Choosing a ferrite bead

[Michael Noone]

In addition to the other suggestions, if at all possible, split the
two 6V busses right at the power supply - that way the power supply
filter will help keep the motor noise out of the GPS. Also, split
their return lines the same way.

A ferrite bead is just a little torus of ferrite that strings on the
power lead just like stringing beads on a string. It adds a little
inductance, and presents a high impedance to higher frequency noise.

But with only 70 mA, you might even use an ordinary RF choke - it
might make it easier to assemble, but only you can determine that.

Good Luck!
Rich

This is how I have it laid out right now. Return line is a ground plane
that everything uses - should I be changing this? Thanks,

-Mike

 

[Michael Noone]

Are you using surface mount parts or through hole?

The board is approximately 90% surface mount at the moment. When I have an
option between through hole and surface mount I always go for surface mount
if they take up the same amount of board space - I find such parts normally
make layouts cleaner, and also I find them to be decidedly easier to
solder.

I think it would. It is fairly small for the energy stored. You may
be able to find a slightly smaller part in through hole in an axial
would part (like a resistor with wire wound around it), but they spray
field out all over the place, where the part I suggested keeps almost
all its field inside.

OK I will try to design it in. I have already laid out this board so space
is tight - but I should be able to find a place for it. It will have to go
on the bottom layer where the ground plane is - will that cause a problem?

Thanks,

-Mike

 

[Michael Noone]

The bigger the cap, the lower the frequencies remaining in the bumps
left by motor operation. I am just guessing how well you need to
filter the 6 volt supply. You may get by with just removing the
higher frequency components of the bumps. In that case, a low E.S.R.
multilayer ceramic surface mount capacitor may be enough. This might
be as small as an 0805 surface mount cap like a X5R 10 uF, 10 volt
unit, like Panasonic ECJ-2FB1A106K. I would avoid the Y5V and F
types, even though they are available in higher capacitance per
volume. Their E.S.R is higher.
http://dkc3.digikey.com/PDF/T061/1165.pdf

Do you have a scope to look at how well various options work?

I do have a scope - but the annoying thing will be that everything will
be printed already - so if it doesn't work I would probabaly need to
make a new board. I guess that's OK though. It'll just be another delay.

A lot depends on how well you lay out the circuit board. When you get
to that point, I would be happy to discus principles and criticize
your artwork.

The board with the GPS module is already laid out (though I still have
about a week before I need to send it off to be printed). The motor
driver boards are going to be interesting to say the least - they'll be
about 1.5x4cm long and control 3 motors each, along with having a load
of sensors and other nonsense on them. Feedback on them would definitely
be awesome. I don't think I'll be finishing them for another month or so
though.

-Mike

 

[John Popelish]

Michael Noone wrote:
(snip)

OK I will try to design it in. I have already laid out this board so space
is tight - but I should be able to find a place for it. It will have to go
on the bottom layer where the ground plane is - will that cause a problem?

No. It will be effective up to higher frequencies if you can run a
ground trace under the inductor, between the pads, with very short
connections to the ground layer (like a few vias under the inductor).
This will reduce the capacitance that bridges across the inductor pads.

That layout will fit the whole series (and several other series) of
different values in that case size. But there is nothing I have seen
that comes close to the Sumida CDRH127/LD (low drop) as far as
resistance in that case size (to preserve as much of the 6 volts as
possible for the GPS unit).

 

[Rich Grise]

Add this to your toolbox: Provided that you have adequate bulk bypass
capacitance near the GPS module, you can add series resistance in the
6V supply line to the GPS. This can be VERY effective at quite low
frequencies. To decide how much resistance to use, determine a voltage
drop budget for filtering. Suppose you decide that you can spare 200
millivolts. That means that you can add 200mV/70mA = ~3 Ohms. The
combination of 3 Ohms with your bypass capacitors can provide a lot of
filtering, without resorting to an inductor. The power rating
dissipation of the resistor is P = I^2*R = 15 mW, so you can use a
really small part. IF the gps module needs a long surge of current at
some point, the resistance can be a problem, and you'll have to use an
inductor instead.
]I agree with the other posters who suggested that filtering spikes at
the motors is your first priority.
Paul Mathews

Would it make sense to use a wirewound resistor in this app?

