WDi to IDE adaptor (3)

[Mike Arnold]

1. The PLCC to 40 DIP adaptors look like the way to go which makes Aron's life easier. There may even be an eZ80 to DIP40 available. Not something for now.

2. I agree with 0.1uF decoupling for the oscillators. Feels safer.

3. I agree with going for unregulated supplies. Much simpler.

4. The MAX232 issue is a pain which is why I proposed the HIN202 originally.

Finally, thanks for all your input on this. I reckon I owe you some beers - just the problem of the Atlantic ocean being in the way to fulfilling that promise!

[Peter Higgins]

Re the MAX232. I suggest we change the design to use the newer MAX232A instead - pinout of the MAX232 and MAX232A is identical. Then capacitors C15, C16, C17, C18, and C19 can all be changed to 0.1uF and R21 can be eliminated.

[Mike Arnold]

Peter, I am not sure if the counterfeit problem also applies to the MAX232A as well. If we leave the circuit as it is it will work with MAX232, MAX232A and HIN202. That was my thinking.

FYI the problem with the fake chips is, I believe, a parasitic scr that can get triggered and shorts out the supplies. This is a well known phenomenon in semiconductor design. The CR network on Vcc slows the rise of Vcc and prevents the pump capacitors from triggering the parasitic scr. I may be wrong though (my wife will testify to my fallibility).

[Peter Higgins]

There is some confusion here...

Mike - your original schematic shows use of either a MAX232A or an HIN202, with 0.1uF charge pump capacitors as required by these newer designs.

Aron's current schematic shows use of a MAX232 with 1.0uF capacitors, as required by that older part. I suggest his schematic be changed to match yours - ie use of the MAX232A with 0.1uF capacitors.

The thing about the MAX232A is that it is still a current production part, and can (should!) be purchased directly from manufacturer's distributors like Mouser and Digikey. When purchased from these sources, the likelihood of purchasing a counterfeit part is essentially nil. Sure, if you are still concerned people may want to save a few dollars by purchasing the MAX232A on eBay and thus run the high risk of buying a counterfeit part, certainly there seems to be no harm with keeping your current limiting resistor R21 in the design.

[Aron Hoekstra]

Ok agreed - I've updated to the MAX232A - attached is the latest schematic. Been a busy week so I haven't had too much time but I have started on the PCB layout. If someone could double-check the recent modifications just as a sanity check that'd be great. Thanks!

Aron

--
You received this message because you are subscribed to the Google Groups "Cromemco" group.
To unsubscribe from this group and stop receiving emails from it, send an email to cromemco+u...@googlegroups.com.
To view this discussion visit https://groups.google.com/d/msgid/cromemco/4656949e-5a2e-41bf-9b0b-d604b6ac9ba0n%40googlegroups.com.

[Aron Hoekstra]

Just wanted to get some feedback on the board layout as I have it so far..  haven't placed the resistors/caps yet or done any traces yet - but let me know how this is looking?

[Mike Arnold]

Aron
I have had a look at the virtual image of the PCB and it looks great. I have a few questions/suggestions.
1. U2 is the 28C256 which is a 24 pin 0.6in device. The device on the board looks like a 0.3in device.
2. Maybe I missed the chat, but is U9 an SMD LS244 rather than HCT244?
3. I couldn't see the pads for the optional diode from pRESET to U45-1.
4. I am probably jumping the gun but I suggest that the trace to J2-41/42 is kept separate from the TTL +5V supply and is taken directly from the Pololu.
5. I suggest that U48's tab is connected to a reasonable area of copper to act as a heat sink. I would guess half a square inch should suffice but be careful as the tab on the regulator is connected the the powerful +16V rail.
6. As is common practice, I suggest using thick ground traces and add in areas of grounded copper where you can.

I have also gone over the schematic and have the following observations.
1. The optional diode between S100 pRESET and U45-1 (not yet added to the schematic) should probably be something cheap like a BAT41 or BAT42. A Schottky diode will be better than a 1N4148 due to its lower forward voltage.
2. IDE pin 21 (DMARQ) should go to ground via 5k6 not +V. Likewise, INTRQ should go to ground via 10k not +V.
3. You may need to check the data sheet for the 3.3V regulator (U50) because they normally need a decoupling capacitor at the input to keep them stable. Also, check the recommended value for the output capacitor. I do not have the part number otherwise I would have done it for you.
4. U45-12 (-RESET in processor circuit) appears to be connected to the clock line when it should be separate.
5. U46 (S-P circuit) does not appear to have its supplies connected.
6. In S-P circuit, U36-14 should go to +5V and U37-14 should go to +5V. U36-7 and U37-7 do not appear to be connected to ground.
7. C72 & C73 appear to be the wrong way round (reverse polarity).
Regards
Mike

[Peter Higgins]

Comments  re Mike's comments...

