Bulding My first class D amp.

ranga

Member
2007-12-18 8:39 am
Hello forum users! I am quite new to this forum but not that new to electronics. During high school the electronics microbe infected me. Since then (i am 26 now) i have made a lot of diy.

This how ever is my first Class D amplifier project! I have chosen this schematics, found in attach. I can not relocate the url :D

So, first of all the components i am going to use are: lm311 as comparator and LF356M as OpAmp. This is not because i think it is better but because these are the ones i have.
I have also found a mistake in the Integrator schematics: pin 3 of IC2A goes to gnd. and the entire net that connects to it.
I am going to use smd tehnology: 0603 for resistors and 1206 for capacitors in the input stages and normal components in rest. I have designed a pcb (not final version yet).
Please have a look and if any-one spots a mistake please comment. Also, if this schematic has been commented here can someone point me to, because i did not found anything for myself
Thank-you.
 

Attachments

  • scheme.zip
    38.5 KB · Views: 472

ranga

Member
2007-12-18 8:39 am
the pcb

I can not attach all the pcb layouts so i am using a hosting:
here it is:
[IMGDEAD]http://i30.tinypic.com/ezr9jo.png[/IMGDEAD]
[IMGDEAD]http://i29.tinypic.com/2ed2zq1.png[/IMGDEAD]
[IMGDEAD]http://i28.tinypic.com/25qrsz8.png[/IMGDEAD]
[IMGDEAD]http://i27.tinypic.com/28hkb5w.png[/IMGDEAD]
[IMGDEAD]http://i30.tinypic.com/k0ips2.png[/IMGDEAD]

I have a splash spill on both sides that represents the gnd but i did not show it in the pictures. The gnd rail is highlighted on the copper side in some of the shots.
If any body would like to have the kicad .brd and .sch please contact me!
 

ranga

Member
2007-12-18 8:39 am
Thank you

I have read the pdf! Very good info in it. :bigeyes:

All capacitors that are not smd or electrolytic are tantalum capacitors. The driver schematics is the one recommended by International Rectifiers for IR2110. Old design may it be but i would like to go with it because it is my first class D and so it is more to learn out of than to actually use it.
The trouble to change the schematics is this one: I have already purchase all the components (resistors, capacitors, semiconductors... even a 3kva toroid transformer and the electrolytic capacitor for the power supply (about 40 x 330uF/200v)) and i have to go around with them.

I am currently working to minimize the high current loops on the pcb. I don't think that i will be able to do much good in this section except to try to isolate them from the rest of the tracks. Updated pcb coming up soon...
One question though... i am missing only few components :the 74ac04 in smd package and the toroid core for the output inductor. Can i use yellow toroids for it, cause i have a lot of those (pwm frequency is 400-500 kHz) ? I saw the post's made by Eva regarding this topic but i am sure I didn't saw: "Don't use yellow cores for Class D output filter" anywhere. I also have a lot of "E+I" ferrite cores used in computer power supply, but i reckon that they are worse.
 

ionutgaga

Member
2006-07-03 12:36 pm
You can use 3f3 gapped toroidal core (by hand) - white (tips: search metrafo dot ro), or you can order a samples from micrometals.com (like i did) - T200-2 red/clear.
Take care at max voltage of your fet's. Read on this forum why bootstrap technique is causing trouble at clip condition. You should note that this design is not very scalable (like you want to try).
 
I'm sorry to say this but you have very much to improve in that layout. Ordering this PCB as shown would be a waste of money.

You can attempt to use yellow/white cores (micrometals #26 iron powder and equivalents) but core losses are likely to be too high resulting in a "burning hot" working temperature and very short life of the core and anything around it. This is unless you use a really big amount of turns to keep peak magnetic flux low, but then you are likely to end up with too high an inductance for full range usage. For a first try you can use the #26 cores without problem (as long as you turn power off before they melt :D:D:D )

Search a bit the forum and you will find info on inductor flux, turns, saturation and losses calculations, and on web sources for cores suitable for class D.
 
Eva said:
I'm sorry to say this but you have very much to improve in that layout. Ordering this PCB as shown would be a waste of money.

