WDI to IDE adaptor (2)

[Mike Arnold]

Aron,

I started another thread to avoid having to scrolling down such a long discussion.

I am back from holidays now and will be checking the schematics and publishing updates. Give me a day or two because we are having a heatwave at the moment and it is 35°C in my shed (no aircon, this is Britain!) so I have only managed to do a few of the tests that I planned to verify Z80 timings.

I love that Pololu SM regulator: it has great dropout characteristics and should power the drive easily. A bit pricey but good. My only concern is that I could not find any information on ripple and switching noise (upstream and downstream) and I could not see any filter inductors on the its board. It may be wise to add an LC network on its input and have two on the output to stop switching noise from propagating: one for the W2I and drive electronics and the other to the drive motor. Unfortunately, that would mean more board space. I understand that the two +5V pins on the 44-pin connector are split between logic and motor. I assume that the motor includes the head positioner because Peter makes a good point about current "gulps". Encouragingly, in my shed I use a 3A lab PSU which has the +5V supply to the W2I and the drive connected together and I am not seeing anything odd happen with my 3.5in or 2.5in drives. Also, the regulator needs to be away from sensitive circuitry such as the oscillators and the 75107/75110. Remember the fun you had when your SMPS was too close to your 7710!

Great idea to use oscillators to replace two (all?) of the ugly HCT04/xtal circuits. That could result in eliminating U44 altogether by using the spare gates in U47 & U38.

If you do manage to fit a 40-pin header on the board then 3.5in drives (and other adaptors) can use this but will need their own external 5/12V supplies.

Peter answered your question about where pin 27 on the RAM went.

Although I like the suggestion of using a more modern part for the RAM, the 62256 appears to be slower than the 61256. According to datasheets, the former is available in 70-150ns types whereas the latter is 12-25ns. To keep the design simple, I do not specifically decode the Z80 M1 cycle but just use MEMREQ. I measured the MEMREQ time this morning and it is 78ns for an M1 cycle and 120ns for a normal memory cycle. Unless the 62256 is available in a faster variant we might need to keep to the old chip.

Finally, I am happy to pay for the prototype board along with postage (ie reimburse you). I can populate it and debug it before others are ordered.

Mike

[Aron Hoekstra]

Thanks Mike! What are your thoughts on replacing the eligible 74x parts with SMD equivalents?  I'm assuming going from DIP to SOIC/TSSOP that some of the pin# assignments would change?

--
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/0d2cda05-35c7-4059-abe7-de7797eeb0f2n%40googlegroups.com.

[Aron Hoekstra]

Ok I'll proceed with SMD since I'll have them populated by JLCPCB, no need to do any surface mount stuff by hand.

It looks like the 62256 part carried by JLCPCB has a 55 ns timing, according to its datasheet. Would that work?

https://jlcpcb.com/partdetail/2879350-CY62256NLL55ZXIT/C2759940

On Fri, Jul 11, 2025 at 10:53 AM arnol...@talk21.com arnol...@talk21.com <arnol...@talk21.com> wrote:

I do not have a problem with SMD ( apart from the fact that I don't have the technology to do it). I am not too hot on SMD chips but the few that I have looked at (a few 74 TTL) seem to have the same pin outs. More exotic ones may differ. Mike

To unsubscribe from this group and stop receiving emails from it, send an email to unsub...@googlegroups.com" target="_blank">cromemco+unsub...@googlegroups.com.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/0d2cda05-35c7-4059-abe7-de7797eeb0f2n%40googlegroups.com.

--

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 unsub...@googlegroups.com">cromemco+unsub...@googlegroups.com.
To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAD9iBDLaGVNSv8n1ZHWsYP3rooaJqGMLEOmQaZ0ubmgu5DH4%2BQ%40mail.gmail.com.

[Peter Higgins]

JLCPCB stocks several manufacturer's versions of the 62256 with a standard access time of 55ns. By my calculations this should work at the clock speed of the Z80 on this board, and is also well within the margins Mike specified.

I also looked up the SMD oscillators stocked by JLCPCB, and all three frequencies required by this board are stocked.

Mike does raise a good point regarding the switching noise generated by the Pololu regulators. It is certainly not documented by Pololu. There has been some discussion of, and concerns raised, on this issue in the S-100 forum, since all new designs there make use of these Pololu regulators. Despite concerns, it has never been conclusively shown this is a real problem and these regulators continue to be used on every new board design with nothing other than standard input and output capacitors.

Likely all of you do worry (as I do) that the further the design departs from Mike's prototype, the greater the chance something will break which would be "unfortunate" if a bunch of money is spent to have a run of partially-populated boards manufactured. I'm counting on the substitutions we are considering as being fairly conservative, and hence I'm optimistic it will work out :)

[Mike Arnold]

I am with Peter that if we move too far from the original design the debugging of the prototype board will be difficult (do JLCPCB do a prototype service?). The criterion for changes will be board space. If you feel that you can lay it out without a silly number of layers then maybe that is the time to stop.

A 55ns RAM should be fine.
Mike

[Aron Hoekstra]

Yes with JLCPCB you can order as few as 5 PCB's with assembly so it's not like we'd need to make huge investment. I'm guessing we can get the boards made + shipped for under $30 ea and that's with the SMD components.

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/5c089b29-e497-47f3-98e3-5b608e06b372n%40googlegroups.com.

