| BWRX |
| Since everyone seems to be talking about the LM1875 lately, I just came up with a very compact layout for a simple circuit using the LM1875. Attached is the schematic. |
|
|
| BWRX |
Attached is an image of the layout. It's a double sided board (red is the top layer and blue is the bottom layer) utilizing surface mount components. The board dimensions are 1 inch by 1 inch ;)
There are a number of things worth pointing out about the layout since you may miss them at first glance.
First is the use of rail to ground and rail to rail decoupling caps right next to the power pins. This is a good example of how to place the decoupling caps.
Second is the placement of the electrolytic caps very close to the power pins. This allows you to route short, low impedance traces to the power pins. Of course the physical size of the cap will dictate how short you can make the traces, so size the caps accordingly to your design requirements.
Third is the use of ground planes. If you look carefully in the picture you can see that the bottom layer ground pour connecting the electrolytic caps, the decoupling caps, and the power and speaker grounds is intentionally isolated from the other ground pours EXCEPT at the speaker ground. This ensures that all of the high currents are contained in that small ground pour AND that the other ground pours are at the same potential as the speaker ground, which is the ground reference. The 4 vias placed around the board connect the ground pours on the bottom layer to the ground pour on the top layer.
Fourth is the order in which nets are assigned to the connector. From left to right the connections are as follows: IN+, IN-, VEE, GND_VEE, GND_OUT, OUT, GND_VDD, VDD. There are 2 separate supply ground connections to accommodate a power supply with dual secondaries (this is actually my preferred type of supply). Take note that the speaker ground connection is very close to where the electrolytic caps connect to the ground plane to minimize the impedance of the ground returns.
Fifth is the position of the input and feedback resistors right near the input pins of the chip. This is good practice for any kind of sensitive inputs.
Sixth is the routing of the input signal traces away from the power supply traces as well as ground plane isolation between adjacent signals. The two input traces are purposely offset so that each is over a ground plane instead of on top of each other. This minimizes capacitance between the input nodes.
|
|
|
| danielwritesbac |
Well, that's a pretty sweet design!
I'd also like to see room for Ci because the LM1875 is more prone to DC offset than its larger cousins. |
|
|
| gootee |
| quote: | Originally posted by BWRX
Attached is an image of the layout. It's a double sided board (red is the top layer and blue is the bottom layer) utilizing surface mount components. The board dimensions are 1 inch by 1 inch ;)
There are a number of things worth pointing out about the layout since you may miss them at first glance.
First is the use of rail to ground and rail to rail decoupling caps right next to the power pins. This is a good example of how to place the decoupling caps.
Second is the placement of the electrolytic caps very close to the power pins. This allows you to route short, low impedance traces to the power pins. Of course the physical size of the cap will dictate how short you can make the traces, so size the caps accordingly to your design requirements.
Third is the use of ground planes. If you look carefully in the picture you can see that the bottom layer ground pour connecting the electrolytic caps, the decoupling caps, and the power and speaker grounds is intentionally isolated from the other ground pours EXCEPT at the speaker ground. This ensures that all of the high currents are contained in that small ground pour AND that the other ground pours are at the same potential as the speaker ground, which is the ground reference. The 4 vias placed around the board connect the ground pours on the bottom layer to the ground pour on the top layer.
Fourth is the order in which nets are assigned to the connector. From left to right the connections are as follows: IN+, IN-, VEE, GND_VEE, GND_OUT, OUT, GND_VDD, VDD. There are 2 separate supply ground connections to accommodate a power supply with dual secondaries (this is actually my preferred type of supply). Take note that the speaker ground connection is very close to where the electrolytic caps connect to the ground plane to minimize the impedance of the ground returns.
Fifth is the position of the input and feedback resistors right near the input pins of the chip. This is good practice for any kind of sensitive inputs.
Sixth is the routing of the input signal traces away from the power supply traces as well as ground plane isolation between adjacent signals. The two input traces are purposely offset so that each is over a ground plane instead of on top of each other. This minimizes capacitance between the input nodes.
|
Hi BWRX,
WOW. Nice-looking layout!!!!! You seem to have been able to lay out basically everything in the most-ideal ways. Kudos!!
It looks like it's definitely time for me to start using surface-mount parts. What are the case-style designations of the ones you have used, on this PCB? Are there any slightly-larger sizes, that might be easier to hand-solder? Or is that not a big problem?
You have the LM1875 configured as a differential amplifier. Cool. Can it accept both single-ended (i.e. one side grounded, I guess) and balanced inputs? Or maybe I should just ask how it is intended to be used.
Could you explain, in more detail, how and why the grounding scheme works? I am very interested in that part. (And my eyes are getting bad-enough that it's difficult to follow, with both layers included on the PCB-layout image.)
At first glance, it looks like the 'input ground' will share a ground-return conductor with other ground-return currents, on the way to the power supply. Or maybe I'm wrong. Or maybe I'm not wrong but it works OK, somehow.
Oh wait! It's a differential amplifier! So the R3 ground SHOULD be referencing it to the 'new' output ground level. Nice.
Have you tried it, yet??!
P.S. Is there any reason that you might want to also minimize the capacitance between each input and ground, in addition to the capacitance between the two inputs? |
|
|
| BWRX |
Thanks guys. Simple circuits like these involving a chip with a nice pin out are easier to generate good PCB layouts for.
The footprints for the surface mount parts used on this board are 0805 size. Passive surface mount parts are generally classified by a 4 digit size code. This code is a combination of the length and width of the part. So when you see an 0805 size part that means it is 0.08 inches long by 0.05 inches wide. The codes are most commonly referred to using English units, but you will also see codes using Metric units. For instance, 0805 is equivalent to 2012 (2.0mm long by 1.2mm wide).
0805 is one of the most common sizes but 0603 and smaller components are widely used in a lot of consumer electronics. I don't like having to hand solder parts smaller than 0805 because it requires an even steadier hand and it is hard to control the amount of solder applied to the joint. You only need a very little amount of solder to make a good joint with surface mount components. It is also easier to read the numbers printed on 0805 size and larger components. Components smaller than 0603 generally don't have anything printed on them.
About halfway down this this page on wikipedia you can find a chart showing the standard surface mount package sizes: http://en.wikipedia.org/wiki/Surface-mount_technology
Size is of course not the only thing you need to take into consideration when selecting parts. Just like through hole parts, surface mount resistors are offered with different types of resistive elements and construction. The smaller resistors have lower power dissipation ratings and often maximum voltage ratings as well. Temperature coefficient is another parameter to keep in mind - metal film resistors have a lower tempco than the cheaper thick film types. The smaller capacitors have capacitance and voltage limits, but these are increasing as dielectric technology is improved. |
|
|
| BWRX |
| quote: | Originally posted by gootee
You have the LM1875 configured as a differential amplifier. Cool. Can it accept both single-ended (i.e. one side grounded, I guess) and balanced inputs? Or maybe I should just ask how it is intended to be used. |
I haven't really intended it to be used in any specific manner. It could be configured as a non-inverting amp, an inverting amp, or a differential amp. What you don't see on the picture of the layout I provided earlier is that there will be exposed areas of the ground plane next to each input so that they can be bridged to ground should you want to make a non-inverting or inverting amp (these are the most common anyway). As a differential amp it could accept either single ended or balanced inputs. It would be preferred to use balanced inputs because it will work better when being driven from equal source impedances.
| quote: | Originally posted by gootee
Could you explain, in more detail, how and why the grounding scheme works? I am very interested in that part. (And my eyes are getting bad-enough that it's difficult to follow, with both layers included on the PCB-layout image.)
