Jump to content

AOUT_V2 pcb design


illogik
 Share

Recommended Posts

Hey guys, long time.. haha

I havent been active here for a while but did a lot of midiboxing last year, finally built a seq and helped a friend with building one.. needless te say here but still : really nice!!

Anyway, I need to build a few AOUT modules for the 2 seq's and a midibox_cv2 so I decided to have some pcb's made.

I had contact with northernlightx from the forum a few years ago; he was busy with designing a new pcb for the mbhp_AOUT module (max525 version). He had some made but didn't work; he sent them to me so I could help. I found that there were a couple of mistakes on the pcb; had to cut too much traces and the layout wasn't good (confusing, no names/labelling).
Let me say: for me this aout pcb is really something that has to be good quality; ie. clear, efficient, optimized to produce the best signal possible: because it is central in my setup; it provides the connection from midi to modular synthesis AND because it is quite an expensive module (max525ACPP around 35 euros); so that is why i'm quite critical about this pcb.

So I decided to make a new pcb for the AOUT module which I will have made at OSH park soon, but I think if it is a good design it could be put on ucapps as the AOUT_V2 pcb.
So before I have them made, I thought to share it here and see if I forgot something, should do something different etc. If so, let me know so I can make some adjustments/improvements and order some boards. I will then of course build and test them and report back here..

If they work correctly the design can be put on the site as the (long awaited) AOUT_v2 pcb

These are things I had in mind while designing:

-how to adress analog/digital ground stuff

-clear labelling of test points, components, trimmers, in- and outputs

-clear layout, enough room for trimpots that are a bit bigger

-all connectors should be (2x5) IDC connectors

-bipolar option will be possible with extra hardware; more on that later

-power led not included

The design shown below is just to get the idea and to see the stuff I find important. Im actually working on another version with different/better tracing. I'll add the eagle files so you can have a better look.

AOUT_OSH.thumb.png.b42872a26d9d824d690b3

-how to adress analog/digital ground stuff

so I used top and bottom ground planes; top ground plane is analog ground, bottom has 2 groundplanes, the biggest on the right side is analog ground, the smaller left plane is digital ground.
I have the 6007b placed on top (original was bottom); the area on the bottom around the 6007 has no ground plane to avoid capacitance problems.
About tie-ing grounds; he max525 datasheet says connect the 2 grounds together close to the max535 to the best ground trace. JP5 and JP6 connect the grounds together (should I keep this? Have them to be safe because I dont know anything about the math or processes that are involved with proper grounding, I just try to learn& apply the best grounding practice)
I have jumpers JP1 and JP2 so you can decide if you get digital power from the power connector (CON2) and send it to your core (with CON1) or if you only get analog power from CON2 and get digital power from the core (CON1).

-clear labelling of test points, components, trimmers, in- and outputs
-clear layout, enough room for trimpots that are a bit bigger

-all connectors should be (2x5) IDC connectors

first off, I made some icons with pin names next to all of the IDC connectors. I see that in the image above half of the pin names don't show up but ill fix that.

I didn't make separate test pins for calibrating the outputs because the RX-* resistors are perfect for that. Note the labels inducating the CV out number.

The trimpots are in order; top to bottom is cv out 1 to 8. There is room around the trimmers so they can be a bit bigger.

Also the IDC connector for the outputs (CON3) has the outputs in order. Pin 1 to 8 of connector are CV out 1 to 8.

-bipolar option will be possible with extra hardware;

 so I thought A LOT about this since years ago I tried making the bipolar option and had problems. I know for sure that it is possible to make some hardware that will let you switch between an offset of +/- -5V and 0V. (there was some talk about this in the CV-V2 thread and maybe some other forum pages) I would guess it would be possible to make it so you can decide on a patch/preset level wich output should be bipolar; this would be the best approach for me. If I want to send notes to a module want an unipolar out but if im controlling other stuff a bipolar would sometimes be better. But I wouldn't know how to program that so i'm just putting the idea out there.

In practice the expansion hardware could be basically an 2 input inverted opamp mixer with matched resistors for the so you have a gain of exactly 1 on both channels. One mixer input will be the calibrated cv output from the AOUT pcb and the other mixer input should be a signal (provided on the expansion pcb) that you can switch from 0v (unipolar) to -5V (bipolar).To make a stable -5V you could use a zener voltage regulator, and then there should be some kind of digitally controlled switch that can be controlled by a DOUT pin to send either 0V or -5V to the opamp. Haven't designed this yet but should be easy.

The output of the inverting mixer should be inverted again.. Of course you could think; use an non-inverting mixer, but the gain formula of that is not so straightforwrd and I think that was the reason for my problems with using the original bipolar expansion.. But if anyone has a better option; less opamps is always better I guess.

Few questions on this: should we take the calibrated, amplified CV outs or the direct outputs of the max525? I those the first option because then it is a true expansion as in you can use and calibrate the AOUT standalone and just add the expansion if you need it.

To implement the opamp mixer correctly it should have a gain of exactly 1 otherwise the calibrated voltage will be off. Do you think we can do this by using precisely mmatched resistors? 

Hmm sorry that was maybe a bit much about the possible expansion.. now back to the AOUT

finally some questions I still have about the AOUT_v2 pcb design:

-should the 2 gate outputs be there? I guess so right, doesn't cost a lot and you have some visual aid to see if the module is responding to midi/core

- should there be a connector for chaining th SPI port (dunno if I name it correctly) but like port J2 at the original out module? Is it ever possible to chain more AOUT modules together? I did put it in the design (CON4) but don't know if I did the connections right; maybe someone could check that?

Allright guys lemme know what you think..

cheers, marcel

 

 

AOUT_V2_prot.zip

Edited by illogik
image didn't show up
Link to comment
Share on other sites

  • 4 months later...

Hi, somehow I missed your post.

I'd make the following points about your design:

  • Ground scheme/trace layout isn't the best, the digital stuff has free reign to interfere with the analogue by way of coupling through the top layer plane.
  • Some quite thin traces (10mil), going through capacitors and the like.
  • Power connector is non-standard (suggest a Eurorack 2*5 DIL or polarised Molex SIL). Also note that the "digital power and ground" comes in on J19 (CONN1 on your layout); but I notice jumpers for connecting/disconnecting these.

 

In the meantime I've come up with my own solution:

It's a four-channel board and uses two quad op amps for this. But you get range and offset switching plus a fine tune control out of the box. It stacks with an associated control board with 3.5mm jacks that also carries DOUT gates and indicator LEDs. To be honest, I think the switching can be done manually, presumably as you re-patch at the same time anyway. While it could be done with a digital IC (or FET perhaps?) the risk is that you inject digital noise into the sensitive analogue summing node (op amp inverting input). My concept also uses a switch pole to add/remove a resistor from one op amp stage, which varies the gain. This would be expensive (and a bit risky in terms of noise) with an analogue switch IC. Maybe vactrols would work :), but I made do with mini DPDT switches and indicator LEDs.

@Altitude also did a fully SMT version with eight channels, all DOUT gates, extra triggers and clocks on the one board.

To be honest, I'm not sure how much interest there is in these MAX525 boards. I think the price of the DAC puts people off, even though it has better linearity than TLV5630. If users are keen I'll do a run of them, otherwise I get personalised CV for myself :).

Best,
Andy

 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

Loading...
 Share

×
×
  • Create New...