Maker Pro
Maker Pro

PCB Layout (for ADC and DAC)

J

Jon Slaughter

Jan 1, 1970
0
Reading over some layout issues involving data conversion it seems that most
of the stuff is well covered such as using seperate supplies, grounds,
bypass caps on power pins, etc...

Some issues I'm not sure about are when going from analog to digital and
vice versa.

In a datasheet involving a DAC(DAD1793 from TI) they show the recommended
layout but I'm a bit confused. The DAC is on the analog side but its half
digital. Its digital ground is grounded to the analog side. Would it not be
better to have its digital ground go to the digital ground plane? Of course
since the IC is over the analog ground plane it means that the there would
have to be a little routing but I'm thinking that maybe the digital ground
plane could be extendend to half between the chip and vias would go directly
to it?

Also, is there any reason for the ground plane to be on a seperate layer? Is
it for just convenience and to maximize area or is there some other concept
involved. Since I don't have any double sided pcb boards and if I did(which
I suppose I could make but sticking two single sided ones together) I'm not
sure how to make the vias(drill and solder/maybe use a wire connector). I'm
sure I can get away with using a single side for prototyping though? (As
noise issues won't be the ultimate factor unless its pretty bad)


What I was thinking about was splitting the ground plane/pcb board into two
halfs where the ic's that were partially digital and partially analog would
straddle both sides. This would allow me to sorta seperate the two sides to
some degree but not sure if it would cause other issues.

Also, in this case would using one digital supply for all digital elements
work? In the two layouts I have saw for ADC's and DAC's they use one supply
for the digital and then one supply for the the DAC and/or ADC.

i.e., one supply is completely digital but the one supplying analog power
also supplies the digital for the ADC's and DAC's. Is this necessary(in
that, is it better or worse than having only two supplies one for digital
and one for analog)?

One more question. I didn't realize that the DAC's and ADC's where
synchronous devices and need external clocks(thought they had them build in
and I could use interrupts to transfer data). Can I use the same clock for
both/all conversion ic's? I need a pretty stable and fixed clock because I'm
using it for audio so the pitch needs to be right(I don't think this will be
an issue but I'd like not to introduce more complications by having many
different clocks it isn't necessary).


Thanks,
Jon
 

neon

Oct 21, 2006
1,325
Joined
Oct 21, 2006
Messages
1,325
the input gnd is more inportant as opposed to digital gnd. the noise on the input will clearly be put on the output as a digital error.
 
M

MooseFET

Jan 1, 1970
0
Reading over some layout issues involving data conversion it seems that most
of the stuff is well covered such as using seperate supplies, grounds,
bypass caps on power pins, etc...

Some issues I'm not sure about are when going from analog to digital and
vice versa.

In a datasheet involving a DAC(DAD1793 from TI) they show the recommended
layout but I'm a bit confused. The DAC is on the analog side but its half
digital. Its digital ground is grounded to the analog side. Would it not be
better to have its digital ground go to the digital ground plane? Of course
since the IC is over the analog ground plane it means that the there would
have to be a little routing but I'm thinking that maybe the digital ground
plane could be extendend to half between the chip and vias would go directly
to it?

ADCs and DACs always have the issue of the digital circuit messing
with the analog workings. Internally, the chip has a path from the
digital logic ground to the analog ground. You don't want any current
to flow in this path. To prevent this, the digital ground must have a
very low impedance path. You want the digital ground plane to provide
all of the return currents for the digital lines so it needs to be
under them.


Also, is there any reason for the ground plane to be on a seperate layer?

Making a layer for a ground makes it work as a continuous sheet of low
impedance ground. When you combine it with a signal layer, you have
to plow traces through it. This increases the impedance.

And ...
Is
it for just convenience and to maximize area or is there some other concept
involved.

At RF frequencies slots and gaps in planes look like little tuned
circuits and antennas. If you circuit can drive an RF current into
the structure, it will radiate.
Since I don't have any double sided pcb boards and if I did(which
I suppose I could make but sticking two single sided ones together) I'm not
sure how to make the vias(drill and solder/maybe use a wire connector). I'm
sure I can get away with using a single side for prototyping though? (As
noise issues won't be the ultimate factor unless its pretty bad)

Use your single sided PCB with the traces making the top side.
Scatter largish holes (0.05 or more) for the ground connection. Take
an unprocessed sheet of copper clad and place it under your PCB and
match drill smaller holes (0.035) in it for the ground.