[Peter Higgins]

On Friday, July 11, 2025 at 10:23:53 AM UTC-7 Aron Hoekstra wrote:

Yes with JLCPCB you can order as few as 5 PCB's with assembly so it's not like we'd need to make huge investment. I'm guessing we can get the boards made + shipped for under $30 ea and that's with the SMD components.

I would be okay with that.

With regard to your earlier question regarding pinouts of DIP vs SMD devices - in many cases, they are identical. For the specific case of 74-series logic components, pinouts for the DIP and SMD versions are identical.

[Aron Hoekstra]

Ok that makes it easy. & Mike - I'll add a 40-pin header for 3.5" drives to the board, thanks for the reminder. 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/88fc78d1-43b9-4dcb-880e-8e7936415d19n%40googlegroups.com.

[Aron Hoekstra]

Peter, would you mind sharing the links to those oscillator parts?

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/bfe1d737-acc2-4d29-9d19-015ba6a5f038n%40googlegroups.com.

[Aron Hoekstra]

Also SMD Capacitor selection question - I'm pretty sure using MLCC capacitors are non-polarized. Using MLCC for the 40-some odd decoupling capacitors is a no-brainer. What about some of the other smaller capacitors? The caps in the pF range will be fine, I'm sure. What about something like the 22uF or 47uF caps, would those also be ok as MLCC?

I guess what I'm trying to ask is at what point do you cross the threshold into wanting something like a SMD aluminum electrolytic?

[Peter Higgins]

27MHZ SMD oscillator, 5V, TTL output:

https://jlcpcb.com/partdetail/1942480-CB3_3C27M000000/C1851667

3.6864MHz SMD oscillator, 5V, TTL output:

https://jlcpcb.com/partdetail/1942252-CB3_3C3M686400/C1851439

22.5792MHz

I have not been able to find an SMD oscillator that works at 5V (they are all 3.3V parts). In a DIP package with a 5V supply, these are also hard to find.

This oscillator may need to be build from discrete parts per Mike's original schematic. An SMD crystal is available - see https://jlcpcb.com/partdetail/HD-7D022579I01/C648930

Regarding the power supply filter capacitors (recommend organic polymer types) suggest you just use through-hole parts rather than SMD. They need to be mounted near the Pololu regulator, and that regulator needs to be manually installed anyway, so not an issue.

- 

[Aron Hoekstra]

For 22.5792 what about this one? https://jlcpcb.com/partdetail/361103-S7D22579200A20F30T/C387015

To view this discussion visit https://groups.google.com/d/msgid/cromemco/0cb5baff-51ef-4662-9364-c95f9558324cn%40googlegroups.com.

[Aron Hoekstra]

oh nevermind i see its not available for order

[Mike Arnold]

If you use a  22.5792MHz oscillator with a 3.3V supply then this should work because the Vout-high should be ~3V which is within the TTL thresholds. You will have to put a miniature 5V to 3.3V regulator on board (low dropout) plus associated decoupling.  Example datasheet for osc attached (from Mouser). I don't have one of these but if I get time I'll rig up an osc running at 3.3V and test it.

Any capacitors over about 1uF will be electrolytic not MLCC.  
A thought on the 40-way connector. If you are still running short of board space, you could put 40 pads under where the 2.5in drive is located. Then the user can choose to solder in the 44-way and use an on-board drive or else solder in the 40-way header and use an external drive. 

[Mike Arnold]

Oh, and if using an oscillator most have an enable connection that needs to be pulled high.

[Mike Arnold]

Aron

I have done a review of the circuits and also corrected the items highlighted in my master diagrams. I attach the three that have changed.

During my review I noted the following:

  Processor: the legends for U5-14, 7, 13, 8 should be TxA, TxB, RxA, RxB. This is not a wiring issue just the naming.

  WDI I/O: trivial point but suggest remove the Schmitt trigger symbol from U13, the HCT part lacks hysteresis.

  S-P conversion: U24-11 should connect to U39-5.

  S-P: U25-9 (and associated connections) should connect to +WGATE.

  S-P: The legend for U29-5 should read -CMDSEL1.

  S-P: On U29 & U42 are the references to -CMDSEL0, CMDRW, -CMDSEL1, -CMDSTR, -CMDBUS01 and -CMDBUS00 connected through to the relevant pins on the 34-way WDI connector?

  IDE interface: U30-6 should connect to U43-12.

  IDE interface: the pulldown on the IDE connector pin 31 should be 10k.

  Display: the timing capacitors for U102A/B and U103A should be 1uF. That was due to me telling you to change all the 1uF to 0.1uF.

I feel that we are moving forward at quite a pace on this project.

I would be pleased to hear if Peter has spotted anything.

Mike

[Peter Higgins]

On Saturday, July 12, 2025 at 12:41:48 AM UTC-7 Mike Arnold wrote:

If you use a  22.5792MHz oscillator with a 3.3V supply then this should work because the Vout-high should be ~3V which is within the TTL thresholds.

 

Agreed The oscillator you specified has an Voh=90% of Vcc. If Vcc=3.3V, then Voh=2.97V.

That will meet Vih=2V (min) for both the 74F163 and 74HCT163 the oscillator output must drive.

To power the 3.3V oscillator, the design would need to have this SMD 3.3V LDO voltage regulator added:

https://jlcpcb.com/partdetail/onsemi-MC33269DR2_33G/C7301

[Aron Hoekstra]

Thanks Mike, wow I don't know how you even spotted some of these but I've updated all of these on my end. Will share a new schematic after I've updated it with the new oscillators and 40-pin IDE header.

