Having “never designed a PCB before” you’ve created a very nice looking layout.
Will conductive (metal) standoffs be used to mount this board? If so, the two traces on the bottom side (see image) will eventually make electrical contact with that standoff. In my experience solder mask is not a mechanical insulator.
The same caution applies to the top side. If conductive hardware is used the fastener will break through the solder mask and make electrical contact with the ground plane. This may, or may not, be what is intended.
I want to be able to access Gnd, 15V, and 5V in case I forgot to add anything, so I added test points so I can add a turret terminal and easily solder wires to them if need be.
I’ll also change the MCU cap and look into adding the bypass cap. Thank you
When researching how to wire the A4988 stepper drivers it always showed an electrolytic cap. With what you’re saying though I should be able to switch it for a ceramic cap?
Initial I believe I had the DI pin on the Max485 tied to ground, but when testing, the chip wasn’t working. So I removed that connection, but also changed a few other things and it worked. I’ll try reconnecting it again though. Should the enable pin of the A4988 stepper driver be connected to something as well?
Yes, metal screws are going to be used. I will definitely change the layout. I did not think about the screws possibly shorting the 2 traces. Thank you!
I have never used stepper driver.
In any modern switching circuit as effect of switching there are high current pulses. It is because modern circuits are able to switch very fast and can have internal keys with high current capabilities.
Even you read in datasheet that something switches in 5ns it is possible that it switches in 1ns (making loading parasitic capacitances currents being 5 times higher). It is because it can be cheaper in production (search ‘Die shrink’).
It is better if such current pulses flow in as short circle as possible. As these are short pulses you need not a big capacitance as current source for it (100nF is enough). But you need a capacitor with as small ESR and ESL as possible. So ceramic is for that much better then electrolytic. It also can be placed closer to the IC taking those current pulses. So the common solution is to give 100nF as close as possible and electrolytic C somewhere else (distance not critical). 100nF works for current spikes and electrolytic for slower pulses. Since some time ceramics with relatively high capacitance started to be available. They can be more expansive than electrolytic with same capacitance and voltage, but they can replace both (100nF and electrolytic). If you need high capacitance for high voltage then you will have to use electrolytic. I didn’t looked into parameters of elements you used. It was just general information how it should be done.
If you want to read more just see articles I have mentioned few years ago (hope links are still valid):
If driver is not enabled shoring DI to GND should have no effect.
I don’t know A4988 but generally all input pins should be set to known state. Some inputs can have build-in pull-ups or pull-downs allowing you to not polarize them externally.
Reading the data sheet, tying pin 4 DI high or low will force pins 6 & 7 and consequently, Pin 1, into permanent states that cannot be changed by signals into DMX 2 & 3.
The result being Pin 2 of the 328, an external counter input will be disabled.
That’s why I have two parts in my library: a simple drill (also useful from time to time) and a screw, having a keepout zone to prevent accidently routing a trace over it or beeing filled by a ground plane. In your case, the screws will still connect GND to the chassis. This may be ok but be aware of it.
In fact I have a third part for a screw that has a pad to surely connect it.
I would also suggest to reduce the clearance of the GND fill. Set it to 0.3mm and you will get connections under the IC pins resulting in a much stiffer GND connection.
Practically at each of my PCBs there is RS485 driver (not MAX485 but something like it). Not reading its data sheet I don’t believe in what you have read there.
The configuration for that IC is quite different to most others. That is why I went looking after the OP wrote that it wouldn’t work if Pin 4 was grounded.
Mouser and Digikey are good sources for datasheets of elements they have. I used alldatasheet only few times to find datasheet of inaccessible (old) elements.
You are wrong. Check it once more.
Pin 3 set to VCC enables the driver but OP needs to have driver disabled so pin 3 should be connected to GND as he did it.
Since 90s we use (in most of our products) ICs that are MAX485 functional equivalents (+ some extra features we need).
I just had a look at the board I am working on. My clearance is 0.5 mm and that is quite large=conservative for low voltages (voltages under 24V for example). I do not know much about your design, but the large clearance means that the rows of pins for a DIP cause a slit in the ground. In a very critical design this would reduce the effectiveness of your ground plane.
I like big clearance, but even 0.35 mm should not be a problem to work with for low voltages.
I cannot be certain, but I suspect that because your board is mostly through hole (not SMT) that the ICs are older and none of the signals or switching is VERY fast. FWIW any time a forum member is doing a new design and buying the components, I strongly recommend going with surface mount. It is not difficult (and is easier in some ways) so long as you are not using tiny lead pitch devices such as 0.5 mm or smaller. Of course if you have the through hole parts already, you might as well use them. I do that also.
Anyway I think it is unlikely that those slits I observe and mention above are likely to cause problems. That would seem like a more critical design than most of what I think is discussed on this forum.
I’m using 5V and 15V in my board. And I’m using THT because I’ve never hand soldered SMT before, I also have all the components already. I’ll probably reduce the clearance to 0.4 or 0.5mm
