| LM3886 - P19, Any comment? - Click HERE for Original Thread |
| roly3055 |
| The PCB was made in Eagle 4.13, so if someone wants .pcb file let me know |
|
|
| Nordic |
| care to post the schematic or source? |
|
|
| sek |
Hi,
Just as a sidenote to the topic: Why is it that numerous people use their eCAD software for making boards without starting from the schematic?
It defeats most of the purposes of, e.g., Eagle. You would be quicker with a drawing program like Illustrator - or even Paint - if You consider the learning curve. Some of the features You're really missing:
- abstraction between component functionality and physical package (packages can be exchanged while always maintaining electrical correctness),
- electrical "rule checking" (schematics can be tested for plausibility and corrected independent of board layout),
- physical "rule checking" (board layout can be adjusted independent of electrical schema),
- maintainability (schematic or board can evolve and become improved while never risking errors in other parts of the respective other files),
just to name a few... Besides that, discussing it on a forum would be a lot easier (if we had Your schematic that explicitly matches Your board) as Nordic already said.
Just my two cents, have fun!
Sebastian. ;)
PS: I understand that P19 is ESP's Project 19, a Chipamp that Rod Elliot made a couple of years ago, inspired by Siegfried Linkwitz's excellent amplifier project.
But still, how should we check your board against Rod's schematic. That's what Your computer is for... ;)
edit: PS |
|
|
| jpg |
| quote: | | numerous people use their eCAD software for making boards without starting from the schematic |
Maybe roly3055 does have a schematic and just didn't post a screenshot? |
|
|
| Leolabs |
| quote: | | Why is it that numerous people use their eCAD software for making boards without starting from the schematic? |
Because the schematic is so simple or common. |
|
|
| sek |
It's not about complexity.
My point is: would the original poster have used a schematic in Eagle, his question could narrow down to layout beauty doubts. Electrical correctness is hard to verify on a board by looking at it. Before the question wether the board is good comes the question: Was the well-known schematic applied correctly.
Tools are there to rule out this uncertainty, and they are free and in the hands of the poster. ;) |
|
|
| sek |
Hi roly,
to contribute to your question: Your power rail traces have 'regular' with, which is too narrow in this case. Make them as wide as possible, there's no need to keep a ground plane as far as to the chip.
Eagle has 'faston' connectors (which you seem to try to resemble with jumpers) in the library 'con-rib'. The 6.3mm vertical connector is named 'ST6,3', for example.
Try experimenting with larger filter capacitor packages or wider footprints (e.g. 7.5mm or 10mm), which are also available form many parts suppliers. Also, those caps look a little small for the purpose, but you might of course go with the 1000uF approach. ;)
You also micht want to have a read about snubbed supplies for chipamps (just do a search for snubberized gain clones). You can increase filter capacitance while improving the sound, according to many DIYers.
What does LSP2 do? It might sit in an uncomfortable place. I won't stress that I knew if I had a schematic. :D
Cheers,
Sebastian. |
|
|
| roly3055 |
| The schematic is Elliott Sound P115 |
|
|
| BWRX |
As sek suggested, use fast on tabs or through holes for wire connections. You can make your own, use the ones in the library, or find a nice terminal block footprint. I prefer to have the option to use terminal blocks for power, ground, and speaker connections.
Thicker power and speaker traces would be good (also as sek suggested).
I would suggest moving your volume pot in front of the opamp input buffer along with the coupling cap. This has a number of advantages. Now you can get rid of R6, C1, and C4 and change R9 to a 1kohm resistor. It will allow the low output impedance of the buffer to directly drive the input of the 3886 with better results. It also means you can use a smaller value coupling cap due to the higher input impedance of the buffer. You can now change the layout a bit to make the signal trace much shorter and have a more direct route from IC1 to the 3886 input pin. Also, add a ground connection alongside the +/- supply connections for the buffer supply. |
|
|
| sek |
Allright, LSP2 is signal ground.
You include a buffer and a pot connection with your chip amp. That's not Project 19. Which is why I rumbled in the first place. ;)
Cool idea with the jumpers to set the input stage gain.
