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!
(https://i.postimg.cc/hXcVHZ5r/Big-Mac-Drive-PCB.jpg) (https://postimg.cc/hXcVHZ5r)
Also would love to hear any tips on how to make this smaller and neater.
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
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.
QuoteThe 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,
(https://i.postimg.cc/G8XxHfBC/t-trace.png) (https://postimages.org/)
that's the T-trace i was taught.
cheers, Iain
Quote from: Digital Larry on February 14, 2021, 11:37:25 AM
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.
Quote from: iainpunk on February 14, 2021, 11:50:38 AM
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.
QuoteThe 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,
(https://i.postimg.cc/G8XxHfBC/t-trace.png) (https://postimages.org/)
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.
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.
Alright, I cleaned up the labels, fixed the diodes, and fixed the 45 joints. Thanks for all the help!
(https://i.postimg.cc/Q9MGNWXz/Mac-Driver.jpg) (https://postimg.cc/Q9MGNWXz)
Quote from: rockola on February 14, 2021, 12:41:36 PM
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.
Quote from: OiMcCoy on February 14, 2021, 12:56:57 PM
Quote from: rockola on February 14, 2021, 12:41:36 PM
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.
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
by the way, are that two electrolytic caps underneath the pots? i don't think that fits height wise!?!?
cheers
The pots are to be mounted on the other side of the board.
Quote from: OiMcCoy on February 14, 2021, 02:57:51 PM
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.
Quote from: OiMcCoy on February 14, 2021, 02:57:51 PM
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
Quote from: iainpunk on February 14, 2021, 03:22:11 PM
Quote from: OiMcCoy on February 14, 2021, 02:57:51 PM
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?
Quote from: OiMcCoy on February 14, 2021, 03:45:55 PM
Quote from: iainpunk on February 14, 2021, 03:22:11 PM
Quote from: OiMcCoy on February 14, 2021, 02:57:51 PM
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.
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.
(https://i.postimg.cc/xk569FJn/OC1-PCB.jpg) (https://postimg.cc/xk569FJn)
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
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.
Well I took a shot and ordered 3 prototypes printed from OSH.
I know its probably old hat to most of you, but considering I am not a technically inclined guy I am pretty happy that I went from breadboard to PCB printing with in a few days.
Thanks everyone for all the help. This has been a lot of fun.
Glad we could help and glad it went so smoothly for you. I've been stuck at that stage for months now. Oh well, I'll get it done some day...
In the meantime, do you mind telling us where you found those pot footprints? Are they from an external library?
Andy
Its from the standard library. Omeg PC16UB Vertical. I believe in the Pot THT section.
I got to say this is a lot of fun. I am probably biting off more than I can chew but I just laid of the schematic for a Big Muff with a mid control.
Quote from: OiMcCoy on February 15, 2021, 12:16:48 PM
Its from the standard library. Omeg PC16UB Vertical. I believe in the Pot THT section.
I got to say this is a lot of fun. I am probably biting off more than I can chew but I just laid of the schematic for a Big Muff with a mid control.
It is a lot of fun, can become an addictive activity unto itself, i liken it to doing crossword puzzles.
dave
That's exactly it, it's a brain puzzle. Something I never realized how much I needed during this lockdown.
QuoteI know its probably old hat to most of you, but considering I am not a technically inclined guy I am pretty happy that I went from breadboard to PCB printing with in a few days.
that's super fast, i always get stuck on the breadboard stage, and rarely move further, only if i need a certain pedal or if it has very few components.
cheers, Iain
To be fair, I am still on the breadboard stage. But its just a values change choice. My goal is to have it finalized by the time I get the PCBs.
Quote from: davent on February 15, 2021, 12:29:54 PM
Quote from: OiMcCoy on February 15, 2021, 12:16:48 PM
Its from the standard library. Omeg PC16UB Vertical. I believe in the Pot THT section.
I got to say this is a lot of fun. I am probably biting off more than I can chew but I just laid of the schematic for a Big Muff with a mid control.
It is a lot of fun, can become an addictive activity unto itself, i liken it to doing crossword puzzles.
dave
I've found it to be a really fun thing to do. I usually do all rough draft work in DIYLC and then manually route the PCB in Diptrace. It's always thrilling to be pulling datasheets and getting spacing correct and then see what the final board will look like.
Trying my best to do a modded big muff, but man is this one proving to be a challenge. Trying to get it on a 1590b sized board. It's a hot mess!
I am too embarrassed to show off the complete BMP pcb. However, I decided to revisit the first project and apply what I have learned. I am way happier with this layout.
(https://i.postimg.cc/jLWtPnPr/MacDrive.jpg) (https://postimg.cc/jLWtPnPr)
Quote from: OiMcCoy on February 16, 2021, 10:03:33 AM
Trying my best to do a modded big muff, but man is this one proving to be a challenge. Trying to get it on a 1590b sized board. It's a hot mess!