At first glance, it looks like the 'input ground' will share a ground-return conductor with other ground-return currents, on the way to the power supply. Or maybe I'm wrong. Or maybe I'm not wrong but it works OK, somehow.
Oh wait! It's a differential amplifier! So the R3 ground SHOULD be referencing it to the 'new' output ground level. Nice. |
It is a little hard to see everything with both layers displayed. Attached a picture of the bottom layer so you can get a better view of the supply ground connections. It's just a copper pour connecting the supply rail grounds, the electrolytic cap grounds, the decoupling caps grounds, and the speaker ground.
Refer to my next post for comments about the ground plane on the top layer.
| quote: | Originally posted by gootee
Have you tried it, yet??! |
Nope. I just came up with this on a whim last night, but I would like to have some PCBs made to see how the LM1875 sounds. The parts won't cost much so it won't be expensive to build up a number of these. I hadn't planned on doing a group buy of sorts but these are so simple that I could even offer to build these up (or at least populate the surface mount components) if anyone is interested.
| quote: | Originally posted by gootee
P.S. Is there any reason that you might want to also minimize the capacitance between each input and ground, in addition to the capacitance between the two inputs? |
Ideally you want to minimize capacitance everywhere, but it is often better to have capacitance between a signal and ground versus capacitance between two signals. For this amplifier (and considering the very small size of the PCB) it's really not that critical. |
|
|
| tangmonster |
We do a lot of pc board manufacturing ,Since we are a smallish company My job are of selecting components and managing the production schedule amongst a bit of designing.
On most of our boards we still stick to 0805 and many times even 1206
Obviousely the bigger the resistor the higher its wattage , so on our analogue in parts and some digital out parts we still stick to 1206 even though that is still overkill.
Our newest designs have started to use 0603 ,but 0603 proves VERY hard to solder by hand.
And part of my job is troubleshooting and testing the boards ,and then the 0603 parts is a pain. |
|
|
| BWRX |
| quote: | Originally posted by gootee
Could you explain, in more detail, how and why the grounding scheme works? I am very interested in that part. (And my eyes are getting bad-enough that it's difficult to follow, with both layers included on the PCB-layout image.)
At first glance, it looks like the 'input ground' will share a ground-return conductor with other ground-return currents, on the way to the power supply. Or maybe I'm wrong. Or maybe I'm not wrong but it works OK, somehow.
Oh wait! It's a differential amplifier! So the R3 ground SHOULD be referencing it to the 'new' output ground level. Nice. |
Attached is a picture of just the top layer. Look carefully at the pads of the electrolytic caps and the pads of the connector used for the supply rail grounds. I used keepouts around the pads so that they do not connect to the ground plane on the top side. This forces the high currents to stay in that small area of ground plane on the bottom side and allows the use of the top ground plane as a reference and shield. We want the ground reference potential to be the same as that of the speaker ground, which is why only the speaker ground is connected to the ground plane on the top side.
As you noted, a differential amplifier should reference to the output ground potential. That is why the one side of R3 is connected to the ground plane on the top layer. |
|
|
| BWRX |
| quote: | Originally posted by tangmonster
Our newest designs have started to use 0603 ,but 0603 proves VERY hard to solder by hand.
And part of my job is troubleshooting and testing the boards ,and then the 0603 parts is a pain. |
A hot air rework station is VERY handy when soldering, and almost essential when reworking, these smaller components.
Where I work we routinely use 0603 parts and the smallest components we use are 0402. I've had to solder those by hand a number of times and the tweezer tips are nearly as wide as the part! You have to be very careful when breathing or using a hot air pencil around components that small. They're extremely easy to blow right off the table or board. |
|
|
| BWRX |
| quote: | Originally posted by BWRX
What you don't see on the picture of the layout I provided earlier is that there will be exposed areas of the ground plane next to each input so that they can be bridged to ground should you want to make a non-inverting or inverting amp (these are the most common anyway). |
Attached is a picture of the top layer showing the solder stop mask. Areas with hatch marks will not be coated with solder mask. As I mentioned above, note the two small rectangular hatched areas above the input pads of the connector. A non-inverting amp would require R2 to be grounded, so you would simply bridge that connection to the ground plane. Likewise, an inverting amp would require R1 to be grounded, so you would just bridge that connection to the ground plane. |
|
|
| motherone |
These little guys look great!
Any chance on a GB of these PCBs? I've got a big ol' pile of LM1875's (ahem, like 40 or so), and I've been looking for a small PCB to use them with. |
|
|
| tangmonster |
| quote: | Originally posted by BWRX
A hot air rework station is VERY handy when soldering, and almost essential when reworking, these smaller components.
Where I work we routinely use 0603 parts and the smallest components we use are 0402. I've had to solder those by hand a number of times and the tweezer tips are nearly as wide as the part! You have to be very careful when breathing or using a hot air pencil around components that small. They're extremely easy to blow right off the table or board. |
We recently did get a hot air station. I was a bit sceptical , but it actually does work great.
replacing that switch mode powersupply chip (u1 on the picture) with just a soldering iron is a bit hard.
One last thing , A hollow tip solder tip is THE BEST thing for surfacemount.
http://img.photobucket.com/albums/v.../PICT0008_2.jpg |
|
|
| gfiandy |
Before ordering alot of these PCBs I would make a prototype.
The stability criteria of the amp is more critical in an inverting configuration and you have neither a dominant pole capacitor accross the feedback resistor or a Zobel network on the output to be able to adjust the stability criteria should it end up being unstable..
If you are proposing it as a general purpose amplifer it should probably have a output inductor as well. Capacitive speaker cables and even some crossovers can cause the amplifier to oscillate if there is no isolation for the amplifer from capacitance on the ouput. Experiennce suggests than arround 10nF to 100nF is the level of capacitance that normall sets off these chip amps. So if you can be sure that the load capacitance on the output will not be in this region you should be ok.
It may work without these but it also might oscillate especially as you have ground plane arround all the pins which can couple the output signal back to the input in unpredicatable ways at high frequencies which again might lead to oscillation. This amp tends to go off in the 2-5Mhz region if it is going to go unstable.
I am unsure why you are concerned about capacitnace between the input nodes. It is normal practice to keep input traces as close together as possible as this reduces the loop area from which they can pick up noise. Having said this it is unlikey to be a problem in this design. I would however move the input to a seperate connector if it was my design to keep it away from the high power recified currents comming into the local smoothing caps.
Since this is not a high speed digital design I don't think there is any benifit to having a ground plane. There may be some benifit to guard tracks arround the input connected to ground but the rest of the plane is just picking up noise from the high currents flowing in the circuits and injecting it into the ground referance. I am open to hearing a rational for the plane but my experience has been that apart from arround the low power, high sensitivity front end of amplfiers planes should not be used and even then you need to really know what you are doing to use them sucessfully.
Having said that I do like the way you have isolated the decoupling ground from the signal ground using the different layers and there is no reason for the decoupling ground not to remain as a plane as it does not couple into the signal ground.
Regards,
Andrew |
|
|
| KSTR |
For more universality I would add provision for noise gain compensation option (series RC from +IN to -IN) and for output zobel and L//R, various jumper pads etc.
Also I see no need for SMT resistors, but in case of SMT I would prefer MELF form factor.