1. U9 was originally spec'd as an LS244. Aron's schematic also shows it as an LS244. There is no problem keeping that design spec, since the LS244 is in-stock at JLCPCB in both SSOP and SOIC packages.

2. Re filtering for 3.3V regulator U50:

U50 is an ON Semiconductor MC33269 in an SO-8 package. The recommended filter capacitors are:

- on output, a capacitor of at least 10uF. Could use same as C71 and C73

- on input, a capacitor is not necessary but a 0.33uF capacitor is recommended such as this one:

https://jlcpcb.com/partdetail/1967-0603B334K250NT/C1615

3. C72 and C73 definitely need to have their polarity flipped on the schematic

For the "optional accoustic feedback" - Mike, could you suggest a modification to the circuit design that would allow jumpers to be used to disable this, without leaving floating inputs on U104B and U104C when the circuit is disabled?

[Mike Arnold]

Peter, 

I agree that it would be a good idea to put a 0.33uF capacitor at the input of the regulator just in case it decides to oscillate or ring.

Disabling the acoustic feedback should be quite simple. Do not install R10 and BZ1. 

As you will have deduced, I have a thing about "feedback" from computers whether lights or noise. It has allowed me to sense what is going on and if something is going wrong. However, I realise that not everyone thinks like me hence me making the front panel optional. 
Mike

[Peter Higgins]

Thanks Mike. The solution was staring at me in the face, and it really is as simple as making installation of BZ1 optional. Perhaps Aron could put a 2-pin header in series with BZ1, and that way it could easily be disabled, or enabled for diagnostic purposes or if you just like to hear things happening.

[Mike Arnold]

I see where you are coming from. It would be nice to be able to enable and disable the sounder depending on your mood rather then have it permanently set. If a pair of pads (drilled 1mm holes) were put in series with the sounder (or R10) 0.1in apart with a fine (5 thou?) trace shorting them, then if you want to, you can install a 2 pin header and cut the trace. A jumper plug on the header will allow sound to be enabled/disabled at whim.

[Aron Hoekstra]

On Mon, Jul 28, 2025 at 7:56 AM 'Mike Arnold' via Cromemco <crom...@googlegroups.com> wrote:

1. U2 is the 28C256 which is a 24 pin 0.6in device. The device on the board looks like a 0.3in device.

You're right, I think you've mentioned this previously too - I've just updated it to the 600mil width part.

 

2. Maybe I missed the chat, but is U9 an SMD LS244 rather than HCT244?

Ok so after reviewing your discussions it's ok to leave this as LS244, correct?

 

3. I couldn't see the pads for the optional diode from pRESET to U45-1.

Ah! right, still need to add those

 

4. I am probably jumping the gun but I suggest that the trace to J2-41/42 is kept separate from the TTL +5V supply and is taken directly from the Pololu.

Here's that section - the 5V to J2 is coming directly from the Pololu.. Maybe in the view you had you couldn't tell because it was just showing the top layer. (Blue is bottom layer) 

 

5. I suggest that U48's tab is connected to a reasonable area of copper to act as a heat sink. I would guess half a square inch should suffice but be careful as the tab on the regulator is connected the the powerful +16V rail.

How's this look?

 

 

6. As is common practice, I suggest using thick ground traces and add in areas of grounded copper where you can.

I was planning on adding a ground plane on both sides of the board rather than individual traces for GND. In Kicad, you basically save filling your ground planes for last - you just have to be cognizant of it while placing components so the pour can reach all the GND pins/pads.  

 

I'll review your schematic observations in the next day or two when I get some more time. Thanks!

Aron

On Monday, 28 July 2025 at 03:51:52 UTC+1 Aron Hoekstra wrote:

Just wanted to get some feedback on the board layout as I have it so far..  haven't placed the resistors/caps yet or done any traces yet - but let me know how this is looking?