Attached is an image of my recent Tone Bender MKII Layout. As you can see, this is a very tight board going into a 125B enclosure. My design constraint was an aesthetic one and in an effort to get most of the components in line, and also because I am using the larger 10 mm Vishay/Dale metal film resistors, I went through a few iterations.
(https://www.themodernbrewhouse.com/wp-content/uploads/2021/02/VB-MKII.png)
I can't imagine doing a BMP in a small space but my limited experience tells me these suggestions may help:
1.) Depending on board dimensions, you may want to entertain 1/8W resistors;
2.) You'll need the smallest caps you can find
A Big Muff in a 1590B is very doable. I have one in a 1590A, but I really can't remember if I drew the layout by myself or used somebody's layout. Probably the later. Anyway. For a 1590B layout with onboard pots, you can just google for effectslayouts big muff, but using a already made layout can take out some of the fun on doing your own.
One of the challenging parts on creating some layouts are the choices we make for our layouts. Specific in/out/v+/gnd pads position, onboard pots, aesthetic details like symmetry and parts distribution, no jumpers allowed if possible... A layout where you can put one pad for a pot on a corner of the board and another pad at the opposite corner is easier than putting those pads together at a random-ish position, and the later is easier than putting the pads on a specific position to use onboard pots.
Just three things on the MacDrive layout:
1- the pads for the transistors are too close to each other. This can easily results on them being hard to solder without any shorts.
2- you can improve the led track if you rotate R1 and C1, putting them horizontally and running the track under them. You'll have a better tracing route, but will remove the symmetry you created for the resistors (3 on each side). It's up to you what to do, but anyway I'd just at least run this track a bit far from C' and R1 pads, the trace is almost touching them.
3- the same can be said on the track that connects R1 and C1 to that bigger pad (input, probably), it's almost touching the ground pad. Put it a bit closer to R6 lower pad, but not close enough for it to touch R6 lower pad.
Btw, double sided layout?
Quote from: Marcos - Munky on February 16, 2021, 01:58:37 PM
A Big Muff in a 1590B is very doable. I have one in a 1590A, but I really can't remember if I drew the layout by myself or used somebody's layout. Probably the later. Anyway. For a 1590B layout with onboard pots, you can just google for effectslayouts big muff, but using a already made layout can take out some of the fun on doing your own.
One of the challenging parts on creating some layouts are the choices we make for our layouts. Specific in/out/v+/gnd pads position, onboard pots, aesthetic details like symmetry and parts distribution, no jumpers allowed if possible... A layout where you can put one pad for a pot on a corner of the board and another pad at the opposite corner is easier than putting those pads together at a random-ish position, and the later is easier than putting the pads on a specific position to use onboard pots.
Just three things on the MacDrive layout:
1- the pads for the transistors are too close to each other. This can easily results on them being hard to solder without any shorts.
2- you can improve the led track if you rotate R1 and C1, putting them horizontally and running the track under them. You'll have a better tracing route, but will remove the symmetry you created for the resistors (3 on each side). It's up to you what to do, but anyway I'd just at least run this track a bit far from C' and R1 pads, the trace is almost touching them.
3- the same can be said on the track that connects R1 and C1 to that bigger pad (input, probably), it's almost touching the ground pad. Put it a bit closer to R6 lower pad, but not close enough for it to touch R6 lower pad.
Btw, double sided layout?
Thanks for the great response. It is a double sided pcb. I have the ground and 9v running on the bottom layer.
I fixed up a lot of what you pointed out. An easy solution was to swap the IN and LED pads.
And thanks for pointing out the legs of the transistor being close. I will have to be careful when soldering them on the PCBs prototypes I ordered.
I have said it before and I will say it again, thank you everyone for being so incredibly helpful. I think I would be swearing at my computer and then giving up if it weren't for you.
Also, I found out there is a 3D render option.
(https://i.postimg.cc/K40wfMWj/MACdriver.jpg) (https://postimg.cc/K40wfMWj)
You're in deep now, there's no looking back.
dave
There for sure is no going back. I kinda want to go through a list of all the classic small circuits and design PCBs for them. Once I get confident in it, I should offer out my services to others. I mean, until I can go back to work, I have a lot of time on my hands.
Also I noticed that PCB manufacturers charge by the square inch. So I reduced the size of the OC1 Drive.
(https://i.postimg.cc/06k9WHmm/OC1-Drive3-D.jpg) (https://postimg.cc/06k9WHmm)
Quote from: OiMcCoy on February 16, 2021, 04:04:55 PM
An easy solution was to swap the IN and LED pads.