Just so I understand these chip oscillators, all this circuitry in the red gets replaced with the oscillator and the output pin goes directly to clock? Or is U28B part of what gets removed?

This is the only one which includes the HCT74, the others' output to clock come directly from the HCT04.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/d64982af-e438-4cd6-aab2-a7cfb00274e3n%40googlegroups.com.

[Mike Arnold]

If I were starting with the use of oscillator packages I might have done the design a bit differently but I want to minimise change at this point.

Yes, U44B and its associated components (in red box) are replaced by the oscillator chip whose output will go to the clock input of the D type (pin 11). This is the only oscillator that feeds a D type because it is normal practice to use a divide-by-two for CPU clocks to ensure that the CPU clock has a 50% duty cycle: the HCT04 & xtal combination do not provide that.

The spare gate U44B must have its input tied high (or low) to stop it doing stupid things!

Mike

[Aron Hoekstra]

Sounds good!

This is the 22.5792MHz part I'll go with, it's the same footprint as the other 2:

https://jlcpcb.com/partdetail/8433547-SX7M225792B10F20TNN/C7431407 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/a2d31968-4d3f-4b52-ab4a-c8c166211d24n%40googlegroups.com.

[Aron Hoekstra]

Update schematic attached. I've also swapped the MAX232 to the SMD chip, cuz.. why not :)

[Peter Higgins]

Looking at ways to simplify the design.

Question for Mike - in most cases I can see why you specified LSTTL (eg you need to drive an interface) or F series parts (eg to divide down the 27MHz clock) but what about these instances:

1. both U26 and U46 are clocked at 22.5792MHz, yet you specified an F163 for U26 and an HCT163 for U46. Is there some reason that U26 could not also be an HCT163 ?

2. could U24 not be changed to an HCT374, since it is being clocked at a max of 22.5792MHz/4

[Mike Arnold]

Peter, 

thanks for the questions. It is important that members of the group question, suggest and challenge in order to get the best solution. Two heads better than one...

1. The choice of U26 as F is intentional because this counter has to produce tightly timed bursts of 8 pulses between accesses to port 60 by the CPU. Referring to sections A1.3 and A5.7 of the manual, you see that the asynchronous nature of the burst clock and the CPU clock means that I want the maximum separation between the end of the burst and the start of the next port 60 access without having to slow the CPU clock. For safety I chose the F part and have not had any problems as I always have a clear gap. I did also try a F393 for U27 which was slightly better still but not enough to justify the rarity of the part. The primer clock has no such constraints.
2. Although I have not tried it in my prototype I believe that a HCT374 for U24 should be fine.

I am tied up for the next day or two but I will then test the U24 change and a 3V drive from the 22.5792MHz oscillator.

Aron,

My thought on the MAX232 as SMD is apprehension. It is connected to the outside world and the outside world is a nasty place where there are static discharges and accidentally applied high voltages. If I were doing the PCB I would suggest keeping this DIP so that it can be replaced.

Another thought: is it possible to have three solder pads for +8V, ground & -16V so that a newly assembled board can be tested outside the card cage?

Another thought, I would suggest not using SMD LS parts. I say this because I bought some 74LS244 chips from a Chinese supplier. When I used them they seemed unreasonably fast and had a VoH of 4.9V. They were 74HCT244s which were labelled as LS. I am sure that not all suppliers are like that but caveat emptor!

I have been thinking that I should code up a test ROM for newly assembled or faulty boards but that is some way off at the present.

Aron, when you get to the board layout keep us informed on how tight things are. I have an idea for completely deleting two 14 pin DIP chips but that will involve me doing some rewiring of my prototype and a retest.

Mike

[Peter Higgins]

Thank you for the detailed explanation.

Aron - were you planning to include the "F" series parts in DIP packages that are hand soldered by the user, or were you hoping to include them as SMDs?

If SMD, on JLCPCB for the 74F163 I see only one choice that can be pre-ordered in small numbers in a SOIC package, which is the onsemi 74F163AD:

https://jlcpcb.com/partdetail/onsemi-MC74F163AD/C3828634

You could also stay with the original design specifying a 74F374 for U24. JLCPCB allows you to preorder the TI 74F374LC in small quantities:

https://jlcpcb.com/partdetail/TexasInstruments-74F374LC/C3754260

It is however in an LCC package, which has a completely different pinout from the DIP and SOIC versions.

Mike - with regard to your experience buying LS chips from a Chinese supplier, and getting HCT chips instead. I have had the same experience from suppliers in the far east, eBay, and even Jameco. I think the difference is that JLCPCB sources their parts directly from manufacturer's distributors, hence the parts are unlikely to be rebadged/remarked used parts and/or factory sold by secondary sources frequented by hobbyists.

[Aron Hoekstra]

Mike, great point about the MAX232 chip - leaving it as a socketed through-hole would be best. I'll switch it back. It would really suck to get some counterfeit parts. I'm hoping that JLCPCB does its due diligence, it would be awful for their reputation if this ever happened. A brief google search hasn't really turned up any real reports of this, so I don't think it's something we need to worry about. 

Peter, I had planned to leave the F parts as DIP - I hadn't seen any as SMD.. I see that one you linked now, but it is a bit pricey... 😮

To view this discussion visit https://groups.google.com/d/msgid/cromemco/c2f5b500-e0bc-422e-9296-35e52e4eb015n%40googlegroups.com.