To view this discussion visit https://groups.google.com/d/msgid/cromemco/183a37d7-1c4f-41aa-8b17-7f76959bdd56n%40googlegroups.com.

[Mike Arnold]

Aron, 

2. yes U9 should be LS244 which is better than the HCT244 in this position - I was not sure if you had found an SMD version but I see now that you have. 

5. Although I cannot be clear about scale, the copper for the regulator should be ok.

6. I am pleased to hear that you intend to put a ground plane in. I don't think that you need two as we are not in the GHz world and a single plane might keep the price a little lower.
Again, thanks for the time that you are investing in this.

Mike

[Aron Hoekstra]

1. The optional diode between S100 pRESET and U45-1 (not yet added to the schematic) should probably be something cheap like a BAT41 or BAT42. A Schottky diode will be better than a 1N4148 due to its lower forward voltage.

Which direction should this diode face? I apologize if this has already been answered

 

2. IDE pin 21 (DMARQ) should go to ground via 5k6 not +V. Likewise, INTRQ should go to ground via 10k not +V.

Wow not sure how I goofed those up. Fixed

 

3. You may need to check the data sheet for the 3.3V regulator (U50) because they normally need a decoupling capacitor at the input to keep them stable. Also, check the recommended value for the output capacitor. I do not have the part number otherwise I would have done it for you.

I have added the 33uF cap on input (same part as C72 - https://jlcpcb.com/partdetail/Lelon-VZH330M1ETR0606/C249892 is it overkill for this purpose?). Already had the 10uF on output (same part as C71 and C73)

4. U45-12 (-RESET in processor circuit) appears to be connected to the clock line when it should be separate.

Whoops - this is one thing I hate about Kicad, when dragging a wire in the schematic you can accidentally connect something that you didn't mean to, which is what I suspect I did here. Great catch spotting that little dot in the wrong place!

 

5. U46 (S-P circuit) does not appear to have its supplies connected.

Fixed

 

6. In S-P circuit, U36-14 should go to +5V and U37-14 should go to +5V. U36-7 and U37-7 do not appear to be connected to ground.

Fixed. It also looks like I may be missing decoupling caps on U36&37 - should I add them?

 

7. C72 & C73 appear to be the wrong way round (reverse polarity).

So the + side of the cap goes to GND for both of these? Ah - you're right, these are negative voltages...  

I have also added the 2-pin header to one of the buzzer inputs to enable/disable the sound - this is all that was needed for that, correct?

 

 

On Monday, 28 July 2025 at 03:51:52 UTC+1 Aron Hoekstra wrote:

Just wanted to get some feedback on the board layout as I have it so far..  haven't placed the resistors/caps yet or done any traces yet - but let me know how this is looking?

To view this discussion visit https://groups.google.com/d/msgid/cromemco/183a37d7-1c4f-41aa-8b17-7f76959bdd56n%40googlegroups.com.

[Peter Higgins]

1. diode cathode connected to the S100 reset signal, anode connected to U45 pin 1

3. the recommended capacitor on the input side of 3.3V regulator U50 should be 0.33uF (not 33uF) like this one:

https://jlcpcb.com/partdetail/1967-0603B334K250NT/C1615

6. yes the 75107 and 75110 should have 0.1uF decoupling caps from their respective +5V and -5V pins to ground

7. yes the 2-pin header to enable/disable the buzzer is correctly placed in your schematic

[Mike Arnold]

Peter, thanks for your reply - the time shift makes it difficult to respond when the US is awake. Agree with your responses.

Aron, when you get to it could you send me the link to the parts you plan to use for the 470pF and 47pF capacitors? I just want to check their dielectric properties.

Thanks

[Aron Hoekstra]

Hey Mike, here is the 470pF part: https://jlcpcb.com/partdetail/YAGEO-CC0603JRNPO8BN471/C519395

and here is the 47pF part: https://jlcpcb.com/partdetail/YAGEO-CC0603JRNPO8BN470/C519392

1. Does this work?
 

3. Updated to the recommended part, thanks

6. Added!

To view this discussion visit https://groups.google.com/d/msgid/cromemco/253d2bee-9245-4431-b145-8389a7b5e2c9n%40googlegroups.com.

[Peter Higgins]

Aron - please put a 2-pin jumper header between U45 pin 1 and the anode of D3, with no "default" trace between header pins. We want the default board configuration to not respond to the S100 /RESET signal, and make it an option (by installing a shunt on the header) to enable it.

