@paulvdh & al. I read on this forum other day that JLCPCB has online Gerber viewer, which does some error checking as part of the ordering process. I tried it out and got an error in the “Analysis” tab (photo 1). Being a newb, figured let slide until get other things worked out.
Been toiling away on my project, following @paulvdh 's very informative postings, above, using his version as reference and comparison. Took a break and tried JLCPCB’s online tool with his *.pro. I get two errors, the original Edge Cuts error, and a second, drill file error in re non-Gerber format (photo 2).
Can someone offer guidance in resolving this? If I was to submit order, I do not know if JLCPCB will reject based on these errors. In both instances I followed JLCPCB’s linked guide “KiCAD PCB to gerber files.”
The main to know is that ferryte beads are like inductors but with lo quality. At higher frequency inductors resonate but ferryte beads change RF energy to heat and not resonate. In power filtering it is better to not have something resonate so the first choise is ferryte bead. But if you are interested in filtering rather low frequency the ferryte bead is not good as it has rather low inductance and don’t work effectively at low frequency. 1MHz is low, 100MHz is high, but where exactly is the border betwean low and high - may be 10MHz but it depends on many things I think.
If I have a source of unwonted signal (like DCDC converter) I typically put two filtering stages at both sides of it. First - closer to DCDC with ferryte beads and ceramic capacitors (to filter as close to source as possible because high fregueny can use even a few cm of track to RF emmite) and second with inductors (100uH range) and electrolytic capacitors. I use 0603 1k ferryte beads (farryte beads are identified by their R at 100MHz) whenever possible (that means if their DC R is not too high). If DC R have to be very low than I look for less then 1k ferryte beads or for bigger then 0603 ones.
Yes, that’s the URL for the “KiCAD PCB to gerber files” page linked in the footer of their pages. Those are the guidelines I followed. Unsure if error or message, just not a green check mark. Just curious.
Make some errors on your PCB (Too small via’s, faulty PCB outline, traces outside Edge.Cuts, etc) and upload to JLC, and see if they get flagged.
I’m also curious what happens if you swap the filenames of a Silkscreen and a Copper layer.
Note: Ink does not conduct very well, and computers are stupid.
So, I opened symbol editor from Eeschema and dragged the hidden pin 22 to side (photo), tied it to pin 8. This then led to a grey label of my GND symbols as “GND 1”. There was no grey label when pin 22 hidden. Receive no ERC infractions on inspection.
Lots of greyed out GND pins in schematic symbols is a known issue in a lot of the library symbols. I’ve heard (more like “read” actually) that it’s a temporary thing and will probably improve with KiCad 6.
I did see a small bit of room for improvement in the PCB layout.
There were 3 traces between the 2 rows of pins in the top of this screenshot, but I rerouted MOSI to expand the GND plane between the THT pins on the top. This gives a shorter return path for the ISP connector currents. After that I saw I could easily move SDA and SCL to make the GND plane even more continuous, and I added a via for a continuous GND plane around the ISP connector.
These changes are pretty trivial for such a small and simple circuit as this, but for larger & compexer boards a lot of such details all add up.
Did you also remove the LED’s and replaced it with an experimental / kludge area?
With Oshpark you gat 3 or 5 boards, and that makes it easier to use all of your boards.
@paulvdh Yes, I wanted to move that 2x4 header closer to U1 to make tracks shorter than the 2.4 GHz antenna on the radio breakout. I think your mod makes that more practicable. Mahalo!
I got mired in self-tutor in re ferrite beads, inductors, &c. Seek advice (confirmation?) on possible choice ferrite for the L1 component in below capture.
Ferrite Bead With Axial Wire, 5A, 75 Ohms@100MHZ, DCR Max 0.01 Ohm Laird 28L0138-10R-10
This one I can stand up close to the chip, keeping C5 nearby as well.
AVCC is the supply of analog circuitry in U1. Such pin should get clear power. Analog circuitry typically don’t gets so high and short current pulses as digital circuitry. So the filtration is needed at lower frequencies than at VCC. Using here 10…22uH is typical, I think.
As ferryte beads has much lower L I would look for inductance and not ferryte bead here.
If you see that element you selected is for 5A and your AVCC pin gets probably few mA the red-light should lite-on in your head that you are probably doing something wrong. There are probably situations that it could be good choise but I don’t know such.
Look at characteristic of that ferrite bead at place where R is close to 0 and X and Z are the same line. I read that Z=8 ohm at 1MHz. From that you can calculate L=1,3uH (and the designer wonted 10uH).
I don’t understand power filtering as much as others so I can’t comment on value choice, but I can comment on the symbol used. Ferrite beads, while similar to inductors, are different enough to have their own unique symbol. See the Ferrite_Bead symbol in the Device library.
Thank you for the pointer. I think I approached from footprint point-of-view…lead and courtyard spacing…for a presumed axial-leaded component, generic “filler” component for layout purpose.
Thank you very much for your insight. I had been confused as to purpose/function of two different types “inductors”, ferrite vs. wire wound. Your search link helps me. Something like a Bourns 77F or 78F series should suffice, the wire wound kind. For power supply filtering with a ferrite I may forego the “inductor”. (Although, I recall passing my battery leads through a ferrite on a small “robot” few years back, cannot source my notes for the reasoning).
To note, not many of these Arduino-styled 328P breakouts include the 10uH inductor between AVcc and Vcc, as called for by Atmel (nee uchip). Pololu does, but they use a chip bead SMD inductor, which to me said ferrite. The Laird component sited above seemed best cross-ref to THT, Well, that my small brain could figure.
I go with the following: 10uH Inductor
On 2019-03-06 @Efcis suggested to add 2 small tracks to “fill up empty spaces”.
This is not only uselless, it is bad from an EMC point of view.
The loose fingers on the GND plane act as antennas that pick up and radiate noise.
He has also moved the tracks in that area of the board further apart, which is detrimental to the low impedance of the GND plane. The worst modification are the 3 vertical tracks on the top of the screenshot. This forces all GND currents in that area to go complety around all connectors, and this increases loop area.
When I saw this (again) I gave in and started this response.
A near to optimum track layout for this section of this board is:
Copper area on the top of the board is continuous.
Tracks hrough GND plane are close together to minimize discontinuties in GND.
By having 2 tracks between resistors R9+R10 and the IC below them there is room for a GND connection, so GND currents do not have to circumvent around these resistors.
Much more solid copper connection to the north east of Pin 14 of the AVR.
Thicker copper connection between the East side of U2 and the side of the board.