[Patrick Linstruth]

When designing the ESP32 FDC+ serial server, I settled on the ADM3202ANZ because I needed to support baud rates up 460,800. I have not had any problems sourcing them and so far no defective parts. I also socket them.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAD9iBDJYgHGA2sQW2xyikhi7j%2BCYxn%3DKtxcZw8k3eekvrSx0Ww%40mail.gmail.com.

[Peter Higgins]

Yes, the 74F374LC in the LCC package is pricey.

An alternative available for order at JLCPCB is the 74F374D in an SOIC package - you can preorder the minimum of 14 for a total of $9.10 which is cost effective.

[Aron Hoekstra]

Just want to make sure we're looking at the same thing, I am showing the SOIC part is 19 for $8.81:

https://jlcpcb.com/partdetail/TexasInstruments-SN74F374DWR/C2866981

I think the one that is 14 for $9.10 is a SSOP part:

https://jlcpcb.com/partdetail/TexasInstruments-SN74F374DBR/C2869589

To view this discussion visit https://groups.google.com/d/msgid/cromemco/e6847f9d-380f-448b-b027-45bf1189454cn%40googlegroups.com.

[Peter Higgins]

On Monday, July 14, 2025 at 9:32:19 AM UTC-7 Aron Hoekstra wrote:

Just want to make sure we're looking at the same thing, I am showing the SOIC part is 19 for $8.81:

https://jlcpcb.com/partdetail/TexasInstruments-SN74F374DWR/C2866981

I think the one that is 14 for $9.10 is a SSOP part:

https://jlcpcb.com/partdetail/TexasInstruments-SN74F374DBR/C2869589

You are right... and I missed the SOIC version, which would be a better choice. 

[Mike Arnold]

I changed U24 to an HCT374 and put a 3.3V gate between the 22.5792MHz oscillator and the '163s. I ran my test pack (60 mins of intense disk activity under Cromix 31.68) and there were no errors. We are ok to make those changes.

Also, it appears that JLCPCB stock the Z80 ->  https://jlcpcb.com/parts/componentSearch?searchTxt=z84c0020 

[Peter Higgins]

On Tuesday, July 15, 2025 at 10:08:02 AM UTC-7 Mike Arnold wrote:

Also, it appears that JLCPCB stock the Z80 ->  https://jlcpcb.com/parts/componentSearch?searchTxt=z84c0020

Not in stock, but are are listed as available for preorder. That is a bit odd, since Zilog stopped production of all versions of the Z84C00 series one year ago and they are now only available on the secondary market. Or, perhaps JLCPCB is not keeping their parts listings up to date.

[Aron Hoekstra]

> I changed U24 to an HCT374 and put a 3.3V gate between the 22.5792MHz oscillator and the '163s. I ran my test pack (60 mins of intense disk activity under Cromix 31.68) and there were no errors. We are ok to make those changes. 

Do you plan to update/share the schematic? (No rush if you're not available - just checking)

So do you guys think I should swap out for that SMD Z80 or just leave it as DIP?

Just a few questions as I complete part selection:

• For D1, 1N4148 - would this part work? https://jlcpcb.com/partdetail/2456-1N4148W/C2099
• For Q1, PN2222A - would this part work? https://jlcpcb.com/partdetail/CBI-2N2222AU/C21714170
• For R32 (WDI I/O sheet) - what is the value of this resistor? Having a hard time making that out. I think it's 2.2K?

Aron

To view this discussion visit https://groups.google.com/d/msgid/cromemco/26cddad7-1955-422d-b31a-3b366a805d3cn%40googlegroups.com.

[Peter Higgins]

Aron - what Mike Arnold did was a test on his original build to make sure that (a) U24 could be substituted with an HCT374 and (b) a logic element with a 3.3V output could drive the 74F163 and 74HCT163. This confirms your own most recent schematic (which  uses a 3.3V oscillator) and confirms you can use a 74HCT374 for U24.

I think it is okay to use an SMD version of the Z80 - but before going to the trouble of changing the design, I suggest you get confirmation from JLCPCB they really are able to source this out-of-production part. The cost they are quoting is pretty good.

With regard to your other questions:

- D! - JLCPCB part you referenced is okay

- Q1 - JLCPCB part you referenced is okay

-  R32 is indeed 2.2K ohms

[Aron Hoekstra]

Ok so just to confirm, all I have remaining to do on that is to swap out U24 from a 74F374 to a 74HCT374, correct?

I'll reach out to JLCPCB (LCSC) about the Z80

To view this discussion visit https://groups.google.com/d/msgid/cromemco/bbb92c39-cb38-4b98-b74d-89b632d57351n%40googlegroups.com.

[Aron Hoekstra]

Ok so this is just me playing around - I am able to get all the components on a single side.. The chip layout doesn't make any sense at the moment, just wanted to see if it'd fit.. Should I put it all on one side like this or put all the SMD components on the back side?

Any comments on the positioning of the headers, drive or LEDs?  For LEDs I was using through-hole right angle LEDs, but they do make "side view" SMD LEDs.. should I use some of those?

[Walt Perko]

Hi,

 

That looks like an interesting board.  I haven’t been reading all the details about this, but couldn’t there be more SMT chips on the board and just be ready to plug ‘n play? 

