Hey,
I got access to CNC PCB mill and lots of cheap material. It can do single sided PCBs (drills holes and everything). So, I just did my first layout for Big Muff with Eagle.
(http://i.imgur.com/EPL7isC.jpg)
So, even I think it looks messy. ;D I tried to move parts around and redo connections, but that's pretty much best I could on first try. It's going in a 1590BB, so there's lots of room. I tried to put the parts bit more apart to make soldering more easy (no solder mask).
So, could someone more experienced take a look and let me know what immediate problems are there? Will the long connections (for example C2 to C4, C8 to C6 or volume pot to out) cause problems?
Lots of people seem to use 45 degree angles instead of 90 degrees. I've always thought this doesn't matter in audio frequencies (only higher). Does it?
Any other tips or advice?
Thanks!
Edit. One more question: what are those blue patches at bottom right, below volume pot and at top right corner?
I would make the isolation a bit more and also make sure there is more space between traces and pads to reduce the possibility of connecting things that are supposed to be connected:)
Also, at least one trace touches a pad:
(https://uploads.tapatalk-cdn.com/20170123/185bd1924c67e61952d8e9adef3d51a2.png)
Sent from my iPhone using Tapatalk
I once had someone explain to me that circuit boards are like long lines of people standing shoulder to shoulder. Each time the 'power' gets turned on, all that happens is that the people in the lines nudge the person next to them until the end. It doesn't really matter how long the lines are, because this nudging is almost instantaneous.
So in the end, 45 degrees or 90 don't really matter, but they can make routing a little easier at times. Neither does the length of connections, because it takes a really, really long line before the electronic latency is noticeable, and there's no way you could ever fit even the largest enclosure with that much trace length.
As a PCB design guy of some sort, I really encourage people trying to up their game with two things:
1 - look at other PCBs out there. For instance, this is a circuit that has been done again, and again, and again. Doing it yourself feels fantastic, but it's okay to look at someone else's design to learn what they did, see things through their eyes.
2 - when you're designing the layout, don't just think about the traces, think about what it will be like to build the PCB and put it in an enclosure. Are you happy with the way the parts are on the PCB? Have you left yourself enough room in the right places? Is the PCB the right size and shape? Do you have the connections you need to make in the correct place to make the build go smoothly? I personally work hardest at this part first, making sure the orientation and arrangement of my parts are satisfactory, then I start working on the traces themselves, and adjust the parts on the PCB to make both the arrangement and traces work.
But I've done hundreds of layouts at this point, so please don't feel pressure to meet any sort of standard. I still remember making my first layouts, and the learning curve will allow you the experience over time.
Enjoy it! PCB making is fun!
Jacob
that's not bad for a first try. mine looked quite similar. Once you got that step, I've found it nice as a start to set some goals, like "I want the pots in that order/positions" or supply pads arranged a certain way. this constraints make it harder for sure, but the overall ease of building is worth it. you could make your layout a quite bit smaller just by moving components closer together in the arrangement as they are now. No idea what enclosure size or restrictions you have.
the blue patches you've got are probably some "keep out" areas. Check the active layers (upper left corner) and you'll find one that has the correct colour and pattern. keep out areas are usually areas where ratsnest does not fill in and stuff like that.
move r5, r16 and r15 a bit to the left. you'll eliminate the 90 turn to the clr. 90° should generally be avoided for some reason and I would just stick to the 45° drawing tools.
trace going from c8 to c5, check that it's not touching C7. use the DRC tool to check for any errors. it will tell you if traces are too close to pads and stuff like that.
Agree with most comments, especially those aimed at ease of assembly.
If you're going to cnc, try to optimize the cuts and trace widths to make the most of your cutter diameter. In general make sure that your diameter is a little thinner than your cuts, but not too much. Otherwise, it will take more passes to cut (dia too small), or worse (dia too big), you take away material off your traces.
Thanks a lot to everyone for suggestions and information! I moved parts bit more and here's the current version:
(http://i.imgur.com/ZSthKaw.png)
Quote from: PhiloB on January 23, 2017, 08:30:06 PM
I would make the isolation a bit more and also make sure there is more space between traces and pads to reduce the possibility of connecting things that are supposed to be connected:)
I tried moving parts a bit to get more space between traces and pads.
Do you mean the isolation between pads and other stuff? How do I increase that that?
Quote from: jkokura on January 23, 2017, 08:52:36 PM
I once had someone explain to me that circuit boards are like long lines of people standing shoulder to shoulder. Each time the 'power' gets turned on, all that happens is that the people in the lines nudge the person next to them until the end. It doesn't really matter how long the lines are, because this nudging is almost instantaneous.
So in the end, 45 degrees or 90 don't really matter, but they can make routing a little easier at times. Neither does the length of connections, because it takes a really, really long line before the electronic latency is noticeable, and there's no way you could ever fit even the largest enclosure with that much trace length.
