Ok, thanks. I should increase this to at least 0.4mm.
But just to understand it: Do you worry about PCB production (short curcuit) or about capacitive coupling of them?
The latter should be a positive effect in my eyes, as differential mode distortions in power lines are reduced. (Single side distortions are divided into common mode distortions, not being reduced by this effect and differential mode distortions.)
Please correct me if I'm wrong or I miss something.
It looks really fine to me.
For manufacturing reasons*, I'd be a bit more careful with the vias however. They seem very close to some power tracks. No problems when they belong to that track but they could lead to shorts when they're close to another track.
*I've found that drills wandering around by a few mils isn't that uncommon with cheap pcb manufacturers.
For manufacturing reasons*, I'd be a bit more careful with the vias however. They seem very close to some power tracks. No problems when they belong to that track but they could lead to shorts when they're close to another track.
*I've found that drills wandering around by a few mils isn't that uncommon with cheap pcb manufacturers.
Alright, this is nearly unchanged but all via clearances set to at least 0.4mm.
Would you suggest to get it manufactured at its current state?
Would you suggest to get it manufactured at its current state?
An externally hosted image should be here but it was not working when we last tested it.
Good luck with the project, planning the enclosure will be the real battle
I'm looking forward to it
Before that I wanted to finish the interface PCB (stacked on top of the main amp PCB).
This is what it looks like atm:
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
The interfacing consists of a volume pot, an internal dip switch for volume pre attenuation and 3 signal LEDs per channel: -10dBu (signal present) and +16dBu (clipping) for the input stage and +16dBu (clipping and ear damage warning) for the output stage.
My main focus was to achieve minimal coupling of the volume attenuation curcuits and the signal indication curcuits (for minimal distortion of the signal) and to minimize power supply pollution.
Design targets of the signal LED were:
- Well defined on/off level for clear level indication (steep on/off switching flank)
- Minimal power supply line pollution. Achievable through soft switching or rare switching - headed for the latter:
- Minimal switching frequency - even if the signal level is very near on/off switching point
- RMS weighting of the signal (didn't get this, implemented average weighting instead)
Design targets of the peak LED were:
- Well defined on/off level with steep on/off switching flanks
- Peak weighting of the signal
- fast on switching, slow off switching
- didn't bother about power line pollution as the signal most likely gets more distortion in the amp than through power line pollution
What do you think about it?
Just to mention it before: My concerns are mostly the SQ. Every comments and advice is welcome, but I'm most interessted in possible traps regarding SQ.
Thanks!
Looks to me your concerns about power supply purity are an appropriate area of attention.
A couple of things - you've included no series impedance on the supply rails to the opamps. So there's a possibility that noise will couple along the common supply wires between the boards.
You have bipolar transistors being driven from opamps with bipolar supply rails. This means those transistors are going to get reverse biassed B-E junctions when switched off. Since the opamp supplies are 15V they're likely going to go into zener breakdown - this isn't recommended. Either fit a diode across the B-E junction to prevent this or switch the bipolars to MOSFETs. The latter choice has benefits that the current draw from the opamps can be reduced to zero at DC, at AC it'll be determined by the FET's capacitances. So choose FETs with low capacitance. 2N7002 is fine for the N-channel slots, its also dirt-cheap. Infineon has some likely suitable P-channel parts but P-chans are always going to be more expensive.
<edit> On reviewing the schematic once again I see you've only got NPN transistors driven by the TL074s. So no P-channel FETs are called for.
A couple of things - you've included no series impedance on the supply rails to the opamps. So there's a possibility that noise will couple along the common supply wires between the boards.
You have bipolar transistors being driven from opamps with bipolar supply rails. This means those transistors are going to get reverse biassed B-E junctions when switched off. Since the opamp supplies are 15V they're likely going to go into zener breakdown - this isn't recommended. Either fit a diode across the B-E junction to prevent this or switch the bipolars to MOSFETs. The latter choice has benefits that the current draw from the opamps can be reduced to zero at DC, at AC it'll be determined by the FET's capacitances. So choose FETs with low capacitance. 2N7002 is fine for the N-channel slots, its also dirt-cheap. Infineon has some likely suitable P-channel parts but P-chans are always going to be more expensive.