[Aron Hoekstra]

Ah ok I was going to leave the diode as a through-hole component which could be installed by the user if they want that feature. Would that also work?

Aron

To view this discussion visit https://groups.google.com/d/msgid/cromemco/f8559f55-bffd-4c74-822b-7708733ce4b5n%40googlegroups.com.

[Peter Higgins]

Yes, making D3 something that would optionally be installed would be another way to do it.

[Mike Arnold]

Aron, those capacitors are fine. They have NP0 dielectric so they will not change their value too much with temperature.

Mike

[Mike Arnold]

I tried dropping the CPU clock speed from 13.5MHz to 10MHz but got lots of read errors. I don't know if that is a software or hardware thing. Unfortunately, I do not have the time to investigate at the moment.

[Aron Hoekstra]

Hey guys just a quick update - sorry been pretty slammed this week. But did manage to get all the passive components placed and some of the power traces. Going to keep working on those and then let the autorouter do its thing. Here's where things are at:

To view this discussion visit https://groups.google.com/d/msgid/cromemco/274765cd-4924-421f-b60d-97fec4ba48b3n%40googlegroups.com.

[Aron Hoekstra]

So 2-layer routing failed miserably - it was worth a shot but left something like 200+ connections incomplete. We're going to have to make this a 4 or 6 layer board. Fortunately I have a coupon through JLCPCB which makes this option not much more expensive...  will play with it some more

[Aron Hoekstra]

Ok 6-layer autorouting was a success! I went through and fixed/cleared all DRC issues, remaining warnings are not a concern.

At this point I'd really like to get some eyes on the board in Kicad to do a review of the routing, etc - if you're willing? 

Unfortunately I don't think it'd be possible to review in any detail using printouts/PDF?

• Download/Install Kicad 9.0: https://www.kicad.org/download/
• Download and extract the W2I-S100 project files: https://drive.google.com/file/d/1Kst2UWaEPm_NJZzu7-OqE2ak8XuMBSx0/view?usp=drive_link
• In the extracted folder, open the "W2I-S100.kicad_pro" file.
• From there, open the W2I-S100.kicad_sch to view the Schematic, open the W2I-S100.kicad_pcb to view the board.
• First time opening a schematic/board it'll pop up some questions, just accept the defaults and it'll take you in.
• If you accidentally drag/move something, don't worry. Either undo, or exit without saving changes and go back in.
• In the board editor it may be hard to view traces due to the ground plane - hit CTRL+B to "unfill" the plane, making things easier to see (but then it'll show GND components as unconnected). Hit "B" to refill it.
• Signal trace widths are 0.2mm. Most vias are 0.6/0.3mm.
• To view a connected net, select a single trace, then hit the ` key (tilde/backtick), and it'll highlight the whole net.

Let me know if you have any questions.

[Peter Higgins]

Impressive!

Having never gotten to the stage of board design using Kicad I have to ask... does reviewing the routing basically come down to visually following each board trace to make sure it matches the schematic?

[Aron Hoekstra]

Yep, pretty much. I don't think it's really necessary though to verify each & every trace matches the schematic - there are tons of checks built into the software which takes care of that. If the schematic is done right, then the traces should be right. More just looking for feedback like on things I may have overlooked like "this component shouldn't be close to that one" or "why is this capacitor way over here??" or "are you nuts this trace carries 10 amps and you made it only 0.2mm wide!" :)

To view this discussion visit https://groups.google.com/d/msgid/cromemco/c0b2b79b-a3f2-4e46-86b8-ec0fe269f29en%40googlegroups.com.

[Mike Arnold]

Aron, looks like a masterpiece! I never realised that the design was such a challenge to lay out.  Imagine if I had chosen a 16 bit processor!

 I will look at it over the next few days but I am on quite a steep learning curve with Kicad.
Mike

[Aron Hoekstra]

No rush or worries.. In the meantime when I have time, I'll go through a test order to make sure I have all the SMD/BOM parts export working so JLCPCB recognizes all the parts & placement correctly. We can still make changes, I just want to get the process down.. and get a pretty close cost estimate.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/66a3b48a-b486-46a8-81e4-2c953bf181ebn%40googlegroups.com.

