First time designing a PCB

[OiMcCoy]

So after days of frustration I finally found a layout that works for a small drive circuit that I found posted by Mark Hammer [here](https://www.diystompboxes.com/smfforum/index.php?topic=123341.0). So I have been using KiCAD and learning a lot from my failures. I was hoping I could solicit some feedback about my attempt. I know its messy and I need to clean up the labeling badly. Also the clipping diodes image has the cathodes going the wrong way (not sure why). But ya, please check it out and take the wind out of my sails by finding all the big mistakes I have unknowingly made.

Thanks in advance!

[OiMcCoy]

Also would love to hear any tips on how to make this smaller and neater.

[Digital Larry]

If that's your first attempt, you did pretty well.  To make it smaller, put components closer together.  You don't really need to put part values on the silkscreen, unless you REALLY want to for some reason.

The only other thing that jumps out at me is that I never have two traces come together at a 45 degree angle.  I think I was taught that those inner corners tend to get over-etched.  Maybe it's not such a big concern given the width of your traces, but it's also very simple to make them 90 degrees.

DL

[iainpunk]

the two diodes on the left, they should not be in the same direction, but in opposites.
if you can find the right footprint, you could apply upright resistors and diodes, or 1/8W instead of 1/4W resistors.
i think its quite a good looking layout already, some experienced engineers do worse, and i doubt you want to put in in a 1590A if its your first PCB design.

The only other thing that jumps out at me is that I never have two traces come together at a 45 degree angle.  I think I was taught that those inner corners tend to get over-etched.  Maybe it's not such a big concern given the width of your traces, but it's also very simple to make them 90 degrees.

i also have the same concern, but his traces are quite thicc to begin with, but for ''etiquettes'' sake,

that's the T-trace i was taught.

cheers, Iain

[OiMcCoy]

If that's your first attempt, you did pretty well.  To make it smaller, put components closer together.  You don't really need to put part values on the silkscreen, unless you REALLY want to for some reason.

The only other thing that jumps out at me is that I never have two traces come together at a 45 degree angle.  I think I was taught that those inner corners tend to get over-etched.  Maybe it's not such a big concern given the width of your traces, but it's also very simple to make them 90 degrees.

DL

Thanks. It was a rocky road getting to this points. I started it three days ago and finally came up with something that "works" this morning. As far as the 45 degree tracks, I was doing that to avoid 90 degree corners (for some reason I remember someone telling me that those are bad), but I never considered there being problems with the 45s. I guess 90 would be a better alternative.

[OiMcCoy]

the two diodes on the left, they should not be in the same direction, but in opposites.
if you can find the right footprint, you could apply upright resistors and diodes, or 1/8W instead of 1/4W resistors.
i think its quite a good looking layout already, some experienced engineers do worse, and i doubt you want to put in in a 1590A if its your first PCB design.

The only other thing that jumps out at me is that I never have two traces come together at a 45 degree angle.  I think I was taught that those inner corners tend to get over-etched.  Maybe it's not such a big concern given the width of your traces, but it's also very simple to make them 90 degrees.

i also have the same concern, but his traces are quite thicc to begin with, but for ''etiquettes'' sake,

that's the T-trace i was taught.

cheers, Iain

Thanks for the catch on the diodes. I messed that one up when drawing the schematic. Funny thing is I would never make that mistake breadboarding, but this a new medium for me so I really need to spend more time checking my work.

As for the T traces, I will give that a go. I appreciate the help.

[rockola]

If you're planning to socket the transistors, it would be a good idea to change the footprint to one where the legs are in a row. Transistor sockets with that leg pattern are expensive and hard to find.

If you're not planning to socket the transistors, those footprints are fine, but I would strongly suggest to reconsider.

A GND pad close to the +9V pad will make wiring easier.

A ground pour would be cleaner than a ground trace. Are you planning to etch this, or to have it made by eg. Oshpark? If you're getting it manufactured, you have a whole PCB side just waiting to be used as a ground plane.

Always a good idea to use the silkscreen to say what it is. A year later you'll be hard pressed to remember which circuit among the dozens you've done since then that one was. Date is a good idea too.

[OiMcCoy]

Alright, I cleaned up the labels, fixed the diodes, and fixed the 45 joints. Thanks for all the help!

[OiMcCoy]

If you're planning to socket the transistors, it would be a good idea to change the footprint to one where the legs are in a row. Transistor sockets with that leg pattern are expensive and hard to find.

If you're not planning to socket the transistors, those footprints are fine, but I would strongly suggest to reconsider.

A GND pad close to the +9V pad will make wiring easier.

A ground pour would be cleaner than a ground trace. Are you planning to etch this, or to have it made by eg. Oshpark? If you're getting it manufactured, you have a whole PCB side just waiting to be used as a ground plane.

Thanks for the tip on the sockets. Was not even thinking about that. I am having a hard time trying to find a footprint on KiCAD tho. I am sure its in there.

I plan on having PCBs printed in the future. Right now I am using this as a learning tool. I am unfamiliar with a ground pour. but I have envisioned having the traces on the bottom of the board and the labels on top.

