Hi Guys,
I'm trying to convert a project I have into a full PCB with no extra modules. I'm using 8 of those cd74hc4067, and I want a more expert opinion if the main wiring for this is correct:
also 2 questions:
Thanks in advance!
Do you think there will ever be a situaion where you might possibly want to disable one of the ICs?
Hi jim-p, thanks for the quick answer! No, I will not have this situation. They will be used mainly for reading buttons, faders etc. I don't plan on chaining them as well, since the code will get more complicated.
You can tie the E (enable) to GND.
Remember you can mount SMDs (capacitors) on the bottom of your PCB too; one decoupling capacitor per chip.
Got it, so in this case the R1 (10K) is acting as a pullup right?
Pull-up goes to 5V
Pull-down goes to 0V
You do not need the resistor unless you want to disable the chip.
Thanks got it - So if I want to be able to disable all (high on EN) , use the resistor. If that is not the case, just wired strait to ground.
Thanks for the answers! As I update the project I will continue on this post.
Suggest you show us your complete schematic.
Hi sorry for the delay, I was updating the schematics. It's not yet a finished version, but you can have an idea. It's like a breakout board with mux for Analog / digital, later I'm adding 12C and Led matrix, with Midi In/Out ports. So it can be used for controllers as well.
Let me know your thoughts.
Thanks!
Show us the other PCB side i.e. IC traces red and on top.
Personally, I would place the +5v volt headers in the middle; that way turning the IO connector 180° keeps +Vcc in the middle.
Make sure trace clearances are checked with DRC.
What is the diameter of the VIAS And what is your trace width ?
Where are your mounting holes, a power LED is always nice.
Thanks LarryD. I will work a little more on the project and repost. I have to change the 74HC4067D,653 for the 74HC4067DB,118 due to availability. Will be back in a few hours or a day! Thanks for the insights.
Seems a lot easier to just use the modules pictured in post#1, with a 16-way ribbon cable soldered to each module, and then stack them with 2-3mm spacers on the mounting holes.
Bare wires straight through all the pins on the other side, connecting VCC/GND/S0-3/etc.
Leo..
Thanks Wawa. I already have a solution like this, where you can plug the leonardo and the modules. what I'm looking for is a way to have more ready and less solder , integrated pcbs, also to reduce size.. and maybe a little of challenge and fun along the way lol.
Wow, those traces and vias look really really small, and some of the clearances seem to be on the order of a few microns.
JLCPCB will manufacturer your board even if your violate their minimum requirement, but don't expect it to work.
Their min annular ring for a PTH is 12 mils. You have a via dia of 24 with a drill of 12, that gives an annular ring of only 6 mils ((24-12)/2). Their capabilities table is confusing with many contradictions.
I would use the following:
Drill = 20 mils
Via = 48 mils (annular ring = 14)
Trace = 15 mils minimum. Make power and ground as big as possible
Clearance = 15 mils minimum.
Don't tent the vias, they can be valuable test points when debugging.
Awsome! Thanks for the input, I will redo with those parameters. 
Hi Guys,
So i've made a few changes, trying to acommodate the suggested parameters for the board. I had to tweak a little due to the SMD components, but it's looking better. I've also made a bottom GND copper layer, and a top VCC (5V) top layer. Added a TCA9548A for multiplexing 12C ( enabling up to 8 devices, same address ex. oleds) . Componentes were mounted to one side only, for cheaper and easier assembly. Still need to add a Midi in and out and a led driver for led inputs and outputs + power on. Let me know your thoughts!
Top View
Bottom VIew
Quick Question(s) - I'm adding a MAX7219 to drive leds, so when buttons or controls are pressed, the can be used for a panel. I have found 3 different schematics:
MAX 7219 being driven by a 74HCT125 - as I understand, it's used as a signal buffer - Necessary?
If not necessary, I would use the MAX7219 directly into arduino, as the schematics above.
** Update - from the SPI SCK /MOSI/SS* pins. **
But I found a schematics for this approach that has an extra 10uf cap between VCC and GND - Wich one is correct?
Thanks!
Matrixed LED displays can add noise to the power supply rail, that needs to be suppressed.
Google "power supply decoupling".
It is common to have a ceramic cap and an electrolytic cap in parallel. They both cover (kill) a different frequency spectrum. I would have used 47 or 100uF instead of 10uF. Tiny 10uF electrolytic caps tend to dry out (fail) faster.
Leo..