[Aron Hoekstra]

Went to get a preliminary cost estimate (though we are now short a few parts that are now showing low/out of stock). Got through the estimate and on the checkout page, I got hit with this. As if I needed any more reason to absolutely loathe everything about Trump and his despicable cult following. As much as I want to get this board made, I refuse to hand over any cash directly into his coffers. He was in the news again just today about how the corporations pay the tariffs, not the American consumers (a well-known lie from day 1). Sorry, I don't mean to turn this into a political rant, I just haven't placed a PCB order yet since these tariffs went into effect.

Up until this the prices were pretty reasonable for 5 boards, about $70 for the 5 PCBs, and $180 for parts & assembly. so comes to just over $50 ea, considering the number of parts etc, not terrible. I know I said they'd probably be around $30 ea but that was before we added a bunch more SMD parts.

Mike, not sure what import duties might look like from your side of the pond?

Aron

[Mike Arnold]

47% duties and tax is steep. Happy to help on this but it will still, probably, attract 20% VAT. I will message you privately about how to proceed.

[Peter Higgins]

Despite the steep duties and taxes... if you do decide to go ahead, I remain interested in buying a couple of these boards.

[Jay Cotton]

I'm in for one copy.

Tnx

Jc

To view this discussion visit https://groups.google.com/d/msgid/cromemco/70113948-1908-491b-9a13-bfc78eb0fec5n%40googlegroups.com.

[Richard Muse]

I'm also in.

Richard M

To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAE%3DSzZUAn2C8803-sbyaKW-_kSs%2BVd7ikphaBJmh_zADXtdnRg%40mail.gmail.com.

[Aron Hoekstra]

Well ok, I'll go ahead and proceed and we'll collectively have to eat these extra costs. One thing I hadn't realized is that 6-layer PCBs are tariffed higher than 2 or 4 layer PCBs! I have to get a few more components sorted out so cost will go up a bit more, plus there's shipping to consider. 

I have to order in multiples of 5's, and so far have 6 claimed..  so I'll need to order at least 10 - I can't recall who else may have said they wanted one. Is anyone else interested?

Aron H - 1

Mike A - 1

Peter H - 2

Jay C - 1

Richard M - 1

To view this discussion visit https://groups.google.com/d/msgid/cromemco/ba1a20ff-5513-4c19-a209-32ee4fd797b9%40gmail.com.

[Mark Huffstutter]

Hi Aron,

            Please add Me to Your list for one board.

 

Thanks,

Mark H

 

From: crom...@googlegroups.com <crom...@googlegroups.com> On Behalf Of Aron Hoekstra
Sent: Wednesday, August 13, 2025 7:32 PM
To: crom...@googlegroups.com
Subject: Re: WDi to IDE adaptor (3)

 

Well ok, I'll go ahead and proceed and we'll collectively have to eat these extra costs. One thing I hadn't realized is that 6-layer PCBs are tariffed higher than 2 or 4 layer PCBs! I have to get a few more components sorted out so cost will go up a bit more, plus there's shipping to consider. 

 

I have to order in multiples of 5's, and so far have 6 claimed..  so I'll need to order at least 10 - I can't recall who else may have said they wanted one. Is anyone else interested?

 

Aron H - 1

Mike A - 1

Peter H - 2

Jay C - 1

Richard M - 1

 

 

On Wed, Aug 13, 2025 at 3:52 PM Richard Muse <rlm...@gmail.com> wrote:

I'm also in.

Richard M

On 8/13/25 12:28, Jay Cotton wrote:

I'm in for one copy.

 

Tnx

Jc

 

 

On Wed, Aug 13, 2025, 8:19 AM Peter Higgins <higgin...@gmail.com> wrote:

Despite the steep duties and taxes... if you do decide to go ahead, I remain interested in buying a couple of these boards.

On Tuesday, August 12, 2025 at 8:58:41 PM UTC-7 Aron Hoekstra wrote:

Went to get a preliminary cost estimate (though we are now short a few parts that are now showing low/out of stock). Got through the estimate and on the checkout page, I got hit with this. As if I needed any more reason to absolutely loathe everything about Trump and his despicable cult following. As much as I want to get this board made, I refuse to hand over any cash directly into his coffers. He was in the news again just today about how the corporations pay the tariffs, not the American consumers (a well-known lie from day 1). Sorry, I don't mean to turn this into a political rant, I just haven't placed a PCB order yet since these tariffs went into effect.