Solder long lengths of wire into the holes of the copper clad. Don't
use too much solder on the top surface. Bend the bottom side of the
wires over and not the top.

Feed the wires through the holes in the PCB and slide the PCB along
the wires down onto the copperclad. Bend over the wires and solder
and snip.

What I was thinking about was splitting the ground plane/pcb board into two
halfs where the ic's that were partially digital and partially analog would
straddle both sides. This would allow me to sorta seperate the two sides to
some degree but not sure if it would cause other issues.

Beware of increasing the impedance of the digital ground paths.

Also, in this case would using one digital supply for all digital elements
work? In the two layouts I have saw for ADC's and DAC's they use one supply
for the digital and then one supply for the the DAC and/or ADC.

Filter the heck out of your supplies. An RF bead, inductor or
resistor and a couple of 47u capacitors can make quite a difference.


Consider this bit of ASCII art:

---+------[ZT]-------+-------[ZT]--------+-----[ZT]-------+---------
! ! ! !
--/\/--+---A --/\/--+---B --/\/--+---C !
! ! ! ---
--- --- --- ---
--- C1 --- ---C3 !
! ! ! GND
GND GND GND

[ZT} = the impedance of the trace

Notice how if the reistors were zero ohms, some of an AC current
applied to B would flow through C1 and C3 into the local grounds at
those locations. It doesn't take much resistance to reduce this.
 
J

John Larkin

Jan 1, 1970
0
Reading over some layout issues involving data conversion it seems that most
of the stuff is well covered such as using seperate supplies, grounds,
bypass caps on power pins, etc...

Some issues I'm not sure about are when going from analog to digital and
vice versa.

In a datasheet involving a DAC(DAD1793 from TI) they show the recommended
layout but I'm a bit confused. The DAC is on the analog side but its half
digital. Its digital ground is grounded to the analog side. Would it not be
better to have its digital ground go to the digital ground plane? Of course
since the IC is over the analog ground plane it means that the there would
have to be a little routing but I'm thinking that maybe the digital ground
plane could be extendend to half between the chip and vias would go directly
to it?

Also, is there any reason for the ground plane to be on a seperate layer? Is
it for just convenience and to maximize area or is there some other concept
involved. Since I don't have any double sided pcb boards and if I did(which
I suppose I could make but sticking two single sided ones together) I'm not
sure how to make the vias(drill and solder/maybe use a wire connector). I'm
sure I can get away with using a single side for prototyping though? (As
noise issues won't be the ultimate factor unless its pretty bad)


What I was thinking about was splitting the ground plane/pcb board into two
halfs where the ic's that were partially digital and partially analog would
straddle both sides. This would allow me to sorta seperate the two sides to
some degree but not sure if it would cause other issues.

Also, in this case would using one digital supply for all digital elements
work? In the two layouts I have saw for ADC's and DAC's they use one supply
for the digital and then one supply for the the DAC and/or ADC.

i.e., one supply is completely digital but the one supplying analog power
also supplies the digital for the ADC's and DAC's. Is this necessary(in
that, is it better or worse than having only two supplies one for digital
and one for analog)?

One more question. I didn't realize that the DAC's and ADC's where
synchronous devices and need external clocks(thought they had them build in
and I could use interrupts to transfer data). Can I use the same clock for
both/all conversion ic's? I need a pretty stable and fixed clock because I'm
using it for audio so the pitch needs to be right(I don't think this will be
an issue but I'd like not to introduce more complications by having many
different clocks it isn't necessary).


Thanks,
Jon

Splitting planes is almost always a bad idea.

If you are restricted to etching single-sided boards, consider using
double-side copperclad and leaving the back side unetched, a solid
copper ground plane. Drill topside ground pads or, better, islands,
and solder via wires through to the ground plane. This will give you
far better signal integrity than a 1-sided, split-ground layout is
likely able to do.

The big performance cut in pc boards is between boards with true
ground planes, and boards without.

