Anyone interested in an Altera DE1 to 68000 socket adapter?

[Shadowfire]

I'm getting ready to spin a pair of custom board to allow the Altera DE1 dev board to plug into a 68000 socket (as present on the A500/A2000).

The first board is a 2-layer board that plugs into the 40-pin headers on the DE1, which converts them to 80-pin .050" headers with interleaved ground wires.

The second board is a 4 layer board with solid ground and power planes (which I've already done up, but I'm tweaking the layout and routing right now) that accepts the two 80 pin cables, routes the signals out to quickswitches for 5V-3.3V voltage level translation and converges then to a 64-pin-dip header that you can plug into a 68000 socket. As designed it should plug into an A500 or A2000.

I'm thinking about supplying schematics, both boards, a pair of 8" 80-pin cables, and a .csv file for the DE1 pinouts to map them to the signals on the 68000 socket. It's going to be about $100 for the whole deal, assembled + tested.

I believe that the DE2 has expansion headers with a similar pinout, and should work without modification, only the FPGA pin assignments should need to be changed.

The DE0 also has a pair of expansion headers, but is based on the Cyclone 3, and I don't have access to the schematics to verify that the pinouts are the same as on the DE1.

This will allow you to plug a DE1 development board into the 68000 socket of any machine. There is no software or support of any kind supplied, other than the schematic and DE1 pin mappings. If you aren't sure what this is all about, then you should pass on this. It is a tool for mid to advanced level hardware/fpga hackers. I anticipate only two extra sets of boards will be available.

[rkauer]

I may be interested. Price?

[coze]

hmm, yeah I would be interested too !

[RedskullDC]

Hi ShadowFire,

Originally Posted by Shadowfire

The DE0 also has a pair of expansion headers, but is based on the Cyclone 3, and I don't have access to the schematics to verify that the pinouts are the same as on the DE1.

DE0 GPIO pinouts are the same as DE1/DE2/DE2-70 models.

Why not bring the pins out to an 86pin edge connector, to plug onto the side of an A500 instead of the 68k socket?

Then you have acess to a few extra signals which can be handy when taking over the machine: _OVR etc.

Cheers,
Red

[Shadowfire]

Price seems to be $100, for the two custom boards, components & cabling. (Mill-max sockets, Samtec headers, etc.). I am planning on doing the boards through www.expresspcb.com (a 2-layer miniboard pro for the 40->80 pin converter board, and a 4-layer miniboard pro for the voltage converter).

I'll be ordering parts soon and will post gerbers once I've verified all the footprints (see below), so that you can get an idea of what it will look like. I'm also debating a more robust +4.3V supply than the 1N4148/resistor recommended by IDT for the quickswitches.

I'm going to rejig the voltage board to pull the remaining 12 signals off the header (currently I'm running 60 I/O's to the appropriate lines on the socket) and run them thru the level shifters to a .100" header, but I won't be installing the quickswitches or header for them. I would like to include an actual 68000 socket, but there's no guarantee since it's already pretty cramped on a 2.5" wide board. But, what I talked about in the first post is the absolute minimum feature set.

Redskull, an 86-pin socket would limit the board to attaching to A500's. The 68000 socket configuration is far more useful to a hardware hacker... a LOT of things other than the A500 used 68000 microcprocessors. The DE1 was a nice, cheap dev board with SRAM, SDRAM, flash, an SD card slot, video out, rs-232, and audio in/out, switches/buttons/led's, onboard USB programmer, etc. (basically an ideal platform for designing hardware expansions). Part of the problem of hooking these things up is signal integrity, you can hack a pair of 40-pin cables up to a 68000 socket and do almost the same thing as this, but this solution is going to be way quieter/stabler than that.

[RedskullDC]

Hi Shadowfire,

Originally Posted by Shadowfire

...an 86-pin socket would limit the board to attaching to A500's. The 68000 socket configuration is far more useful to a hardware hacker... a LOT of things other than the A500 used 68000 microcprocessors. The DE1 was a nice, cheap dev board with SRAM, SDRAM, flash, an SD card slot, video out, rs-232, and audio in/out, switches/buttons/led's, onboard USB programmer, etc. (basically an ideal platform for designing hardware expansions). Part of the problem of hooking these things up is signal integrity, you can hack a pair of 40-pin cables up to a 68000 socket and do almost the same thing as this, but this solution is going to be way quieter/stabler than that.

Didn't realise you had other 68k targets in mind aprat from the Amiga. Go for it!

Preaching to the converted regarding the virtures of the DE1.
I have a DE1 and DE2-70 this end. Lots of fun

Incidentally, in case you weren't aware, in the last few days Terasic have added a place holder for a Cyclone IV board on their website. Front page graphic says "DE2-115".
Should prove to be most interesting!




Cheers,
Red

[FrenchShark]

Hi,

I am interrested too.
An FPGA accelerator will be fun for my A2000.

Regards,

Frederic

[Shadowfire]

I didn't know that they had started shipping the cyclone 4's yet. Spot check: Digi-key is now showing listings but doesn't have any IC's in stock. Newark is showing a lead time of 30 days.
BTW, Gerbers and schematic will be posted for those who miss the initial order.