@gfiandy
"a dominant pole capacitor accross the feedback" won't work here, we need a constant**) noise gain of >= 10
**) from about half a decade below from the Aol / noise gain intersect and upward. Can be achieved in various ways...
Regarding the GND plane, for those comparativly small currents involved (4 amps max.) a solid GND-plane is as good as it gets, IMHO
- Klaus |
|
|
| danielwritesbac |
Howabout a bridged LM1875?
This could have a more generous soundfield, more generous gain (is more dynamics power), and more generous power output. Sort of like everything you'd want a chip amp to do. ;) |
|
|
| defect9 |
wouldn't just using an LM3875 be as good as bridged 1875s?
honestly, i dont know. havent compared, but it would just seem so. |
|
|
| gfiandy |
Hi Klaus,
I am sure you are right as a dominant pole on an already compensated amplifer is dodgey to say the least. I suppose I should have been more accurate and described it as a frequency compensation shelf. i.e cap and resistor. Thanks for pointing that out. I agree that compensation at the input is probably a more reliable solution though.
Still don't agree on the ground plane, I have seen them cause too many problems on power amplifers as you can't define where the currents will flow and they pick up current return paths from high current paths you weren't expecting. It probably won't make it unstable, but I don't belive it gives you the best possible solution.
Regards,
Andrew |
|
|
| AndrewT |
Hi,
if you don't understand how a component works then what is the point of adding it to a working circuit?
This includes adding Ground Planes. |
|
|
| AndrewT |
Hi Daniel,
adopting bridged for a chipamp does not automatically give| quote: | | more generous power output |
All Chipamps are severely limited by their peak current ability.
Going to bridged asks each chipamp to supply double the current into your selected load.
This is more likely to trigger the protection mechanisms or at least sound wrong because the combination of chipamp + PSU is stressed more highly. |
|
|
| planet10 |
| quote: | Originally posted by gfiandy
I don't think there is any benifit to having a ground plane. |
But with a proper poured ground plane you won't need any groundside electon pools :)
That was one of the features i liked about Brian's design.
I also think things like zobels should be point-to-point if required. I don't think they will be required in any of my applications so provision on the board would be wasted space.
dave |
|
|
| gfiandy |
I don't want to get into a argument about this; but the point was the circuit may not work and having the option to add compensation would then allow you to get it working.
If you have a circuit that is an oscillator because of some unexpected characteristic of the load cable or crossover then the option to add a component even if it has to be derived by trial and error is surely a better option.
If the design was proposed as for a single application with a single defined load then that would be one thing but before getting into group buys the design should be adaptable enough to be made to work in most situations.
A ouput zobel and inductor would almost certainly be enough to achieve this, I mentioned the compensation only for extreem examples (which is partly why I didn't fully expand on how that should be achieved and partly because I just didn't think it through, should have know better there is always someone to pick you up on a sloppy point)
Regards,
Andrew |
|
|
| AndrewT |
I will add to my last post.
If one modifies a working circuit by removing a component because one does not understand it's function then that is likely to lead to trouble. |
|
|
| danielwritesbac |
| quote: | Originally posted by AndrewT
Hi Daniel,
adopting bridged for a chipamp does not automatically give [more generous power output]
All Chipamps are severely limited by their peak current ability.
Going to bridged asks each chipamp to supply double the current into your selected load.
This is more likely to trigger the protection mechanisms or at least sound wrong because the combination of chipamp + PSU is stressed more highly. |
In practice, its quite difficult to trigger the protection scheme on the LM1875. And, it isn't the screechy spike system either.
The LM1875 can do 4 ampers; however, if it is set up in the efficient ways you have mentioned, then. . . If/when one doesn't bump into the 4 amper limiter, then the transients are good for 12 ampers.
In practice, the actual limit is heat. Using two chips seems like a great solution, because it spreads the heat out of the way.
The part that I really like is that the chips will be operating at half gain. Therein is a lot of potential. Personally, that's ever so much more sensible than using two amplifiers in series (as with buffers and active pre).
So, I'm saying that this bridged LM1875 has every reason to succeed with only a passive preamp. I'd like to give the precedent of the miniature BTL Tripaths as an example.
The LM1875's, if bridged, will also be operating on a slightly lower voltage. I don't know about that one.
Personally, I find the prospect of a bridged LM1875 to be very exciting, unlike yet another pcb for just one chip. There's already so many of those. |
|
|
| AndrewT |
Hi Daniel,
do the numbers.
50W into 4r0 needs 20Vk and 5Apk. That's about the same amp set up as 27W into 8r0, requiring only 2.6Apk.
A bridged pair will do 100W into 8r0 needing 40Vpk and 5Apk.
Now attach a real speaker. 100W into 8ohms.
The transient peak current can be as high as 14Apk.
Those numbers apply to a 27W into 8r0 amp, with it's very much reduced supply voltage.
If one chooses to start with a 60W into 8ohm chipamp you don't have any hope of getting the amp to perform well in bridged mode, because the peak current requirement jumps to around 21Apk.
Don't be silly, just think about it and if need be, do more background reading. |
|
|
| danielwritesbac |
| quote: | Originally posted by AndrewT
Hi Daniel,
do the numbers.
50W into 4r0 needs 20Vk and 5Apk. That's about the same amp set up as 27W into 8r0, requiring only 2.6Apk.
A bridged pair will do 100W into 8r0 needing 40Vpk and 5Apk.
Now attach a real speaker. 100W into 8ohms.
The transient peak current can be as high as 14Apk.
Those numbers apply to a 27W into 8r0 amp, with it's very much reduced supply voltage.
If one chooses to start with a 60W into 8ohm chipamp you don't have any hope of getting the amp to perform well in bridged mode, because the peak current requirement jumps to around 21Apk.
Don't be silly, just think about it and if need be, do more background reading. |
I'm so glad to hear this news. Yes. Please disregard everything that I said about bridge application for this chip. Its apparently unviable, nonworking and inadvisable. So, I sincerely hope that nobody makes a bridge LM1875. |
|
|
| Zero One |
On bridging for the LM1875.
I can think of 3 reasons why one might wish to bridge this amp, and they have little to do with liberating maximum power, if that is what one want then it would be best to go for another chip.
Reason 1: You have a limited voltage power supply to play with like for example 12Volts, all Nat Semi chips produce around 6 watts on such a supply.....well in fact according to the Nat Semi data the LM1875 actually produces more than the other chips at that voltage, including the 3886.
Reason 2 In my experience the LM1875 actually sound sweetest running on 12 volts, many folk who have tried it say much the same, but maybe you need more power than 6 watts. Bridge application will of course do this, though you will only end up with around 24W equavilent to the std LM1875 trafo set-up.
Reason 3 You want the best sonic performance and that means (in my experience again) you need to run either SLA or SMPS power supply, to do this you need to run either 12V, 15V (using SMPS which is actually hard to locate at this voltage) or 24V (4 batteries) or SMPS. Having tested all of these except 15v the 12V sounds better in either config. Trafo set-ups to my ears are either grainy sounding and/or dull in the mids/highs.
So bridged application is probably not as daft as it might seem, and it is worth noting that the LM1876 is actually designed to be used in such a way, and of course the LM1876 is basically just a pair of 1875s in one package with a few small changes.