John
 
J

John Devereux

Jan 1, 1970
0
Jon Slaughter said:
Also, is there any reason for the ground plane to be on a seperate layer? Is
it for just convenience and to maximize area or is there some other concept
involved. Since I don't have any double sided pcb boards and if I did(which
I suppose I could make but sticking two single sided ones together) I'm not
sure how to make the vias(drill and solder/maybe use a wire connector). I'm
sure I can get away with using a single side for prototyping though? (As
noise issues won't be the ultimate factor unless its pretty bad)

What I like to do is use double sided PCB material, but dedicate one
side as a ground plane. This side does not need to be etched, so it is
just like making a single-sided board from the processing point of
view. All ground signals go to a via (and all vias are to
ground). Then, for these "ground" vias just drill them and use tinned
copper wire (or resistor leads etc) to make the connection. This works
very well for surface mount boards, and is much easier than a full
double-sided layout (no alignment issues). Since there is no ground
routing on the "tracking" side (the component side) a single sided
layout is not too difficult. You could use the same artwork for
production boards too. (Actually I now only make my own boards for quick
prototypes of tricky bits of the circuit).
 
J

John Popelish

Jan 1, 1970
0
John said:
What I like to do is use double sided PCB material, but dedicate one
side as a ground plane. This side does not need to be etched, so it is
just like making a single-sided board from the processing point of
view. All ground signals go to a via (and all vias are to
ground). Then, for these "ground" vias just drill them and use tinned
copper wire (or resistor leads etc) to make the connection. This works
very well for surface mount boards, and is much easier than a full
double-sided layout (no alignment issues). Since there is no ground
routing on the "tracking" side (the component side) a single sided
layout is not too difficult. You could use the same artwork for
production boards too. (Actually I now only make my own boards for quick
prototypes of tricky bits of the circuit).

I haven't tried this technique, but it sounds very useful.
For through hole boards, I would use one of those spur or
brad point bits (that cut a circle around a central point,
made for drilling wood) to clear the ground plane from a
little circle around the lead hole where components are
passed through the plane to connect to traces on the other
side. Do you think that is practical?

The biggest problem might be finding bits smaller than 1/8".
http://www.japanwoodworker.com/prod...JE0V0E3H0U7L26&pf_id=54.521.125&dept_id=12815

I'd probably have to grind my own low rake versions to cut
copper without diving through the board.
 
J

John Popelish

Jan 1, 1970
0
John said:
I haven't tried this technique, but it sounds very useful. For through
hole boards, I would use one of those spur or brad point bits (that cut
a circle around a central point, made for drilling wood) to clear the
ground plane from a little circle around the lead hole where components
are passed through the plane to connect to traces on the other side. Do
you think that is practical?

The biggest problem might be finding bits smaller than 1/8".
http://www.japanwoodworker.com/prod...JE0V0E3H0U7L26&pf_id=54.521.125&dept_id=12815
I'd probably have to grind my own low rake versions to cut copper
without diving through the board.

I found a 2mm version, but look at the price!
http://www.mikestools.com/570-7020-Stern-Brad-Point-Drill-Bit-Metric-2mm-Hss.aspx
 
G

Glenn Gundlach

Jan 1, 1970
0
s=JapanWoodworker&mimid=XS...

I found a 2mm version, but look at the price!http://
www.mikestools.com/570-7020-Stern-Brad-Point-Drill-Bit-Metric-...

Not to pick on anybody, particularly John Popelish, but but when I
think of folks spending several hundred bucks on computers and cell
phones and $100+/month on cell service, internet and cable TV, I'm
always a bit taken aback when there is a comment on a 1 time expense
like a carbide drill bit being expensive.

As for the technique, I've seen low quantity broadcast gear with one
side ground planes manually drilled for clearance.

GG
 
L

linnix

Jan 1, 1970
0
3/32" and 1/16" are quite common at your local hardware store.

That link is broken, can't see the price. I got a few 1.2mm and 1mm
steel bits if you want them.
Not to pick on anybody, particularly John Popelish, but but when I
think of folks spending several hundred bucks on computers and cell
phones and $100+/month on cell service, internet and cable TV, I'm
always a bit taken aback when there is a comment on a 1 time expense
like a carbide drill bit being expensive.

Carbide bits are easy to break, especially for these sizes.
 
J

John Popelish

Jan 1, 1970
0
Glenn said:
Not to pick on anybody, particularly John Popelish, but but when I
think of folks spending several hundred bucks on computers and cell
phones and $100+/month on cell service, internet and cable TV, I'm
always a bit taken aback when there is a comment on a 1 time expense
like a carbide drill bit being expensive.

As for the technique, I've seen low quantity broadcast gear with one
side ground planes manually drilled for clearance.

