LM3886 component selection - Page 4 - diyAudio
Go Back   Home > Forums > Amplifiers > Chip Amps

Chip Amps Amplifiers based on integrated circuits

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 17th December 2012, 11:11 PM   #31
diyAudio Member
 
Join Date: Nov 2012
Location: Bavaria
Quote:
Originally Posted by gootee View Post
You can estimate the cap inductance pretty well by using 1 nH per mm, times the lead-spacing in mm. And you can estimate the self-inductance of a trace or wire with the same figure, for now.
Thanks, that was exactly the information that was missing in the datasheets!
As I said, I didn't find any suitable information about inductance, so I just calculated the values I could (ripple current, impedance, ESR).
But now I can clearly see that inductance will be much lower.

Here are the inductance values (just for the leads, traces are omitted here):
56F has a 2.5mm pitch, so lead inductance will be about 2.5nH.
With 4 of them, that results in 0.625nH.
220F and 820F both have 5.0mm pitch, which results in 5.0nH.
So the parallel version is by factor 8 lower than a single cap with same capacitance, quite impressive.

Then I think I'll go with the paralleled version.
May I - or should I even - then omit the small foil bypass caps at the chip's supply pins, and still maintain optimal performance?

Quote:
Originally Posted by gootee View Post
You could chop off the part of your PCB with the big caps and replace it with a separate 1mm-thick 2-sided PCB, maybe 48 x 48 mm. Keep one side solid copper, for ground. Divide the other side in two, by removing copper to from one slot along the diagonal. DON'T make any traces or remove any other copper, except as described. Lay out positions for 15 8 mm caps on each half (rows with 5, 4, 3, 2, and 1 cap). Drill one hole per cap, for the lead that goes to the bottom side. Remove a little copper from around each hole, on the top side. Bend the top-side lead flat against the copper and solder. One end of the diagonal "slot" will go near the chip. Connect the power pins' traces from there, with something thick or wide. Connect the rails from the PSU to the opposite corners, at the other end of the diagonal slot.
I'll try to implement a configuration like you described.

I have just made a new version of the rectifier board.
Both versions are equipped with dual rectifiers with 16K/W heatsinks per diode, bleeding resistors and space for diode snubber RC.
They have 2 outputs per rail (for stereo usage), and a third GND terminal for safety ground connection (via safety loop breaker).

My original version used a single 10,000F capacitor per rail and provided space for a small film bypass cap.
(power planes have not been drawn, layout just for size estimation)

The new version uses 12x 820F per rail and power planes on both sides.

Please ignore the thin lines around traces and pads, they are just clearance marks in KiCad.
Attached Images
File Type: png PSU_Rev2.png (93.2 KB, 274 views)
File Type: png PSU_Rev3.png (114.2 KB, 274 views)
  Reply With Quote
Old 17th December 2012, 11:45 PM   #32
Reality first!
diyAudio Member
 
ClaveFremen's Avatar
 
Join Date: May 2005
Location: Milan, Italy
I've made for you a PS only version of my board to illustrate some concepts:

Click the image to open in full size.

  • keep diodes traces as simple as possible, try to avoid overlaps
  • after smoothing caps try to keep V+ and V- traces paired on the ground plane, it will have an effect similar to twisting cables
  • power traces on the groundplane have constant impedance if they mantain their width constant
  • power traces on a groundplane will have a greatly reduced inductance (circa 40% less)
  • When using groundplanes take in account current returns, HF current will follow power traces, LF will seek the least impedance path.
  • Avoid slots in groundplanes, particularly on the current return path
  • Sometime, though, slots are useful to isolate sections of the groundplane (see the small slots on the smoothing caps to sepate diode's plane from the general one)
  • when routing traces avoid 90 angles, they will cause impedance changes and reflections that can possibly smear the signal.
two additional notes:
  • it's unlikely that those diodes will ever need an heatsink...
  • do not remove the bypass caps on V+ and V-, use R2R bypassing if you want.
Attached Images
File Type: jpg My_Ref_FE RC - PCB.jpg (214.7 KB, 608 views)
__________________
Dario
ClaveFremen "Bailando Salsa en el Sietch"
  Reply With Quote
Old 18th December 2012, 01:33 AM   #33
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Yes, I agree. Do not remove the small bypass caps. Could allow high-frequency instability.

SirPA,

Now you are getting the idea!

But the best performance should come from the easiest-possible layout: NO traces. One board for one power rail. Double-sided PCB. One side power and one side ground. All you need is a drill.