Bridging from my investigations can bring many benefits (power supply issues being covered), it appears that the only real deficit is that it will not improve cross-over distortion, which could in fact be a little worse. However I must say if power is all you want then there are probably far better options to be had with other chips, the thing is up till now most folk have only considered bridging on the grounds of power liberation. Anyhow I am interested enough in the idea to try it and will do so in the next few weeks, if it doesn't cut the sonic mustard it won't have cost me much to find out. |
|
|
| danielwritesbac |
| Hey, the guy who started this thread has a really good LM1875 monobloc design there. I really do hope he makes some boards. ;) It would be really nice to see what the powerful little chip can do with his elegant and compact design. |
|
|
| ttan98 |
| I am interested in purchasing the PCB's. |
|
|
| danielwritesbac |
| Is it possible to use the little LM1875 to drive a FET output, and at the other end, also have a buffer input? |
|
|
| Iván Francisco |
| Maybe something like this? |
|
|
| BWRX |
| quote: | Originally posted by danielwritesbac
Is it possible to use the little LM1875 to drive a FET output, and at the other end, also have a buffer input? |
It would make much more sense to use the LME49810 or one of its siblings to drive a FET output stage, even though it's roughly twice the price of the LM1875. |
|
|
| danielwritesbac |
| quote: | Originally posted by BWRX
It would make much more sense to use the LME49810 or one of its siblings to drive a FET output stage, even though it's roughly twice the price of the LM1875. |
Hey, it looks like your mini project really is the best option. Have you made one? I sure would like to see what it sounds like. |
|
|
| BWRX |
| I haven't done much of anything audio related for days - been sick with the flu since wednesday :dead: |
|
|
| Bob_Sled |
| I bet you're audible in the bathroom! :D |
|
|
| BWRX |
| quote: | Originally posted by Bob_Sled
I bet you're audible in the bathroom! :D |
Indeed I was ;) but that's off topic...
In terms of the design, I've decided to try two different layouts - a basic and a full version. The basic version is just the basic components and fits on a 1"x1" pcb. A picture of the basic version schematic and layout are attached. |
|
|
| BWRX |
The full version includes options for components suggested by others and fits on a slightly larger 1.15"x1" pcb. A picture of the full version schematic and layout are attached.
I'll be putting both layouts on one board and have them made using expresspcb's miniboard service, which is three 3.8"x2.5" boards, no silkscreen or soldermask, for $59.90 shipped (very fast turn around too). If anyone knows of a better place to have these proto boards made feel free to let me know ;) Two basic and two full layouts plus another little layout will fit on each board. These will just be used for testing the design. |
|
|
| defect9 |
Do I smell a group buy in the future?
-Jared |
|
|
| renfrow |
I just came across this, on ebay, I have not tried it, and can not vouch for it. sureelectronics, the chinese company selling cheap class-d boards is offering pcb prototyping, look for them as a seller or, try this link.
Tom. |
|
|
| BWRX |
| quote: | Originally posted by defect9
Do I smell a group buy in the future? |
It's possible, but right now I'm drained from the Jordan JX92S group buy (which is close to being finished!).
| quote: | Originally posted by renfrow
sureelectronics, the chinese company selling cheap class-d boards is offering pcb prototyping, look for them as a seller or, try this link. |
They're dirt cheap all right! Quality may be a bit iffy but a lot of people have bought the class d amps from them... I've used other Chinese board houses and had good results but I'll probably stick with expresspcb for the first set of prototype boards. They have good quality and the turn around time is very fast for the price - mainly because there's no soldermask or silkscreen but you don't need that for proving out a design. |
|
|
| dfdye |
Hey Brian,
I typically use Advanced Circuits $33 deal , but they require you to buy 4 (unless you get the student discount, in which you can order only one, but I am guessing you don't exactly qualify for that). Thus, I don't really think they would be a good fit for this project, but for something a little larger, the $33 price is good for any board up to 60 square inches. The prototype boards are full spec (1oz. copper, top and bottom mask/silk), and are VERY nice. |
|
|
| BWRX |
| I've used Advanced before and they are good. I would consider going with them if this were higher quantity but they're not as cheap for doing prototype stuff. Plus, they charge $50 for multiple part numbers on one board (almost all places do that anymore). Their barebones sevice, however, is almost the same price as expresspcb for the same size and quantity of boards. They would still probably tack on the $50 charge for multiple part numbers on one board. |
|
|
| dfdye |
Yea, no doubt regarding the no multiple parts per board being a deal breaker for this project.
If, however, you make the panels yourself and send them the Gerbers as one file, I don't think they care as long as you are willing to cut the boards yourself. I haven't ever tried, but it may be worth it if you have a couple of small projects that you could cut and paste into one file. . . .
Just thinking out loud. . .
David |
|
|
| BWRX |
| quote: | Originally posted by dfdye
If, however, you make the panels yourself and send them the Gerbers as one file, I don't think they care as long as you are willing to cut the boards yourself. |
That is exactly what Advanced charges you the extra $50 fee for. Most places charge a similar fee or won't make your boards if you send them files like that. They do that because they don't make much on small orders as it is. |
|
|
| motherone |
Well, if it helps a GB along, I would probably be in for something on the order of 40 boards (since I have about 40 LM1875s sitting around), depending on the price.
I can't imagine boards this small being much more than $2.50/pcb in any appreciable quantity. IIRC, the Guzzler USB DAC group buy from head-fi was around that price, even though it was shipped from Europe. I would guess these boards to be of similar size. |
|
|
| BWRX |
| quote: | Originally posted by motherone
(since I have about 40 LM1875s sitting around) |
Perhaps you'd like to trade some of those chips for boards? ;)
I just finished the other "little layout" I mentioned earlier. It's a differential buffer that when used with the LM1875 configured as a differential amp makes a 3 op amp instrumentation amp. This is the same configuration I'm using with my LM3875 amps.
I managed to squeeze all that stuff on a 1"x1" pcb, make the power connections line up with those of the other two LM1875 boards, and make the outputs of the differential buffer line up with the inputs of the LM1875 boards so they could easily be stacked. |
|
|
| dfdye |
| With no mounting holes, how do you propose stacking? |
|
|
| BWRX |
That's an excellent question! I had originally planned to place a small mounting hole in the upper right corner of each board but it seems I forgot to do that while laying out everything :cannotbe:
I guess since the board will be so small and light that just running the 7 wires down from the upper board to the lower board will be enough to hold it in place. What do you think? |
|
|
| theAnonymous1 |
BatchPCB does a nice job for a very reasonable price, the only down side is it can take almost 3 weeks to receive your order. They are an excellent deal for small prototype orders. There are probably better places for large quantities.
Below is a pic of some boards they made. Six boards cost $59.60 and that included setup, silkscreen, soldermask, and shipping.
http://i30.tinypic.com/30b0i80.jpg |
|
|
| BWRX |
Those look real nice Anon. 6 of those for $60 (including shipping) is a pretty good deal. Too bad the lead time is so long.
How big are they? They look to be about 1.25" x 1.75". |
|
|
| AndrewT |
| quote: | Originally posted by BWRX
That's an excellent question! I had originally planned to place a small mounting hole in the upper right corner of each board but it seems I forgot to do that while laying out everything :cannotbe:
I guess since the board will be so small and light that just running the 7 wires down from the upper board to the lower board will be enough to hold it in place. What do you think? |
7 off 0.6mm wires will be quite rigid. If you are unsure, then increase the hole diam to 1mm and use 0.9mm wire. |
|
|
| BWRX |
| Hi Andrew. Thanks for the assurance :) The diameter of the plated holes for the 9 pole connector should end up being around 1.1-1.2mm, so there's room for 0.9mm wire or maybe even a really tight fit of 2 0.6mm wires. |
|
|
| theAnonymous1 |
| quote: | Originally posted by BWRX
How big are they? They look to be about 1.25" x 1.75". |
Wow, good eyes.:magnify:
They are 1.25" x 1.7". |
|
|
| BWRX |
| It's amazing what you can do with photoshop ;) |
|
|
| theAnonymous1 |
| quote: | Originally posted by BWRX
It's amazing what you can do with photoshop ;) |
Cheater! |
|
|
| AndrewT |
| quote: | Originally posted by BWRX
Hi Andrew. Thanks for the assurance :) The diameter of the plated holes for the 9 pole connector should end up being around 1.1-1.2mm, so there's room for 0.9mm wire or maybe even a really tight fit of 2 0.6mm wires. |
then use 1mm or 1.1mm wires.