I remember checking the Cyclone 4 and I recall reading that the C4's have a maximum I/O tolerance of 3.0V. This is getting close to 2.5V. The quickswitch VCC's could be dropped to 4.0V to support this, but the C4 is going to have less of a noise margin for high level signals.

[FrenchShark]

Originally Posted by Shadowfire

I didn't know that they had started shipping the cyclone 4's yet. Spot check: Digi-key is now showing listings but doesn't have any IC's in stock. Newark is showing a lead time of 30 days.
BTW, Gerbers and schematic will be posted for those who miss the initial order.

I remember checking the Cyclone 4 and I recall reading that the C4's have a maximum I/O tolerance of 3.0V. This is getting close to 2.5V. The quickswitch VCC's could be dropped to 4.0V to support this, but the C4 is going to have less of a noise margin for high level signals.

The Cyclone III has the same issue. The chip is a lot better at driving 2.5V and 3.0V I/Os than 3.3V I/Os.
The Cyclone III and IV are indeed very similar. For the moment, just the C4 GX is available in small quantities, the C4 E is not available yet.
The C4 E has also a Vcc Int of 1.0V only

Regards,

Frederic

[Shadowfire]

Finally got the board down to 350 vias, had to change out the header strips for clearance problems, which needed a bit more tweaking of the board routes (new strips had .025 square posts instead of .025 round posts, requiring larger pads, making clearance violations on tracks which were already routed there, etc.)

I'm working on prettying up the board. I managed to stick in the 68000 socket, and the remaining 12 signals from the DE1 header also go through more Quickswitches then out to a 16-pin .100 header, so you can tap out other signals if you want. Going to place an order at Digikey and Newark this weekend to get some parts and verify footprints.

[Shadowfire]

OK, for those of you who expressed interest, the preliminary schematics/layout for the voltage converter board has been posted in the Zone. It's a 3.8" x 2.5" 4-layer board. I managed to get it within ExpressPCB's criteria for a mini-board, including the pass-through socket for a real 68000, a header for the extra 12 signal lines (all running through a quickswitch), as well as layout for a 4V quickswitch power supply for the Cyclone 3 / Cyclone 4 boards. Should be possible to swap zener/resistors on that circuit to put almost any arbitrary VCC up to 5V on the quick switches.

I'm prepping to do the interface board, right now plan is for dual -layer, with bottom side a ground plane, and jumpers in each signal line that you can cut and install an 0603 resistor if you want additional termination. Will post that as soon as I am done with it.

[rkauer]

OK, now I can start to drooling or I must wait a little?

[Shadowfire]

These things take time when they aren't your day job. I like to do quality work, as you can see. Therefore, the boards won't be done overnight
5/3: Parts ordered from Digikey and Newark. Digikey is out of stock of SM 10K 0603 resistors :/ FYI, parts and connectors for both boards came to almost $100 (no extra connectors, some extra passives/quickswitches, and I forgot to order a pair of 80 pin cables).

[Shadowfire]

Comment                        Description                              Designator                        Qty Supplier  Supplier Part Number
Parts for Voltage converter board....
Cap SM 0603 .1uf 10V          Johanson Dielectrics 100X14W104MV4T       C1, C2, C3, C4, C5, C6, C7, C8    8   Digi-Key  709-1101-1-ND
Diode SM SOD223 1N4148        Fairchild 1N4148WS                        D1                                1   Digi-Key  1N4148WSFSCT-ND
Header Male SM 80pin .050     Samtec FTSH-150-01-L-DV (80 pins)         J1, J2                            2   Digi-Key  SAM1161-50-ND
Socket DIP 64pin              Millmax 110-44-964-41-001000              J3                                1   Digi-Key  ED90061-ND
Header DIP 64pin              Samtec TS-132-T-A                         J4                                2   Digi-Key  SAM1050-32-ND
Header Male 16pin             Samtec TD-108-T-A                         J5                                1   Digi-Key  SAM1114-08-ND
Res SM 0603 10K               Vishay CRCW060310K0FKEA                   R1, R2                            2   Digi-Key  541-10.0KHCT-ND
IC SM IDTQS3384 QSOP24        IDT QUICKSWITCH QS3384                    U1, U2, U3, U4, U5, U6, U7, U8    8   Digi-Key  800-1739-1-ND
LT6200CS8                     Linear Technology LT6200CS8-10#PBF        U9                                1   Digi-Key  LT6200CS8-10#PBF-ND
MAZS039GHL                    Panasonic MAZS039GHL                      ZD1                               1   Digi-Key  MAZS039GHL CT-ND

Parts for Interface board...
Header Male SM 80pin .050     Samtec FTSH-150-01-L-DV (80 pins)         J1, J2                            2   Digi-Key  SAM1161-50-ND
Receptacle, 40pin .100        Harwin M20-6112045                        J3, J4                            2   Newark    03M3404

[Shadowfire]

Final gerbers/schematics/BOM has been posted to the zone for the Voltage coverter board. I will press Go on the boards later on this week.

