| bill1961 |
This is my first try to make a single side pcb for LM4780.
I'm using the following schematic, (from National website).
[IMG]D:\PCB's\LM4780\schematic.gif[/IMG]
I've got no much experience about pcb making, so please make your comments, post your advise, about my pcb.
[IMG]D:\PCB's\LM4780\pcb.gif[/IMG] |
|
|
| Netlist |
Bill,
welcome.
Instead of trying to post the picture with the IMG button, try inserting the path into the 'Attach file' box.
/Hugo :) |
|
|
| bill1961 |
| OK, this is the schematic |
|
|
| peranders |
| The high current traces are rather thin. If you check the datasheet you can get a picture of how much current you can get. 23 A may occur as short circuit current. |
|
|
| Kevin Haskins |
I don't know from personal experience how critical it is but you will notice that National separated the power & output ground plane from the low level signal input ground plane via a 2.7 Ohm resistor. This may help keep noise out of the input.
Also... lead length & width for the high current traces is important. I'd try and add some width to them from the pins to the two big caps. Also... you may want to add some more capacitance. I see your running it in parallel and 2000uF isn't much. National also suggest 10uF OR bigger for the smaller electrolytic bypass. I've only used 10uF with my board (and it works very well) but I plan to experiment with larger values.
I'm not sure how you plan on mounting this to the heatsink but having the one edge of the PCB flush for easy surface mounting makes life a little easier.
Just for space constraints I left the 1.0uF input cap off the board. The good quality MKP caps are large in relation to the board size and I've always just used leaded caps on the input RCAs if DC blocking was needed. |
|
|
| bill1961 |
| Is it better now? |
|
|
| bill1961 |
| A new version of the schematic to include a 2.7Ohm to seperate signal ground from power ground plane. Also added more cappacitance (2200uF). All, thanks to Kevin's suggestions. |
|
|
| Upupa Epops |
| To signal ground you must connect also shunt resistors from input and feedback resistors - not only ground of input connector :cool: . |
|
|
| bill1961 |
And a newer pcb, according to the schematic changes.
Maybe i need more space for the bigger capacitors, but i'll fix that later. Small board is not my first priority, so i'll leave the 1u capacitor onboard. I also changed the width of some power and ground traces.
Kevin, if it's easy to you, why don't you post your pcb? |
|
|
| bill1961 |
? shunt resistors from input and feedback resistors
Could you be more specific please? |
|
|
| jackinnj |
| the 2.7R resistors should be 2 watt. the 100nF should be polypropylene. |
|
|
| Upupa Epops |
| To signal ground must be connected R3, C7, C8. |
|
|
| Kevin Haskins |
The 2.7 ohm in series with the output needs to be 2-3W but the other 2.7 ohm resistors can be 1/4W. My board is double sided and I use both sides so it won't do you much good.
Using a MKP 100n cap is probably a good suggestion. It doesn't cost much more than a ceramic but does take up more real estate on the board.
Upupa is correct.... you need to have shunt & feedback grounds separate from power ground also. The grounds from your power supply & the speaker output grounds (along with the zobel ground reference) are all I have on the power ground. All other ground references I have to a singal ground point (star ground) and then I connect the two grounds via the 2.7 ohm resistor (1/4W). My amp is dead quite without any noise on even very efficient speakers when the inputs are shorted.
Spend some time studying the National board. That is what I used as a reference. That and I looked over some of the arguements from the members of this forum to optimize my PCB & ground layout.
Thanks guys!
 |
|
|
| Mr Teal |
| One other thing to think of, with the mute and top ground trace where they are, you'll only be able to mount the heatsink if it's resting on the PCB. If you plan to do that it'll work fine, but it might limit your mounting options. |
|
|
| bill1961 |
Many ideas!!!
Working out... |
|
|
| bill1961 |
This is the newer version of my pcb.
So: R3, C7, C8 (shunt and feedback) and pins 12 & 19 (according to National reference board) to signal ground (star ground)
Grounds from power supply & the speaker output grounds (and zobel ground) are all on the power ground.
The two ground planes are separated with the 2.7Omh (1/4W) resistor.
Tolerance of the two feedback resistors is 0.1%.
As for the two 0.1Ohm/3W resistors i have in mind the VISHAY SFERNICE RPL3.
