An Improved MENSCH™ Microcomputer

[plasmo]

You can certainly fit the layout in 100mmX100mm which is significantly cheaper. Measure QFP100 pad length; the fingers need to extend about 20 mil (0.5mm) beyond the leads to help with manual soldering. The default library for QFP100 is likely designed for machine soldering which is too short for manual soldering. I don’t use KiCad, so I can’t help you checking the QFP footprint.
Bill

[barnacle]

Nothing really leaps out at me, except perhaps that I'd move D5 and R9 to the left, so they're out of the way of the tracks which you'll be running between most of the pins on the ram and the eeprom. I might consider moving the RTC oscillator parts left as well, to clear the space where you're likely to have a lot of data and address lines changing direction.

Neil

[Dr Jefyll]

Just a suggestion, but an important one, IMO. I'd replace the single-row headers with double row headers. This would reduce the headers' length by half, leading to a more compact design and shorter connections between the '265 and the outside world.

Or -- and this is the option I'd favour -- stick with the double row headers, but add 50% more pins, thus enabling you to improve signal integrity by interspersing ground/vcc connections among the signal connections. For example, the pattern on a header could be GND pin, signal pin, signal pin, VCC pin, signal pin, signal pin [...] and so on. (And the length of the header is still only 75% of what you have now, supporting the goal of shorter connections between the '265 and the outside world.)

Also on the theme of a more compact design and shorter connections, I think it'd be best if the '265 were located pretty much in the center of the board... but right now that position is occupied by the crystals. [Edit: Neil hinted at this too.] I'd be looking for some way to relocate them, or at least reduce the space between the '265, the crystals, and the memories. This'll help in getting the '265 in the center (more or less).

-- Jeff

[Martin_H]

Thanks for the helpful feedback. Here's my punch list:

Code: Select all

* Try to shrink PCB to 100mm x 100mm to decrease cost.
* For the QFP100, use larger pads 20 mil (0.5mm) beyond the leads to help with manual soldering.
* Move D5 and R9 to be out of the way of traces between the EEPROM and RAM
* Centralize the w65c265 to make for shorter connections.
* Moving the RTC oscillator parts left.
* Reduce the space between the '265, the crystals, and the memories. This'll help in getting the '265 in the center (more or less).
* Consider replacing the single-row headers with double row headers. This would reduce the headers' length by half, leading to a more compact design and shorter connections between the '265 and the outside world.
* Alternately, stick with the double row headers, but add 50% more pins to improve signal integrity by interspersing ground/vcc connections.

FYI: My initial idea for the headers was to plug one side into a breadboard and prototype. Basically like a larger version of the W65C265QBX. But I may forgo that and use the double row W65C265SXB expansion header design, because add on board already exist for that. I can easily make a protoboard for that format.

[Martin_H]

Here's the updated board layout with most of the suggested changes. It's now 100mm square, and uses headers that are pin compatible with the W65C265SXB, although their placement is different. This result is a board that look suspiciously like the W65C265SXB. But it has some features that I wanted:

* The ability to power it from an unregulated battery pack.
* A conventional 32K EEPROM.
* More RAM, and the ability to move the RAM in the memory map.

There's no room for an onboard 65c22 which would have been nice.

To do:
I haven't figured out how to change the Package_QFP:PQFP-100_14x20mm_P0.65mm footprint to a version with larger pads.
I haven't found a place for most of the chip select LED's. I may delete them.
I am wondering if I should replace the crystals, resistors, and loading caps with a TTL can oscillator.

Can you just feed the output of a TTL can oscillator into FCLK or CLK?

[barnacle]

I know, everyone's a critic... but I wonder if you can fit the memories side by side (as you had them originally), move the processor down (away from the centre!) and under one of the memories, and move the memories left. That would leave you space for a 6522 on the right (though you might want to mirror the whole thing as its ports are all on the left).

Given the relative paucity of memories in DIP packages, you might find it handy to add footprints for SO versions inside the DIP spaces - they do fit, just.

Sorry

Neil

[J64C]

gfoot wrote:

That's a nice point - while you can get away with using the generic symbols and footprints, for large more complex connectors it makes a lot of sense to create your own symbols and footprints just the way you want them (especially which pin is which, and maybe custom silkscreen) - at least be aware that it is an option.