You can attempt to use yellow/white cores (micrometals #26 iron powder and equivalents) but core losses are likely to be too high resulting in a "burning hot" working temperature and very short life of the core and anything around it. This is unless you use a really big amount of turns to keep peak magnetic flux low, but then you are likely to end up with too high an inductance for full range usage. For a first try you can use the #26 cores without problem (as long as you turn power off before they melt :D:D:D )

Search a bit the forum and you will find info on inductor flux, turns, saturation and losses calculations, and on web sources for cores suitable for class D.

eva,

what's the difference with yellow/white cores and light green/yellow cores? from what I can tell, they are also powdered metal. and while we're at it, what about light green/red? I have lots of those over here. :D
 

ranga

Member
2007-12-18 8:39 am
http://i32.tinypic.com/21jx3zb.png
http://i30.tinypic.com/30kwwus.png

I have shortened the high current loops, and by moving the components closer together i think i can shorten them some more. I placed the capacitors as close as possible to the power MOSFETs . I have separated the high current section from the low current section as best as i could. I still have some limitations in design because i have to keep room for heat radiators and IR made their mos-fet with the G terminal so close to the D and S terminal :cannotbe:

Seriously now: i will try to improve the layout but i am not sure how much will be possible considering the limitations that i have(the shear size of the electrolytic capacitors rated at 200V for example) . I will separate the low current zone by making a screen out of aluminum or copper foil that i will ground. I also made a star like ground for low level current side and another for the high. i will connect these 2 in a single point at the power supply. Also i will splash the gnd and -Vcc as described in the pdf posted upper. Also studying the bootstrap 10uF capacitor suggestion right now.

@ eva: I am not ordering anything. I am making it using photo method. Drill it with my CNC and manually construct vias.

Regarding the inductor core... i will make tests using what i have and supply with +/- 25 V on the rails. After that i will order some high quality cores. If i finish before this weekend the design part than on Monday i will have the pcb corroded and some stages already on it.
 

ionutgaga

Member
2006-07-03 12:36 pm
There is no need to put 200v big electrolytic caps in proximity place of your mosfet. Tips: 2-3 smd cap 0.1uF + 220-470n/MKP + 10uF.
If you do not have a limiter/compressor or a special modulator to obtain controlled duty cycle (max at say 95%) you cannot use bootstrap technique on hard clipping without flames of different colours... Maybe you should try a charge pump with NE555 on high side, or Workhorse technique, or floating smps supply.
 
The layout can be improved further, it's true that you have rearranged it but you still run into most of the previous pitfalls. I think you are not understanding some key concepts. Some hints:

- Have you ever read about continuous ground planes? In high performance class-D you need one of these, but yours is full of cuts so it's mostly useless.

- Star grounding only works at audio frequencies, for RF it's mainly useless. A reasonably low RF impedance is only achieved when current is made to flow in opposite directions through continuous conductive planes in opposite PCB layers. The RF inductance of conventional PCB tracks is not negligible and increases considerably for smaller widths, so supply traces should be as wide as possible and should have a return path in the opposite PCB side (that may be just a continuous ground plane).

- Capacitor paralleling is evil, particularly when you mix several types and sizes because it results in several supply impedance peaks and long ringing tails excited by every switching event, and thus very noisy rails. This is terrible for audio. You have to place the switching MOSFETs as close as possible to a small bank of parallel electrolytics. Paralleling medium-sized same value-electrolytics cuts inductance dramatically, it's far more effective than films or tantalums (forget abot this junk). Ceramic chip capacitors placed directly at switching MOSFET solder pads are the final touch. Small electrolytics may be required to damp the resonance between ceramics and the bank of electrolytics. The most critical RF loop is the cross-conduction one, so think a bit about how to improve it...

- Supply inductance (from layout and capacitors) and MOSFET package inductance (from legs and bonding wires) will ring with MOSFET internal die capacitance. RC snubbers are required to damp this mess. You can model the resulting LCLC networks (with data from datasheets) and find component values of suitable RC or RLC dampers.

- Most of the RF is radiated by wiring rather than by the PCB and components, but I don't see any RF filter in your supply rails. You need pi filters in the rails.

- A LC lowpass filter with too much parasitistic inductance in series with the capacitor will happily leak plenty of RF to the output. Be careful with filter capacitor package choice and layout.

This page is fun to read:
http://www.audioholics.com/educatio...ics/switching-amplifier-class-d-basics-page-2
 

ranga

Member
2007-12-18 8:39 am
ionutgaga said:
There is no need to put 200v big electrolytic caps in proximity place of your mosfet[...]Tips: 2-3 smd cap 0.1uF + 220-470n/MKP + 10uF
VS
Eva said:
- Capacitor paralleling is evil, particularly when you mix several types and sizes[...]You have to place the switching MOSFETs as close as possible to a small bank of parallel electrolytics. Paralleling medium-sized same value-electrolytics cuts inductance dramatically, it's far more effective than films or tantalums (forget abot this junk). Ceramic chip capacitors placed directly at switching MOSFET solder pads are the final touch. Small electrolytics may be required to damp the resonance between ceramics and the bank of electrolytics. [/B]

This two snippets slightly contradicts each other.
-330uf/200v capacitors are big and there is nothing i can do about it! I will instead replace them with 2*47uf types that are not that much space consuming.-I have in the schematics 100nf ceramic parallel with them, but on the pcb i chosen to place them as close as possible to MOSFET transistors.
-I will add CLC low pass filters on the rails (PI filter).
-About cross-conduction there is no issue that i know of for this schematics. So i will have to build it first and see after. Correct me if i am wrong. I will re-study the ir2110 application note and datasheet.
-Continuous ground plain is my focus right now.
Update after all this is done...
 

