DipTrace troubles with PCB

[MikeRamsey]

Hi all...I've been building clones for a bit and feel comfortable doing builds on perf, vero, and PCB's just fine. So I decided to try my hand at DipTrace and see if I can recreate a known circuit from schematic to PCB as an experiment before going all in on my own designs.. So cracked open DipTrace, loaded up the rubywow libraries, went through the tutorial(s) and I "thought" I had a handle on it... sent off the Gerber to JLCPCB and ordered 5 boards to test out... few days later, i get the boards and go straight to soldering... And then it all went to doo doo..

I get zip for sound when testing the board, and the LED doesn't even light up. tried two of them, carefully inspected all solder joints and connections and things "seem" ok.. so clearly I flubbed something in either the schematic or the PCB.

So I'm asking the brain trust here because A.) this forum rocks and B.) there are some VASTLY more knowledgeable people here than I, who always help out.. Would any of you gurus take a peek at my schematic and PCB layout and see if you can spot what I did wrong. I am 10000% positive it is my mistake, I just don't know enough to know what I goofed.

Screenshots attached are my attempt at recreating the Ginormous Fuzz (based on the insanely awesome Frost Giant Massif)

I can provide the DipTrace files as well, if needed.

Any assistance is much appreciated!!

 

[Robert]

Your transistors are routed backwards in the layout. The schematic is correct and they're marked correctly (EBC) on the PCB but the connections are reversed.

For example, the collector of the BC548 is connected to ground in your layout. The emitter should be connected to ground instead.

You should be able to remove/reinstall them rotated 180 degrees to correct that.

 

[Robert]

When you created your PCB layout, did you just manually place all of the components by hand or did you import the schematic?

If you import the schematic when starting a layout it will display "ratlines" to show which points need to be connected. This also allows you to run tests to compare your layout to the schematic and ensure everything is connected according to the schematic.

For example:

 

[MikeRamsey]

Your transistors are routed backwards in the layout. The schematic is correct and they're marked correctly (EBC) on the PCB but the connections are reversed.

For example, the collector of the BC548 is connected to ground in your layout. The emitter should be connected to ground instead.

You should be able to remove/reinstall them rotated 180 degrees to correct that.

Thanks!! i will give that a shot!

When you created your PCB layout, did you just manually place all of the components by hand or did you import the schematic?

If you import the schematic when starting a layout it will display "ratlines" to show which points need to be connected. This also allows you to run tests to compare your layout to the schematic and ensure everything is connected according to the schematic.

yeah I imported from the schematic, positioned all the components manually based on the rat lines, and then ran autorouter. a few fine tune adjustments for positioning and ERC tests passed.

 

[Brett]

Where does your power come into the board?

 

[Brett]

The pad marked "V" should be your "SW" pad on the schematic. The connection to the LED anode is also wrong, coming off of R5 which connects to D100's anode (rather than cathode). This is just on a quick look. Did you try running a DRC on the board? I've only used DipTrace briefly (horrible GUI on macOS), but I'd assume it has a DRC feature.

 

[Robert]

Where does your power come into the board?

Good catch, it looks like the +9V pad is missing.

+9V and VC(+) are both just net labels, not physical pads.


You'll need to connect 9V directly to the anode of the 1N5817 diode.

 

[MikeRamsey]

Thank you both!!! @Robert & @Brett looks like i goofed the 9v pattern in the schematic and didn't even notice it was missing from the PCB.. I'll redo that and give it another comb over.. Side question, is there a way to actually test the board without having to print it.. I ran all the verifications in Diptrace that were there and cleared the ERC fails but i could not figure out how to simulate a test, do i need something like LTSpice to do that?

apologies for the n00b questions... sincerely appreciate your help!!

 

[Brett]

You'll need to connect 9V directly to the anode of the 1N5817 diode.

I wouldn't power it up after just that change. The CLR resistor is connected incorrectly as well. With this one, I'd probably scarp this board and make another attempt. If DipTrace has a DRC feature, be sure to utilize it. I'm sure more than just myself would be happy to take a look at your board before you send it off to JLC again. This one is just going to require quite a bit of surgery to get working.

 

[Brett]

I ran all the verifications in Diptrace that were there and cleared the ERC fails

It goes without saying here, but if you have fails on the ERC/DRC, you probably don't want to clear them without fully investigating. It probably would have saved you some headache, money, and parts on this one. Chalk this up to a learning experience and give it another go! You got this!

 

[MikeRamsey]

I wouldn't power it up after just that change. The CLR resistor is connected incorrectly as well. With this one, I'd probably scarp this board and make another attempt. If DipTrace has a DRC feature, be sure to utilize it. I'm sure more than just myself would be happy to take a look at your board before you send it off to JLC again. This one is just going to require quite a bit of surgery to get working.

yeah i'm going to quadruple check the schematic and then reimport it to pcb. seems i borked this one proper bad.