Parts in small quantities are expensive. Contact me if you want a preassembled board. I can pass through board costs + shipping if you want to source your own components and solder your own board. There are some caveats. I can give you a pair of each diode 1N4148, 4.0V, and 4.3V. (I purchased 10 of each, and will likely never use any of the spares again...)

1. Some of the components, especially the 68000 socket & the 12-pin header, have been designed around Mill-max (i.e. *round* .025") pins and .025" square pins will not fit. Also, the layout is designed to fit inside a mill-max 64DIP.900 socket, other sockets may need to have the interior cut down. J1/J2 pads have been enlarged, maybe you can find a cheaper SM .050" dual header to put on there, the ones I speced are over $8 each in quantities < 10. When cutting down the headers, I recommend cutting it down to 82 pins then removing the last two carefully with needlenose pliers.

2. J4 header as specified fits great, other headers may need to have the tails cut down since there is minimal space betweent the board and the socket on the front side.

3. The diodes are really >>small<<. They are SSMINI-2 and SOD323F foot prints. I will be using my 30X microscope to attach these to my board, but you could probably get by using 10x or 8x mangification.

4. The rest of the parts are .5mm pitch, .050" pitch, or 0603 components. They aren't terribly difficult if you know how to solder surface mount pieces.


I've also done a bit of work on the 40->80 pin converter board. 0603 resistors are too big, so I will have to go at least one size smaller for optional termination resistors.

[FrenchShark]

Originally Posted by Shadowfire

Final gerbers/schematics/BOM has been posted to the zone for the Voltage coverter board. I will press Go on the boards later on this week.

Parts in small quantities are expensive. Contact me if you want a preassembled board. I can pass through board costs + shipping if you want to source your own components and solder your own board. There are some caveats. I can give you a pair of each diode 1N4148, 4.0V, and 4.3V. (I purchased 10 of each, and will likely never use any of the spares again...)

1. Some of the components, especially the 68000 socket & the 12-pin header, have been designed around Mill-max (i.e. *round* .025") pins and .025" square pins will not fit. Also, the layout is designed to fit inside a mill-max 64DIP.900 socket, other sockets may need to have the interior cut down. J1/J2 pads have been enlarged, maybe you can find a cheaper SM .050" dual header to put on there, the ones I speced are over $8 each in quantities < 10. When cutting down the headers, I recommend cutting it down to 82 pins then removing the last two carefully with needlenose pliers.

2. J4 header as specified fits great, other headers may need to have the tails cut down since there is minimal space betweent the board and the socket on the front side.

3. The diodes are really >>small<<. They are SSMINI-2 and SOD323F foot prints. I will be using my 30X microscope to attach these to my board, but you could probably get by using 10x or 8x mangification.

4. The rest of the parts are .5mm pitch, .050" pitch, or 0603 components. They aren't terribly difficult if you know how to solder surface mount pieces.


I've also done a bit of work on the 40->80 pin converter board. 0603 resistors are too big, so I will have to go at least one size smaller for optional termination resistors.

Do you know if your quickswitch is compatible with the NXP's CBTD3384 ?
It is a 10-bit level shifter with output enable. I have a bunch of them.
Moreover, it does not need the external diode to lower the voltage.

EDIT : actually it must be compatible since yours is called QS3384 .

It looks like I have everything to populate the board.
Can I directly solder the 68000 on it and disable it with some jumpers ?

Regards,

Frederic

[Shadowfire]

I pulled up the datsheet for the CBTD3384 and it will not work. The pinout is different and the footprint is different, the NXP is a bigger IC using .635mm pitch leads while the IDT is a QSOP with .5mm pitch..

There is a socket, J4, which you can populate with a standard 64DIP900 68000 processor, however, there is no disabling logic on the board. (See the schematic for details.) All the pins from the 68000 socket (j4) to the 68000 header (j3) are tied together. What kind of disabling circuit would you suggest? I had plans of using a regular 68000 until my soft core is completed, then just removing it from the board when I was ready to go live with it.

[tnt23]

Do J1 and J2 pinouts correspond to DE1's J1 and J2 correctly? I remember attaching an LCD to J1(GPIO0), and pinout was like this:

IO_A0 ---  1  2  --- IO_A1
IO_A2 ---  3  4  --- IO_A3
IO_A4 ---  5  6  --- IO_A5
IO_A6 ---  7  8  --- IO_A7
IO_A8 ---  9  10 --- IO_A9
VCC5  --- 11  12 --- GND
...

, as opposed to the adapter's schematics in the Zone, where all even pins are grounded.

I am checking with DE1_Schematic.PDF from the DE1's CDROM, page 16.

[Shadowfire]

Yes, J1 & J2 mirror the DE1's pinouts on the odd pin #'s. The even pins are grounded to prevent signal crosstalk.

[tnt23]

Originally Posted by Shadowfire

Yes, J1 & J2 mirror the DE1's pinouts on the odd pin #'s. The even pins are grounded to prevent signal crosstalk.

I see. I was under the impression the board would plug directly into DE1 without any cables.