You won't need two DC blocking caps around the volume potentiometer, one at the input side of the amp section (as in P19) will be sufficient.
220uF for supply buffering is definitely too little for a 24V supply and 4-16Ohm speakers, except you use separate supply regulation/filters (which P19 requires). Other than that, it works good to have both filter caps at the same side of the chip.
As you have the buffer/preamp onboard, I would recommend a star grounding scheme instead of a ground plane. You have a ground loop around your preamp section, and the copper that connects signal ground to power ground also shares current flow with the poweramp section.
Also, you don't seem to connect the preamp supply's ground onboard - which actually requires another ground star in the supply...
You left out the fuses. That's good as long as you're okay with that and take care of safety in the main power supply.
Increasing your R9 to 3k3 will increase input impedance and thus shift input bias a little. This could result in DC output, but you could give it a try like this and experiment with the value.
Your drawup of the jumpers and connectors looks a little odd! Did you hardwire the TL's supply by hand? Look at Eagle's 'invoke' command, either in the toolbar or as a console command. It lets you place the opamp's power pins independent of the amp symbol. You didn't do that (or at least I can't seem to see it), which is why you had to be creative with the circuitry around J4/J5. :D
Last, not least: I already pointed out the too thin traces for power and the missing scheme for ground. This would impact sound quality and fun the most, everything else I mention is peanuts compared to the power and ground layout and wiring problems you could have.
What project would you like to use it in?
Cheers,
Sebastian.
EDIT: Uh, Oh! I take it back. Brian's suggestion with the pot will influence the sound the most! (He was quicker typing than me ;)) But everything else is still important... |
|
|
| BWRX |
| quote: | Originally posted by sek
220uF for supply buffering is definitely too little for a 24V supply and 4-16Ohm speakers, except you use separate supply regulation/filters (which P19 requires). |
If he plans to use larger bulk filter caps off the board then 220uF on board should be ok. A separate power supply just for the input buffer opamp would be best, but it is possible to make a simple regulated supply off of the higher voltage power supply rails with a handful of components. In the attached schematic in this post check out the components on the far right side. That's just a basic emitter follower with a zener reference that is used to derive the opamp's +/- supply rails from the higher voltage +/- supply rails.
| quote: | Originally posted by sek
As you have the buffer/preamp onboard, I would recommend a star grounding scheme instead of a ground plane. You have a ground loop around your preamp section, and the copper that connects signal ground to power ground also shares current flow with the poweramp section. |
A ground plane is ok if you know where the currents will be flowing. If you don't then a star grounding scheme will force the currents to flow where you want them. If the opamp's rails are derived from the higher voltage supply rails then ground paths should all return to one point. If separate supplies are used then separate ground points may be used as long as they are connected to each other. |
|
|
| sek |
Okay, I start digging it. Finally.
Project 115 is reusing project 19, that's why the pot is in the middle. Rod did this because it's more simple, no other reason (as he writes himself).
It's also using parts of Project 88 for the preamp section.
Roly, there's no need for you to do so, unless you have project 19 and parts of project 88 at hand. :)
Have you had a look into e.g. Carlos' snubberized, buffered amplifier project?
@Brian,
of course I see your points, but all this is assuming a background Roly doesn't give us...
Cheers. |
|
|
| BWRX |
| quote: | Originally posted by sek
of course I see your points, but all this is assuming a background Roly doesn't give us... |
True :) I'm sure he'll give us more details sooner or later. |
|
|
| roly3055 |
Thanks for all your reply's.
They are very usefull.
Here's the updated board |
|
|
| sek |
Many changes applied :)
A couple of things from first glance:
#
Look at the triangle between LSP2, J3 and the LM3886's ground pin. This is a loop. You have two power supplies and one signal cable. All three of them have one ground. All those three ground potentials have to be united somewhere. Currently, amp power ground and signal ground unite in a loop onboard and buffer supply ground is not shown. I'd suggest it would be better to have one star-like scheme where all three of them meet - either off- or onboard. This scheme may well be implemented as a ground plane, but a thin triangle is not a plane...
