ClassD Open Source Development Board - diyAudio
Go Back   Home > Forums > Amplifiers > Class D

Class D Switching Power Amplifiers and Power D/A conversion

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 15th February 2013, 07:36 PM   #1
TroelsM is offline TroelsM  Denmark
diyAudio Member
 
TroelsM's Avatar
 
Join Date: May 2003
Location: AARHUS. DK
Default ClassD Open Source Development Board

So here it is: the COSDB (seems that abbreviations are hot in classD ).

I've been looking at this forum for the past 10 years, and never before has so many classD-designs been available for us amateurs. But a lot of these designs apparently don't care about EMC, EMI and switch mode-circuits.

Chokoholic's thread here: SystemD_2kW, any interest for an open design? looks like the most thought-through and ambitious project so far. I have no doubt that Chokoholic have forgotten more about classD than I'll ever know, but I still dare to present an alternative to his fantastic effort.

I'm thinking that "we" need a platform to experiment with classD. The platform I envision shall strive to meet these points:
  • TO220 mosfets on underside of PCB
  • Only tracks on bottom of PCB. Top reserved for GND plane(s)
  • Lots of SMD. 0805 minimum
  • Best possible layout with regards to EMC, but still homemade
  • Regulated supply for mosfet-driver and modulator
  • Daughter-PCB's for: modulator, protection and Mosfet-driver
  • Usable up to +/-65V, 10A minimum
  • Usable as "real amplifier" but focus on development and learning

I've done preliminary schematic and PCB-suggestion. I'm not sure that I'll find the time to actually build the amp, but the design-process is fun as well.

I'm hoping that all the knowledgeable members here will chime in and perhaps someone will make a few PCB's to verify the function.

We can never design a PCB that will fit every need or cater for every wish, - that's simply not possible with classD because space around the critical components are so limited.

The component-values on the presented schematic is not final. Some of them are probably way off. At this stage we are focusing on the connections in the schematic as these will dictate PCB-design.

Click the image to open in full size.

PCB will follow if there is any interest.

Regards
__________________
Need more time...

Last edited by TroelsM; 15th February 2013 at 07:48 PM. Reason: Picture not showing
  Reply With Quote
Old 15th February 2013, 08:48 PM   #2
TroelsM is offline TroelsM  Denmark
diyAudio Member
 
TroelsM's Avatar
 
Join Date: May 2003
Location: AARHUS. DK
A quick look at the PCB-suggestion. All red tracks are on the bottom, Green (looks yellow, sorry) is jumpers on bottom side.

White is (leaded)components on topside, yellow is (SMD)components on bottom.

Click the image to open in full size.

Biggest compromise is the placement of the (big) output coil. The torroid is close to the Mosfets and therefore the switching node is as small as possible. This means that the PSU-caps are pushed away from the mosfets, but tracks are wide and loop-area are minimized. With a solid plane on the toplayer critical loops will be smaller.

On the proposed layout it is possible to place a shield between torroid and control-circuitry. All switchning-tracks and critical components are on bottoms-side and a solid layer on the top-side will confine the noisy parts between toplayer and heatsink.

Do-able, worthwhile or rubbish. Tell me.

Some of the notes used for inspiration:
AN-1135
AN-978
Cool and small 2x150W class D full-range car amplifier

Regards
Attached Images
File Type: png ClassD PCB bottom and comp_1.png (91.2 KB, 493 views)
__________________
Need more time...

Last edited by TroelsM; 15th February 2013 at 08:51 PM. Reason: minor errors, attach picture
  Reply With Quote
Old 16th February 2013, 05:05 PM   #3
diyAudio Member
 
Join Date: Dec 2003
Location: Munich
This is looking like the birth of a nice experimental board.

The footprint of L1 seems to overlap with the pins of M1 and M2. How is this intended in detail?