 

Not that I would need one, but for the future, I think taking advantage of the SMT is better than having a mix on the board if the SMT is all available … or at least cover more of the chips etc. 

 

 

 

 

==============================================================================================
C U L8r,  °|°  Walt Perko  °|°        "Kids ... teach them the good stuff, and they still learn the bad stuff on their own."

http://www.R2Pv1.com/  RoboGuts™ Intelligent content for 3D printing making S.T.E.A.M. education better, easier and more affordable 

 

Experiments to learn how to use various Electronic Components, Structured Computer Programming, Phonemes for Speech &Song in any language, and Art.

                         "The World Needs a New Economic Model"
==============================================================================================

            Sent from the Cyber7

 

 

From: crom...@googlegroups.com On Behalf Of Aron Hoekstra
Sent: Wednesday, July 16, 2025 9:40 PM
To: crom...@googlegroups.com
Subject: Re: WDI to IDE adaptor (2)

 

Ok so this is just me playing around - I am able to get all the components on a single side.. The chip layout doesn't make any sense at the moment, just wanted to see if it'd fit.. Should I put it all on one side like this or put all the SMD components on the back side?

 

Any comments on the positioning of the headers, drive or LEDs?  For LEDs I was using through-hole right angle LEDs, but they do make "side view" SMD LEDs.. should I use some of those?

 

 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/CAD9iBDK5sHgBnptbh0k-WzmUt%3DOkcMQrJWG-i3JPOLQnsPMGLg%40mail.gmail.com.

[Peter Higgins]

My suggestions:

- standard SMD LEDs would easily be visible from most any angle

- put all components on the same side of the board. I would be worried about not paying attention and accidentally knocking off SMD components mounted on the "back side" of the board
- J3 (the serial connector) should ideally be located at the top edge of the board

- the Pololu regulator should be located at the bottom left corner of the board where the S100 +8V bus connection is located

- the -5V regulator has a low power draw on it, and can be located near the two ICs it powers

- the J2 external power connector will ideally also be located near the lower left corner of the board, near the Pololu regulator

[Peter Higgins]

Re "why not have more/all the chips on the board be SMT?'

The reason is that not all the chips are available in SMT versions that can be purchased from the PCB manufacturer:

- there are several old chip designs (like the 74xx and 74Fxx series, and the 2681 UART) not produced as SMT versions

- we are not yet certain the Z80 is available as an SMT version from the PCB manufacturer, since these parts are no longer in production

The program ROM is best left as a socketed IC, so that it is removeable for programming/reprogramming.

I suspect you are right that several of the older chips could be substituted with newer versions available in an SMT package. We are however trying not to deviate very far from Mike Arnold's original, tested, proven design by using chips that do not have identical specs (74F vs 74HCT, or 74LS vs 74HCT for example) or would require a redesign.

[Mike Arnold]

Just a thought: should we run pRESET from the S100 bus into the W2I?

[Peter Higgins]

On Thursday, July 17, 2025 at 5:30:38 AM UTC-7 Mike Arnold wrote:

Just a thought: should we run pRESET from the S100 bus into the W2I?

My first thought would be no, since the "standalone" version presumably does not require this, and the adapter board has its own power-on reset circuit.

Do you know if there are any issues with power up/down sequencing of the S100 WDI controller board vs the WDI-IDE adapter vs the IDE drive?

[Mike Arnold]

I don't know of any issues or interactions for power up/power down. I have not had any problems. The only irritation is that the PIOs on the WDI have rather random outputs when power is first applied but I handle this in the software. 

The time it takes for the IDE to come ready means that you cannot boot immediately (5-30 seconds delay depending on model) but the IMI 7710 takes 15s to spin up and everyone lived with that.

[Peter Higgins]

On Thursday, July 17, 2025 at 10:08:57 AM UTC-7 Mike Arnold wrote:

I don't know of any issues or interactions for power up/power down. I have not had any problems. The only irritation is that the PIOs on the WDI have rather random outputs when power is first applied but I handle this in the software. 

The time it takes for the IDE to come ready means that you cannot boot immediately (5-30 seconds delay depending on model) but the IMI 7710 takes 15s to spin up and everyone lived with that.

Thanks!  If there was a concern with the WDI-IDE adapter not being reset whenever the S100 WDI controller board is reset, carrying the S100 reset signal to the WDI-IDE adapter board would be desireable. Since your prototype adapter works fine without a reset that happens whenever the S100 WDI controller board is reset, it would seem to be fine to have the WDI-IDE adapter board ignore the S100 reset signal.

[Peter Higgins]

Mike - what was the reason you chose 7438s vs 74LS38s to drive the WDI bus? Both versions have the same maximum sink current. The older 7438s are only available on the secondary market, whereas the 74LS38 is current production.

[Aron Hoekstra]

Well, I heard back from LCSC on the Z80 SMD:

" Sadly the item is not available for quotation currently."

Good thing we checked first. But this also begs the question, weren't there a few other parts we selected that were "pre-order"?

Aron

To view this discussion visit https://groups.google.com/d/msgid/cromemco/9f4b06f1-d2ba-43a6-b573-26845960db15n%40googlegroups.com.

[Mike Arnold]

7438s are specified in the 7710 manual (albeit for the controller) and are used in the drive itself. My datasheet (TI rev March 1988) says that the max sink current for LS38 is 24mA whereas 7438 is 48mA. U17 & 18 are only driving terminators at the WDI so will have to sink 22mA whereas U19 & 20 drive terminators at both ends so need to sink 44mA.