#
You could jump over the +24V trace with R7 and/or C10 in order to tie them directly to the power ground trace there.
#
After having played with R7/C10, try to move R3 a little lower and J7 to the very right side where the power connection is. This will help R42/C5 to free up this huge board area in the middle of the 'triangle'.
#
Now, move the TL072 a little to the left in order for the power connectors to line up properly at the right edge. Invoke the TL's power pins in order to model the power supply correctly.
#
Replace all jumpers with ST6,3 from 'con-rib'. Introduce another ST6,3 for the buffer supply ground and then another one for speaker return connection. Keep all those 'fast on' connectors 5mm apart, as anything more narrow is unsafe during testing and setup. You can even buy fast on block connectors in that spacing.
Now you're almost done. ;)
BTW, C1 looks a little small (you need between 1uF and 3.3uF; e.g. at least MKS 5.5x7mm or MKP 5x13mm), C2 and C4 look a little large (you can use the same type for C2, C3, C4, C8; e.g. 100nF/63V, 2.5x7.5mm). Also, C7 and C21 could be turned 45 degree by choosing 'rotate', clicking at the part and moving the mouse without releasing the mouse button... ;)
Cheers,
Sebastian. |
|
|
| BWRX |
| quote: | Originally posted by sek
BTW, C1 looks a little small (you need between 1uF and 3.3uF; e.g. at least MKS 5.5x7mm or MKP 5x13mm), C2 and C4 look a little large (you can use the same type for C2, C3, C4, C8; e.g. 100nF/63V, 2.5x7.5mm). |
It's always difficult to do a proper layout when you aren't sure what parts you want to use ;) |
|
|
| juergenk |
the unused amplifier has no connections
literature recommends grounding of in+ and connecting in- to vout
I´ve always done this, so I´ve no experience with leaving the pins open.
maybe this could interfere with your circuit, maybe not
regards |
|
|
| roly3055 |
Ok, another update
thanx everyone again for their help!
Roly
:smash: |
|
|
| sek |
I was thinking of something like this, going even a step further. Especially the connectors and number of ground plugs.
The area right of the 6,3mm plugs could contain the central ground point (where the grounds meet). Also easily forgotten: mounting holes... :D
Just a thought, anyway. How you do it is of course totally up to you.
Cheers. |
|
|
| roly3055 |
The new version, sorry for no comment, my english is basic.
Thank for replys
Cheers.
Roly |
|
|
| roly3055 |
New Changes
Cheers
Roly:smash: |
|
|
| sek |
Cool! :cool:
Now on to some details:
#
The feedback resistor R2 doesn't need to be any bigger than the rest, but it should have a direct, short connection to the chip. Try to give it it's own traces to pins 3 and 9 (independent to R7/R3).
#
The amp has to move left, you have to be able to mount it to a heatsink. Give it at least 1mm overlap over the board edge. Take care of R5, though. ;)
#
The ground copper does reach some of the parts only insufficiently. But sill, the grounding scheme of amp power ground, buffer power ground and signal ground looks difficult.
Normally, you would model this by giving the three grounds three different ground symbol designators from the libraries 'supply1' or 'supply2'. You don't have to. But keep in mind that the currents flowing between power and ground will influence noise and distortion quality of the finished amp. They must not overlap when flowing through the copper!
Look at C6, it only has this tiny little strip above C1 for it's currents to flow to amp power ground. Either try moving C1 a little lower or (better :)) move the copper trace between C1 and R9 up, so that the ground plane is cut underneath C1 and spreads from R9 to C6.
Look at R13, it connects to the same ground as C5 and C6. But it belongs to the buffer, so it refers to the buffer supply ground. Try rotating it 90degree and have it jump over the trace to R6. It then connects to the ground copper at JP1, which is derectly connected to the buffer supply ground. ;)
Look at JP1, it is only connected to it's ground by the little strip above the fast-on connector. Move the upper five ST6,3's down one grid step, that should be okay.
