4 x IIC PCB for SEQ

[Altitude]

**edited

This is the latest version for the Kobiconn DIN8 connector available at mouser and reichelt. Previous versions removed.

Pinswap fixed

Edited September 27, 2010 by Altitude

[matoz]

it is a very good idea.

Why did'nt you put some midi input?

[Altitude]

it is a very good idea.

Why did'nt you put some midi input?

Additional midi inputs are not supported on Seq4 atm. This is out only

Edited August 25, 2010 by Altitude

[TK.]

Nice idea, I'm interested on a board for my MBSEQ :)

Proposals:

• Currently the jumper settings are ID 10, 12, 14, 16 - I would place the first IIC port at the right, and the last IIC port at the left side (ID 16, 14, 12, 10), so that the ports numbers are in the right order if you look to the sockets from the backpanel side
  
• if people don't like this order, just add the jumpers again ;)
  
• if no jumpers are required, you could also leave out the pull-up resistors and clamp the appr. ID pins directly on Vdd (+5V)
  
• would it be possible to consider a 5th DIN socket (but with 7 pins) at the left side for an optional BLM connector? Distance between the IIC sockets and the BLM socket should be one "left out" socket
  
• distance between mounting holes and "socket side" should be at least 20 mm (like on the MBHP_CORE_STM32 module), or better: 25 mm for compatibility with the MBSEQ aluminum case
  
• add 2 additional mounting holes at the other side for more robustness (it's worth the PCB area)
  
• make jumper J2 compatible with J4 of the core module (the middle pin is used for a receive interrupt, but the MIDI IN option isn't used anyhow)
  

See also my backpanel as reference: http://www.ucapps.de/midibox_seq/mbseqv4_backpanel.png

Best Regards, Thorsten.

[Altitude]

Thanks TK, just the input I was looking for.

5th socket for the BLM connector: is there a diagram for the wiring?

Also, if I read your comment correctly, I can clamp the 5V rail directly to pins 12/13 with no 10K for a no jumper board? (I was wonder about this before laying this out)..

When you say 20mm between mounting holes and "socket side" at least, you are referring to the clearance for the profile in the case correct?

Edited August 25, 2010 by Altitude

[TK.]

5th socket for the BLM connector: is there a diagram for the wiring?

Not yet, but currently it isn't relevant.

It's only important that the socket can be mounted and soldered.

You could add a 7-pin SIL header, the connections can be defined later (there is no equivalent socket on the core module anyhow, cables have to be soldered directly at different places)

This socket could be used for other purposes as well by people who don't own a BLM.

Also, if I read your comment correctly, I can clamp the 5V rail directly to pins 12/13 with no 10K for a no jumper board? (I was wonder about this before laying this out)..

yes, thats allow.

When you say 20mm between mounting holes and "socket side" at least, you are referring to the clearance for the profile in the case correct?

yes

Best Regards, Thorsten.

[Altitude]

Ok,

Here is the revision.

• No jumpers
  
• IIC order changed
  
• holes changed
  
• DIN7 connector added
  

[Echopraxia]

Most excellent!

Where do I sign up :thumbsup:

[TK.]

Please move the BLM connector to the left side of the PCB! :)

(-> right side of the backpanel)

Best Regards, Thorsten.

[Altitude]

Please move the BLM connector to the left side of the PCB! :)

(-> right side of the backpanel)

Best Regards, Thorsten.

hehe. left is in the eye of the beholder :) How's this?

[sineSurfer]

I'd move the left mount holes to the right of DIN7 (between this connector and the others) and move every part but din5 connectors a little bit to the left, including right mount holes.

Both changes just to shave off some pcb width ;)

And, fix the couple of weird angle traces before nILS notices!

[nILS]

You'll prolly run into some problems with the current isolate/track width settings on DIY etching. I'd rather add a few jumper wires than run tracks between pins. Also, most DIY etchers find it hard to etch and drill those small pads - unless you have a really nice way of making PCBs (share it!) you probably want to increase the size ond everything that's copper.

Oh and fix those weird angles!

If you don't mind sharing the .brd, some people (like me) might find it easier to look over it ;)

[Altitude]

SS: Good point about the board size

nILS: Define "weird angles". I can get rid of the traces between the pins without any major changes but the isolate is a big as I can make it before I start getting into problems with the ground plane, what should I have it at ideally?. I also use the "drill assistant" ULP so the final product will have that layer added.

Thanks for the input.

[TK.]

