First PCB-design: 32C eq

GroupDIY Audio Forum

Help Support GroupDIY Audio Forum:

This site may earn a commission from merchant affiliate links, including eBay, Amazon, and others.

wlinart

Well-known member
Joined
Jan 19, 2012
Messages
282
Location
Belgium
Hi All,

I started with my first pcb design: the harrison 32C eq. Because it's my first time, I'm not sure it's a good design.
Could you maybe check if the pcb is useable?
I included the scematics in this post
 
Here is the brd file (eagle)
I've decided to use 4 gang pots, just because it was cheaper. I only used 2 gangs of them. (this is the pot: http://www.mouser.be/Search/ProductDetail.aspx?R=PTD904-2015K-C503virtualkey65210000virtualkey652-PTD9042015KC503)
For the gain pots, i've decided to mount them offboard. 2 reasons for that: the layout can be the same as the original and to save space.

Thanks for helping me out!
 
People here use different pcb software and browse forums on mobile phones.
It would be cool if you could do a PDF file or some simple JPG with board and schematic...
:)
 
Looks good
Maybe some more experienced members can check for mistakes

You should give it a try and have few boards manufactured!
 
Thanks for the reply.
I want to be sure that's everything is allright before ordering, hence the question.
 
the pots look to be board mounted and look rather close. Imagine what the front panel will look like and if you will have enough space around the knob for markings etc, you may need to allow additional space for this.

and further to this, the push switches may need to sit further back depending on how you plan on mounting it, once the cap goes on the switch can stick out a lot, so make considerations for this as well.
 
I am unable to open the board file with Cadence Allegro. If you attach a  manufacturing file such as Gerber I could look at it with LPKF circuitpro.  I also need practice running the Protolaser...
 
This is exactly why i wanted other people to check it  :)
warpie said:
no ground plane?
I don't know actually, I thought i did it, but I'm not sure. How can I check in  Eagle?

Humner said:
the pots look to be board mounted and look rather close. Imagine what the front panel will look like and if you will have enough space around the knob for markings etc, you may need to allow additional space for this.

and further to this, the push switches may need to sit further back depending on how you plan on mounting it, once the cap goes on the switch can stick out a lot, so make considerations for this as well.
Wow, this is just embarrassing, that i hadn't even thought of that. Well, I guess i can rework it a lot, or start over.

walter said:
I am unable to open the board file with Cadence Allegro. If you attach a  manufacturing file such as Gerber I could look at it with LPKF circuitpro.  I also need practice running the Protolaser...
I will, when the corrections above are made.
 
A few things to change. It looks like you made a polygon on layer 1 to do a copper pour, but you must name the polygon with a node name in the circuit, and then also do a 'ratsnest' command to get it to fill. You could add a copper pour to  layer 16 as well - why not keep as much of the copper on the board as possible.

You should do a "design rule check". The default parameters are probably OK but you can change them first to match your PCB house's specs.

There area number of places where there is extremely little clearance between traces, at the same time that there is ample space nearby.  The traces near the three bourns pots are a good example - these traces should not be right at the design rule minimum - spread it out!

There's a via near the leftmost e-switch that is extremely close to the pads for the switch. You need to have clearance around drill holes, and the pads cannot be that close together either. You can easily move some traces around and sort that out.

The library parts for your polarized electrolytic caps should have a square pad for the positive pin and round for the other. The little "+" in the silkscreen is great, until it flakes off or gets removed during re-work. The general tradition is to use a square pad for pin 1 and a round pad for all other pins - this will also help you with the 8 and 14 pin DIP ICs. For surface mount, the tradition is to put some sort of line or mark near pin 1, since the pads have to be a specific shape for soldering reasons. So, sometimes you need to rely on the silkscreen legends, but with through-hole , you can alter the pad shape without causing problems.

To fix that, you can edit the part in the library, save the library, then do a library 'update all' command. These components are stored in your PCB file, so changing the library won't affect a placed part unless you run the 'update' command.
 
Great work!  :) How are you getting along with this build? Everything working OK?

I'm very interested in some boards. Could you please let me know how much 16 PCBs will be?

All the best,
Leigh
 
Well, I'm actually making progress, so it's gonna be allright.
I hope the pcb's will be ready around the end of april at last.
I'm not sure if i want to sell them, but i can just order some more of my own run for you. Price won't be high, i guess €20 max per pcb.

Kind regards,

Wouter
 
good call, Monte McGuire

Wouter,

It's very hard from outside to check other peoples work without knowing all their exact design parameters. Like mechanics. Budget. Availability of parts. Preferred mounting methods etc etc

..and note that perfect prototype pcb's does not exist outside of one's mind. At least I have never managed to get it right in first shot. It's all about doing your best, make the pcb (or have it made), build it to find the problems, then revise and make a new board. After a couple of revisions it'll get quite good, but trust me: You'll ALWAYS find an annoying detail when you commit and have 100 PCB's made...

Yes DRC's, netlists, simulation and automatic integrity checks makes the job faster and somewhat easier - I have just last year upgraded my 27 years old (!) PCB drawing software package to get these functions - but it's still limited to help prevent only certain categories of error. While generating others..

Jakob E.
 
If all stages are unity gain you need to change the THAT1240 to a 1246  to get unity gain through your unit.
Also think you should remove the R48 as the THAT1646 need as low source impedance as possible.
 
I'm coming a little late at the party, but I think you need at least one pair of electrolytic caps on the power rails, like 100 or 220uF.
I don't know why you favored the TL074's, maybe in order to make it period-accurate, but I don't like quads generally. Duals offer much more flexibility for opamp-rolling.
OPA 4134 could offer better THD/headroom performance, but not as much improvement in terms of noise as some bipolars.
Ideally, I would have used duals and a combination of OPA2134's and 5532's.
 
abbey road d enfer said:
I'm coming a little late at the party, but I think you need at least one pair of electrolytic caps on the power rails, like 100 or 220uF.
I don't know why you favored the TL074's, maybe in order to make it period-accurate, but I don't like quads generally. Duals offer much more flexibility for opamp-rolling.
OPA 4134 could offer better THD/headroom performance, but not as much improvement in terms of noise as some bipolars.
Ideally, I would have used duals and a combination of OPA2134's and 5532's.

I agree with you, but imho, TL074 is cheaper, easy to get, and very unlikely to be a counterfeit/fake, especially if not sourcing the OPA2134 from respectable vendors such as DigiKey-Mouser-etc.
 
metalb00b00 said:
I agree with you, but imho, TL074 is cheaper, easy to get, and very unlikely to be a counterfeit/fake, especially if not sourcing the OPA2134 from respectable vendors such as DigiKey-Mouser-etc.
Agreed, TL074 is dirt-cheap, but OPA2134 is available at less than $4 from reputable vendors such as Farnell, Mouser, DigiKey... Now, it can be justified only by a desire to improve measurable performance over the genuine period-correct article.
 
Wlinart,
If you were going to post a schematic or board design directly from a piece of design software, I can't think of a better program than Eagle. Aside from being free, it has a decent following in the DIY community and is a good choice for low frequency, 2 layer boards.
However I'm not really qualified to  error check.  ;)
Just giving you a thumbs up and my 2 cents,  since I read you caught a little flack for it. :)
-Boji
 
Back
Top