[rockola]

If you're planning to socket the transistors, it would be a good idea to change the footprint to one where the legs are in a row. Transistor sockets with that leg pattern are expensive and hard to find.

If you're not planning to socket the transistors, those footprints are fine, but I would strongly suggest to reconsider.

A GND pad close to the +9V pad will make wiring easier.

A ground pour would be cleaner than a ground trace. Are you planning to etch this, or to have it made by eg. Oshpark? If you're getting it manufactured, you have a whole PCB side just waiting to be used as a ground plane.

Thanks for the tip on the sockets. Was not even thinking about that. I am having a hard time trying to find a footprint on KiCAD tho. I am sure its in there.

I plan on having PCBs printed in the future. Right now I am using this as a learning tool. I am unfamiliar with a ground pour. but I have envisioned having the traces on the bottom of the board and the labels on top.

If you're using KiCAD, it's called a "filled zone". Choose the filled zone tool and click somewhere outside your edge. Choose GND as the net from the dialog that appears, and tick B.Cu (back copper layer). Draw around your PCB. Hit B to refill the zone. You now have a ground pour on the back side.

It's not a problem to have labels on the same side as traces and even on top of them.

[Fancy Lime]

Hi OiMcCoy,

welcome to our little nuthouse!

I am in the same position as you, doing my first PCB designs and using KiCad. So everything I say is strictly one clueless noob to another.

First, +1 on the ground pour and on the transistor sockets.

You have two GND pads for some reason. That does not hurt but is unnecessary.

Do you want to home-etch or have it fabricated? If you home-etch, I would suggest making the traces a lot thicker to make it harder to mess up the etching. I use 1mm traces and 1mm minimum distance between traces for that. You can set those parameters in the preferences/design rules. If you send it to be fabricated, the trace thickness is probably fine (check the design rules of the fab house first). Most fab houses don't even have single sided PCBs anymore or charge the same for single or double sided. So I would put the ground plane on one side and everything else on the other.

If you want a smaller board, you can use a smaller pitch footprint for the resistors and diodes.

Your pots seem to be installed on the same side as the other components. I assume you want to use pots that are installed directly (without wires) because you used the footprints for those. Depending on the length of the pot legs and the height of the electrolytic caps beneath them, this may not fit. Consider installing the pots and LED from the other side as the rest of the components. There is a function for that in KiCad, I think if you right-click on the footprint in the PCB editor.

BTW, where did you find those pot footprints? Are those 16mm alpha angled print? What are they called officially?

HTH,
Andy

[iainpunk]

by the way, are that two electrolytic caps underneath the pots? i don't think that fits height wise!?!?

cheers

[OiMcCoy]

The pots are to be mounted on the other side of the board.

[Fancy Lime]

The pots are to be mounted on the other side of the board.

The way they are drawn at the moment, I am pretty sure that they are on the same side as the rest. That does not matter for anything that is unpolar or polar with only two leads (those can be flipped around) but it matters for the pots and the transistors. I think you need to flip the pots around so that pin 1 and 3 trade places.

[iainpunk]

The pots are to be mounted on the other side of the board.

in that case, the pots are mounted in reverse, if you don't want to mess with the layout, you might want to put them upside down onto the board, they will be correct again.

cheers

[OiMcCoy]

The pots are to be mounted on the other side of the board.

in that case, the pots are mounted in reverse, if you don't want to mess with the layout, you might want to put them upside down onto the board, they will be correct again.

cheers

That's a pretty big thing to get wrong.

In terms of flipping them, is there a way to override the fails safes that prevent you from wiring things wrong? Or do I need to invert it in my schematic?

[Fancy Lime]

The pots are to be mounted on the other side of the board.

in that case, the pots are mounted in reverse, if you don't want to mess with the layout, you might want to put them upside down onto the board, they will be correct again.

cheers

That's a pretty big thing to get wrong.

In terms of flipping them, is there a way to override the fails safes that prevent you from wiring things wrong? Or do I need to invert it in my schematic?

No, you just need to click on the component (the teal colored part that is the silk screen markings) and hit "F" or rightclick and choose "Flip". Then the teal should change to some kind of pink, indicating it is now on the back side and flipped. Make sure the "B.SilkS" layer is active.

[OiMcCoy]

I am overwhelmed by the help I have gotten. Thank you everyone.
Sadly, due to a crash, and a corrupt save file, I lost the design. However, I took all of what you have been teaching me and applied it to a simple one knob drive circuit I have been working on with hopes of putting it in 1590A enclosures.

[iainpunk]

what did you base it on?
might be one of those pedals where your guitar volume and tone knobs are the gain and contour controls.

i generally don't like putting gain controls on simple pedals i build for myself, i change my volume control constantly to control the gain, which is super convenient since its right at my finger tips

cheers, Iain

[OiMcCoy]

It's kinda based off of Electra Distortion and kinda based off of the clipping section of a big muff. Basically it is a  asymmetric soft clipping gain stage.

I built one with a gain control and have been passing it around to different players to get feed back. All of them say it's pretty uninspired until you drive the gain up near full, then it comes alive. So why not just keep it as simple as possible and try putting it in a 1590a.