Much stiffer than twin 0.6mm. (~4times stiffer) |
|
|
| motherone |
| quote: | Originally posted by BWRX
Perhaps you'd like to trade some of those chips for boards? ;)
I just finished the other "little layout" I mentioned earlier. It's a differential buffer that when used with the LM1875 configured as a differential amp makes a 3 op amp instrumentation amp. This is the same configuration I'm using with my LM3875 amps.
I managed to squeeze all that stuff on a 1"x1" pcb, make the power connections line up with those of the other two LM1875 boards, and make the outputs of the differential buffer line up with the inputs of the LM1875 boards so they could easily be stacked. |
I'd be happy to send a few your way if they help get these boards moving forward. The LM3875/3886/4780 have had a ton of support, but there hasn't been nearly as much for the 1875.
If you're interested in the chips, you can e-mail me at m i k e a!t m o t h e r o n e d a w t co m.
Oh, and the awesome thing about these chips is evidently Radioshack in Canada sold them, so they're in the little radioshack cardboard/plastic parts packs.
Any chance you could put some holes on the board in the resistor areas so we could tombstone some if we wanted to go with something other than SMD? I certainly don't mind using SMD parts (having built quite a few projects with them), but it'd be fun and possibly more versatile if you had the ability to throw some boutique stuff on there. I can't imagine it would drastically increase the layout size.
Mike |
|
|
| BWRX |
| You can position through hole resistors vertically and solder the leads to the SMD pads on the board if you really want to (don't need through holes for that), but there is really no point if you use good quality metal film surface mount resistors. If you want to use some film caps for supply bypass instead of ceramic you can solder them to the pins on the underside of the board. |
|
|
| Nordic |
I call it the 1 incher |
|
|
| BWRX |
| quote: | Originally posted by Nordic
I call it the 1 incher |
But it's 1.5"x1" not 1"x1" ;)
Marketing... :p |
|
|
| dfdye |
| quote: | Originally posted by BWRX
I guess since the board will be so small and light that just running the 7 wires down from the upper board to the lower board will be enough to hold it in place. What do you think? |
Well, I have used double sided foam tape under PCB's to mount stuff for lab gizmos in the past, so I probably shouldn't offer my opinion! :D
Seriously, the wire hanging trick sounds like a winner. I am not even approaching being concerned about the weight of both of the boards being supported by the chip. |
|
|
| dfdye |
| quote: | Originally posted by BWRX
. . . .there is really no point if you use good quality metal film surface mount resistors. |
While we are on the subject, I was tooling through Digikey the other day, putting together a BOM for a project I am working on and noticed that the Rohm resistors were literally half as much as the Vishay/Dale resistors. Have you ever used the Rohm resistors? Heard anything about them?
Not that there would be that much difference in cost for a few parts, but it definitely made me wonder what was up and whether the Rohm parts were to be trusted. |
|
|
| BWRX |
I'm not entirely sure why there is such a difference in price between something like the Vishay/Dale CRCW resistors and the Rohm MCR10 since both are thick film types and have similar specs, but it could be due to differences in construction and composition of the resistive element. It could also be that Rohm makes such a large quantity that they can offer them for cheaper (economies of scale at work).
The resistors I like to use are the Susumu RR series. They are categorized as thin film and they have a metal film resistive element. Priced at $1.40 for 10, they have low 0.5% tolerance and low TCR (the RR????P... resistors have a TCR of 25ppm/C). Or if you feel like spending a little more for 0.1% go with the Panasonic ERA6AEB???? resistors which are $2.04 for 10. As always, if anyone knows of good resistors for less, we'd all love to hear what and where to get them :) |
|
|
| dfdye |
Thanks for the suggestion, but the Susumu's don't seem to come in 1206's (which is what I need)--at least not at Digikey. :(
Not to veer too much more off course, but do you notice any difference between the thin and thick film resistors? I have seen the "more direct conduction route" argument for thin film, which is voodoo as far as I am concerned, but if you have a reason you prefer one over the other, I am all ears.
Either way, I am certain any of these resistors should work just fine, but now is the tweaking stage! :D |
|
|
| Nordic |
1206 is huge man!, you need to be over 60 to have to have to use those.
I see you are designing double sided, maybe you can copy my idea of useing SMT electrolytics, mounted on the bottom layer, which allows you to shorten the board drasticaly...
After the clever quip above, I reduced my board to 1.3inch square.
useing moslty 0805, they are quite easy to work with I find, even when soldering them with an iron like a caveman.
It seems a shame to make them this small as the suggested heatsink (if it will be exposed - isolated)is quite big, 10 x 10 x 3cm per channel.
 |
|
|
| BWRX |
| quote: | Originally posted by dfdye
Thanks for the suggestion, but the Susumu's don't seem to come in 1206's (which is what I need)--at least not at Digikey. |
As Nordic indirectly said, why are you using 1206 size resistors? Is it for the slightly higher power rating? If not, use 0805.
| quote: | Originally posted by dfdye
Not to veer too much more off course, but do you notice any difference between the thin and thick film resistors? |
Honestly, I haven't AB tested amps with thick film versus metal film resistors, but I probably wouldn't be able to tell the difference. Technically, the metal films are better so I prefer to use them. |
|
|
| dfdye |
Yea, the 1206's are indeed huge, but they have part numbers on them! :D
Actually, the reason I like them is because I can use 1/4W parts and not think about the conversion from "OLD" designs to SMP's. I know I should use 0805's, but I guess I am just slow to convert, and, though I don't think I am near the limit for any parts. the 1/10W thing sort of puts me off. Also, with the 1206's I can run traces between the pads, which I don't feel comfy doing with 0805's.
This really helps when making double sided boards at home since vias on small signal traces are notoriously hard to line up and I generally try to avoid them at all cost! The exception obviously being vias going from small traces into a ground plane that you don't have to align carefully.
Plus, that heat sink is INSANE overkill IMHO. I know what the recommendations are, but who in their right mind would push this chip to get hot enough to need THAT heatsink??? If you need that much power, use a different chip (or a grown up amp! :) ) |
|
|
| BWRX |
| quote: | Originally posted by Nordic
I see you are designing double sided, maybe you can copy my idea of useing SMT electrolytics, mounted on the bottom layer, which allows you to shorten the board drasticaly... |
Those surface mount caps are physically the same size, so they wouldn't allow me to shorten the board at all. Surface mount parts are nice but there is really no benefit for using surface mount electrolytic caps if you're hand soldering them. |
|
|
| BWRX |
Most 0805 size resistors have values on them too ;) The Susumu and Panasonic resistors do.
If you design the footprint well you can comfortably run up to a 16 mil trace between the pads of an 0805 size part.