[Peter Higgins]

On Thursday, July 17, 2025 at 11:13:15 AM UTC-7 Mike Arnold wrote:

7438s are specified in the 7710 manual (albeit for the controller) and are used in the drive itself. My datasheet (TI rev March 1988) says that the max sink current for LS38 is 24mA whereas 7438 is 48mA. U17 & 18 are only driving terminators at the WDI so will have to sink 22mA whereas U19 & 20 drive terminators at both ends so need to sink 44mA.

Yes you are absolutely correct and that makes perfect sense. I misread the data sheets. 

[Peter Higgins]

On Thursday, July 17, 2025 at 11:11:10 AM UTC-7 Aron Hoekstra wrote:

Well, I heard back from LCSC on the Z80 SMD:

" Sadly the item is not available for quotation currently."

Good thing we checked first. But this also begs the question, weren't there a few other parts we selected that were "pre-order"?

That response from LCSC is what I expected. Zilog stopped ,manufacture of the Z80 in June 2024, hence these parts are now only available through secondary distribution channels. LCSC certainly wouldn't want to be involved in the risks associated with buying ICs on the secondary market.

All the other parts that need to be pre-ordered are current production. I think I checked that most are obtainable from distributors like Mouser and Digikey. My assumption is that any parts we are able to source from these distributors could similarly be obtained by LCSC.

[Walt Perko]

Hi,

 

It is possible that if you buy the chips from another distributor/vendor, you could probably send the chips to JLCPCB to be installed. 

 

JLCPCB was allowing that a few years ago, but I don’t know if they continue that service. 

 

 

 

 

==============================================================================================
C U L8r,  °|°  Walt Perko  °|°        "Kids ... teach them the good stuff, and they still learn the bad stuff on their own."

http://www.R2Pv1.com/  RoboGuts™ Intelligent content for 3D printing making S.T.E.A.M. education better, easier and more affordable 

 

Experiments to learn how to use various Electronic Components, Structured Computer Programming, Phonemes for Speech &Song in any language, and Art.

                         "The World Needs a New Economic Model"
==============================================================================================

            Sent from the Cyber7

 

 

From: crom...@googlegroups.com On Behalf Of Peter Higgins
Sent: Thursday, July 17, 2025 11:33 AM
To: Cromemco <crom...@googlegroups.com>
Subject: Re: WDI to IDE adaptor (2)

 

On Thursday, July 17, 2025 at 11:11:10 AM UTC-7 Aron Hoekstra wrote:

            Sent from the Cyber7

 

 

From: crom...@googlegroups.com On Behalf Of Aron Hoekstra
Sent: Wednesday, July 16, 2025 9:40 PM
To: crom...@googlegroups.com
Subject: Re: WDI to IDE adaptor (2)

 

Ok so this is just me playing around - I am able to get all the components on a single side.. The chip layout doesn't make any sense at the moment, just wanted to see if it'd fit.. Should I put it all on one side like this or put all the SMD components on the back side?

 

Any comments on the positioning of the headers, drive or LEDs?  For LEDs I was using through-hole right angle LEDs, but they do make "side view" SMD LEDs.. should I use some of those?

 

 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/ad43c0fa-7050-4d6c-af82-cfc3b3cfc602n%40googlegroups.com.

[Peter Higgins]

I think there is a FAQ question about that on the JLCPCB web site, and the answer is no.

[Walt Perko]

Hi,

 

I figured they stopped that.  It’s extra work for them now days.  Back a few years they didn’t have access to such a large catalog of SMD components. 

 

 

 

 

==============================================================================================
C U L8r,  °|°  Walt Perko  °|°        "Kids ... teach them the good stuff, and they still learn the bad stuff on their own."

http://www.R2Pv1.com/  RoboGuts™ Intelligent content for 3D printing making S.T.E.A.M. education better, easier and more affordable 

 

Experiments to learn how to use various Electronic Components, Structured Computer Programming, Phonemes for Speech &Song in any language, and Art.

                         "The World Needs a New Economic Model"
==============================================================================================

            Sent from the Cyber7

 

 

From: crom...@googlegroups.com On Behalf Of Peter Higgins
Sent: Thursday, July 17, 2025 12:09 PM
To: Cromemco <crom...@googlegroups.com>
Subject: Re: WDI to IDE adaptor (2)

 

I think there is a FAQ question about that on the JLCPCB web site, and the answer is no.

On Thursday, July 17, 2025 at 11:37:47 AM UTC-7 Walt Perko wrote:

Hi,

 

It is possible that if you buy the chips from another distributor/vendor, you could probably send the chips to JLCPCB to be installed. 

 

JLCPCB was allowing that a few years ago, but I don’t know if they continue that service. 

 

 

 

 

==============================================================================================
C U L8r,  °|°  Walt Perko  °|°        "Kids ... teach them the good stuff, and they still learn the bad stuff on their own."

http://www.R2Pv1.com/  RoboGuts™ Intelligent content for 3D printing making S.T.E.A.M. education better, easier and more affordable 

 

Experiments to learn how to use various Electronic Components, Structured Computer Programming, Phonemes for Speech &Song in any language, and Art.

