PCB Layout Improvement using BMP example

Stompboxes circuits published in magazines, books or on DIY electronics websites.

PCB Layout Improvement using BMP example

Postby FlyingWild » 10 Nov 2019, 20:29

Following a discussion in another thread, http://www.freestompboxes.org/viewtopic.php?f=7&t=29980&start=20#p277589 I have asked Mookyj, if he would be so kind as to suggest how I improve the PCB layout for a BMP that I have recently etched a board for.

I can only upload one file in this post so I've attached a PDF of my PCB layout, and in DropBox I have the Eagle files for the schematic and board layout I did: https://www.dropbox.com/sh/qlk62u7b589fuyh/AACS-8egSb-HGxEVA3uuv8Dba?dl=0

Also in the DropBox folder is a photo of the bottom of the PCB showing the ground plane fill (sorry not sure of the technical term) but I undid it on the Eagle file as I don't know how to turn it on or off. This was done because I discovered how to do it, not, alas, because I understand what it does other than surely it's better than individual ground tracks. My layouts are for home etching, hence limited to two layers and using vias, or the legs of resistors to transition from one layer to the other.

My methodology for PCB layout is to first establish where the pots are going, as I use board mounted pots, then draw a ground track around the perimeter, then try and find a sensible place for the power filtering, after that I'm sorry to say my method is trying to make everything fit and limit the number of vias were possible.

I started learning Eagle (free version) a year ago, I don't have any electrical understanding by way of a formal education, just picked bits up, but would describe myself as still in the painting by numbers phase with the occasional glimmer of understanding.

What I'm hoping to learn is a better methodology for laying out a PCB. Any advice would be gratefully received from anyone who wishes to comment.

For this message the author FlyingWild has received thanks:
Satch12879 (11 Nov 2019, 15:11)
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby FlyingWild » 10 Nov 2019, 20:44

The file upload didn't work, here is the PDF of the board.
You do not have the required permissions to view the files attached to this post.
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby mookyj » 11 Nov 2019, 01:39

I need to look further at details, here's what I see in initially looking at it:

It's is organized, and nice attention to clean routing. In and outs are separated from each other and it makes for a nice counterclockwise signal flow. We can do a lot with this layout and I think you will like what it will end up at. This is a good start.

1. I would keep pot placements,
2. In and outs, maybe a littler wider but likely to stay as is. I would move power in down, and closer to main filtering. Or move cap and filtering section up. As I think of it, I would ove out more to the left past C16
3. Instead of tidy columns, think about having parts placements more closely follow as drawn in schematic. Schematic is well drawn.
4. Routes can be shorten by improving placements and orientations. Note- this is improving what is not a bad layout as one can visually follow the signal path in the layout, it does flow.
5. I personally would go a little wider on traces.
6. Return paths and consistent impedance is lacking with the ring around the periphery concept. Much like the old days of rack cards with V+ on one end, gnd on the other. Sets up longer return paths. You want to get the lowest impedance path you can for your return currents, We can get this to have a good reference plane on the bottom with plenty of coverage.

Mike

For this message the author mookyj has received thanks: 2
FlyingWild (11 Nov 2019, 09:04), Satch12879 (11 Nov 2019, 15:11)
User avatar
mookyj
 
Posts: 18
Joined: 17 Jul 2018, 03:13
Location: Cortland, NY
Has thanked: 10 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby FlyingWild » 11 Nov 2019, 09:09

Hi Mike,

Thank you for taking the time to look over my schematic and board layout. It will be this evening before I can really turn my attention to your suggestions, but I'm very grateful for your advice, and probably have many follow up questions.

Chris
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby Satch12879 » 11 Nov 2019, 15:11

This is a great thread. Thanks, guys for doing this.
Satch12879
 
Posts: 15
Joined: 09 Jun 2010, 00:41
Has thanked: 2 times
Have thanks: 2 times

Re: PCB Layout Improvement using BMP example

Postby FlyingWild » 11 Nov 2019, 22:02

Hi Mike,

mookyj wrote:I need to look further at details, here's what I see in initially looking at it:

It's is organized, and nice attention to clean routing. In and outs are separated from each other and it makes for a nice counterclockwise signal flow. We can do a lot with this layout and I think you will like what it will end up at. This is a good start.