#
The buffer IC2 still has it's second amp IC2B open loop. It's better practice to mute it as Jürgen suggested. It's just one net/copper trace. Try invoking the second amp from IC2 and place it anywhere on the schematic, then give it a net between out and (-) in, then place a ground at it's (+) in. The trace fit's underneath the package of IC2, ground is already there. :)
Also I again recommend to buy C3/C8 in the same size as C2/C4/C10. Easier to buy less types of components and looks better. ;)
Note that if you plan to use anything better than the TL072, you'll have to integrate more parts near it to compensate and decouple.
#
Make the amp power supply and amp output tracks much wider. The ground copper under C7/C21 can be reduced to the same width as the supply tracks. Output can be of same width as amp power. Generally choose as much width as possible, you have plenty of room.
#
I would compact everything to the left, you can then reduce your board size to your original idea (or even smaller). In general, suplly traces should be as short as possible, ground copper should be of same width as supply copper, tracks with high current should be distant to tracks with sensitive signals and hot parts (such as power resistors) should not be close to sensitive parts (such as signal resistors and opamps). ;)
Cheers. |
|
|
| roly3055 |
| New modifications |
|
|
| sek |
Hi Roly,
that's a little too compact. When was you last design rule check (DRC)? ;) |
|
|
| sek |
Hi again,
I received the project via email (upon request) and will fiddle around with it as soon as I find the time. :cool:
But one thing is important: What do you want to use as a power supply?
I'm asking because nothing has been said about the PSUs so far.
The project requires an amp supply of +-20 to +-30V with a 60VA to 150VA trafo and a buffer supply of +-15V with about 5VA to 10VA, depending on what you want to connect and how much power you need.
It's also importand how you want to integrate the PSU with the amp(s) into an enclosure. If you're unsure, please do a search on the forum for gainclone or lm3886 supply or PSU and report back on what you decide to do.
Cheers,
Sebastian. |
|
|
| Nordic |
| Move those dcoupling pins closer to their respective power pins... they are almost useless way out there... |
|
|
| roly3055 |
| I have a toroid 400VA 18-0-18, and 4x 4.700/50V filters. |
|
|
| sek |
You also need rectifiers and voltage regulators for the buffer (it can't use the same supply as the amp).
You can use the same trafo for amplifier and buffer, but not the same PSU output.
Project 115 from ESP contains a suggested PSU. Do you intend to use this? |
|
|
| roly3055 |
| Ok, for the buffer ESP P05 |
|
|
| sek |
The Project 115 PSU already contains a supply connection (+-15V) for the buffer, so you don't absolutely need Project 05 additionally.
OTOH, P05 is of higher quality, but it won't fit on the board and will increase your PCB and parts costs. |
|
|
| roly3055 |
| I already have p05 mount on other board. |
|
|
| sek |
Hi,
okay, I know there are enough GC projects out there, but this one is special.
I have adapted and corrected the schematic. Now I want to know if I did it right. ;)
Please have a look and tell me what can be improved upon.
Constraints:
- schematic initially according to ESP projects 88 (buffer) and 19 (amp),
- split buffer and amplifier supplies,
- low component count due to small board size,
Changes to the former version:
- put documentation field on page,
- changed hole size from 2.8mm to 3.2mm (M3/3mm bolt plus washer diameter),
- replaced TL072 with TL071 (higher quality amps available in this package),
- separated PSU wirings from signal nets; split signal and power ground,
- adapted connector symbols in schematic to ease drawing,
- introduced star ground network with jumper (for optional resistor),
Okay, here goes.
Thanks,
Sebastian.
PS: The board is nearly finished, I just need corrections and critique. :) |
|
|
| juergenk |
if the circuit is still open for debate... :confused:
I won´t do it that way.
routing the naked in+ pin of the opamp to the input connectors is not a good thing. At least there should be a current limiting resistor. Maybe a resistor of reasonnable size is to small to offer good protection, but it gives a better feeling. ;)
This could also be used for impedance matching at jfet-inputs. Jfet opamps are supposed to be sensible to commonmode distortion.