I'm not very proud about the four jumpers, especially those to the Vee and Vcc lines. |
|
|
| Upupa Epops |
| Uncorrect : you must lead ground line beside R7 directly to the geometrical middle between elyts C3 and C4. Beside R7 you can't connect to this line any devices. |
|
|
| Upupa Epops |
| P.S. : And at the same point ( middle between elyts ) you must connect ground terminal for speaker. |
|
|
| Tekko |
| What PCB program are you using ? |
|
|
| soundNERD |
| If I had to guess it looks like eagle |
|
|
| bill1961 |
| You guess right, it is Eagle. |
|
|
| WorkingAtHome |
| Cast thee out jumpers! Though now it has to change anyway... |
|
|
| bill1961 |
But is it better that "loop", or the jumpers?
BTW Upupa i think you mean resistor R13 (2R7). Am i right? |
|
|
| WorkingAtHome |
Fewer solder joint. Also, I typicaly use a ground plane, so that would negate the big looping ground.
-b |
|
|
| bill1961 |
Here again with another version of my pcb.
Trying hard... |
|
|
| Upupa Epops |
| It is much more better, but don't forget " minus " outlet for speaker :cool: . |
|
|
| bill1961 |
Many thanks to Upupa (and all the others of cource) for helping me.
Still having some questions:
1. Capacitor C3 must be closer to LM4780 or it's ok?
2. Input capacitor (1u) must be MKT or better MKP?
3. Is VISHAY SFERNICE RPL3 a good choise for the output resistors?
4. Are lines Vee, Ground and Vcc lines to close one another? |
|
|
| bill1961 |
| Vishay Sfernice RLP3 (this is the correct type) is of wirewound type 0.1Ohm 1% tolerance and has a TCR 50ppm/°C. I saw that the IRC resistror has a TCR 20ppm/°C. Don't know if the difference is critical. |
|
|
| Upupa Epops |
| You have three outlets : Uee, ground and Ucc. These outlets lead to the rectifier and center tape of transformer - it is OK. But you haven't still ground outlet for speaker, which must be between C2 and C3. :cool: |
|
|
| bill1961 |
| So, you suggest another line from the center of C3 - C4 to the speaker ground, and i was wrong planning to connect speaker ground in the middle of R12 - R13. |
|
|
| Upupa Epops |
| If you can have both outlets for speaker close, shift main ground line closer to Uee line and lead new separate ground line for speaker along main ground line and connect both together in geometrical middle between C2 and C3. Only in this case will be hum minimal. |
|
|
| bill1961 |
| You mean something like this: |
|
|
| Upupa Epops |
| It's OK now :cool: . |
|
|
| bill1961 |
or like this one?
I saw that this is the National proposal (on demo board). |
|
|
| WorkingAtHome |
Hi Bill
I don't understand your ground node. Either it doesn't make sense or I need to learn more about it.
Why does it loop around like that and use a jumper? Why not just come off the end of the ground line? And why not just connect to R13 there (rather than jumper to the short lead)? Isn't it (electricly) all the same node?
Nice work btw.
Thanks-
b |
|
|
| WorkingAtHome |
Just saw Upupa Epops post about the hum. Interesting. Need to learn more about this.
Would a ground plane help reduce hum even further?
-b |
|
|
| BrianGT |
| quote: | Originally posted by bill1961
You mean something like this: |
How about something like this?
Also, if you use the smaller resistors (5mm spacing, 3.2mm body length, 0.5w), you can make the feedback paths shorter and the board smaller.
EDIT: looks like you beat me to it, as I was referring to the earlier design..
--
Brian |
|
|
| bill1961 |
I really can't help you (WorkingAtHome).
Just following the suggestions of Upupa Epops.
So, which design do you thing is better? |
|
|
| WorkingAtHome |
BrianGT's last post makes more sense to me, but Upupa was talking about hum and such, so I think there be more that I do not yet understand. Though I would trust BrianGT's suggestions as well.
I guess we need to hear back from Upupa...
-Brian |
|
|
| pinkmouse |
| Just my usual comment; if you move the component designators from under the footprints, it makes debugging later easier. |
|
|
| bill1961 |
Of cource BrianGt has done excellent work in his LM4780 project and his opinion is important.
On the other hand it is difficult to ignore Upupa's suggestions.
Upupa prefers a double star (if i can call it that) ground a signal star and a power star with its center between the two big capacitors. |
|
|
| Upupa Epops |
| To bill : Second version is still better :cool: . To Brian : Your version is way to unstability ( by output current are " modulated " input circuity - you must imagine, that ground line haven't zero resistance ). |
|
|
| BrianGT |
| quote: | Originally posted by Upupa Epops
To bill : Second version is still better :cool: . To Brian : Your version is way to unstability ( by output current are " modulated " input circuity - you must imagine, that ground line haven't zero resistance ). |
I see what you are referring to, and I agree that the input ground path should go from the more central point. Is this better?