I usually keep a notepad document which I copy and paste the text from, once you determine which components you require. I only use a handful of different footprints most of the time. So, if I place a capacitor, I select it, press E and paste in the footprint. Then it’s a matter of copying that capacitor and the pasted one will have the same attributes.

Better still, if you have an existing project that you were happy with, you can have two instances of KiCad running side by side. Then you can simply select a component from one project and paste straight in to the other.

Even to the extent where you can copy over whole sections using this method, as the pull-ups etc on your 6502 are often going to be the same between projects, so you can just copy that whole section over.

[Martin_H]

barnacle wrote:

Given the relative paucity of memories in DIP packages, you might find it handy to add footprints for SO versions inside the DIP spaces - they do fit, just.

I have mused on the idea of going with SMD for the quad nor gate and RAM. That would free up space and might allow for a 65c22.

I have seen some SMD practice kits on Amazon which include various sizes of components and types. I plan to order one and give it a try.

I know I can solder 0805 devices. But seeing if I can solder SOIC and QFP devices would open up some avenues.

[Martin_H]

I think we're getting somewhere with this layout. I switched the quad nand gate to a SOIC package and gained enough room to add aa 65c22 with I/O ports that match my 6502 SBC. Although crowded, I could remove the top and bottom keep out zones and stretch the layout vertical.

Put a Forth implementation in the EEPROM and it would be a fun robot controller. With the onboard UARTS you would have a wireless radio link, a serial local keyboard, and serial video output.

[barnacle]

Aligning the rom and ram at the 0v end will simplify the parallel feeds (but isn't critical; you've lots of room in there).

Neil

[plasmo]

Plenty of room still. You can also put resistors, capacitors at the back of the board under IC. You can probably route everything in 2 layers although 4-layer is so cheap, no reason not to do 4 layers.
Bill

[Martin_H]

Changes:

Code: Select all

* I increased the vertical spacing of the components.
* I aligned the 0-volt pins of the RAM and ROM.
* I made sure that no resistors or diodes are in the parallel feed area.
* I removed the unused chip select indicator diodes. I can add them to any cards that use the expansion header.
* I moved the interrupt select header and diode above the 65c22 because that area was available.
* For the 65c22 chip I used a5b for cs1 and cs1b for cs2b. This should map it to 0xDFC0.

Changes I'd like to make.

Code: Select all

* Any suggestions for a panel mount power switch? Boards lacking them can get annoying when power cycles are needed.
* Any suggestions for a more compact voltage regulator? Possibly in a sot-223 package? I'm using the LM7805 TO-220 because I'm familiar with it. But it's taking up a lot of space and is probably overkill for this board. I'm also laying it on its side because it's tall when standing vertically and I've been bitten by that in the past.
* I'm open to moving resistors and decoupling capacitors to the back of the board. But how do you do that in KiCad?

[gfoot]

Martin_H wrote:

* Any suggestions for a panel mount power switch? Boards lacking them can get annoying when power cycles are needed.

Over here I implemented a soft power on/off arrangement, it was very convenient but uses two buttons and some additional components, so maybe too much real estate for your needs.

Quote:

* Any suggestions for a more compact voltage regulator? Possibly in a sot-223 package? I'm using the LM7805 TO-220 because I'm familiar with it. But it's taking up a lot of space and is probably overkill for this board. I'm also laying it on its side because it's tall when standing vertically and I've been bitten by that in the past.

In the above linked circuit I put a TO-220 MOSFET horizontally on the back of the board to get it out of the way, that worked very well and you could do the same for your voltage regulator. See the bottom centre portion of the I/O board in the above post.

Quote:

* I'm open to moving resistors and decoupling capacitors to the back of the board. But how do you do that in KiCad?

Just select the part and press 'F' for "flip", I believe.

[barnacle]

F for flip, yes.

You might consider the LM1117 range; depending on your power requirements they're available in various SM formats; I like the SOT-223 package which handles up to an amp (but remember any linear regulator is limited by how much heat it can dissipate!)

Neil

[Dr Jefyll]

Myself, I prefer that a SBC circuit board has no voltages greater than VCC. This massively reduces the potential damage from an accidental short circuit. Instead, I'll locate the regulator off-board.

-- Jeff