$10 for a carbide bit might not be so bad, but that one:
http://www.mikestools.com/570-7020-Stern-Brad-Point-Drill-Bit-Metric-2mm-Hss.aspx
was high speed steel.
 
E

Eeyore

Jan 1, 1970
0
John said:
Splitting planes is almost always a bad idea.

And almost universally done in audio or you'll hear low-level 'birdies' in the
signal.

Graham
 
J

John Devereux

Jan 1, 1970
0
John Popelish said:
I haven't tried this technique, but it sounds very useful. For through
hole boards, I would use one of those spur or brad point bits (that
cut a circle around a central point, made for drilling wood) to clear
the ground plane from a little circle around the lead hole where
components are passed through the plane to connect to traces on the
other side. Do you think that is practical?

Yes, in fact that is precisely what I used to do. You can buy special
bits from Farnell IIRC. (It has been so long since I made a through
hole board that I had genuinely forgotten all about this)!
 
J

John Devereux

Jan 1, 1970
0
(replying to own post)
Yes, in fact that is precisely what I used to do. You can buy special
bits from Farnell IIRC. (It has been so long since I made a through
hole board that I had genuinely forgotten all about this)!

Thinking about this, it might be better to have the components on the
groundplane side, and the tracks on the "solder" side. Then you use a
normal ~3mm bit to countersink the area around non-ground pins. The
ground pins can then be soldered on the component/ground plane
side. Can be tricky when the pins are under the device.

It's much easier with surface mount.
 
J

Joerg

Jan 1, 1970
0
Eeyore said:
John Larkin wrote:




And almost universally done in audio or you'll hear low-level 'birdies' in the
signal.

Until the audio gear is used near a strong transmitter and then any
split will cause some real birdies. Or worst case a fzzzzt ... poof.
 
V

Vladimir Vassilevsky

Jan 1, 1970
0
Joerg said:
Until the audio gear is used near a strong transmitter and then any
split will cause some real birdies. Or worst case a fzzzzt ... poof.

Well. Indeed the star grounding is very common in audio. As for the EMC
susceptibility problem, Graham is aggressively unaware of it.

Here are some practical considerations for the split ground:

1. A separate island in the ground plane can be usefull if you want to
isolate something very noisy or very sensitive from the rest of schematics.

2. Using common ground plane as the universal signal/power return path
may not be a good idea if the high currents flow through it.

3. There may be other connections to the ground. It may not always be
possible to connect everything to the ground at your board. So you have
to spit the grounds to avoid or alleviate loop currents.


Vladimir Vassilevsky

DSP and Mixed Signal Design Consultant

http://www.abvolt.com
 
J

Jon Slaughter

Jan 1, 1970
0
Thanks for all the info guys.

I'm curious as to just how bad not having a ground plane is. Surely the
circuit will still function properly? How much noise will be introduced? I'm
willing to sacrifice quality for ease to make at this point. (since if the
only issue with the layout is going to be noise once I get everything
working through a prototype I can add a ground plane to the layout and then
send off and get it fabricated)

I think here there won't be any issues masking noise from other sources but
that might be a problem. (I think at this point I'm just trying to get the
system to work as a whole)

I assume that the issue is with the analog domain or is there a reverse
issue with digital? i.e., can the digital be affected by the analog domain
also when not using these special precautions such as a ground plane? (so
that the circuit could actually not function properly rather than just
having noisy conversions)

I think that I will end up doing the 2 sided boards though. I'm sure its
much easier to route/layout ;) Since there are vias that I can buy that look
like a snap to use and it will just involve a drilling a few holes.

(mainly just curious about the consequences of not using a ground plane. I
know its not as good but I don't think any mentions just how bad. (remember
its for prototyping so I can sacrifice some things))


Thanks,
Jon
 
J

Jon Slaughter

Jan 1, 1970
0
Jon Slaughter said:
Thanks for all the info guys.

I'm curious as to just how bad not having a ground plane is. Surely the
circuit will still function properly? How much noise will be introduced?
I'm willing to sacrifice quality for ease to make at this point. (since if
the only issue with the layout is going to be noise once I get everything
working through a prototype I can add a ground plane to the layout and
then send off and get it fabricated)

I think here there won't be any issues masking noise from other sources
but that might be a problem. (I think at this point I'm just trying to get
the system to work as a whole)

I assume that the issue is with the analog domain or is there a reverse
issue with digital? i.e., can the digital be affected by the analog domain
also when not using these special precautions such as a ground plane? (so
that the circuit could actually not function properly rather than just
having noisy conversions)

I think that I will end up doing the 2 sided boards though. I'm sure its
much easier to route/layout ;) Since there are vias that I can buy that
look like a snap to use and it will just involve a drilling a few holes.