--
Brian |
|
|
| WorkingAtHome |
Is this type of consideration unique to chipamps? I don;t mean the general layout theory, just the tendency to instability?
-b |
|
|
| bill1961 |
To Brian: An earlier design was allmost like yours.
To Upupa: what's your opinion? |
|
|
| Upupa Epops |
| I mean, that now all will be quite silent :cool: . This type of grounding is common for all amps : "Star " with separate ground lines, which have center in geometrical middle between supply elyts. If you make it by this mode, SNR will be commonly around 120 dB ( in case of PA ). |
|
|
| soundNERD |
Those speaker traces still look pretty thin
Looks good other than that |
|
|
| bill1961 |
| Keeping in mind all (allmost) the suggestions, here is the latest design. |
|
|
| bill1961 |
| This is the correct pcb!!! |
|
|
| bill1961 |
This is the bottom side of the pcb.
Placement as above. |
|
|
| bill1961 |
Regulated or unregulated psu?
I'm planning to use something like this one (by Carlos Filipe): |
|
|
| Tekko |
| Where can i get eagle or whatever the pcb prog was named ? |
|
|
| bill1961 |
EAGLE Light Edition (freeware) limitations:
* The useable board area is limited to 100 x 80 mm (4 x 3.2 inches).
* Only two signal layers can be used (Top and Bottom).
* The schematic editor can only create one sheet.
http://www.cadsoftusa.com/ |
|
|
| Mr Teal |
| Are you sure the footprint of the 0.1 Ohm resistors is large enough? It looks quite small. |
|
|
| dgaxeman |
| so how is your project going just ordered some 4780 chips. |
|
|
| baskiria |
I'm interested too. How's your project going?
My five chips just arrived, i'm on building your pcb. Thank you for it! |
|
|
| PierreG |
| Is there somebody here who tried this PCB with any success? |
|
|
| bill1961 |
| Didn't have the time to complete the project, so i dont't know if and how it works. |
|
|
| PierreG |
Too bad.
Thanks for the answer bill1961. |
|
|
| gmphadte |
Here is mine. Meant for 2chs and parallel and bridged.
Cut the pcb at appropriate length as required
Gajanan Phadte |
|
|
| PierreG |
Thank you Gajanan.
1- What plan did you use?
2- Do yiu have the silkscreen?
3- Did you made it, and did it work? |
|
|
| builderandy |
Hi Bill, nice pcb work you have done. I'm aware of that it isn't nice to ask for files needed to import the design into Eagle, but I do it anyway. It would spare me a lot of time. If you think I'm rude a nice NO would do. Give me an e-mail if you don't want to answer in the thread.
Regards
/Andy |
|
|
| gmphadte |
PierreG wrote| quote: | Thank you Gajanan.
1- What plan did you use?
2- Do yiu have the silkscreen?
3- Did you made it, and did it work? |
I have modified this from an earlier thread, and there is a thread at
http://www.diyaudio.com/forums/show...&threadid=53526
The one I have shown is improved for all purpose.
What plan... I have no pcb design software on this mac, and the demo eagle does not work on my, one step less OS. It is an artwork on Mac word. So just use it and follow the ways it is done. Read Big PAPAs comment and u will know.
Don't worry, it works, but u have to trace the component location from other post in the earlier thread stated above.
This design is a further modification to accomodate all the three ways...2chs, parallel and bridged.
Gajanan Phadte |
|
|
| bill1961 |
| The schematic and board file. |
|
|
| PierreG |
Thanks Bill.
I tried to open the brd and sch files in your zip file......but it didn't work with eagle.....
These are eagle files right? |
|
|
| builderandy |
Hi Bill, I also have problem to get the files into Eagle. I'm using Eagle 4.13, is it nessesery to use 4.15? Please do another try?
Thanks in advance.
/Andy |
|
|
| bill1961 |
| Sorry, Eagle 4.11 files |
|
|
| PierreG |
| I have 4.16 and it doesn't work. I think you might have to reupload thems. Sorry. |
|
|
| dsmith4021 |
I have a lot of experience with the LM4780 and have found that using the basic reference design circuit from the datasheet works OK, but the amps can oscillate and shut down when driven hard.
You should add the compensation circuitry that is shown in Figure 5 of the datasheet (Special Audio Amplifier Application Circuit, page 7). You will need to add 2 caps and a resistor for each channel. |
|
|
| bill1961 |
| Eagle 4.16 light files. |
|
|
| builderandy |
Thanks Bill
/Andy |
|
|
|