<edit> On reviewing the schematic once again I see you've only got NPN transistors driven by the TL074s. So no P-channel FETs are called for.
Last edited:
What exactly do you suggest? Maybe I could add a 10R resistor in every rail directly after branching from the main power line (max current draw is below 10mA per rail, >90% of this is just bias current).
My simulations show that due to the low pass filtering of the switching singal below every accoustic signal (3Hz first cut off, the second in low accoustic range) this current is mostly DC.
At an input level where the signal LED switches on (about -13.7dBV atm, about 0.6Vpp) the current drawn is about -126dBA@fundamental, -132dBA@1st harmonic, -154dBA@2nd harmonic (nearly independent of frequency) - and about the same values of power supply pollution in dBV for 1ohm source resistance.
For an input level of about 11dBV (10Vpp - a high level, but below peak warning) the pollution level relative to signal level at first harmonic raises to about 95dB (again at 1 ohm source impedance), the second harmonic stays at about 120dB suppression.
Would you trust these simulation results?
An interessting alternative. I think I could cut down the DC current draw a bit. However zener breakdown shouldn't be an issue due to the voltage divider, where there shouldn't be much more than +-1V on B-E, which shouldn't affect the transistor, especially as there is moderate C-E bias voltage about 11V.
Yet there is one downside of an FET due to technology: For npn I have a very well defined switch on point of the transistor. For FETs, there is a large spread of the Vth, so I maybe have to pre-select the transistors before assembly to achieve a reliable switch on point, which again isn't an issue at about 3€ I would have to pay for 100 of them.
Last edited:
I suggest include a pair of series Rs, value somewhere between 2.2 and 10R. You could determine the noise levels empirically rather than rely on simulation.
A voltage divider from the opamp output would need to be in excess of 50% reduction to ensure no zenering of your transistors. Looking at the schematic only T3 has such a divider, the other two are considerably below 50% reduction.
I agree about the spread of threshold voltage, its a significant drawback for FETs. 3 euro cents each sounds like you're being over-charged. Here the going rate on Taobao is around $16 for a reel (3k) so ~200 per USD.
A voltage divider from the opamp output would need to be in excess of 50% reduction to ensure no zenering of your transistors. Looking at the schematic only T3 has such a divider, the other two are considerably below 50% reduction.
I agree about the spread of threshold voltage, its a significant drawback for FETs. 3 euro cents each sounds like you're being over-charged. Here the going rate on Taobao is around $16 for a reel (3k) so ~200 per USD.
Alright, sounds good. I'll fit them in and update the post.
Oops, sry, my mistake. The schematics around T9 are wrong. It should be the same curcuitry as around T3. So 220k series to B and 22k parallel to B-E.
<edit>Regarding T5, there is only positive voltage applied, as it gets (half-wave) rectified by D3, R34 and low pass filterred by the SK low pass filter.</edit>
Oh ok. Do you know some cheap distributors for Europe? I regularly use Digikey, Mouser and Farnell, but all of them charge between 2 and 3 ct per unit, even if ordering a whole reel (3k).
Last edited:
Now that you have considerable attenuation, the need for FETs disappears.
The issue of component prices in Europe (and US) is an interesting one. I ran up against this problem when employed as a designer in UK and ended up sourcing some high value items for my design through a contact in Taiwan as I couldn't get reasonable prices through any distributor. So the answer to your question is 'no, I know of no cheap distributor in Europe' (I suspect there's something of a cartel in operation)- if you're interested in purchasing significant quantities of parts I could put you in contact with someone locally who might be able to help you. PM me.
The issue of component prices in Europe (and US) is an interesting one. I ran up against this problem when employed as a designer in UK and ended up sourcing some high value items for my design through a contact in Taiwan as I couldn't get reasonable prices through any distributor. So the answer to your question is 'no, I know of no cheap distributor in Europe' (I suspect there's something of a cartel in operation)- if you're interested in purchasing significant quantities of parts I could put you in contact with someone locally who might be able to help you. PM me.
Ah, good, then I will stick with the bipolar ones, which simplifies assembly. (No need for measuring and selection.)
Good to know I didn't miss something until now. It would have been annoying having paid too much, if there was some simple alternative.