Or, I suppose you could use one board with one side ground plane and the other side could be split into two (+ and -) power planes.

ClaveFremen is right about not having a large gap between the + and - power rails, too. Enclosed loop area = antenna.

What you are doing is almost identical to what is described in the second half of post $1214, here: Power Supply Resevoir Size

And here is some VERY good news about a similar setup: Power Supply Resevoir Size
(like, you could get about 1 nH or TOTAL inductance, for ALL of the caps AND their "wiring"!)

And here are some construction secrets: Power Supply Resevoir Size

And here's much of the real story, probably about $20000 of consulting, all in one free post: Power Supply Resevoir Size\

It basically started here, which also has some key points: Power Supply Resevoir Size

It seems to me that we should simply use two capacitor arrays to connect the rectifiers to the chipamp power pins. (At that point, THEN you can remove the small bypass caps. <grin>)

Cheers,

Tom

Last edited by gootee; 18th December 2012 at 01:47 AM.
  Reply With Quote
Old 19th December 2012, 04:48 PM   #34
diyAudio Member
 
Join Date: Nov 2012
Location: Bavaria
Quote:
Originally Posted by ClaveFremen View Post
I've made for you a PS only version of my board to illustrate some concepts:
  • keep diodes traces as simple as possible, try to avoid overlaps
  • after smoothing caps try to keep V+ and V- traces paired on the ground plane, it will have an effect similar to twisting cables
  • power traces on the groundplane have constant impedance if they mantain their width constant
  • power traces on a groundplane will have a greatly reduced inductance (circa 40% less)
  • When using groundplanes take in account current returns, HF current will follow power traces, LF will seek the least impedance path.
  • Avoid slots in groundplanes, particularly on the current return path
  • Sometime, though, slots are useful to isolate sections of the groundplane (see the small slots on the smoothing caps to sepate diode's plane from the general one)
  • when routing traces avoid 90 angles, they will cause impedance changes and reflections that can possibly smear the signal.
two additional notes:
  • it's unlikely that those diodes will ever need an heatsink...
  • do not remove the bypass caps on V+ and V-, use R2R bypassing if you want.
Thanks!
I will try to implement that, as far as I haven't done yet, and where ever possible.

Regarding the diode heatsinks: The datasheet states that above ca. 3.5A, a heatsink is required.
For getting 60W@4 Ohm loudspeaker output power, a current of about 3.9A will flow. And for 2*20W@4 Ohm, even 4.8A.
I know the average power consumption will be quite less, but you never know.
So I thought it would be wise to include at least the option of a heatsink.

How warm do your diodes get, when you hear music a little louder?

Regarding the diode traces: Thanks for the hint, I've overlooked that! I could reduce it to exactly one crossing at 90, if I swap the pins at the input terminals.

Quote:
Originally Posted by gootee View Post
Yes, I agree. Do not remove the small bypass caps. Could allow high-frequency instability.
...
And here is some VERY good news about a similar setup: Power Supply Resevoir Size
(like, you could get about 1 nH or TOTAL inductance, for ALL of the caps AND their "wiring"!)
Because of that, I thought of omitting the 100nF film caps at the chip's power input pins, I thought they could perhaps even provide the possibility of HF instability.
But I will leave them in place.

Quote:
Originally Posted by gootee View Post
Now you are getting the idea!

But the best performance should come from the easiest-possible layout: NO traces. One board for one power rail. Double-sided PCB. One side power and one side ground. All you need is a drill.

Or, I suppose you could use one board with one side ground plane and the other side could be split into two (+ and -) power planes.

It seems to me that we should simply use two capacitor arrays to connect the rectifiers to the chipamp power pins. (At that point, THEN you can remove the small bypass caps. <grin>)
Sure, this would be the absolute optimum.
But, as far as I could follow the "Power supply reservoir size" thread, it was referred to discrete power amps, with power stages consisting of perhaps multiple paralleled output transistors.
Connecting that to a massive cap array will be much simpler than a single (and comparatively small) all-in-one chip.
Because the other parts have to be connected to the chip in an optimal way, too.

Quote:
Originally Posted by gootee View Post
What you are doing is almost identical to what is described in the second half of post $1214, here: Power Supply Resevoir Size
Exactly from that post I took the inspiration for the PS board, although my approach isn't as good.

Quote:
Originally Posted by gootee View Post
And here's much of the real story, probably about $20000 of consulting, all in one free post: Power Supply Resevoir Size
In that post, there is a lot interesting about SMT caps.
And, if I get it right, it would be the best to use the smallest case size possible to not ruin all efforts made so far.