ranga

Member
2007-12-18 8:39 am
much better

I inserted 2 pi filters on the rails! 2*C+1*L for each. Haven't yet decided the values but i guess that experiments will tell.
I now have short and thick rails. I also now have a splash gnd on the copper side that is continuous and uninterrupted. I replaced the capsules of the huge capacitors with 2 parallel small (but tall) capsule 47uF/250v.
I also have space for a heat sink that will act like a screen between the low and high current sides.
[IMGDEAD]http://i29.tinypic.com/110f13t.png[/IMGDEAD]

I am now reading about cross-conduction, bootstrap and the other advices i received, but i am note sure that i am able to make the decision to modify the schematic in a good way. All i know about class D i read, no practical experience. The only encounter with PWM was with an all2old 555!


Thank you guys (and Eva)! I-ll get back on theory now.
 

ionutgaga

Member
2006-07-03 12:36 pm
You should minimise the curent loop at the gate of mosfet. Run in parallel (close proximity) the 2 traces representing signal from gate and source to the IR2110. Also, take the signal for pin 5 (Vs) from source of high side mosfet, not drain of the other; put pin 2 on source of low side mosfet; feedback take from other point, not drain of mosfet - the best is at L pin...

Like Eva said, you should read some theory about high speed pcb.
Read about local loops and how to minimise this...
 
Hey, this is looking really much better now (and simpler!) Auto-routers are ugly. I suppose you found some of my published layouts ;)

You may want to put two or three 100nF capacitors in front of each MOSFET instead of one. This further reduces leakage inductance. The closer the capacitors are placed to TO-220 leads, the better, but remember that the current has to flow through the ground plane too, so the closer the two MOSFET are placed the better too.

Remember the RC snubbers between D and S.

Do you think that your inductors are going to fit in the space that you left for them? I hope so...

Concerning cross-conduction, it always happens in some degree. MOSFETs have d-s capacitance (that becomes high for low Vd-s) so when one device turns on, there is always a short current spike from one rail to another even if the other device was dead off. Then we have diode reverse recovery, this will also cause sharp current spikes flowing from one rail to another when the body diode is "asked" to stop conducting. These spikes should be confined in a small loop, they will (and should) tend to flow through the 100n capacitors.
 

ranga

Member
2007-12-18 8:39 am
let' see:
- rc snubbers: Added 500pF with 10 ohm as chocoholic did for his design. Checked!
-Bootstrap... Apparently i had in schematics a 330 nF one... i will twik it's value ... Checked!
-Yellow ferrite cores for toroid output filter are in fact ... well... yellow, so it does not fit the color code from micrometals. I will live an see how they behave. They are recovered from old computer SMPS's.
-PI filters for rails, i will use same cores as for the output filter and 100nf capacitors. Yes they will fit nicely (15.5 x 45.5 mm clearance). Checked.
-Added ceramic capacitors for the rails of IR2110 right next to it. Hope they will do.
-Splash gnd, uninterrupted for the high signal area. Checked!
-Power mosfet as close together as possible and decoupling capacitors as close to them as possible... Well let say checked but i will solder some caps right on their terminals. I am not sure about it for now.
- Minus rail is splashed under the IR2110 ... done but is very interrupted so i have to improve this.
-Regarding the feedback route that Ionut suggested... well ... the only way for me to do that is by putting a via and so braking a little the splash gnd continuity. I have to make a decision.

Thanx for the help given so far. If it works i will publish schematics and pcb in cad format.
Hope i am not missing anything....

I did not use an auto-router for the first, ugly pcb layout and nor i found any of your published layouts Eva! It was only me all along. I will search the web for your work, starting with diyaudio before corroding this pcb.
here it is... :
[IMGDEAD]http://i30.tinypic.com/vp9r3o.png[/IMGDEAD]
No splash zone is displayed in 3d mode but there sourly is one! Final touches tomorrow and in the weekend i will corrode it. Actually what i want from this amp is knowledge and for it to be solid (protections will be added) and powerful, not necessarily HI-FI. It will be used (if so) in a small biker bar playing heavy metal. So noise is not that important :cannotbe: :cannotbe:
For home i have a nice 30W class A amp :angel:
 
In the right side you have a long cut in the ground plane that you could avoid or convert into a smaller cut in another place. Consider for example crossing supply traces in the middle of the capacitor bank and swapping right side inductors. Also, you don't need or want a too high inductance for rail filtering, the offending frequencies are above 10Mhz (and particularly above 30Mhz) so one or more ferrite beads are usually enough. Always study resonance of LC systems, you don't want high Q ringing generators ;) Oscilloscope will tell you if your supply rails are calm or not.