Thanks for your offer. I may take you up on that later. As I'm not yet professionally enganged in this business (only student yet), I only order for private needs atm and I don't think these are "significant quantities"
. But I'll contact you, when this changes.
Mouser and Digikey are mostly reasonable in prices if you don't order in huge quantities. Farnell and RS are usually overpriced.
What you pay extra to the big distributors is the fast shipping, the clear indications of inventory and the guarantee of genuine parts. As an individual, it's very difficult to assess the reliability of Chinese distributors and I would avoid them as a rule. It's different if you're a business able to do quality tests in house.
In Europe, Reichelt.de has reasonable prices for small quantities. But you have to be careful: if the brand of the part isn't specified, it's probably not coming from the main manufacturers but from something like CDIL.
What you pay extra to the big distributors is the fast shipping, the clear indications of inventory and the guarantee of genuine parts. As an individual, it's very difficult to assess the reliability of Chinese distributors and I would avoid them as a rule. It's different if you're a business able to do quality tests in house.
In Europe, Reichelt.de has reasonable prices for small quantities. But you have to be careful: if the brand of the part isn't specified, it's probably not coming from the main manufacturers but from something like CDIL.
So, version 2 of the Interface PCB is ready:
What do you think? Do you see any relevant flaws?
<edit>
Changes are:
- decoupled local power rail from common power rails by 10R resistors
- added input resistors for sound signals to "deactivate" signal detection by just removing these resistors + power decoupling resistors
- inserted slicing of ground plane to improve seperation of common ground currents (running through every PCB) and local ground currents
</edit>
@00940:
As a german company I also knew Reichelt. I prefer it for small quantities where I don't have any particular quality demands. Beside that, high quality electrolytical caps and pin header are very cheap there.
Regarding Farnell I noticed that for some products they have even lower prices than Digikey or Mouser. Especially the standard parts (resistors, caps, the 220uH inductor, common active devices like BC847 or TL072) were less expensive at Farnell in my comparance.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
What do you think? Do you see any relevant flaws?
<edit>
Changes are:
- decoupled local power rail from common power rails by 10R resistors
- added input resistors for sound signals to "deactivate" signal detection by just removing these resistors + power decoupling resistors
- inserted slicing of ground plane to improve seperation of common ground currents (running through every PCB) and local ground currents
</edit>
@00940:
As a german company I also knew Reichelt. I prefer it for small quantities where I don't have any particular quality demands. Beside that, high quality electrolytical caps and pin header are very cheap there.
Regarding Farnell I noticed that for some products they have even lower prices than Digikey or Mouser. Especially the standard parts (resistors, caps, the 220uH inductor, common active devices like BC847 or TL072) were less expensive at Farnell in my comparance.
Last edited:
Hi tobias32,
First of all I am not a professional PCB designer but I see a couple of possible problems with your layout. First you have a ground plane cut under the signal trace below the potentiometer (upper left corner of your PCB).
The -15V power trace to the left of R61 on the PCB does not have ground plane below. Also instead of making so many cuts into the ground plane by traces diving from one layer to the other and then back again I would use wire jumpers. I understand that this board is not so critical as it is mostly not in the signal path but still.
Also, series resistors R60 and R61 should probably be before the bulk capacitors C3, C8 but not after them. And you probably do not need R59 because the reg does the power supply isolation. May be I do not understand the design idea but I guess R60 and R61 are there to isolate the local power supply from the power rails shared between many of your boards.
To make a layout a bit nicer around the R10,C8,C4 you could shift the R10 below the C8 and C4 and then all caps will align nicely along the power connector. If you wish to gain a couple of mm of space you can solder R10 from below.
If you plan to daisy chain the boards using angled pin-headers/sockets I would advise to check distances. Usually you would need around 12 mm or more from the center of the pin-header through holes to the center of the socket through holes. In Eagle CAD you can easily add the socket and see how it fits together.
Just my two cents.
Regards,
Oleg
First of all I am not a professional PCB designer but I see a couple of possible problems with your layout. First you have a ground plane cut under the signal trace below the potentiometer (upper left corner of your PCB).
The -15V power trace to the left of R61 on the PCB does not have ground plane below. Also instead of making so many cuts into the ground plane by traces diving from one layer to the other and then back again I would use wire jumpers. I understand that this board is not so critical as it is mostly not in the signal path but still.