I have some sections of that heatsink Nordic posted a picture of. It would work well as the heatsink for many LM1875s! |
|
|
| dfdye |
| quote: | Originally posted by BWRX
Most 0805 size resistors have values on them too ;) The Susumu and Panasonic resistors do.
If you design the footprint well you can comfortably run up to a 16 mil trace between the pads of an 0805 size part. |
I hate you so much right now. Now all of my excuses are out the window. . . . :bawling:
Still, I'll be building one last project that's underway with 1206's, so I have a little reprieve before I have to bust out the microscope. :D |
|
|
| BWRX |
| quote: | Originally posted by motherone
I'd be happy to send a few your way if they help get these boards moving forward. |
I sent an email to expresspcb asking to place an order for some boards using the gerber files generated by eagle and they said they only accept boards designed and routed using their software! :xeye: I have no idea why they would turn down business like this when every other board house known to man will accept regular gerber files... Needless to say, I won't ever be doing business with them again.
In the meantime I stared at the layout some more, saw ways to rearrange components, and shrank the size of the full version board down to 1"x1". Since there isn't much point in having the basic version made anymore, the plan is to put 2 LM1875 boards and 2 differential buffer boards onto a 2"x2" board and see what kind of pricing I can get from some other places even though they will charge an extra fee for more than one part number per board. |
|
|
| dfdye |
Hmm. . . . . If you tie the signal traces between the inputs of the chip board into the outputs of the buffer board and tie some of the power leads together, you could almost make this "one" part. You can always cut through the leads when you separate the boards.
Again, this is clearly trying to skirt the rules, but it may work. . . .
Worst case, you can go with Olimex. :D Talk about long turn around time, but the price is right! |
|
|
| BWRX |
I've already tried that before with multiple little layouts on one board and most places aren't that dumb. Just like any other business, they won't miss out on a chance to charge you more!
Olimex may be the best way to go pricewise but I'd have to check to see if the boards meet their minimum requirements. Either way, I'm also looking at having them made by pcbex. They make great quality 2 layer boards with a pretty fast turn around for pretty cheap. The multiple layout fee might be like $50 though. |
|
|
| shallbehealed |
| I'm in for a few sets if a GB goes through. I don't have anything technical to add, but I've been reading with a keen interest. |
|
|
| renfrow |
I haven't seen much discussion of power supply for this. Earlier there was mention of 12v, 15v and 24v, SLA and SMPS. However, the board clearly is designed for split power supply. How are you planning on powering it?
Tom. |
|
|
| BWRX |
| I plan on using a dual secondary transformer and dual diode bridges to derive the +/- rails. The target rail voltage is around 25V but you could use 12V to 35V. It would work equally well with a center tapped transformer if one wanted to go that route. |
|
|
| danielwritesbac |
| quote: | Originally posted by BWRX
I plan on using a dual secondary transformer and dual diode bridges to derive the +/- rails. The target rail voltage is around 25V but you could use 12V to 35V. It would work equally well with a center tapped transformer if one wanted to go that route. |
Hi Brian! I just wanted to mention that, in practice, these LM1875 max at 32.5v, but do it well. In the U.S. that would relate closely to a 40vct (20+20) transformer. . . and Nordic's heatsink. ;)
For an economical, yet well made, center tap, there's a Stancor, White Rogers 40vct available with sufficient amperage for several LM1875.
The heatsink won't be economical unless its a "recycle" like a thrifty shop discovery.
At max voltage, the power caps onboard with the amplifier would be in the neighborhood of 100uF to 330uF, because larger "may" promote heat. I don't have details on that observation.
Reason to use the maximum. . . there are some configurations possible to "promote" dynamics to an unusual extent. Personally, I find this helpful for popular music and/or stubborn (inefficient) speakers that the other chip amps drive poorly. In my opinion, there's no such problem with LM1875's.
That's all I've got for now, except. . .
The mention of such voltages has me curious about safer, lower, voltage, but a parallel layout. |
|
|
| BWRX |
Hi Daniel. Quite right about the supply voltage. I was thinking about the LM3875 when I mentioned 35V rails! The max recommended voltage is +/-30VDC for the LM1875.
Most any transformer will work. That rating you would want would depend on how many circuits it will be powering. 30VA per chip is what I would use as the minimum. 50VA per chip would yield a nice beefy supply.
The value of the electrolytic caps on board shouldn't have anything to do with power dissipation in the chip. If different caps yield different amounts of power dissipation than you are probably having oscillation problems. The footprint I've used is for a 5mm lead spacing, 10.5mm diameter cap. I selected a 220uF 35V Panasonic FM to use because it has a height of 15mm which will leave room for a screwdriver to access the screw that will hold the LM1875 to the heatsink. If you have another way of fastening the chip to the heatsink you can use up to a 560uF 35V Panasonic FM (which is 25mm high). If you use lower voltage rails you can use a lower voltage cap and get more capacitance in the same size. For instance, 560uF 35V is the same size as 820uF 25V or 1200uF 16V for the Panasonic FM series. |
|
|
| dfdye |
Daniel, what you are saying about the caps at the chip doesn't make any sense. Those caps merely serve to clean up the power and to provide "quick" reserve, but the power dissipation (heat) of the chip would not be affected by changing those values.
(Woops, didn't see Brian's post there before I posted) |
|
|
| danielwritesbac |
| quote: | Originally posted by BWRX
Hi Daniel.
. . .
Most any transformer will work. That rating you would want would depend on how many circuits it will be powering. 30VA per chip is what I would use as the minimum. 50VA per chip would yield a nice beefy supply.
The value of the electrolytic caps on board shouldn't have anything to do with power dissipation in the chip. If different caps yield different amounts of power dissipation than you are probably having oscillation problems. The footprint I've used is for a 5mm lead spacing, 10.5mm diameter cap. I selected a 220uF 35V Panasonic FM to use because it has a height of 15mm which will leave room for a screwdriver to access the screw that will hold the LM1875 to the heatsink. . . |
At from $12 to $14 each, 36va, 36vct (18+18ac), Canadian made Allied store brand, #227-2060 looks good for Monoblocs. No rice paper, no gaps. Actual amperage, well, she'll hold 1x LM1875 quite well with about 4400uF per rail. Pairs of Mallory 2200uF SEK or something nice from Nichicon, are quite economical performers for $1.
There's also MR. . . oh heck no! They've only got OnSemi--ridiculous variances per sample. I was hoping for Motorola Litespeed goodies. Oh well, at least there's a lot of KBPC bridge rectifier units, perfectly matched inside, at about $2 (per bridge).
So, power for two monoblocs would be about $38 + shipping.
The local smoothing cap size makes difference in oscillation problems? Oh thank you! I had no idea why there would be a difference in heat. I was just reporting an observation and hoping for an explanation. ;) Thanks!!
Also, thanks for leaving room for the screwdriver!!! :D :D :D
If someone's looking for a speaker idea, then a possible speaker partner for LM1875 might be W6-789S, Tang Band, 91db, 6-1/2, 8R (DC6R). Despite specs saying large box and 15w, its perfectly happy with small ported box (from 0.5 to 1 cubic foot), works fine sealed or ancheloc (can't spell it)--and a LM1875 with the above 36vct (18+18) transformer matches closely on power handling, as I am testing it right now. Its got that high crossover point, extra fast lightweight coated paper, and, a non-screech fiber dust cap--so practically no effort for the crossover. Anyway, like the LM1875 amps, there's power and fidelity with not much labor to get it.