IRF530 has poor body diodes. Very high Qrr.
Hm, if you really want to use IRF530, you should use shottkys for freewheeling which ensure lower drop than the body diodes at any current. With normal diodes you will not prevent the body diodes from being flooded at higher load situations.
The entire Qrr topic in the half bridges is an interesting area, especially at high loads. IRF530 is for sure a scientifically interesting choice and examining its short comings and possible work arounds as well (gate drive timing and/or shottkys).

If you want the half bridge simple and trouble free - better use MosFets like IRF540Z, with phantastic body diodes and you won't need external freewheeling diodes.
  Reply With Quote
Old 16th February 2013, 08:57 PM   #4
TroelsM is offline TroelsM  Denmark
diyAudio Member
 
TroelsM's Avatar
 
Join Date: May 2003
Location: AARHUS. DK
Thanks for the input.

It might not be clear from the proposed layout, but there are no tracks on the topside below the toroid. The mosfets could be mounted SMD-style without drilled holes at all. - that way of mounting makes replacing the mosfets a lot simpler and the main switching nodes can be completely covered with a solid plane on top layer.

The 530 is just a quick pick from the component library. I'm guessing that IRF530 will only be used for this project if its the only part folks can get. - or if you happen to have a big pile in the stash. I've looked at the mosfet-selection From Farnell and it seems that we can get nice mosfets for 5$ and Ok ones for half.

The diodes from D to S are meant to be fast ones. The symbol is just me being lazy and using the same for all diodes. I should update that. I have a pile of MUR340 rated at 400V / 3A for testing.

My biggest doubt so far is whether I should move the main capacitors closer right up to the mosfets on expense of longer connection to the toroid. Shorter current-path or bigger switching node? I like the current layout, but at the same time it looks like a linear amp layout which is rarely good...

With regards to GND-planes: any experience on the difference between solid gnd-planes and planes divided into:input-gnd, output-gnd and Vss as suggested in the previous mentioned ap-notes?

Keep the inputs comming

Kind regards
__________________
Need more time...

Last edited by TroelsM; 16th February 2013 at 09:00 PM. Reason: terrible spellling and grammar.
  Reply With Quote
Old 16th February 2013, 11:00 PM   #5
diyAudio Member
 
Join Date: Dec 2003
Location: Munich
...still not getting the MosFet-choke-overlap.
More detailed what I am wondering about:
MosFets and torroid are white, means on top.
Consequently also the leads of the TO220 are on the top - but the torroid overlaps with the leads and solder pads.

Fast diodes from D to S:
The internal body diodes remain existing and connected, even if we place additional external diodes.
Both diodes are in parallel, current will split according to the specific diode characteristics and parasitic inductances partially to the body diode and partially to the external diode and if the gate is pulled high also through the N chanel.
The headache starts, when the body diode will be used in a way that the junction stores substantial charge. As soon as I_bodydiode x t > Qrr you can anticipate that the junction is flooded and the D-S-path is acting conductive until Qrr has been removed again. The external diode is only helpful if it can avoid flooding the body diode. Means the external diode does not just need to be fast, but also has to provide a Vf < 0.4V at the concerned current.

Your concern about the position of the large rail caps is correct from fundamental view, but referring to the simulations of my open design , I would not expect issues with your geometry and normal currents (say up to 10..15A).
The positions of your small rail caps and snubbers are good, means correct parametrization should allow operation without uncontrolled HF ringing.
You are doing much better than your shy words make the readers believe!

GND planes:
To me the key are the resulting inductances of the concerned loops and disturbances which are injected from high current areas to the small signal areas.
Typically loops with forward path in one layer and return path right below on the opposite layer are hard to beat and a closed GND plane is often used to provide the closest return paths everywhere. Unfortunately the critical return path is not always GND... So a GND plane alone does not automatically solve all issues.
Your approach is looking OK to me, even if the screw between the MosFets is not fully my cup of tea, because it enlarges the critical loop (M1-M2-C41). The chosen trade offs in a PCB are always sort of a personal signature and overall your arrangement appears OK to me.
Give it a try and see what you like and what to improve in future designs.
I did not experiment with Vss planes.
In my last design , SystemD_MD, I used a GND plane which shaped the different GND areas by a cut. The result was fine from signal integrity - but I have not EMI measurements.
For the open design I am going the next step in evolution.
No cut in the ground plane, but shaping the GND areas by the position of the components and the geometrically resulting current density distribution of load currents. ...still assembling the PCB, so I cannot tell whether reality has understood my theory or not.
  Reply With Quote
Old 17th February 2013, 02:02 PM   #6
diyAudio Member
 