 

 

Up until this the prices were pretty reasonable for 5 boards, about $70 for the 5 PCBs, and $180 for parts & assembly. so comes to just over $50 ea, considering the number of parts etc, not terrible. I know I said they'd probably be around $30 ea but that was before we added a bunch more SMD parts.

 

Mike, not sure what import duties might look like from your side of the pond?

 

Aron

 

 

 

 

 

 

On Mon, Aug 11, 2025 at 12:02 PM Aron Hoekstra <null...@gmail.com> wrote:

No rush or worries.. In the meantime when I have time, I'll go through a test order to make sure I have all the SMD/BOM parts export working so JLCPCB recognizes all the parts & placement correctly. We can still make changes, I just want to get the process down.. and get a pretty close cost estimate.

 

On Mon, Aug 11, 2025 at 11:59 AM 'Mike Arnold' via Cromemco <crom...@googlegroups.com> wrote:

Aron, looks like a masterpiece! I never realised that the design was such a challenge to lay out.  Imagine if I had chosen a 16 bit processor!

 I will look at it over the next few days but I am on quite a steep learning curve with Kicad.
Mike

On Monday, 11 August 2025 at 16:43:08 UTC+1 Aron Hoekstra wrote:

Yep, pretty much. I don't think it's really necessary though to verify each & every trace matches the schematic - there are tons of checks built into the software which takes care of that. If the schematic is done right, then the traces should be right. More just looking for feedback like on things I may have overlooked like "this component shouldn't be close to that one" or "why is this capacitor way over here??" or "are you nuts this trace carries 10 amps and you made it only 0.2mm wide!" :)

 

On Mon, Aug 11, 2025 at 10:24 AM Peter Higgins <higgin...@gmail.com> wrote:

Impressive!

Having never gotten to the stage of board design using Kicad I have to ask... does reviewing the routing basically come down to visually following each board trace to make sure it matches the schematic?

On Monday, August 11, 2025 at 8:02:02 AM UTC-7 Aron Hoekstra wrote:

Ok 6-layer autorouting was a success! I went through and fixed/cleared all DRC issues, remaining warnings are not a concern.

 

 

At this point I'd really like to get some eyes on the board in Kicad to do a review of the routing, etc - if you're willing? 

 

Unfortunately I don't think it'd be possible to review in any detail using printouts/PDF?

• Download/Install Kicad 9.0: https://www.kicad.org/download/
• Download and extract the W2I-S100 project files: https://drive.google.com/file/d/1Kst2UWaEPm_NJZzu7-OqE2ak8XuMBSx0/view?usp=drive_link
• In the extracted folder, open the "W2I-S100.kicad_pro" file.
• From there, open the W2I-S100.kicad_sch to view the Schematic, open the W2I-S100.kicad_pcb to view the board.
• First time opening a schematic/board it'll pop up some questions, just accept the defaults and it'll take you in.
• If you accidentally drag/move something, don't worry. Either undo, or exit without saving changes and go back in.
• In the board editor it may be hard to view traces due to the ground plane - hit CTRL+B to "unfill" the plane, making things easier to see (but then it'll show GND components as unconnected). Hit "B" to refill it.
• Signal trace widths are 0.2mm. Most vias are 0.6/0.3mm.
• To view a connected net, select a single trace, then hit the ` key (tilde/backtick), and it'll highlight the whole net.

Let me know if you have any questions.

On Sat, Aug 9, 2025 at 10:17 PM Aron Hoekstra <null...@gmail.com> wrote:

So 2-layer routing failed miserably - it was worth a shot but left something like 200+ connections incomplete. We're going to have to make this a 4 or 6 layer board. Fortunately I have a coupon through JLCPCB which makes this option not much more expensive...  will play with it some more

 

On Fri, Aug 8, 2025 at 5:57 PM Aron Hoekstra <null...@gmail.com> wrote:

Hey guys just a quick update - sorry been pretty slammed this week. But did manage to get all the passive components placed and some of the power traces. Going to keep working on those and then let the autorouter do its thing. Here's where things are at:

 

 

On Sat, Aug 2, 2025 at 4:59 AM 'Mike Arnold' via Cromemco <crom...@googlegroups.com> wrote:

I tried dropping the CPU clock speed from 13.5MHz to 10MHz but got lots of read errors. I don't know if that is a software or hardware thing. Unfortunately, I do not have the time to investigate at the moment.