But film caps are only available in 1210 case or bigger.
So wouldn't it be better to use a X7R ceramic in 0603 instead of film?

Quote:
Originally Posted by gootee View Post
ClaveFremen is right about not having a large gap between the + and - power rails, too. Enclosed loop area = antenna.
Hmm, to close the gaps, I would have to use Faston tabs for the transformer connections.
But somehow I don't quite like these, because of the tension stress for the PCB.
A few years ago I have seen Faston tabs with a molded plastic support base, to provide a bigger contact surface for the PCB.
That would have been ideal, but unfortunately I don't find them anymore...

Regards, Stefan
  Reply With Quote
Old 19th December 2012, 10:38 PM   #35
Reality first!
diyAudio Member
 
ClaveFremen's Avatar
 
Join Date: May 2005
Location: Milan, Italy
Quote:
Originally Posted by SirPlanALot View Post
Thanks!
I will try to implement that, as far as I haven't done yet, and where ever possible.
You're welcome, Stefan.

Quote:
Originally Posted by SirPlanALot View Post
Regarding the diode heatsinks: The datasheet states that above ca. 3.5A, a heatsink is required.
(...)
How warm do your diodes get, when you hear music a little louder?
They never get hot to the touch.

BTW the heatsink wouldn't harm.

Quote:
Originally Posted by SirPlanALot View Post
Regarding the diode traces: Thanks for the hint, I've overlooked that! I could reduce it to exactly one crossing at 90, if I swap the pins at the input terminals.


Quote:
Originally Posted by SirPlanALot View Post
Hmm, to close the gaps, I would have to use Faston tabs for the transformer connections.
???

BTW the fastons I use are solidly bonded to the PCB (better if soldered on both sides) and are mechanically really strong...
__________________
Dario
ClaveFremen "Bailando Salsa en el Sietch"
  Reply With Quote
Old 20th December 2012, 03:33 AM   #36
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by SirPlanALot View Post
Thanks!
I will try to implement that, as far as I haven't done yet, and where ever possible.

Regarding the diode heatsinks: The datasheet states that above ca. 3.5A, a heatsink is required.
For getting 60W@4 Ohm loudspeaker output power, a current of about 3.9A will flow. And for 2*20W@4 Ohm, even 4.8A.
I know the average power consumption will be quite less, but you never know.
So I thought it would be wise to include at least the option of a heatsink.

How warm do your diodes get, when you hear music a little louder?

Regarding the diode traces: Thanks for the hint, I've overlooked that! I could reduce it to exactly one crossing at 90, if I swap the pins at the input terminals.


Because of that, I thought of omitting the 100nF film caps at the chip's power input pins, I thought they could perhaps even provide the possibility of HF instability.
But I will leave them in place.
The film caps actually might cause HF instability, if they happen to resonate with some inconvenient value of inductance, such as that of a large electrolytic. You are correct that X7R ceramic should be safer, there, in that sense. But if you have an oscilloscope, you could try the film caps and just check, under various conditions (square waves might be a good test, for that). The bottom line is that you need to have a low impedance at high frequency, there, between the pin and ground. How you acheive that doesn't matter to the high fequencies themselves.


Quote:
Sure, this would be the absolute optimum.
But, as far as I could follow the "Power supply reservoir size" thread, it was referred to discrete power amps, with power stages consisting of perhaps multiple paralleled output transistors.
Connecting that to a massive cap array will be much simpler than a single (and comparatively small) all-in-one chip.
Because the other parts have to be connected to the chip in an optimal way, too.
Well I didn't say it would be trivial to figure out how to make it optimal. <smile>

And I haven't found a "perfect" way to do it yet, either. But here are some more spur-of-the-moment thoughts about possible methods and configurations:

The dual-triangular-arrays idea (which was just off the top of my head at the time) "might" work OK, since it gets two of the corners of the two triangles to end up near the same place that your original layout had the power traces going to the chip.

OR, maybe more likely to work well, you could have two rectangular arrays on one board and have them taper down somewhat, as they approach the chipamp area.

But I'm also thinking that maybe a more-three-dimensional solution could be better. Maybe a cap-array board parallel to the amp board. Or maybe two of them, with one above and one below (possibly like a "card cage", or, using standoffs). Then drop some large low-inductance conductors directly to the chip pin areas on the amp board, with power and ground.