Thanks,
Rich

 

[Rich Grise]

This is how I have it laid out right now. Return line is a ground plane
that everything uses - should I be changing this? Thanks,

I'd say, no, you want as much continuous metal as possible for a "ground
plane". You might want to look at the layout, and kind of trace what the
current paths would look like, and how they might interact, But I wouldn't
even begin to know how to fix it if there's some kind of situation.

In fact, I was wondering about mounting the choke (heck, a bead with leads
is pretty much a choke, right? ) on the ground plane side - would you
cut a little notch for it and go right to a via? I also like John's idea
of a bridge under it.

Cheers!
Rich

 

[David Harmon]

On Wed, 11 Jan 2006 21:40:41 GMT in sci.electronics.design, Rich

In fact, I was wondering about mounting the choke (heck, a bead with leads
is pretty much a choke, right? ) on the ground plane side -

Yes, it is exactly a choke. However, if it is laying on the ground
plane then it is a capacitor, right?

 

[Rich Grise]

On Wed, 11 Jan 2006 21:40:41 GMT in sci.electronics.design, Rich


Yes, it is exactly a choke. However, if it is laying on the ground
plane then it is a capacitor, right?

Well, it has capacitance to the ground plane, yes, of course; but I'd
presume that the power line would be in series with the inductor, and
the capacitance to ground is in parallel with the whole thing, kind
of like a distributed pi/T filter.

Thanks!
Rich

 

[Michael Noone]

Michael Noone wrote:
(snip)

No. It will be effective up to higher frequencies if you can run a
ground trace under the inductor, between the pads, with very short
connections to the ground layer (like a few vias under the inductor).
This will reduce the capacitance that bridges across the inductor
pads.

That layout will fit the whole series (and several other series) of
different values in that case size. But there is nothing I have seen
that comes close to the Sumida CDRH127/LD (low drop) as far as
resistance in that case size (to preserve as much of the 6 volts as
possible for the GPS unit).

I finally was able to fit it onto the top of my board. I decided that
putting it on the bottom would be a constant annoyance as it is a good
deal taller than all the other components on the bottom. After a fierce
battle and many a moved trace I was able to fit it along with the two
capacitors on the top of the board right next to the connector for the
GPS module. Very glad to have that done! One question though: should
this ground trace be just a single trace? Reason is I also have a ground
plane on the top of the board in that area to provide some shielding for
another component. So right now it has the full ground plane going
between its pads, not just a thin trace. I could change that if that
would be better though.

Have to finish up a couple last details on this board and then I can
finally send it out to be made! (been working on this one 8.5x10cm board
since September or October). Anyways, thanks for the help. I'll report
back on how well it works when I get that far.

-Mike

 

[John Popelish]

I finally was able to fit it onto the top of my board. I decided that
putting it on the bottom would be a constant annoyance as it is a good
deal taller than all the other components on the bottom. After a fierce
battle and many a moved trace I was able to fit it along with the two
capacitors on the top of the board right next to the connector for the
GPS module. Very glad to have that done! One question though: should
this ground trace be just a single trace? Reason is I also have a ground
plane on the top of the board in that area to provide some shielding for
another component. So right now it has the full ground plane going
between its pads, not just a thin trace. I could change that if that
would be better though.

That is fine, as long as this trace has a low inductance path to the
ground layer. But I'll bet you have that, just by virtue of the two
capacitor ground connections.

Have to finish up a couple last details on this board and then I can
finally send it out to be made! (been working on this one 8.5x10cm board
since September or October). Anyways, thanks for the help. I'll report
back on how well it works when I get that far.