1. I would keep pot placements,
2. In and outs, maybe a littler wider but likely to stay as is. I would move power in down, and closer to main filtering. Or move cap and filtering section up. As I think of it, I would ove out more to the left past C16

By moving the power input closer to the filtering, would this help reduce potential power supply noise? As it is at the moment, the 9v I/P track runs past all the resisters of the final transistor stage before reaching the filtering. With regards to the input and outputs, I've not consciously kept them widely apart, after all they arrive at a switch with the solder lugs just a few millimeters apart.

mookyj wrote:3. Instead of tidy columns, think about having parts placements more closely follow as drawn in schematic. Schematic is well drawn.
4. Routes can be shorten by improving placements and orientations. Note- this is improving what is not a bad layout as one can visually follow the signal path in the layout, it does flow.

I’m looking at the schematic and my currently layout and considering how to shorten the routes, by repositioning components etc, but could do with an approach to follow, which I'll ask you about below.

mookyj wrote:5. I personally would go a little wider on traces.

My current width is 28, I’m guessing going wider lowers resistance? Do you have a suggestion regarding width? I'm assuming Eagle is talking 1/1000's of an inch.

mookyj wrote:6. Return paths and consistent impedance is lacking with the ring around the periphery concept. Much like the old days of rack cards with V+ on one end, gnd on the other. Sets up longer return paths. You want to get the lowest impedance path you can for your return currents, We can get this to have a good reference plane on the bottom with plenty of coverage.

The ring around the periphery was intended to ensure all grounds were at the same potential, the idea of considering impedance was not even on my horizon. This, I’m assuming is why a ground plane is desirable? I would use the term resistance, but you have used impedance, is that because there is an AC signal involved?


Taking several steps back, after establishing where key components are going i.e. potentiometers and switches, where is a sensible place to start? For example should I decide where the input, output, GND & DC wire pads need to be, with the input and output well spaced, then the power filtering?

And lastly are you able to read the Eagle files or would PDF exports be better?

Thanks again for you help, and any advice would be very welcome.
Chris
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby mookyj » 12 Nov 2019, 00:19

By moving the power input closer to the filtering, would this help reduce potential power supply noise?

Response:
Incrementally yes, in a high gain pedal you would notice differences. Same goes for powering the LED as it can act as an antenna, I might power it after C16 & the series resitor.

As it is at the moment, the 9v I/P track runs past all the resisters of the final transistor stage before reaching the filtering. once through the series resistor, and filter cap, then you may like to go wider with your V+ even partial poor that you might be able to do after tweaking placements.

With regards to the input and outputs, I've not consciously kept them widely apart, after all they arrive at a switch with the solder lugs just a few millimeters apart.

Response:
Yes, they do get close at the footswitch, but the less you have that happen the better in other places. A lot of designs have inputs/outputs close together for neater wiring, not a fan of it. If you go high enough gain or looking to achieve lower noise or lower bleedthrough it is better to reduce proximity. Getting away with it, or "good enough:" as some like to say is not the same as getting the best result.

I’m looking at the schematic and my currently layout and considering how to shorten the routes, by repositioning components etc, but could do with an approach to follow, which I'll ask you about below.

mookyj wrote:
5. I personally would go a little wider on traces.

My current width is 28, I’m guessing going wider lowers resistance? Do you have a suggestion regarding width? I'm assuming Eagle is talking 1/1000's of an inch.

Response:
In the pcb lingo, that would be 28mils what you might think about is what the cross-section is of the trace. would you favor 24-26ga wire or 30-32 wirewrap wire? There are calculators that give you this data, I favor Saturn PCB, they have a great tool and it is free, there are others that many designers like.

mookyj wrote:
6. Return paths and consistent impedance is lacking with the ring around the periphery concept. Much like the old days of rack cards with V+ on one end, gnd on the other. Sets up longer return paths. You want to get the lowest impedance path you can for your return currents, We can get this to have a good reference plane on the bottom with plenty of coverage.