(mainly just curious about the consequences of not using a ground plane. I
know its not as good but I don't think any mentions just how bad.
(remember its for prototyping so I can sacrifice some things))

Oh, not sure if I mentioned this but its for audio. I'm not doing really
high speed stuff and my sample rate will actually be 96khz or max 192khz but
definitely nothing past 100Mhz.

I suppose though that it is actually in the mhz range since these are
oversampling so I guess I do have to look at it as high speed?
 
J

Joerg

Jan 1, 1970
0
Vladimir said:
Well. Indeed the star grounding is very common in audio. As for the EMC
susceptibility problem, Graham is aggressively unaware of it.

Here are some practical considerations for the split ground:

1. A separate island in the ground plane can be usefull if you want to
isolate something very noisy or very sensitive from the rest of schematics.

It can help but a good design wouldn't need such islands :)

2. Using common ground plane as the universal signal/power return path
may not be a good idea if the high currents flow through it.

It's the only way to avoid RF interference. Star grounds don't work well
in such situations because a connection to that star point will act as a
loop antenna and inject noise currents into wherever it ends. When I was
a young ham radio operator I had to remedy lots of those cases, mostly
stuff like electronic organs. To the point where I almost got sick of
it. Luckily copper stock was cheap in those days and I was often
rewarded with a nice tune played on the instrument (I can't play myself).

3. There may be other connections to the ground. It may not always be
possible to connect everything to the ground at your board. So you have
to spit the grounds to avoid or alleviate loop currents.

#3 is usually a sure sign that somthing went wrong. You brought up
exactly the point that is often misunderstood: Systems do not operate in
isolation, there is stuff connected to them or people wouldn't need the
system. A really good system will not have a problem with ground loops.

Of course you might not know the other end of the cable and sometimes
things like isolation transformers are needed, especially in audio.
Splitting grounds inside a system is, however, IMHO rarely a good idea.

The best class to learn ground structures would be to open up some
surplus military stuff. They know how to do it right because they have
to pass much stricter EMI tests than we do. OTOH if everyone would do
that a third of my business would shrivel up ;-)

The last star architecture I ripped out was about a couple of weeks ago.
Lower end of the audio range, noise up to kazoo. Now there is only the
normal background hiss left.
 
M

MooseFET

Jan 1, 1970
0
On Jul 22, 4:39 pm, Vladimir Vassilevsky <[email protected]>
wrote:
[... grounding ...]
1. A separate island in the ground plane can be usefull if you want to
isolate something very noisy or very sensitive from the rest of schematics.

The sensitive bit is usually analog and the noisiest is usually a DC-
DC converter or the like. Neither of these need as many routing
layers as the digital part so you can use up a layer as a local ground
plane above the overall one. In crosss section it may look lile this:

Power Logic Analog
Parts -> -[==]- -[==]- -[==]-
Top -> TTTTTTTT TTTTTTTT TTTTTTTT
Inner1 -> GGGGGGGG VVVVVVVV GGGGGGGG
Inner2 -> TTTTTTTT TTTTTTTT TTTTTTTT
Inner3 -> GGGGGGGGGGGGGGGGGGGGGGGGGGGG
Inner4 -> TTTTTTTTTTTTTTTTTTTTTTTTTTTT
Bot -> TTTTTTTTTTTTTTTTTTTTTTTTTTTT


T = Traces
G = Ground
V = Voltage

If you are careful, you can put the noisy nodes of the power supply
all above its local ground. This allows the rest of the layers to get
by without picking up too much noise.
 
M

MooseFET

Jan 1, 1970
0
Oh, not sure if I mentioned this but its for audio. I'm not doing really
high speed stuff and my sample rate will actually be 96khz or max 192khz but
definitely nothing past 100Mhz.

I suppose though that it is actually in the mhz range since these are
oversampling so I guess I do have to look at it as high speed?


The important number is the gain * bandwidth value. Even with only
audio signals, having a gain of a million and no ground plane is
asking for it.
 
Top