On Saturday, 2 August 2025 at 09:13:44 UTC+1 Mike Arnold wrote:

Aron, those capacitors are fine. They have NP0 dielectric so they will not change their value too much with temperature.

Mike

On Saturday, 2 August 2025 at 03:47:48 UTC+1 Peter Higgins wrote:

Yes, making D3 something that would optionally be installed would be another way to do it.

On Friday, August 1, 2025 at 7:45:17 PM UTC-7 Aron Hoekstra wrote:

Ah ok I was going to leave the diode as a through-hole component which could be installed by the user if they want that feature. Would that also work?

 

Aron

On Fri, Aug 1, 2025, 8:51 PM Peter Higgins <higgin...@gmail.com> wrote:

Aron - please put a 2-pin jumper header between U45 pin 1 and the anode of D3, with no "default" trace between header pins. We want the default board configuration to not respond to the S100 /RESET signal, and make it an option (by installing a shunt on the header) to enable it.

On Friday, August 1, 2025 at 3:42:58 PM UTC-7 Aron Hoekstra wrote:

Hey Mike, here is the 470pF part: https://jlcpcb.com/partdetail/YAGEO-CC0603JRNPO8BN471/C519395

and here is the 47pF part: https://jlcpcb.com/partdetail/YAGEO-CC0603JRNPO8BN470/C519392

 

1. Does this work?
 

 

 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAD9iBD%2By%3D-gUzYazQMVd_Bg3KWVcpKpkFpCNuT3ccih4nhacYA%40mail.gmail.com.

[Richard Muse]

I would like a second one. So 2 for me. If you get an even 10 from unique folks with only 1 for me then 1 will work. But I do have 2 machines I'd like to use one in.

Richard M

To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAD9iBD%2By%3D-gUzYazQMVd_Bg3KWVcpKpkFpCNuT3ccih4nhacYA%40mail.gmail.com.

[Christopher Mallery]

I will take one

To view this discussion visit https://groups.google.com/d/msgid/cromemco/f5510a56-8569-418e-8d88-cb5b0a62c97d%40gmail.com.

[Aron Hoekstra]

Ok that makes 9. If we have enough interest and need to bump it to 15, that's fine too.

Aron H - 1

Mike A - 1

Peter H - 2

Jay C - 1

Mark H - 1

Richard M - 2

Christopher M - 1

To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAPKaxwJsCGSPsvqSuQh6F%2BZ%3DE8Ky_gaotmBRAPHPq5XKrT4%2Bug%40mail.gmail.com.

[Aron Hoekstra]

So, doing a sample order for 10 - here are the problem parts - I'll need to find replacements for these. Everything else shows in stock & ready. Peter if you have a chance would you lend a hand sorting through these? otherwise I can take a closer look in the next day or two.

[Peter Higgins]

I looked into all the parts you listed, and they are either not in stock, or not in stock in sufficient numbers. However, all the parts in that list can be "pre-ordered" with small minimum order numbers:

https://jlcpcb.com/help/article/What-is-JLCPCB-Parts-Pre-order-Service

[Mike Arnold]

I want to be realistic about the first batch of boards made. Although I have double checked my schematics there could still be an error and Aron has had to lay out an extremely complex board so there could be a mis-route hiding somewhere. As you know, manually reworking a multi-layer SMD board post production is very challenging. My thought is that we order the minimum number, test, debug and then order some more. Maybe that is just my English reserve against the American "just do it" attitude :-)

I am still happy to get a price for shipping to UK if you want.

[Aron Hoekstra]

Oh thank you for this info - I will look into doing the pre-order for just those selected parts then & see - I was thinking it would give me the option to do that during checkout but maybe it's more of a manual thing.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/65f3ba85-9717-438c-afb3-9dc56f61f510n%40googlegroups.com.

[Aron Hoekstra]

Agreed, there's definitely potential for needing to do some bodging and with more than half of these components being SMD, that wouldn't be fun. Would need a very steady hand and some 30 AWG Kynar. :)

Mike, I'll send you the files & instructions on how to generate the quote - just so we can compare.

Aron

To view this discussion visit https://groups.google.com/d/msgid/cromemco/45d21db3-22b4-48c5-a2fd-ea611abfede3n%40googlegroups.com.

[Mike Arnold]

Aron, I have been playing with Kicad viewing the schematic/PCB layout and, where things need to be close, you have put them close (eg C35 close to U45-5). Great job.