The distance between DIN7 and MIDI connectors is not correct, it seems that you added the size of the clip at the left side by accident:

Best Regards, Thorsten.

[Altitude]

ok, Rev4

Edited September 1, 2010 by Altitude

[nILS]

:tongue: And I always thought I was the only one using windows to measure things!

[vcfool]

Nice! My 2 cents:

Would the extra resistors for the LEDs fit on the PCB? Maybe somebody wants to use them, so they may be a good addition. At least adding only a soldering pad next to pins 6 and 10 of each PIC, without resistors, so one can add the resistors and LEDs if needed. Just a thought...

Then, looking at your PCB vs the schematics, I see you have connected pin 6 of the PICs to J2 (SV6 on your PCB). As far as I see, Pin 6 should be the "Power ON" LED, and pin 7 is the one that should go to J2. Am I wrong?

:)

[Altitude]

Nice! My 2 cents:

Would the extra resistors for the LEDs fit on the PCB? Maybe somebody wants to use them, so they may be a good addition. At least adding only a soldering pad next to pins 6 and 10 of each PIC, without resistors, so one can add the resistors and LEDs if needed. Just a thought...

Then, looking at your PCB vs the schematics, I see you have connected pin 6 of the PICs to J2 (SV6 on your PCB). As far as I see, Pin 6 should be the "Power ON" LED, and pin 7 is the one that should go to J2. Am I wrong?

:)

Damn, good eye. Your right, totally missed that. It should be connected to pin 7, not pin 6. Adding LEDs should not be a problem, i'll look at it tonight..

[TK.]

Unfortunately DIN7 sockets are not available at Reichelt anymore, therefore I've to change the spec: use a 8pin socket

Reichelt Order numbers: MABP 8SN for the print socket, MAS 80SN for the plug

Best Regards, Thorsten.

[TK.]

And here another idea: since the BLM will require an additional optocoupler and some resistors (a common TTL->MIDI IN and OUT circuit), these components could be added to the PCB as well (if still possible)

Best Regards, Thorsten.

[Altitude]

And here another idea: since the BLM will require an additional optocoupler and some resistors (a common TTL->MIDI IN and OUT circuit), these components could be added to the PCB as well (if still possible)

Best Regards, Thorsten.

Done. I routed the pins for convenience with pin one and two being the midi in and out. I suppose one of those 8 pins should be gnd also..

V5 Changes:

LEDs added

MAB08 was MAB07

Added Midi IN and Out

Edited September 9, 2010 by Altitude

[Altitude]

And the Rev 5 Schematic (which I cant attach for some reason)

Rev 5 Schem

Edited September 9, 2010 by Altitude

[TK.]

Thanks for the enhancement! :)

Could you please change SV8 to a 5x2-pin socket header? The layout should match with J11 of the MBHP_CORE_STM32 module (MIDI Link port). MI2 and MO2 can be used as spare pins.

Just to ensure a certain consistency.

The BLM socket and the surrounding circuit should use Vdd from this 5x2 pin socket, and not from somewhere else, so that it is possible to supply the BLM from a dedicated PSU if required.

Vss should be connected together with the ground of the IIC circuit

In order to make it more clear, I created a schematic for this circuit

http://www.ucapps.de/midibox_blm/blm_connector_mbseq.pdf

Please note: the socket is drawn from the rear side, I'm not sure if this is also the case in your schematic (check with the layout view)

And btw.: a typical error is that people swap the MIDI IN/OUT pins when working with Eagle (ask Smash or Nils ;)) - please doublecheck the pinning with existing MBHP_* layouts.

(Update: I compared your layout with the MBHP_IIC_MIDI PCB, it seems to be correct)

Best Regards, Thorsten.

[nILS]

And btw.: a typical error is that people swap the MIDI IN/OUT pins when working with Eagle (ask Smash or Nils ;)) - please doublecheck the pinning with existing MBHP_* layouts.

Hehe, who would do such a thing :whistle:

To clarify that: The reason isn't/wasn't Eagle, but the fact that in TK's schem the MIDI sockets are viewed from behind, which apparently can confuse some simple minded people (like Smash and me obviously). If you wanna be cool, join the fun, be part of the group, swap the pins :yes:

[Altitude]

ok,

double row in place, layout adjusted.

I have the isolate on the small size (16) which may cause some problems for DIY etchers. I can do this no problem but I will release a revision with some jumpers and a 24 isolation as soon as this is done. My window is closing on access to the lab to make these so i want the basic layout done ASAP

As far as pins go, I just go by the numbers. The deltron sockets I use are all numbered..