Can you show me the layout for comments before it goes out?

 

[John Perry]

...

Yes, it is exactly a choke. However, if it is laying on the ground
plane then it is a capacitor, right?

Hm. I'm not an rf type, but I distinctly remember my lead engineer in
the 70's, who was an rf type, telling me that ferrite beads were
predominantly lossy, so acted more to increase trace resistance than
like chokes. That's why he could get about as much effect from tacking
one on top of the trace as he could cutting the trace and running it (a
connecting wire, actually) through the bead, as I wanted to.

Am I misremembering, or are things different now, or...?

John Perry

 

[John Popelish]

Hm. I'm not an rf type, but I distinctly remember my lead engineer in
the 70's, who was an rf type, telling me that ferrite beads were
predominantly lossy, so acted more to increase trace resistance than
like chokes. That's why he could get about as much effect from tacking
one on top of the trace as he could cutting the trace and running it (a
connecting wire, actually) through the bead, as I wanted to.

Am I misremembering, or are things different now, or...?

The effect is certainly reduced when the core does not wrap all the way
around a conductor, but there is measurable and, I guess useful effect
in having the material only on one side of flat circuits. Steward
now sells thin, flat squares and disks of ferrite with pressure
sensitive adhesive, to be placed over some flat circuit elements.

http://dkc3.digikey.com/PDF/T061/0999.pdf

I haven't used them for this purpose, but someone must be.

 

[Michael Noone]

That is fine, as long as this trace has a low inductance path to the
ground layer. But I'll bet you have that, just by virtue of the two
capacitor ground connections.

It should have that - but I think I'll give it some vias just to be
sure.

Can you show me the layout for comments before it goes out?

I would love to have somebody look at the layout. It is my first
'serious' board - all my other layouts have been much smaller boards
that had a small fraction of the components that this board has (I think
it's now at about 110 parts). Are you familiar with Cadsoft's Eagle? I
could post the raw Eagle files. Otherwise I could just post the files as
jpegs, though they'll have to be fairly high resolution (due to the
complexity of the board).

Thanks,

-Mike

 

[John Popelish]

I would love to have somebody look at the layout. It is my first
'serious' board - all my other layouts have been much smaller boards
that had a small fraction of the components that this board has (I think
it's now at about 110 parts). Are you familiar with Cadsoft's Eagle? I
could post the raw Eagle files. Otherwise I could just post the files as
jpegs, though they'll have to be fairly high resolution (due to the
complexity of the board).

I used to have Eagle loaded, but I deleted it for lack of use.

You are welcome to email graphics of the layout and the schematic, but
please, use GIF or PNG encoding, instead of JPG. It keeps all the
edges sharp and encodes only 256 or fewer colors per pixel, which is
fine for drawings. I have a 5 meg inbox.

If you put the files up on a web page or something, I guess could
reload Eagle but I hate downloading and installing software in a box
that is working well.

 

[Michael Noone]

I used to have Eagle loaded, but I deleted it for lack of use.

You are welcome to email graphics of the layout and the schematic, but
please, use GIF or PNG encoding, instead of JPG. It keeps all the
edges sharp and encodes only 256 or fewer colors per pixel, which is
fine for drawings. I have a 5 meg inbox.

If you put the files up on a web page or something, I guess could
reload Eagle but I hate downloading and installing software in a box
that is working well.

Hi John - I have just sent you an E-mail with both PNGs of the schematic
and layout as well as the actual Eagle files. I'm very interested to here
someone else's take on the boards as they represent my first attempt at
making a fairly sophisticated board. Thanks,

-Mike

 

[John Popelish]

Hi John - I have just sent you an E-mail with both PNGs of the schematic
and layout as well as the actual Eagle files. I'm very interested to here
someone else's take on the boards as they represent my first attempt at
making a fairly sophisticated board. Thanks,

Got it. I hope to devote some time to it this evening. I'm sure I'll
have questions. I'll email them.