Yep, sometimes this kind of thing solves some stuff. I like to put the in pad on the lower right corner with a gnd pad right next to it, the out pad on the lower right corner with a gnd pad right next to it, or both in and out pads as close as possible (again with gnd pads right next to it). Gnd pads right next to in/out pads makes wiring way easier if you're using shielded wires. Power pads on the exact middle of the top side of the board, and usually don't care too much on the led resistor. But if this positions make me have too much work, I just use what makes the tracing easier and call it a day lol. The very board I'm building now have the output wire soldered directly to the colume pot because it was a long (and with jumpers) way to get a trace from the pot position to the out pad position I usually like to use.
Your boards are nice looking, with parts well distributed along board space. You probably can go with a bit smaller resistors, if you bend their legs as close as possible to their body they'll need a bit less of space. Or use standing resistors when space is an issue. Of course, those are just suggestions. So far, things are looking good.
Quote from: Marcos - Munky on February 17, 2021, 07:45:51 AM
Quote from: OiMcCoy on February 16, 2021, 04:04:55 PM
An easy solution was to swap the IN and LED pads.
Yep, sometimes this kind of thing solves some stuff. I like to put the in pad on the lower right corner with a gnd pad right next to it, the out pad on the lower right corner with a gnd pad right next to it, or both in and out pads as close as possible (again with gnd pads right next to it). Gnd pads right next to in/out pads makes wiring way easier if you're using shielded wires. Power pads on the exact middle of the top side of the board, and usually don't care too much on the led resistor. But if this positions make me have too much work, I just use what makes the tracing easier and call it a day lol. The very board I'm building now have the output wire soldered directly to the colume pot because it was a long (and with jumpers) way to get a trace from the pot position to the out pad position I usually like to use.
Your boards are nice looking, with parts well distributed along board space. You probably can go with a bit smaller resistors, if you bend their legs as close as possible to their body they'll need a bit less of space. Or use standing resistors when space is an issue. Of course, those are just suggestions. So far, things are looking good.
Thanks. I thought about doing standing resistors, but that limits the caps as my only trace jumps. I think it will come down to the enclosure limits if I choose to really make it compact.
One Knob Fuzz from Colorsound. (no pop or polarity protection)
(https://i.postimg.cc/GBhVBnr9/1knobfuzz.jpg) (https://postimg.cc/GBhVBnr9)
I think I am just going to make PCB layouts for a bunch of classic circuits. Since I live in Canada, and our access to PCBs can be limited, maybe there would be a market here for PCBs. I don't know, just trying to think of ways to capitalize on my new found obsession.
Quote from: OiMcCoy on February 16, 2021, 05:48:38 PM
Also I noticed that PCB manufacturers charge by the square inch.
Oshpark does. Most of the usual suspects in China charge the same up to 100mm x 100mm.
By-the-square-inch is very good for stuff like this.
(https://ola.rinta-koski.net/Pedals/Pimentero/gutshot.jpg)
OiMcCoy, where did you find the 3D rendering? Is that a plug-in? I can only render the board but not the components.
Cheers,
Andy
Even if it weren't your first attempt it'd be very neat! Well done!
(And get yourself a NAS or put those electnronics files on a Google drive and work on them online. Says someone who lost EVERY Cubase arrangement file he ever did to a HD crash some years ago.)
Quote from: Fancy Lime on February 19, 2021, 12:08:55 AM
OiMcCoy, where did you find the 3D rendering? Is that a plug-in? I can only render the board but not the components.
Cheers,
Andy
It just under VIEW > 3D viewer
No extra plug in. Maybe your version is out of date?
Quote from: Fancy Lime on February 19, 2021, 12:08:55 AM
OiMcCoy, where did you find the 3D rendering? Is that a plug-in? I can only render the board but not the components.
Cheers,
Andy
There's a graphic option in the 3D viewer. You'll have to toggle the items you would like to see (TH, SMD, paste and so on).
Also - some parts don't have the models set automatically. So you'll have to change the 3D properties through PCB new (right click the part, properties and the 3D tab).
By the way - great first layout! Only needed minor cleaning.
Turns out, the 3D component library called packages3d is not bundled with the other libraries under Debian Linux, and I did not have it installed. This is probably so because the 3D library is quite big and not really essential. Anyway, installed it, now it works.
Thanks,
Andy
Quote from: KarenColumbo on February 19, 2021, 12:27:13 PM
And get yourself a NAS or put those electnronics files on a Google drive and work on them online.
I put mine on Github... See eg. https://github.com/rockola/superduro
It took a lot of effort, and I am not exactly pleased with the layout... but I got the Big Muff laid out.
I am going to get this one printed and build it for myself. It's one of my all time favorite pedals and I no longer own one.
(https://i.postimg.cc/TKL2Fzq4/Grand-FUPA.jpg) (https://postimg.cc/TKL2Fzq4)