I feel the dc-blocking capacitor is also best at the circuit input and not somewhere in the middle.
Regards
Jürgen |
|
|
| sek |
I wouldn't do it that way, too. ;)
But it's ESP Projects 19 and 88... :cannotbe:
The cap in the middle is there in order to protect the potentiometer contact from corrosion due to DC bias currents.
An alternative option (that was already mentioned above) is to move the pot to the input. |
|
|
| juergenk |
ok, it´s reasonnable to stick with a real world design.
Maybe I was confused by your last schematic.
Regards
Jürgen |
|
|
| sek |
I recently found the time to determine component sizes, parts orientation and signal routing on the board. It came out as 40x45mm small, with the mounting holes and connector description print occupying the 'outer' 5mm. :cool:
Roly, I now need to know what parts are available to you. After all, you (or anyone) should be able to build it... ;)
The following standard parts are to be on the current board:
- low power resistor packages '0204'
- 100nF cap sizes 2.5x5mm, pitch 2.5mm
- C1 value anything between 1uF and 4.7uF, size 7.5x7.5mm, pitch 5mm
- 200uF caps 35V, 8mm diameter, pitch 3.5mm
- 22uF caps 35V, 5mm diameter, pitch 2mm
- output resistor packages '0207' and '0411'
- buffer opamp like TL071, NE5534, OPA134 or OPA627 in package 'DIL8'
Please check your ability to source such parts in case you haven't got them. I need to know what parts you can get, so that the board has enough mounting space for the parts you (or everyone) wants to buy.
I took a picture of a layout print (in actual size) together with most components of the right size. See attachment. :)
Cheers,
Sebastian. |
|
|
| roly3055 |
OK, no poroblem with this parts and the buffer TL071
Cheers.
Roly |
|
|
| sek |
Hi Roly,
hmmm. Good.
I will need a couple of days to resume on the layout, because I'm into work right now.
I attach the current state of development. Parts positioning is done but copper has still to be drawn, 'cause I've been waiting for the reply regarding the components choice.
The autorouter already proves that it fits on a single sided board, but it can use some readjustment and fine tuned layout by hand, which I currently don't have the time for.
Cheers,
Sebastian. |
|
|
| sek |
Finally! ;)
The schematic came out like this: |
|
|
| sek |
| This is the solder side: |
|
|
| sek |
| And that is the component layout: |
|
|
| sek |
If anyone can still make use of this design, please provide some feedback.
I post low-resolution pictures here, but hi-res data is available.
Next step will be prototyping. Anyone? :D
Cheers,
Sebastian. |
|
|
| Russ White |
I have not looked closely, but I would say the electrolytic cap package you used is a bit small. I would make it a bit bigger to allow for more flexibility in cap selection. Around 11mm is pretty good choice.
Cheers!
Russ |
|
|
| sek |
Hi Russ,
the original design is intended for use with separate amplifier PSU and preamplifier PSU.
Roly, the thread starter, said he has both. ;)
Cheers,
Sebastian.
PS: You need +/-15V for the opamp, so you need a separate PSU anyway... |
|
|
| Russ White |
| quote: | Originally posted by sek
Hi Russ,
the original design is intended for use with separate amplifier PSU and preamplifier PSU.
Roly, the thread starter, said he has both. ;)
Cheers,
Sebastian.
PS: You need +/-15V for the opamp, so you need a separate PSU anyway... |
Thats good to know, but I would still offer the same advice. |
|
|
| sek |
Those in the current layout are 8mm devices, i.e. 220uf/35V.
There's room for 11mm caps, but then the film caps would have to go (even farther away from the chip pins). The board shouldn't go larger, and it shouldn't go SMT either.
I thought electrolyte capacitors of higher quality and a set of film caps close to the chip would be superiour to larger bulk caps and no film bypass. Would increasing elco size and moving film caps away be an alternative to try? I just checked a supplier - 220uf/35V caps are available as low ESR type in 10mm cans.