P.S. That little driver, can't stand up to the "highly optional" 32v rails hotrod LM1875's, but its a can-do with a efficiency-based Harbeth Monitor 40 clone, like this one: http://www.partsexpress.com/project...t=MagnaCumLaude or similar. But, hey! see what the normal stuff will do, unless you're one of those people accustomed to removing drywall in high fidelity. :D :D |
|
|
| BWRX |
| quote: | Originally posted by danielwritesbac
The local smoothing cap size makes difference in oscillation problems? Oh thank you! I had no idea why there would be a difference in heat. |
As dfdye and I said above, the cap size should NOT make a difference (i.e. not cause oscillation problems).
| quote: | Originally posted by danielwritesbac
ancheloc (can't spell it) |
I think anechoic is the word you were looking for. |
|
|
| dfdye |
| quote: | Originally posted by danielwritesbac
The local smoothing cap size makes difference in oscillation problems? |
No. It won't. It will potentially affect rapid transient response of a device (thus the reason bypassing PSU caps can be a good idea), but not stability. |
|
|
| danielwritesbac |
Transient speed. . . as in h2 vs h3 and bass speed resolution. . . makes a lot of sense. Less puuuushing a boom with consequently more pretty bass rumbles, would seem possible to run cooler.
But, there's no problem. Brian has used the centerline tolerance that just happens to agree with my rather mysterious heat management observation. . . so the potential problem is absent.
:D :D :D Let's just keep it simple and say that "room for the screwdriver" is a very, very good thing. :D :D :D |
|
|
| danielwritesbac |
| quote: | Originally posted by Nordic
I call it the 1 incher |
Howabout throw the terminal blocks away and cram both a preamp and power supply on there instead? That would be great fun.
EDIT: P.S. Center pin is v- |
|
|
| BWRX |
| quote: | Originally posted by danielwritesbac
Transient speed. . . as in h2 vs h3 and bass speed resolution. . . makes a lot of sense. Less puuuushing a boom with consequently more pretty bass rumbles, would seem possible to run cooler. |
The "transient speed" of any decent cap should be much faster than any audio waveform. The basic equation i=C(dv/dt) is what governs the amount of current that a capacitor can source or sink. The lower the load impedance is the larger the amount of current that will flow through the capacitor, and the larger the voltage drop that will occur across the capacitor. This is the reason that larger capacitors can provide better bass performance - higher capacitance values can supply more current with less voltage sag. But larger capacitors also tend to have higher inductance, which is governed by the other basic equation V=L(di/dt). This is more or less trivial for class ab amps, but it has more of an effect in class d amps where the output transistors are switched on and off very rapidly.
| quote: | Originally posted by danielwritesbac
Brian has used the centerline tolerance that just happens to agree with my rather mysterious heat management observation. . . so the potential problem is absent. |
Ironically, the 220uF 35V cap I chose coincides with the value that works for your amps. I'd be willing to bet that different values of caps will work equally as well with my board. We'll see soon enough since I've ordered some boards earlier today. |
|
|
| danielwritesbac |
| quote: | Originally posted by BWRX
. . . This is the reason that larger capacitors can provide better bass performance. . . |
Hey bud, sorry about the elipses, but I nearly fell off my chair when I read that part.
I've tried and tried to think up an explanation, but, couldn't do it. My apologies.
Instead, here is my selection method for that part:
Too big for more bass adds noise in proportion to the additional bass, including problems of slow bass resolution, problems with general speaker compatibility--in which case the approach can backfire and become bass shy due to insufficient impact.
If just the right size. . . well you get hifi.
Likewise, too small can make an "extra generous" upper midrange, like the chipamp.com kit. One amplifier like that in my collection is more than sufficient.
I like amplifiers best described by what they don't sound like--no extra bass, no extra mids, no extra details, no distracting extras whatsoever. Does that make sense?
Again, I apologise that I couldn't come up with a better response on the topic of the caps onboard with the amplifier. Well, I just wish I could have given an explanation, but the three comparisons above is all I can do.
And, I can't name the optimum part to use--that will vary by application. I didn't say to use only 220uF, but what I did say is that its a great place to start because its the centerpoint of a range that's likely for hifi results. There's probably still going to be a hunt because many other factors (probably all) will affect the outcome of which part is optimal.
Some of that is fun. I hope the boards arrive soon. :D |
|
|
| BWRX |
| quote: | Originally posted by BWRX
This is the reason that larger capacitors can provide better bass performance |
Perhaps that statement was a little too general. You need to look at the power supply and amp as a whole and not just focus on the electrolytic caps closest to the chip. Since all chip amps use feedback, they will try correct the output voltage to match the input voltage regardless of power supply fluctuations. Even so, that doesn't mean that we don't want good stiff supply voltages. If an amp has a very stiff power supply then it will be able to supply a lot of current without any droop in voltage.
Consider an amp that does not have feedback. Any power supply ripple or sagging will affect the output voltage. When asked to deliver large amounts of current the supply rails will sag the most. What this looks like on a frequency response plot is a low end that starts to roll off. |
|
|
| danielwritesbac |
| That was a fantastic explanation. Thanks! |
|
|
| danielwritesbac |
| quote: | Originally posted by BWRX
. . .We'll see soon enough since I've ordered some boards earlier today. |
Hi Brian!
Hey, did the boards come in? ("Are we there yet, are we there yet?") :D :D |
|
|
| BWRX |
| No, I ordered them from PCBEX with a 5 day turn. They only have 2 day delivery so I should get them around the 16th. I don't have all the parts to build them up ayway. |
|
|
| danielwritesbac |
A heads-up. A great resource (mentioned above) is going away.
A very much ideal driver for this lm1875 project, is currently on a clearance sale. Its 92db, 6-1/2 inches woofer, and it works in boxes from 0.5 cubic feet ported (or sealed) to 1 cubic foot ported (or sealed). Normally, its $43, but on closeout special its $26.
http://www.partsexpress.com/pe/show...tnumber=264-852
It can enable your LM1875 projects to hit home theatre volume levels.
Another option, also using this driver, is http://www.partsexpress.com/project...t=MagnaCumLaude without about 98db efficiency, good for popular music.
That is easily driven by a single LM1875, although it makes a wonderful tri-amp or quad-amp project.
Hey Brian, I guess some of us are going to find out just how much that little amp can do. ;) |
|
|
| danielwritesbac |
Here's some thoughts on the potential of the LM1875
According to the LM1875.pdf from National Semiconductor, and if I read the graphs right. . .
The LM1875 tops out at 42 watts, which it cannot pass because of its size--the heat won't go into the heatsink fast enough.
And a slight break for some collected empiric data. . .
The LM1875 is frequently enjoyed at voltages less than 16vdc or more than 25vdc.
Using it. . .
Okay, so, the recommendable transformer is a 36vct/18vds (18vac rectifies to about 26v rails, sometimes 27v rails).
Back to the PDF. . .
Since we shouldn't increase the voltage, we can increase the load, as long as we never pass the 42w barrier. Okay, if I read the charts right, that's a 6 ohm load.
Applying it. . .
The little 92db driver mentioned above, can make 6 ohm MTM's (two woofers per speaker) with a laid-back midrange (helpful to chipamps).
This would be 1 pair of drivers per each lm1875.
To make 12 ohms for each driver, add a 4 ohm resistor to the + terminal of each driver. There are two drivers, so that means two resistors (1 resistor per each driver).
This would be paralleled to make 6 ohms.
I believe the crossover to be one 0.5mh with one 16uf, second order.
And, I'm guessing that's about 94db, of hifi, at the very first watt.
