

>> They may have several levels (of cost) with different requirements.
>>
>>
>> If you board shop is NOT giving you a promise that the boards theya have
>> built will be "successful", then I would not touch them.
>
> They don't charge for boards that don't work, of course. But the parts that get thrown out are mine. I was a bit surprised to find out they actually expect to see 20% fall out because of parts not properly picked up. They get pulled off the tape, but if they are not aligned well enough, they get flung into space. One of the parts on my previous build had a $200 part on it. We lost some 40 or so, I don't recall the exact number. They recovered a few of them from various nooks and crannies. I've always been told about losses, but I thought that was mostly the tiny passives that don't matter. This was a pretty small, TSSOP-20.

So, you aren't using a good CM, as they aren't using a good board shop,
or at least didn't give you their expected failure rates up front. Yes,
there are loss factors for parts, but if they didn't give you those when
you started to negotiate the contract when you indicated you will be
supplying some of the parts, they aren't doing their job.

Yes, it may be "cheaper" to use a shop like that, but you pay for it in
those sorts of costs.

>
>
>> Yes, capabilities do vary a lot, so I always like to talk with my CMs
>> about what shops they use for the sort of class board we are working on,
>> and check with the shop on their requirements.
>>
>> We also keep a general idea of capabilities, so if one shop is a bit
>> better on one spec, we might try not fully using that so other shops are
>> likely able to handle it.
>
> I got the "Award Letter" the other day and with the onerous conditions, I may not be able to accept the order. Two years ago, we went through this via a third party CM who did their integration. It took months to resolve the issues. They want prototypes in May. Ain't gonna happen.
>
> They want me to guarantee all manner of things that I can't guarantee, such as being able to manufacture the boards for 10 years. They want indemnifications for all manner of things. They even claim ownership of any "unpatented knowledge or information" that is disclosed to them is considered to be "part of the consideration for this Agreement". I believe this is what is called "trade secrets".
>
> This is far more onerous than what had been negotiated previously though their CM. Now, I have to start all over again.
>

Yes, some "customers" are not worth it.

John Larkin

unread,
Jan 14, 2023, 11:10:54 PM1/14/23
to
On Sat, 14 Jan 2023 17:52:45 -0800 (PST), "gnuarm.del...@gmail.com"
That's because you're obnoxious.

gnuarm.del...@gmail.com

unread,
Jan 15, 2023, 12:04:57 AM1/15/23
to
Wow! Talk about sensitive. What is going on with you???

--

Rick C.

--++ Get 1,000 miles of free Supercharging
--++ Tesla referral code - https://ts.la/richard11209

John Larkin

unread,
Jan 15, 2023, 1:37:04 PM1/15/23
to
On Sat, 14 Jan 2023 21:04:55 -0800 (PST), "gnuarm.del...@gmail.com"
Just trying to help. My mistake.

gnuarm.del...@gmail.com

unread,
Jan 15, 2023, 11:11:37 PM1/15/23