But I honestly think that both ways would sound good and work well with a large-capacitance PSU. ;)
Cheers,
Sebastian. |
|
|
| sek |
Okay, as per Russ' request I did a version for 11mm capacitor devices.
It features 3.5mm and 5mm pitch holes, the 5mm footprint is rotated 45 degree.
This now opens up the possibility to employ any capacitor size and value up to, say, 470uF/35V.
The original recommendation of 220uF/35V as a low ESR type also features 11mm diameter.
Here goes, cheers! |
|
|
| sek |
| The amplifier supply traces (lower portion of the board) actually improved in terms of cross section and solderability. |
|
|
| desert_rainbow |
| The resistor under the LM3886...? |
|
|
| sek |
That's right, some of the resistor are underneath the LM3886.
The IC is elevated about 15mm above PCB level, so the resistors are inbetween it's legs.
Shortens the signal path and helps to optimize the layout.
Cheers,
Sebastian. |
|
|
| BWRX |
| quote: | Originally posted by sek
The IC is elevated about 15mm above PCB level, so the resistors are inbetween it's legs.
Shortens the signal path and helps to optimize the layout. |
Why not just use SMDs? ;) |
|
|
| sek |
That would be boring, as all GC projects before by myself here on diyaudio.com have been SMT, e.g. the two-channel module with included PSU measuring just 100mm x 80mm x 35mm (of which I continuously use two modules since april 2005)... :cannotbe:
No kidding, the project in question is intended for beginners and people who want to try a design that is easy to build. I basically just helped out with a PCB optimization.
After all, this thread is about a simple LM3886 amp, yet with variable preamp/buffer and volume control. It helps to make it as easy to build as possible. ;)
Cheers,
Sebastian. |
|
|
| BWRX |
It would be boring because all of the GC projects before you were SMT? On the contrary, the vast majority have used through hole components. I've only seen a few (including mine) that used SM components.
In all honesty I would have to say surface mount components are easier to solder than through hole components. It's just like soldering through hole components. Once you get the technique down you can do it no problem.
I'm not bashing your board in any way, in fact it looks like a very good single sided layout, if not a bit unconventional elevating the chip up off the board quite a bit to accomodate those large, bulky, through hole resistors ;) |
|
|
| sek |
Hi,
| quote: | Originally posted by BWRX
It would be boring because all of the GC projects before you were SMT? On the contrary, the vast majority have used through hole components. I've only seen a few (including mine) that used SM components. |
Oops, perhaps I wasn't clear. I wrote "GC projects before by myself here". By that I mean that I (myself) only made SMT GC projects before. Of course the vast majority of projects by others aren't. Sorry for the confusion, but I thought the words "by myself" would make it clear in English as they would in my language.
Again, this project is intended to use through-holes parts only - simply because the thread starter asked for assistance in such a project.
| quote: | | I'm not bashing your board in any way, in fact it looks like a very good single sided layout, if not a bit unconventional elevating the chip up off the board quite a bit to accomodate those large, bulky, through hole resistors ;) |
Thanks for the kind words. :cool:
In fact, the through-hole resistors underneath the LM3886 aren't that bulky at all. The parts' size is '0204' with 5mm lead pitch. They have the actual parts body size of 1206 or regular mini-melf SMD resistors (minus the bent solder leads)! That's very small for through-hole parts. They're actually fitting inbetween the IC's pins nicely and comfortably, there's no trick and no cheating in mounting the IC above the resistors. My estimate of 15mm elevation above PCB level was a rough guess on the regular IC placement and does not indicate any special mounting (and maybe it's 10mm, that won't harm the resistors). You'd just have to take a little care with soldering. ;)
A nice technique practiced by many others who want short signal paths is to mount through-hole components from the solder side. This would help everyone out who is in doubt about resistor placement within this project. But you don't have to, trust me. ;)
Cheers,
Sebastian. |
|
|
| sek |
| And just for comparison, here's the current layout (with some minor improvements from the one I posted recently). It's the rough editor's view and has no software optimization applied to e.g. edges, corners and drill holes. |
|
|
|
|