                         "The World Needs a New Economic Model"
==============================================================================================

            Sent from the Cyber7

 

 

From: crom...@googlegroups.com On Behalf Of Aron Hoekstra
Sent: Wednesday, July 16, 2025 9:40 PM
To: crom...@googlegroups.com
Subject: Re: WDI to IDE adaptor (2)

 

Ok so this is just me playing around - I am able to get all the components on a single side.. The chip layout doesn't make any sense at the moment, just wanted to see if it'd fit.. Should I put it all on one side like this or put all the SMD components on the back side?

 

Any comments on the positioning of the headers, drive or LEDs?  For LEDs I was using through-hole right angle LEDs, but they do make "side view" SMD LEDs.. should I use some of those?

 

 

To view this discussion visit https://groups.google.com/d/msgid/cromemco/5505fbe2-d508-49c6-9d53-4fbcb6fd4692n%40googlegroups.com.

[Mike Stein]

Just in case anyone needs or wants some original Zilog or Mostek DIP40 Z80(A)s, I've got  afew to get rid of.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/ad43c0fa-7050-4d6c-af82-cfc3b3cfc602n%40googlegroups.com.

[Aron Hoekstra]

Peter, thanks for your suggestions on the board layout, these are all great ideas & will be implemented.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/50435d1f-dac1-4d89-b6a9-294ee6509e57n%40googlegroups.com.

[Mike Arnold]

I was thinking again about -RESET from the S100 bus and I agree that it is probably not necessary but then came up with a thought. If there were two pads 0.4in spaced with one going to -RESET (S100 bus pin 75) and the other to U45-1 then it would be possible to install a 1N4148 if it were ever needed. However, that depends on how the layout is going.

[Mike Stein]

Another silly question since I've been out of the loop: I know it only works with the 7710, but can it emulate two drives?

And does it work with a WDI-II as well as a WDI?

Apologies; I'm too lazy today to read the docs ;-)

To view this discussion visit https://groups.google.com/d/msgid/cromemco/d4b12a78-91f3-48d9-b079-5320e03bf2e9n%40googlegroups.com.

[Peter Higgins]

On Saturday, July 19, 2025 at 12:44:34 AM UTC-7 Mike Arnold wrote:

I was thinking again about -RESET from the S100 bus and I agree that it is probably not necessary but then came up with a thought. If there were two pads 0.4in spaced with one going to -RESET (S100 bus pin 75) and the other to U45-1 then it would be possible to install a 1N4148 if it were ever needed. However, that depends on how the layout is going.

3-pin header block:

- pin 2 goes to U45 pin 1

- pin 1 goes to S100 bus pin 99 ie /POC

- pin 3 goes to junction of C12/R18/D1, with D1 (the SMT version) factory installed

Can then use a 2-pin shunt to select which circuit the board uses for power-on reset.

[Peter Higgins]

On Saturday, July 19, 2025 at 8:58:29 AM UTC-7 Mike Stein wrote:

Another silly question since I've been out of the loop: I know it only works with the 7710, but can it emulate two drives?

And does it work with a WDI-II as well as a WDI?

Mike Arnold's adapter design:

- emulates four IMI7710 drives

- works with both the WDI and WDI-II controller boards

I have attached a copy of his writeup which was originally posted at the start of part 1 of this long discussion.

[Mike Stein]

Great! Thanks very much, Peter.

--
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/68f0aa20-a03c-4ad3-bc44-4afd3366788en%40googlegroups.com.

[Peter Higgins]

Mike and Aron - a couple of issues that arose while I was looking into sourcing of U4 (2681 UART) and U2 (28C256 EEPROM):

U4 - a 2681 UART. Mike's original design uses the 24 pin 0.4" wide "compact DIP" version, and I did notice Aron has got the correct footprint for this part shown on the trial board layout. The 2681 was originally manufactured in 40, 28, and 24 pin DIP versions, so you need to look carefully at what you are buying. The Phillips part number is SCN2681AC1N24.

U2 - a 28C256 EEPROM. Mike's original design specifies this to be the fastest 120ns version, which is not easy to source. The fastest current production part is the AT28C256-15PU with an access time time of 150ns, which is probably insufficient. Current production flash memory devices come in much faster versions and are also less expensive - like the SST39SF040-70 with an access time of 70ns. The SST39SF040-70 comes in a 32 pin DIP (just 4 more pins than the 28C256) and would require a change to the schematic to ground the extra 4 address lines.

[Aron Hoekstra]

Thanks for identifying the right 2681 part # - do you know what the part # would be for a 120ns 28C256? Or are they so rare that we really should swap out to the  SST39SF040?

--

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/5bb68ee9-5f81-405c-a619-27ce302189c3n%40googlegroups.com.

[Peter Higgins]

The only 120ns version of the 28C256 that I could find is the CAT28C256. It is no longer in production, and needs to be sourced on the secondary market, for example eBay (around $10) or UTSource in China (around $5).

Pending Mike's approval, my recommendation is to switch to the SST39SF040 (70ns version) and make the necessary design change to accommodate it. It is in active production, and stocked at Digikey and Mouser ($4). I believe all modern device programmers are able to program it.

Incidentally - are you planning to use only SMT parts for all ICs except:

- Z80

- ROM

- 2681 UART

- 7438 x3

- 75107 and 75F110

It seems all other parts are available (either in-stock or for pre-order) at JLCPCB.