The ring around the periphery was intended to ensure all grounds were at the same potential, the idea of considering impedance was not even on my horizon. This, I’m assuming is why a ground plane is desirable? I would use the term resistance, but you have used impedance, is that because there is an AC signal involved?

Response:
In terms of DC resistance, you will have milliohms in differences, AC signals travel path of least impedance. When they don't, they can exhibit antenna behavior as it creates a ground loop. Ground plane solves many things if done right, mess up your circuit if not. You can also create low impedance returns with matching ground traces on the opposite side. Once you run through looking at how signal currents travel you begin to pick up on how parts placement for signal flow is more important than neat rows and columns. Neatness does count of course, but making longer taces to create a lined up row or column is for art not so much for function.


Taking several steps back, after establishing where key components are going i.e. potentiometers and switches, where is a sensible place to start? For example should I decide where the input, output, GND & DC wire pads need to be, with the input and output well-spaced, then the power filtering?

Response:
I think your pot(s) placement would stay, in and pouts further to the ends or leave as is. I would move the power in down towards C16. Also, add a ground pad for input and output should you want to use shielded wire for any reason. If you are fine with a single wire, it won't hurt a thing. By doing so, you can also play with grounding schemes in your wiring for the best result.

And lastly are you able to read the Eagle files or would PDF exports be better?

Response:
I have subscriptions to a number of tools including Eagle, that works fine. Eagle also ports to KiCad if you are inclined.

For this message the author mookyj has received thanks:
FlyingWild (17 Nov 2019, 18:33)
User avatar
mookyj
 
Posts: 18
Joined: 17 Jul 2018, 03:13
Location: Cortland, NY
Has thanked: 10 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby mookyj » 12 Nov 2019, 00:22

Sorry I did not format this correctly:

As it is at the moment, the 9v I/P track runs past all the resisters of the final transistor stage before reaching the filtering.

Response:
once through the series resistor and filter cap, then you may like to go wider with your V+ even partial poor that you might be able to do after tweaking placements.

For this message the author mookyj has received thanks:
FlyingWild (17 Nov 2019, 18:33)
User avatar
mookyj
 
Posts: 18
Joined: 17 Jul 2018, 03:13
Location: Cortland, NY
Has thanked: 10 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby FlyingWild » 13 Nov 2019, 19:59

Alas I'm tide up for the next few evenings but will try and implement your suggestions in a revised board layout and will put it in the drop box folder once done over the weekend.

Thank you again for taking the time to respond to my questions,

Chris

For this message the author FlyingWild has received thanks:
mookyj (13 Nov 2019, 20:29)
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby FlyingWild » 17 Nov 2019, 18:32

Hi Mike,

I have revised the board layout as follows:

    1. C16 is now closer to the filtering section.
    2. The output is further away from the input and to the left of C16
    3. The LED is now powered after the series resistor.
    4. Power now comes in at the bottom.
    5. Input and Outputs have additional ground pads.

Schematic File: https://www.dropbox.com/s/e8jsc5t0eixhbqn/bmp%20red%20army%20v1.1.sch?dl=0
Board File: https://www.dropbox.com/s/uisk2jcijl9syye/bmp%20red%20army%20v1.1.brd?dl=0

I have not attempted to improve the placement of the other components yet thinking a step by step approach would be better rather than potentially diving off in the wrong direction.

The track widths are still at 28mil because I’m still not sure what a sensible width is, regarding your examples, I’d not come across Wirewrap before so it was nice to learn something new, however I can’t answer the question as to which wire gauge I’d prefer, as surely that answer is dependent on a number of criteria. Given your examples a 30 AWG wire, the cross section would be almost twice that of my 28mil track, the copper being 35 micron, the 26 AWG wire would be over five times the cross section (I’m hoping my maths and conversions are correct at this point). I feel the expected response is that 26 AWG wire would be preferred, but I don’t suppose you are proposing I increase the width of my track five times?

