First PCB design.

[Daniel Pitts]

I've completed my first PCB design in Eagle. Thinking of sending it off
to one of those small-batch fabs.

But, I'm wondering if anyone would be willing to take a look at my
design and giving me any pointers or gotchas? I'm looking for both
aesthetic and technical input.

On a related note, what's the best way to share my design/PCB on this
group?

Thanks,
Daniel.

 

[George Herold]

On Tuesday, January 21, 2014 12:44:35 AM UTC-5, Daniel Pitts wrote:

I've completed my first PCB design in Eagle. Thinking of sending it off

to one of those small-batch fabs.



But, I'm wondering if anyone would be willing to take a look at my
design and giving me any pointers or gotchas? I'm looking for both
aesthetic and technical input.

On a related note, what's the best way to share my design/PCB on this
group?

Hmm for sharing I 'prin't the schematic or PCB to a pdf. and then put the pdf on dropbox. But maybe there is an easier method.
(here's a chaos schematic I did a year or so ago.)
https://www.dropbox.com/s/afy4kb63ftdo1ke/chaos2.pdf

George H.

Thanks,

Daniel.

 

Daniel Pitts <newsgroup.nospam@virtualinfinity.net> wrote:

But, I'm wondering if anyone would be willing to take a look at my
design and giving me any pointers or gotchas? I'm looking for both
aesthetic and technical input.

[in a later message]

http://virtualinfinity.net/electronics/LED%20Display%202%20-%20board.pdf
http://virtualinfinity.net/electronics/LED%20Display%202%20-%20schematic.pdf

Aesthetic:

C1 should be labeled as 22 pF, not 22 pV.

Technical:

You're using a regulated power supply, right? I ask because there is
no regulation in the schematic; that is OK if you are using a well-
regulated power supply.

You will probably want at least one bypass capacitor - say 10 to 47 uF
directly across the +5 V input, near J1. Maybe also an 0.1 uF or so
across the power and ground of the ATTiny and the 74238, and perhaps an
0.1 uF or 1 uF across each of the LED driver chips and the TD62783.

Looking at the datasheet for the TLC5916 LED driver, most of the useful
LED current adjustment range (120 mA to about 10 mA) happens between 0
and 2K ohms of Rext. If you use the 10K ohm pots for Rext, all of the
adjustment will happen very close to one end of the pot rotation. Using
a 2K pot (if you can find one) or a 5K might be better. If you are
willing to set an upper limit on how much LED current you can get, you
might use a small fixed resistor of 100 to 200 ohms or so, in series
with a 1K pot. This gives you a range of (say) 100 to 1100 ohms, which
is roughly 100 to 18 mA of LED current.

You should somehow mark pin 1 of your ICSP header, because you will
forget. Usually pin 1 has a square solder pad instead of round.
(This doesn't always help if the board is mounted and the square pad is
on the side you can't see, though.) If you are going to have a
silkscreen, you can put a dot or a "1" by pin 1. You could also mark
pin 1 of the TD62783 with either a square pad or a dot. For the smaller
chips, about all you can do is a silkscreen dot. Even if you don't have
a silkscreen, putting a dot near pin 1 with a fine-tip marker will save
you trouble some day.

Your schematic doesn't seem to show the power and ground connections to
the TD62783. They are there on the board layout (I think - pin 8 and
9), just not on the schematic.

You may want the power traces to the TD62783 to be as thick, or thicker,
than the ones between the TLC5916s and the LEDs. Try to make the power
trace come straight from J1 if you can.

You probably want the ground traces to the TLC5916s to be as thick, or
thicker, than the ones between the TLC5916s and the LEDs. Try to make
the ground traces go straight to J1 if you can.

How are you going to mount the board? If you need mounting holes in the
corners, I think Eagle knows how to specify that. (Or maybe that layer
is there and just didn't print in the PDF.)

Matt Roberds

 

Daniel,

See my reply in sci.electronics.design .

Matt Roberds

 

[Daniel Pitts]

On 1/21/14 7:05 AM, George Herold wrote:

On Tuesday, January 21, 2014 12:44:35 AM UTC-5, Daniel Pitts wrote:
I've completed my first PCB design in Eagle. Thinking of sending it off

to one of those small-batch fabs.



But, I'm wondering if anyone would be willing to take a look at my
design and giving me any pointers or gotchas? I'm looking for both
aesthetic and technical input.

On a related note, what's the best way to share my design/PCB on this
group?
Hmm for sharing I 'prin't the schematic or PCB to a pdf. and then put the pdf on dropbox. But maybe there is an easier method.
(here's a chaos schematic I did a year or so ago.)
https://www.dropbox.com/s/afy4kb63ftdo1ke/chaos2.pdf

Okay, PDF it is.

<http://virtualinfinity.net/electronics/LED%20Display%202%20-%20board.pdf>
<http://virtualinfinity.net/electronics/LED%20Display%202%20-%20schematic.pdf>

Eagle files:
<http://virtualinfinity.net/electronics/LED%20Display%202.brd>
<http://virtualinfinity.net/electronics/LED%20Display%202.sch>

Before I order my parts and boards, any suggestions?