You could also consider using card-edge connectors (like the old-fashioned type of PC motherboard card slots), with the card-edge connectors mounted on a "motherboard" PCB that contained ONLY power and ground planes running between the card-edge connectors, in order to run those between the cap-array boards and the chipamp board. You would use multiple connector "fingers" for each plane. i.e. The cap and amp PCBs' edges would have two (cap arrays) or three (amp board) solid copper areas that slid into the connectors and each solid copper edge-area would contact multiple fingers inside the card-edge connector.

I still like the idea of building-up a multi-layer PCB, from single and double-sided PCBs. Imagine not having ANY power or ground traces to worry about, in your layout, but having all of those available everywhere on the board, almost exactly where needed.


Quote:
Exactly from that post I took the inspiration for the PS board, although my approach isn't as good.
It's good. Just remember that there is a big advantage in keeping the planes solid, i.e. unbroken, as much as possible, all the way to the point of load if possible.


Quote:
In that post, there is a lot interesting about SMT caps.
And, if I get it right, it would be the best to use the smallest case size possible to not ruin all efforts made so far.

But film caps are only available in 1210 case or bigger.
So wouldn't it be better to use a X7R ceramic in 0603 instead of film?
The 0603 size should be better than the 1210, in terms of inductance. And that should then be better overall. But if you implement and connect the cap-array planes fairly well, the SMT caps would probably just be like a little extra dab of icing on an already-very-good cake, unless you were doing a digital circuit that had fast edge times. I could be wrong about that, though.

Quote:
Hmm, to close the gaps, I would have to use Faston tabs for the transformer connections.
But somehow I don't quite like these, because of the tension stress for the PCB.
A few years ago I have seen Faston tabs with a molded plastic support base, to provide a bigger contact surface for the PCB.
That would have been ideal, but unfortunately I don't find them anymore...

Regards, Stefan
Eliminating gaps, to minimize enclosed loop area, is extremely important, too. I haven't looked at your transformer configuration so I can't comment on that. But it sounds like ClaveFremen has provided a viable solution for you.
  Reply With Quote
Old 20th December 2012, 06:48 PM   #37
diyAudio Member
 
Join Date: Nov 2012
Location: Bavaria
Quote:
Originally Posted by ClaveFremen View Post
They never get hot to the touch.
Thanks, good to know.
I'll keep the heatsinks as an option.

Quote:
Originally Posted by ClaveFremen View Post
BTW the fastons I use are solidly bonded to the PCB (better if soldered on both sides) and are mechanically really strong...
Ok, maybe my bad experience was, because I used them on a home-etched single side PCB.
On a double side PCB with plated holes they will hopefully be much more robust.
Btw, I just found Faston tabs with bended stabilizers on the top side, I think I will use these.

Quote:
Originally Posted by gootee View Post
The film caps actually might cause HF instability, if they happen to resonate with some inconvenient value of inductance, such as that of a large electrolytic. You are correct that X7R ceramic should be safer, there, in that sense. But if you have an oscilloscope, you could try the film caps and just check, under various conditions (square waves might be a good test, for that). The bottom line is that you need to have a low impedance at high frequency, there, between the pin and ground. How you acheive that doesn't matter to the high fequencies themselves.
Unfortunately I don't have an oscilloscope or other tools that might come in handy (as for example a network analyzer).
So I'll better use a ceramic type here.

Quote:
Originally Posted by gootee View Post
Well I didn't say it would be trivial to figure out how to make it optimal. <smile>

And I haven't found a "perfect" way to do it yet, either. But here are some more spur-of-the-moment thoughts about possible methods and configurations:

The dual-triangular-arrays idea (which was just off the top of my head at the time) "might" work OK, since it gets two of the corners of the two triangles to end up near the same place that your original layout had the power traces going to the chip.

OR, maybe more likely to work well, you could have two rectangular arrays on one board and have them taper down somewhat, as they approach the chipamp area.

But I'm also thinking that maybe a more-three-dimensional solution could be better. Maybe a cap-array board parallel to the amp board. Or maybe two of them, with one above and one below (possibly like a "card cage", or, using standoffs). Then drop some large low-inductance conductors directly to the chip pin areas on the amp board, with power and ground.