Given the LM1875's abilities to make 39 watts on a 6 ohm load. . . and typically overstated specs that actually means 32 watts of music (with 39w of heat). . ., that's a whopping 110 db per each lm1875 (113db stereo), if I did the math right.
Did I do the math right?
If so, it seems that this system would outperform most high-power systems. It also seems like the laws of physics are on vacation, so can somebody check the figures? Thanks!! |
|
|
| gfiandy |
Haven't you lost a third of your power into the 4R resistors?
Regards,
Andrew |
|
|
| danielwritesbac |
| quote: | Originally posted by gfiandy
Haven't you lost a third of your power into the 4R resistors?
Regards,
Andrew |
It looks funny, doesn't it.
Well, in practice, the 92db driver with the 4 ohm resistor does still play noticably louder than an 89db driver that has no resistor.
Here's what's happening.
Viewed by itself, the 4r does decrease the loudness, but mostly at the mids. :D I think that this approximately compensates for the boost of the cap in the crossover. So, it doesn't require the masking and power loss of an RC (zobel). Is it break-even? I don't know. But, there's no masking.
Power,
Two of eight ohm speakers, each one having a 4 ohm resistor on their + terminal, still comes out like a single 6 ohm speaker, so I think that the LM1875 amplifier doesn't lose any power.
Well, I got very loud hi-fi out of LM1875, without stressing it out. But, I think that my figures must be off a bit.
My goal here is setting up the very dynamic amplifier with a very dynamic speaker. I think that this is helpful to modern recordings. The amp is unsuited to continuous high spl, but it can deliver a big wallop on dynamics, especially with efficient speakers. Maybe its a bit more like a live performance?
EDIT: I keep wanting to give the little amp a big "push" and this is my "most seemly" idea yet. Of course, from 1 to 2 cubic feet (either size sealed or ported), is almost a floor stander. But, its still a nice compact size, sort of like my cousin's speakers over at Devore Fidelity. Well, there is a slight difference in price. Oh, but the tweeter crossover can just be a 1.5uF cap (that's a guess) and an Lpad, so research time is more like 8 minutes (no cap in the voice band--the easy way). :D |
|
|
| AndrewT |
Hi,
to get 110db/m from a 92db/W/m driver, one would need 63W delivered to the driver.
If the feed also has a resistor in the line then the power wasted in the resistor must be added to find the total power required from the amplifier.
Of course, this assumes there are no losses in the cables nor in the crossover.| quote: | | Did I do the math right? |
no.
Then, one would have to consider the effect the series resistance will have on the speaker Q and design the box accordingly. |
|
|
| BWRX |
| quote: | Originally posted by danielwritesbac
Here's some thoughts on the potential of the LM1875
....
If so, it seems that this system would outperform most high-power systems. |
How do you figure the LM1875 will outperform most high-power systems? I don't see anything that allows you to draw that conclusion based on what you stated. |
|
|
| gfiandy |
Hi,
Here is my pennies worth, I am a bit dopey at the moment as I am off work unwell so I may have made mistakes.
The Zoble network (assuming it is a 10R and 100nF to GND) dissipate very little power in the audio band. As for masking the sound this is a subjective thing and I find it depends on the type of capacitor, resistor and the the return path you use for the ground currents.
However 4R in series with the load will dissipate 1/3 of the power in the region where the drive unit is about 8R. (Agreed it will be much less arround the bass region where the drive uinit starts to resonate)
If you apply 1W in the mid range, 1/3W is lost in 4R 1/3W is dissipated in each of the drive units. This means the output of each drive unit will be down by approx 9.5dB (20*log(1/3)) but because there is two of them, then assuming perfect summation you get +6dB so the output level will be 92 - 3.5 approx 88.5dB. If the drive units in fact dip to arround 6R then the situation is much worse. The capacitor in the crossover does not make up for the loss it just increases the reactive load on the system (reducing the impedance further) drawing more power from the amplifer so for your nominal 1W in you don't get any more output.
Also you will have lost alot of control over the drive unit as it is being driven from such a high impedance, tending to cause an under damped response in the driver. Meaning the driver will tend to flap a bit creating harmonics much like the sound you get from Tube amps. This will also affect the frequency reponse tending to cause a lift a low frequencies. This does mean that it will sound louder than an 89dB speaker especially in the bass region.
This is in effect the reverse of conjugate loading as it will tend to amplify the effects of the speaker impedance changes.
However in the end if you like it, that is all that really counts, but I would just turn the rails down a bit and take the 4R resistors out or use another amplifer if you want more power.
Regards,
Andrew |
|
|
| danielwritesbac |
| quote: | Originally posted by BWRX
How do you figure the LM1875 will outperform most high-power systems? I don't see anything that allows you to draw that conclusion based on what you stated. |
EDIT: I just received notes over email. There is an error. The application with LM1875, the little efficient hifi driver, and the resistor, results in a sealed box application--with resistor it can't do ported.
Brian,
Compare 86db speakers at 128w for 107db (stereo 110db).
So, an LM1875 system as in teamed with 93db (or so) speakers can, indeed, outperform an average high power system.
I did say "average" and I did say "system" as an amplifier makes no sound until you add a speaker.
EDIT2: I'm sorry that those specifics weren't mentioned.
I think that this table below illustrates what happens if we use efficiency *somewhere* in the 90's decibel efficiency range. . .
Attempt at possibly the correct figures here:
One driver, 12R with resistor, maybe 90db.
MTM, 6R, 93db.
1w, 93db
2w, 96db
4w, 99db
8w, 102db
16w, 105db
32w, 108db
Stereo (2 lm1875, 4 drivers) 111db.
Other ways it outperforms the average hi power system:
1). Non-peakish response means no zobel required in the speaker's crossover (no masking). I wasn't talking about amp zobel.
2). High crosspoint avoids tweeter capacitor in the voice band (no noises at the ear's most senstive frequencies).
3). A more dynamic presentation, from both amplifier and speaker (system) is potentially more helpful to modern recordings.
For #3 compare the awful noise of modern CD source with a high power 128w amplifier pushing a stubborn speaker in contrast to the beauty of the LM1875 on an efficient speaker. I think there's no contest whatsoever.
In a nutshell, your amplifier, if given some good, efficient speakers, can, as a system, present high-end audio, at force, and it can do it on a small budget.
The speaker that I was talking about (above posts) is like the amplifier in that its small, its cute, its affordable, its easy, its hi-fi, and its loud. ;)
I said "hi-fi" and this, to me, means that we're going to be specific on applications. Well, choose any efficient fidelity speaker. EDIT3: I was just trying to get the conversation started on whole system application for the LM1875 amps.
Your designs are great, and the SMD approach is very interesting. This upgrade to the well-loved little amplifier is why the post has more than 4600 views. ;)
gfiandy,
Yes, that makes perfect sense. I had tested this in a sealed box, and without the need for a zobel on the woofer and with the LM1875's talents at driver command, it made quite the presentation, clear, lovely, and it shook the house. ;)
The amplifier's zobel has remained in-place. I wasn't discussing it. Sorry for the confusion. Your writing with the flu is better than my writing on any day.
I knew my math was outta-wack because the little system didn't blow out the windows. Maybe next week? :D :D :D |
|
|
| danielwritesbac |
Well, this (photo) is as small as I could get a PCB on hole-thru components. There were lots of notes about possible sizes of SMD, and I just couldn't figure it which of those were actually available for purchase.
Its one layer. Is the 2" size is okay for having 7 caps | | | |