Thanks for all your help, Chris
You do not have the required permissions to view the files attached to this post.
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby mookyj » 17 Nov 2019, 22:59

FlyingWild wrote:
The track widths are still at 28mil because I’m still not sure what a sensible width is, regarding your examples, I’d not come across Wirewrap before so it was nice to learn something new, however I can’t answer the question as to which wire gauge I’d prefer, as surely that answer is dependent on a number of criteria. Given your examples a 30 AWG wire, the cross-section would be almost twice that of my 28mil track, the copper being 35 micron, the 26 AWG wire would be over five times the cross section (I’m hoping my maths and conversions are correct at this point). I feel the expected response is that 26 AWG wire would be preferred, but I don’t suppose you are proposing I increase the width of my track five times?




34ga has a cross-section of 0.0201sq.mm
32ga has a cross-section of 0.0320sq.mm
30ga has a cross-section of 0.0509sq.mm
26ga has a cross-section of 0.1288sq.mm
24ga has a cross-section of 0.2047sq.mm

28mil 1-oz copper has a cross-section of 0.024sq.mm
28mil 2-oz copper has a cross-section of 0.035sq.mm

50mil 1-oz copper has a cross-section of 0.043sq.mm
50mil 2-oz copper has a cross-section of 0.065sq.mm

For this message the author mookyj has received thanks:
FlyingWild (18 Nov 2019, 00:03)
User avatar
mookyj
 
Posts: 18
Joined: 17 Jul 2018, 03:13
Location: Cortland, NY
Has thanked: 10 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby FlyingWild » 18 Nov 2019, 00:02

Thank you for the table Mike, alas in the UK the copper thickness is quoted in Microns, not ounces for example:

Specifications
Thickness: 1.6mm
Copper foil: 35 micron
Dissipation factor: 35
Dielectric constant: 5.4

However, using your table 26ga has a cross-section of 0.1288sq.mm and 28mil 1-oz copper has a cross-section of 0.024sq.mm, so 0.1288 divided by 0.024 equals 5.367, as I said in my previous post, over five times. However, I really don’t feel I’m any further forward in trying to determine what you were suggesting by:
5. I personally would go a little wider on traces.

Five times is, to me, significantly wider than “a little wider”. I fear I have missed some key point in your question:
would you favor 24-26ga wire or 30-32 wirewrap wire?
And that the answer to track width is self evident, but unfortunately it is not to me.

I really don’t mind researching things and I don’t want to be spoon fed, I would like to produce better PCBs, but feel it is likely to be frustrating for both of us to continue with this as I'm obviously not at a level to really benefit from your knowledge. I will endeavor to find a book on PCB design to fill in the many holes in my knowledge, and I do appreciate the help and time you've given me,

Chris
FlyingWild
 
Posts: 27
Joined: 28 Oct 2018, 22:01
Has thanked: 9 times
Have thanks: 7 times

Re: PCB Layout Improvement using BMP example

Postby mookyj » 18 Nov 2019, 00:19

It is not that daunting as it all traces back to simple equations, ohms law, etc. As you can see, 28mil tace is of similar cross-section of very thing wire-wrap wire. It's not any more complicated than that. If you go thru your parts placements and positioning you will find your traces much shorter and a 40-50 mil trace width will work just fine. The idea here is that you can go smaller when using smaller parts such as SMD packages as it is impractical to do that globally on say 0402 style passives, on another hand, the length of traces would likely be much shorter. As you go further I will be glad to help you with any questions you have or to review and recommend as needed.


Mike

For this message the author mookyj has received thanks:
FlyingWild (18 Nov 2019, 18:51)
User avatar
mookyj
 
Posts: 18
Joined: 17 Jul 2018, 03:13
Location: Cortland, NY
Has thanked: 10 times
Have thanks: 7 times


Return to DIY Stompbox designs

Who is online

Users browsing this forum: No registered users and 6 guests