I don't know how to see the trace widths so I assume they are 0.2mm for the main. There are a couple of thoughts on trace widths for the IMI serial lines (RWDAT+, RWDAT-, SYSCLK+, SYSCLK-) which might be thicker if possible. They are current driven and only 12mA but it might reduce the risk of ringing if a bit thicker. Also, DIOR/DIOW for the IDE interface are quite long way from the driver chip to the two connectors. If they could be shorter and thicker that would be better but, with the ground plane, it will probably be ok as it stands. Just worried about ringing which can upset the IDE drive.

Finally, the PCB image shows the ext power connections as a male header. I suggest leaving these as simple pads because if fitted with a header it could short and Cromemco's power supplies are small welding sets!
As I have found how to view the schematics, I will give them another check. I am assuming that if the schematics are right the layout is right.

Mike

[Peter Higgins]

Agree with Mike's comments. With regard to the external power connector - you could leave the pads as designed for a male header, but leave installation of the header as a project for the end user.

Mike raises an excellent point regarding manufacture of a trial batch of (say) five boards vs going straight into full production. These boards will not be inexpensive, since they come fully assembled with the exception of a half dozen sockets for through-hole ICs.

[J Slade]

With respect to a first run of a multi-layer board, based on personal experience from 40 years ago - adding jumpers is one thing, but having to eliminate traces from an internal layer with a high current battery charger is nothing you ever want to have to do ... especially any more than you absolutely have to.

Jason

[Mike Stein]

Is anyone else in Canada besides me? If there were 5 people would it make sense to order 5 boards separately once the bugs are out of the first batch? AFAIK we wouldn't have the same kind of tariffs unless we retaliate against their 75% canola tariffs which in turn were retaliation for our 100% EV tariffs... madness!!

m

To view this discussion visit https://groups.google.com/d/msgid/cromemco/c7c88c35-eace-4e5a-babb-e1562dedea9an%40googlegroups.com.

[Peter Higgins]

On Thursday, August 14, 2025 at 10:02:42 AM UTC-7 Mike Stein wrote:

Is anyone else in Canada besides me?

I am located in Canada. At the moment I think all we'd have to pay is, depending on province, either HST or PST/GST.

[Dominique Le Bel]

Hi,

I am also interested in one.

Located in Canada

Dominique

---

De : crom...@googlegroups.com <crom...@googlegroups.com> de la part de Peter Higgins <higgin...@gmail.com>
Envoyé : 14 août 2025 13:29
À : Cromemco <crom...@googlegroups.com>
Objet : Re: WDi to IDE adaptor (3)

 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/4a8c12c5-bde5-47ce-881f-172bde66973en%40googlegroups.com.

[Mike Arnold]

Ironically, next week my wife and I fly to Canada for our summer holiday exploring Quebec province.

[Richard Muse]

Since it has come up. I have to agree regarding a first run. Of the several boards I have used from John Monahan (S100 Computers), all have been laid out with Kicad and are at least R2 if not later and they are all just 2 layer. Easier to test and patch.

I am following the discussion with great interest and desire to utilize the board, but have to admit, most of this is way outside of my wheelhouse. That said, it seems there are a number of opportunities for necessary or at least desirable 'revisions' for both basic function and reliability once a run of real boards is produced and tested.

Sooo, I have to agree that a short run up front is a good strategy. I'm in the US and not sure what the tariff impact is, but I certainly want to participate whatever strategy is pursued.

Richard M

To view this discussion visit https://groups.google.com/d/msgid/cromemco/c7c88c35-eace-4e5a-babb-e1562dedea9an%40googlegroups.com.

[Aron Hoekstra]

Ok that sounds good, when we're ready we'll go with the smallest batch possible (5 boards) so we can do some debugging. Once we've had some time with them, we'll do a larger order for the group.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/ff2a8058-d03f-49f0-bf65-d5cbbc960835%40gmail.com.

[Jay Cotton]

I am willing to build up the 1st prototype board.  I have WDI and IDE disk available.

[Aron Hoekstra]

Sounds good Jay will let you know when they come in. Haven't ordered yet, I'll reach out when that gets closed. Mike is going to keep the spare from this rev 1 purchase as a backup.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/6ac2eb49-3619-4890-b3c8-93050b429e91n%40googlegroups.com.