Join Date: Dec 2003
Location: Munich
...or do you intend to place M1 and M2 on the backside, showing with their metal back away from the PCB - and you just used the normal footprint unflipped?
  Reply With Quote
Old 17th February 2013, 07:32 PM   #7
TroelsM is offline TroelsM  Denmark
diyAudio Member
 
TroelsM's Avatar
 
Join Date: May 2003
Location: AARHUS. DK
Yes, M1 and M2are indeed placed on the bottom-side with metal-back away from the PCB.
Yes, I was to lazy to correct the footprint.
Yes, I will/should correct it:-)

Could you please elaborate on why the single screw will make the loop larger? I haven't done any high-current switchmode like this and I'm probably missing a point somewhere.

About the body-diode: I see the problems, but lack experience with it. Any hints as to where I find some good info on it?

Thanks again for the valuable input.

Kind Regards
__________________
Need more time...
  Reply With Quote
Old 17th February 2013, 10:18 PM   #8
diyAudio Member
 
Join Date: Dec 2003
Location: Munich
Single screw:
The issue is less the single screw, but its position inbetween both MosFets.
In order to minimize the geometry of the loop M1-M2-C41 it would be most fortunate to place both MosFets close together.
But no need to panic, your geometry already has a reasonably small loop. Shifting the screw away and moving both MosFets close together would theoretically reduce the loop inductance, but the visible difference in unsnubbered ringing frequency and unsnubbered damping would be small.

Body diode and reverse recovery:
Strolling through the google hit list - this paper appears to describe the issue pretty fine.
bbs.dianyuan.com/bbs/u/41/1148348695.pdf
  Reply With Quote
Old 17th February 2013, 10:48 PM   #9
TroelsM is offline TroelsM  Denmark
diyAudio Member
 
TroelsM's Avatar
 
Join Date: May 2003
Location: AARHUS. DK
PCB-update:
-Changed footprints for M1 and M2.
-Different placement and routing around Regulator for Vss-Low
Click the image to open in full size.
__________________
Need more time...
  Reply With Quote
Old 21st February 2013, 09:50 PM   #10
TroelsM is offline TroelsM  Denmark
diyAudio Member
 
TroelsM's Avatar
 
Join Date: May 2003
Location: AARHUS. DK
So, I thought about other possible arrangements of the critical paths around the mosfets and tried a layout that optimizes the layout with regards to lengths of loop: M1-M2-C41 and at the same time minimizes the area and length of the switching node.

I'm keeping the possibility of a solid GND-plane above the mosfets and that limits me a alot.

Downsides with this layout: longer paths for free-wheling diodes and longer paths for snubbers. The diodes might not be nessacary in the final design and I havn't been able to simulate the influence of some additional 10-30nH in the snubber-loop.
Click the image to open in full size.
What do you think?

Kind Regards
__________________
Need more time...
  Reply With Quote

Reply


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

Advanced Search

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

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


Similar Threads
Thread Thread Starter Forum Replies Last Post
Volume / Source selector - open source project ? AuroraB Analog Line Level 22 22nd September 2012 02:21 PM
Crystal CS5501 A/D development board Bargain UK gbullimore Swap Meet 2 16th January 2011 05:31 PM
Open call for suggestions on Open Source DIY Audio Design gfergy Everything Else 1 15th April 2007 07:33 AM
DSP development board suggestions starn02 Digital Source 0 14th April 2006 07:06 AM
Development board Atmel ATmega Freddie Everything Else 1 16th August 2003 03:27 PM


New To Site? Need Help?

All times are GMT. The time now is 01:29 AM.


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

Content Relevant URLs by vBSEO 3.3.2