You could also consider using card-edge connectors (like the old-fashioned type of PC motherboard card slots), with the card-edge connectors mounted on a "motherboard" PCB that contained ONLY power and ground planes running between the card-edge connectors, in order to run those between the cap-array boards and the chipamp board. You would use multiple connector "fingers" for each plane. i.e. The cap and amp PCBs' edges would have two (cap arrays) or three (amp board) solid copper areas that slid into the connectors and each solid copper edge-area would contact multiple fingers inside the card-edge connector.
I already thought of something similar, using dual row pin strips (multiple pins for each rail) to sit the amp board on top of the rectifier board.

But unfortunately this will only work for mono or dual-mono configurations.
Powering two amp boards from one rectifier board (as intend to use it for small output power) will not be possible, at least it will be far more complicated.

Quote:
Originally Posted by gootee View Post
I still like the idea of building-up a multi-layer PCB, from single and double-sided PCBs. Imagine not having ANY power or ground traces to worry about, in your layout, but having all of those available everywhere on the board, almost exactly where needed.
I have, for earlier projects, already thought of homebrew multilayer PCBs.

But it will be quite complicated.
One would have to use 1x 0.5mm double-sided base material and 2x 0.5mm single-sided base material.
Then one must think of placing all vias in an appropriate place, and how the inner layers can be contacted.
And that will be quite tricky and prone to errors.

One could also think of ordering the 3 PCB parts from a PCB manufacturer and laminate them at home.
But most pooling services only provide standard thickness of 1.6mm, and for the extra cost of the thinner base material there won't be much difference from ordering a 4 layer PCB...

Quote:
Originally Posted by gootee View Post
Eliminating gaps, to minimize enclosed loop area, is extremely important, too. I haven't looked at your transformer configuration so I can't comment on that. But it sounds like ClaveFremen has provided a viable solution for you.
I am just reworking the power supply board to close most of the gaps.

The transformer will be a dual secondary type.
Center-tapped toroids are hardly available, I think because dual secondary is more versatile.

Regards, Stefan
  Reply With Quote
Old 20th December 2012, 10:11 PM   #38
diyAudio Member
 
Join Date: Nov 2012
Location: Bavaria
I've just completed the changes to the power supply layout.

Transformer inputs are now Faston tabs between the diodes, just like ClaveFremen proposed.
And the power planes have been closed, too.

As a nice side effect, the width decreased also by 11mm.

Red is top layer, green is bottom layer.
Attached Images
File Type: png PSU_Rev3_top.png (80.0 KB, 218 views)
File Type: png PSU_Rev3_bot.png (88.6 KB, 75 views)
  Reply With Quote
Old 21st December 2012, 11:24 PM   #39
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by SirPlanALot View Post

<snipped>

I have, for earlier projects, already thought of homebrew multilayer PCBs.

But it will be quite complicated.
One would have to use 1x 0.5mm double-sided base material and 2x 0.5mm single-sided base material.
Then one must think of placing all vias in an appropriate place, and how the inner layers can be contacted.
And that will be quite tricky and prone to errors.

One could also think of ordering the 3 PCB parts from a PCB manufacturer and laminate them at home.
But most pooling services only provide standard thickness of 1.6mm, and for the extra cost of the thinner base material there won't be much difference from ordering a 4 layer PCB...

<snipped>

Regards, Stefan
Stefan,

To get to the inner layers, you could just drill large holes in the other layers, as needed. You could use holes that are something like 5 mm in diameter, or more, so you could solder down inside of them, without having solder touch the in-between layers. With a multi-layer PCB-layout software package, it should be simple-enough to plan and execute such a layout correctly.

But if you were going to have a professional PCB fabricator make boards for you, then you should probably use a "real" mutli-layer layout and PCB.

Cheers,

Tom
  Reply With Quote
Old 1st January 2013, 07:05 AM   #40
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by SirPlanALot View Post
I've just completed the changes to the power supply layout.

Transformer inputs are now Faston tabs between the diodes, just like ClaveFremen proposed.
And the power planes have been closed, too.

As a nice side effect, the width decreased also by 11mm.

Red is top layer, green is bottom layer.
I can hardly wait to hear about the results...
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Help with Tubelab SE component selection OneLiterPeter Tubelab 43 22nd August 2012 05:08 PM
Basic chipamp component selection bcdzt5 Chip Amps 32 12th January 2008 01:05 AM
Component selection for best performance (LM3886). CJ900RR Chip Amps 0 24th February 2006 02:10 PM
Component selection eitanwaks Tubes / Valves 31 4th February 2006 06:27 AM
Need help on speaker design, and component selection BrianGT Multi-Way 5 5th February 2002 03:39 PM


New To Site? Need Help?

All times are GMT. The time now is 04:43 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2