Also, series resistors R60 and R61 should probably be before the bulk capacitors C3, C8 but not after them. And you probably do not need R59 because the reg does the power supply isolation. May be I do not understand the design idea but I guess R60 and R61 are there to isolate the local power supply from the power rails shared between many of your boards.
To make a layout a bit nicer around the R10,C8,C4 you could shift the R10 below the C8 and C4 and then all caps will align nicely along the power connector. If you wish to gain a couple of mm of space you can solder R10 from below.
If you plan to daisy chain the boards using angled pin-headers/sockets I would advise to check distances. Usually you would need around 12 mm or more from the center of the pin-header through holes to the center of the socket through holes. In Eagle CAD you can easily add the socket and see how it fits together.
Just my two cents.
Regards,
Oleg
How severe do you see this problem?
(Concerning both: The -15V track and the track at the pot crossing the GND section.)
I just thought: It's not an RF layout. Surely it's always the best to keep the area of the current loop as small as possible. But isn't it good practice, too, to use wires or simple tracks for GND in audio layouts? Shouldn't any GND plane perform better than that? (Especially if only connecting two points as under the pot.)
Concerning the track to the pot: I know it's a bit of a mess of GND planes here, but I get two GND signals from two different areas of the amp board. I want to use both - each GND signal for the appropriate channel - to avoid coupling of induced signals into the signal chain.
But I also don't want to simply connect both planes as it would result in a GND loop - always very dangerous.
I could just place two tracks to connect the pot GND and pin header GND, but isn't a whole plane covering only some parts of the signal track performing better?
If you know a solution to this dilemma I would be happy to know it
Oh, you're absolutely right. They are completely useless in this configuration
(at least in audio frequency range). My thoughts were to avoid the inrush currents to the caps as it extremely increases the currents I have to layout the resistors for. But that's how I corrupted the intent, too.Right. But by reworking the decoupling I think some more things will change in this board region. Placing some THDs to the bottom will be necessairy in more cases.
A good thought, too. I will check and if it fails, switch to straight headers (mounted on the bottom) in component assembly.
Thank you very much to occupy yourself with my project
Many helpful thoughts.If you like, I would be happy to hear your thoughts about my questions, too.
Hi,
I am probably not more skilled than you So be careful with what I suggest.
Concerning both, the -15V track and the track at the pot crossing the GND section:
While the -15V supply may not be so critical as it is now, the cut under the signal trace around the pot does look pretty bad to me. Just think for a moment how the signal return should go in the current configuration?
As for the power supply traces (+ and -15V as well as +12V) to the left of R61, they can go to the underside of the board. This would allow you to lift to the top layer the LEDs control traces and would remove some via. You can also turn LED4 and LED2 to align with the other LEDs. It would not only help routing their control/supply traces on the top layer but will also prevent you from soldering them wrongly - one orientation is always easier to get right...
If you plan to hand solder the boards you may have problems accessing some SMD pads due to tight spaces. Just print the board in its true dimensions and place a couple of resistors/capacitors where they have to be soldered. Now try fit the tip of your soldering iron as if you would solder them... Reflow soldering on the other hand should be fine.
Regards,
Oleg
I am probably not more skilled than you
So be careful with what I suggest.Concerning both, the -15V track and the track at the pot crossing the GND section:
While the -15V supply may not be so critical as it is now, the cut under the signal trace around the pot does look pretty bad to me. Just think for a moment how the signal return should go in the current configuration?
As for the power supply traces (+ and -15V as well as +12V) to the left of R61, they can go to the underside of the board. This would allow you to lift to the top layer the LEDs control traces and would remove some via. You can also turn LED4 and LED2 to align with the other LEDs. It would not only help routing their control/supply traces on the top layer but will also prevent you from soldering them wrongly - one orientation is always easier to get right...
If you plan to hand solder the boards you may have problems accessing some SMD pads due to tight spaces. Just print the board in its true dimensions and place a couple of resistors/capacitors where they have to be soldered. Now try fit the tip of your soldering iron as if you would solder them... Reflow soldering on the other hand should be fine.
Regards,
Oleg
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.