Jacob
Thanks Jacob! Really informative post. I actually tried to look a bit for other peoples designs, but I think I was trying to look for way too specific stuff (like placements for all active components and so on). I'll try to study more of those. :)
Quote from: m-Kresol on January 23, 2017, 08:57:27 PM
No idea what enclosure size or restrictions you have.
It's going into 1590BB with top mounted jacks. No other restrictions.
Quote from: m-Kresol on January 23, 2017, 08:57:27 PM
move r5, r16 and r15 a bit to the left. you'll eliminate the 90 turn to the clr.
Thanks. I moved those around and I think its bit better now :)
Quote from: wgc on January 24, 2017, 02:21:11 AM
If you're going to cnc, try to optimize the cuts and trace widths to make the most of your cutter diameter. In general make sure that your diameter is a little thinner than your cuts, but not too much. Otherwise, it will take more passes to cut (dia too small), or worse (dia too big), you take away material off your traces.
Alright! I'll need to check to CNC mill next Monday to see what size are the cutters. I've only ran a single test layout with it so far.
Quote from: Jebus on January 24, 2017, 07:57:48 AM
I tried moving parts a bit to get more space between traces and pads.
Do you mean the isolation between pads and other stuff? How do I increase that that?
Ah, it was directly at polygon properties. I tried increasing it, does this look better:
(http://i.imgur.com/jZmPu0d.jpg)
Did some more moving around and increased the isolation bit more. This is surprisingly addictive.. ;D
(http://i.imgur.com/Ksdl45f.png)
check your schematic too. it seems to me that your power section is wrong. 9V goes to D5 (protection diode??), but the other end of the diode is also connected to 9V via a resistor...
the traces from R12 to R5/R16/CLR you can save the turn and run a straight line if you go from R12 to R5 rather than R16.
any reason for the increased leg spacing on C10? also if you move C10 directly under the right pad of D3 and align the lower pads of C9 and R13 with the lower pad of C10 you will make things easier too.
rotate Q2 90° to the right, this will also clean things up. also you can rotate R10 180° and reroute the trace that is now going from its lower pad to D1/D2
Quote from: m-Kresol on January 24, 2017, 05:27:05 PM
check your schematic too. it seems to me that your power section is wrong. 9V goes to D5 (protection diode??), but the other end of the diode is also connected to 9V via a resistor...
Good catch! Yeah, I thought I could do it like this:
(http://i.imgur.com/nC65HWp.png)
Where +9V(T) would only mean the pad and +9V would automatically connect to other +9Vs in schematic, but that doesn't seem to be the case. Now it should be fixed.
Quote from: m-Kresol on January 24, 2017, 05:27:05 PM
the traces from R12 to R5/R16/CLR you can save the turn and run a straight line if you go from R12 to R5 rather than R16.
any reason for the increased leg spacing on C10? also if you move C10 directly under the right pad of D3 and align the lower pads of C9 and R13 with the lower pad of C10 you will make things easier too.
rotate Q2 90° to the right, this will also clean things up. also you can rotate R10 180° and reroute the trace that is now going from its lower pad to D1/D2
Oh yeah, good ideas all. No reason for C10, probably just picked wrong component while drawing the schematic. :) I'll post updated layout later..
I've heard that the 90 degree thing is for REALLY REALLY high frequencies, places where straight traces act like antennae and the frequency ends up polluting something else that the trace is pointing at. But that might be BS, you know? ;)
Brian told me that some fab houses might actually have problems doing them properly as well.
Quote from: midwayfair on January 24, 2017, 06:24:19 PM
I've heard that the 90 degree thing is for REALLY REALLY high frequencies, places where straight traces act like antennae and the frequency ends up polluting something else that the trace is pointing at. But that might be BS, you know? ;)
Brian told me that some fab houses might actually have problems doing them properly as well.
Yeah, I asked couple of friends, who work lot with higher frequency electronics, and they both said it won't matter at all with audio frequencies. Well, I guess its still good habit to avoid those. :)
I updated the PCB with Felix's ideas, did you mean something like this?
(http://i.imgur.com/47L0nuU.png)
Edit. updated image. :)
looking good! minor thing, more of a personal perfectionism actually.
you can run the R5 to R3 trace horizontally instead of diagonal.
Quote from: m-Kresol on January 24, 2017, 07:40:17 PM
looking good! minor thing, more of a personal perfectionism actually.
you can run the R5 to R3 trace horizontally instead of diagonal.
Good idea, will do that tomorrow. Also should move R2 and R4 bit to left so I can lower Q1 and ground plane fills that "hole". :)
Quote from: Jebus on January 24, 2017, 08:02:54 PM
Also should move R2 and R4 bit to left so I can lower Q1 and ground plane fills that "hole". :)
that won't do the trick as the pour won't go in between the pins of the transistor. are you going to have some kind of solder mask?