Thanks,
Daniel.

 

[Daniel Pitts]

On 1/21/14 12:55 PM, mroberds@att.net wrote:

Daniel Pitts <newsgroup.nospam@virtualinfinity.net> wrote:
But, I'm wondering if anyone would be willing to take a look at my
design and giving me any pointers or gotchas? I'm looking for both
aesthetic and technical input.

[in a later message]

http://virtualinfinity.net/electronics/LED%20Display%202%20-%20board.pdf
http://virtualinfinity.net/electronics/LED%20Display%202%20-%20schematic.pdf

Aesthetic:

C1 should be labeled as 22 pF, not 22 pV.
Ah yes. Thanks

Technical:

You're using a regulated power supply, right? I ask because there is
no regulation in the schematic; that is OK if you are using a well-
regulated power supply.

Yes. I don't know how "well-regulated" it is, but the idea was to use a
regulated 5v power supply. This thing will pull enough current that I'd
rather not add a linear regulator if I could avoid it. Perhaps I'll
look into adding a DC-to-DC step-down regulator, and marking the supply
as +12v instead.

You will probably want at least one bypass capacitor - say 10 to 47 uF
directly across the +5 V input, near J1. Maybe also an 0.1 uF or so
across the power and ground of the ATTiny and the 74238, and perhaps an
0.1 uF or 1 uF across each of the LED driver chips and the TD62783.
This is just to smooth out voltage ripple?

Looking at the datasheet for the TLC5916 LED driver, most of the useful
LED current adjustment range (120 mA to about 10 mA) happens between 0
and 2K ohms of Rext. If you use the 10K ohm pots for Rext, all of the
adjustment will happen very close to one end of the pot rotation. Using
a 2K pot (if you can find one) or a 5K might be better. If you are
willing to set an upper limit on how much LED current you can get, you
might use a small fixed resistor of 100 to 200 ohms or so, in series
with a 1K pot. This gives you a range of (say) 100 to 1100 ohms, which
is roughly 100 to 18 mA of LED current.

Thanks for looking so deeply into the details here. I was actually
playing with the idea of doing a small resistor in series with a smaller
pot. I may do that.

You should somehow mark pin 1 of your ICSP header, because you will
forget. Usually pin 1 has a square solder pad instead of round.
(This doesn't always help if the board is mounted and the square pad is
on the side you can't see, though.) If you are going to have a
silkscreen, you can put a dot or a "1" by pin 1. You could also mark
pin 1 of the TD62783 with either a square pad or a dot. For the smaller
chips, about all you can do is a silkscreen dot. Even if you don't have
a silkscreen, putting a dot near pin 1 with a fine-tip marker will save
you trouble some day.

The place I'm sending the gerber files is expecting a top and bottom
silkscreen file, so I'm guessing I have a silkscreen. I'll add the dot.

Now if only I have a gerber viewer on my Mac.

Your schematic doesn't seem to show the power and ground connections to
the TD62783. They are there on the board layout (I think - pin 8 and
9), just not on the schematic.

The part in the library I used labelled them +UB and -UB, they are
connected, though maybe not in an obvious way.

You may want the power traces to the TD62783 to be as thick, or thicker,
than the ones between the TLC5916s and the LEDs. Try to make the power
trace come straight from J1 if you can.

When I first was putting this together, I was concerned about the
available surface area for everything. I can re-route it with larger
traces. Though the 74238 pads are small, so I'll need to switch to
smaller traces there. It should be drawing minimal power though. The
big power hogs will be the TLC5916s and TD62783.

Actually, what I'll try first is to add a ground fill on the bottom, and
a Vcc fill on the top.

You probably want the ground traces to the TLC5916s to be as thick, or
thicker, than the ones between the TLC5916s and the LEDs. Try to make
the ground traces go straight to J1 if you can.
Someone mentioned flood-filling GND. Would that help?

How are you going to mount the board? If you need mounting holes in the
corners, I think Eagle knows how to specify that. (Or maybe that layer
is there and just didn't print in the PDF.)

I hadn't thought about mounting at all. I guess I just envisioned it
dangling from the power cord ;-)

I probably will just have a couple of rubber feet put onto the bottom it.


Thanks again for all your suggestions. I'll reply with my updated board
soon.

 

[Jasen Betts]

On 2014-01-21, mroberds@att.net <mroberds@att.net> wrote:

Looking at the datasheet for the TLC5916 LED driver, most of the useful
LED current adjustment range (120 mA to about 10 mA) happens between 0
and 2K ohms of Rext. If you use the 10K ohm pots for Rext, all of the
adjustment will happen very close to one end of the pot rotation.

use a 10K audio taper pot. most of the rotation will be between 0 and 2K





--
For a good time: install ntp

--- news://freenews.netfront.net/ - complaints: news@netfront.net ---