 

[MikeRamsey]

It goes without saying here, but if you have fails on the ERC/DRC, you probably don't want to clear them without fully investigating. It probably would have saved you some headache, money, and parts on this one. Chalk this up to a learning experience and give it another go! You got this!

yeah i learn by failing and have become an expert at learning! its' questionable if im richer for it though.. shipping from jlcpcb is mad! $2.00 boards and $20 in shipping.. think i'll take a hard pause on ordering until i have these correct..

Again.. thank you for the help!

 

[PedalBuilder]

yeah i learn by failing and have become an expert at learning! its' questionable if im richer for it though.. shipping from jlcpcb is mad! $2.00 boards and $20 in shipping.. think i'll take a hard pause on ordering until i have these correct..

Again.. thank you for the help!

If you're in the US, make sure that you change the shipping to from DHL or whoever the default option is to Global Standard Direct Line. That drops shipping down to $1.50.

 

[MikeRamsey]

If you're in the US, make sure that you change the shipping to from DHL or whoever the default option is to Global Standard Direct Line. That drops shipping down to $1.50.

oh wow.. thanks for that tip!!

 

[Big Monk]

I'm certainly not an expert, but here is a down and dirty overview:



Notice that nodes like GND and VCC do not have pads attached. I could have easily connected the two Vcc nodes but wanted to illustrate that the naming convention means they connect:



All the nodes with (T) have pads attached. I gave your schematic multiple ground pads assuming that you'll want to ground jacks near the top for convenience.

I personally like laying things out so that everything connects directly on the schematic, instead of floating pads. For instance, an improvement on your schematic could be to use an I/O footprint and then just use padless net ports:



Here's what the initial stab looks like based on your order and original schematic:





Here is is cleaned up and slightly re-designed:




Running the QC checks, i.e. DRC, Check Net Connectivity, and Compare to Schematic:





In my opinion, you have to really try and fuck this process up once you have it dialed in going from Schematic to PCB.

With that said, you still have to make sure your schematic is correct. Frankly, I spend an inordinate amount of time laying out schematics and making sure they are correct and I've seen my error % in delivered boards go to Zero.

 

[MikeRamsey]

I'm certainly not an expert, but here is a down and dirty overview:

View attachment 78548

Notice that nodes like GND and VCC do not have pads attached. I could have easily connected the two Vcc nodes but wanted to illustrate that the naming convention means they connect:

View attachment 78549

All the nodes with (T) have pads attached. I gave your schematic multiple ground pads assuming that you'll want to ground jacks near the top for convenience.

I personally like laying things out so that everything connects directly on the schematic, instead of floating pads. For instance, an improvement on your schematic could be to use an I/O footprint and then just use padless net ports:

View attachment 78550

Here's what the initial stab looks like based on your order and original schematic:

View attachment 78551
View attachment 78552


Here is is cleaned up and slightly re-designed:

View attachment 78556
View attachment 78557

Running the QC checks, i.e. DRC, Check Net Connectivity, and Compare to Schematic:

View attachment 78558View attachment 78559
View attachment 78560


In my opinion, you have to really try and fuck this process up once you have it dialed in going from Schematic to PCB.

With that said, you still have to make sure your schematic is correct. Frankly, I spend an inordinate amount of time laying out schematics and making sure they are correct and I've seen my error % in delivered boards go to Zero.

Immense thank you!! for taking the time to do this. Supremely helpful!! And if there’s a possibility of me fucking up doing this, I’ll find it!!

I struggle with the named nets vs pads and see your point about laying it out the way you did. Off to update mine!!

Love this forum and members like y’all!!

 

[Big Monk]

Immense thank you!! for taking the time to do this. Supremely helpful!! And if there’s a possibility of me fucking up doing this, I’ll find it!!

I struggle with the named nets vs pads and see your point about laying it out the way you did. Off to update mine!!

Love this forum and members like y’all!!

When you first start out, the tendency is to get excited and rush and to also do things manually because you have not figured out the quality checks built into the program.

Once you get your own libraries together and understand the process from schematic to ordering, errors go way down.

 

[MikeRamsey]

When you first start out, the tendency is to get excited and rush and to also do things manually because you have not figured out the quality checks built into the program.

Once you get your own libraries together and understand the process from schematic to ordering, errors go way down.

Fully agree.. I saw no ERC errors and thought... Ship IT!!! Lesson learned!

Cannot thank you all enough.. pointing out my dumb has been helpful!! I'll post my updated schematic in a bit.. I can already see the need to start building my own component library so i'm not placing the wrong symbols and patterns on the schematic.. doggy paddling my way out of the deep end and putting on my floaties because i'm not ready to swim yet!!!