That's true. Probably wont have any kind of solder mask. Should I swap the transistor in Eagle for ones that have more space between legs?
no, I wouldn't. I think you're fine the way it is, however, if you feel you need to adjust it, you could move C4 down a little bit, then the pour would go around the left pad of C4, and around the transistor.
Jacob
there's no reason why you would need the gnd pour in that area anyways. everyting that is supposed to be grounded is and that little piece won't make much of a difference concerning noise anyways.
you could shift the trace under the vol pot a bit further down away from the pads. Soldering in the pots is trickier with one sided layouts, especially if you use board mounts and thus it's easier to have a solder bridge. that's why I asked about the solder mask. btw. remember that madbeans pots are designed for boardmount, ie. on the BACK. if you have them on the component side and want to use board mounts too, you need to turn them
Quote from: m-Kresol on January 25, 2017, 07:32:13 PM
there's no reason why you would need the gnd pour in that area anyways. everyting that is supposed to be grounded is and that little piece won't make much of a difference concerning noise anyways.
Except that you need to recognize that he's doing this with a machine that drills out the PCB, and making it easier/quicker is not a bad goal.
Jacob
Quote from: wgc on January 24, 2017, 02:21:11 AM
If you're going to cnc, try to optimize the cuts and trace widths to make the most of your cutter diameter. In general make sure that your diameter is a little thinner than your cuts, but not too much. Otherwise, it will take more passes to cut (dia too small), or worse (dia too big), you take away material off your traces.
Alright! I'll need to check to CNC mill next Monday to see what size are the cutters. I've only ran a single test layout with it so far.
[/quote]
Just FYI
There's free gcode simulators online that should help you see if you have a problem.
Also, best to use your own cutters vs community stuff. They're cheap on amazon.
I moved parts around at left down corner and now I think it's looking better:
(http://i.imgur.com/EiOp4DS.png)
Quote from: m-Kresol on January 25, 2017, 07:32:13 PM
btw. remember that madbeans pots are designed for boardmount, ie. on the BACK. if you have them on the component side and want to use board mounts too, you need to turn them
I was thinking I would do them boardmounted at the solder side (like any commercial PCB, the soldering would just be bit different). So are those currently the wrong way around? ;D
if you put the pot on the solder side then it's ok as is. Looking really good btw. The learning curve is high and it is really addicting too. I like to spend long train rides doing pcb layouts :)
Alright, thanks!
I'm still wondering if I should move the trace that goes between the
legs of sustain pot. It could be easily routed under C2 and around the whole pot. What do you guys think?
Often, you'll be asking that question forever. There is, in many ways, no end to tweaks and adjustments. At the end of the day, you just have to call it down when it meets your design criteria and passes the electrical and design checks in eagle.
Jacob
The 90 degrees are fine except for high voltage traces, but I rarely do them except on a T intersection (If I don't add an angle).
Don't forget to do a design rule check. Find a set of rules you are comfortable with and stick with it. Often on the contract work I do, I find many errors that are simply found running a check, this applies to the schematic and PCB. ALWAYS run a check, and if you don't understand the error, google is your friend.
Also make yourself a checklist to follow during your design and at the end. This will eliminate things like the pots being on the wrong side.
Sometimes I have two layouts going for the same circuit after the constraints are met. Often there is a better arrangement than your initial parts placement, so save an alternate file in case it isn't. My last design I just wrapped up was extremely complex and running two layouts saved a lot of time, instead of having to keep backtracking my work, I could move forward on both and then I finished up the one that was the more efficient layout. This is especially helpful when you're tight on space.
Save versions while you are working so you can revert back and also have a backup. I usually save by name and date.
Granted these are more useful for complex designs and things beyond the DIY realm but good habits to get into.
Josh
Okay, I tweaked it bit more. Probably good enough now. :)
(http://i.imgur.com/YnffT5p.png)
Now I need to start wondering how the CAM Processor works and what all the options do. I asked the guy who has used the CNC machine before about the files, but he just said "yeah, you need Gerber files". ::)
You need a way to go from gerber to gcode. There may be a way to convert to gcode using a bw jpg too, but probably less desireable for efficient milling/ drilling.
There's some free programs for either approach but I haven't tried them.
This looks promising: http://flatcam.org
You'll need to know what controller the cnc has, and have the appropriate profile setup in your cam to make sure you get gcode that the machine can run.
Hey!
Got it! They had the CAM job ready for Eagle, so all I had to do was export the files and insert them to the controller program which turned them to gcode. :) Took 24 minutes to make the board and at least I think it turned out pretty darn good!
(http://i.imgur.com/qWN8Yk3.jpg)
Sorry about the fingerprints.. ;D
that is super cool! and so much easier and less messy than home etching and DRILLING
Looks great, awesome you could just drop the files and go.
looks good, especially for a first layout. Nice job!