[Aron Hoekstra]

Let me take inventory of what's still through-hole in my schematic:

• Buzzer_12x9.5RM7.6 (intentional to make it optional? though it would probably also be easy enough to add a jumper)
• IDC headers (34 & 40 pin)
• 2.0mm pitch 44 pin header (incidentally I requested samples of these from the mfg and have 4 remaining! - got em for free, so first come first serve - they fit the 2.5" drive perfectly - will send them out with the boards)
• LEDs, though I shared some SMD parts I chose with Mike, he's reviewing them
• Resistor arrays - the values may change depending on the LEDs but we could easily swap these out for some SMD resistors?
• DIP switch - we could probably find a SMD version?
• MAX232 - intentionally through-hole/socketed
• 74F84 x2 (U6 & U7) DIP-14
• 74F138 x2 (U14 & U16) DIP-16
• 7438 x2 (U17 & U18) DIP-14
• 74LS38 x2 (U19 & U20) DIP-14
• 74F163 (U26) DIP-16
• 75107 (U36) DIP-14 (no SMD equivalent)
• 75110 (U37) DIP-14 (no SMD equivalent)
• 74F04 (U39) DIP-14
• 74F00 (U40) DIP-14
• 74F08 (U41, U42) DIP-14
• 74HCT163 (U46) DIP-16

I'd happily swap out these remaining DIP parts if there are SMDs available? I've attached the current full BOM.

You said 3x 7438 but I only count 2, did I do something wrong?

To view this discussion visit https://groups.google.com/d/msgid/cromemco/04bc2824-5283-4978-bdb6-42f366ac5b00n%40googlegroups.com.

[Aron Hoekstra]

No worries there, no progress on the layout the last couple of days :D Probably a good thing, as Peter is mentioning, maybe swapping a few additional 74 parts to SMD to I'll wait til that's finalized.

Feel free to share a little schematic of the proposed change.

To view this discussion visit https://groups.google.com/d/msgid/cromemco/d4b12a78-91f3-48d9-b079-5320e03bf2e9n%40googlegroups.com.

[Peter Higgins]

Comments:

1. I miscounted the 7438s. Based on the original schematic there are four 7438s driving the WDI bus:  IC17, IC18, IC19, and IC20. This needs to be fixed in your schematic.

2. All the following are available in SMT versions for preorder - look for the "D" versions from TI

7438

74F74

74F138

74F163

74F04

74F00

74F08

74HCT163

4. Suggest we use standard through hole resistor arrays and DIP switches for the user to install.

[Peter Higgins]

Two questions for Mike Arnold:

1. your thoughts on substituting a 70ns SST39SF040 for the hard to source 120ns 28C256.

2. what is the purpose of connecting the MAX232A Vcc to the 5V bus via a 10 ohm resistor? The MAX232A datasheet shows Vcc connected directly to 5V, with a 0.1uF bypass cap to ground.

[Mike Arnold]

I have done some calculations, taken some measurements, checked circuits and gone through the parts lists. Here is my update to Aron and Peter.
1. The memory timings are not going to be a problem. My earlier post of 72ns for -MREQ was the refresh cycle (my mistake) and therefore irrelevant. Also, I insert two wait states when the ROM is in so you will see that the "ROM in" timings are 148ns slower than when running at full speed (give or take). The measurements of -MREQ low are:
  ROM in   refresh cycle 72ns
                  op code fetch 262ns
                  mem read  296ns
  ROM out   refresh cycle  72ns
                   op code fetch 112ns
                   mem read 146ns
A 28C256-150 will be fine. I have some of these so I will test one as soon as I have got my EEPROM programmer working.
2. The supply to the MAX232 is explained in section A5.14 of the reference manual. It is to prevent lockup. Here is a link to a chat about it -> https://e2e.ti.com/support/interface-group/interface/f/interface-forum/233847/max232-overheat-problem .

3. Having looked at the spec sheets for the LEDs I suggest the dropper resistors as follows: red 360R, yellow 270R, green 160R. I used low current LEDs in my prototype so they needed less current.
4. You can delete LED10 and its dropper resistor as this is simply a power on light which is not really needed when on an S100 card.
5. RP1 and RP2 must be in sockets as they are terminator resistors that may need to be removed depending on other drives connected to the WDI bus.
6. C3 in the front panel monostable should be 1.0uF not 0.1uF.
7. I see that the decoupling capacitors for the oscillator modules are 0.01uF. If that is what their datasheet recommends then stick with that otherwise up to 0.1uF.
8. IC19 and IC20 should be 7438 and not LS38. They need a bit of grunt.
9. There should be a resistor in series with the piezo sounder to control the volume. I suggest that this is through hole so that the user can decide how loud it is.
10. On the -pRESET discussion... I feel that it is better to give the option of using -pRESET rather than -POR because the W2I already has its own POR circuit. I was thinking that it might be wise, if pressing the system reset button, to reset the W2I as well. Hence the suggestion of a couple of pads to add a diode.

In the tradition of two steps forward, one step back, I have managed to blow up one of the WDI interface chips on my prototype (I must have shorted something to Vcc) so I need to track down which chip it is and replace it. This is why I am so keen to see interface chips (serial port, WDI) socketed so that they are easy to fix.

Mike

[Peter Higgins]

Thanks for those detailed comments Mike!

1. Re the 28C256. Based on your calculations, the AT28C256-15 (a current-production 150ns version of the 28C256) will work great.

2. I have never encountered the issue discussed in that TI support forum re the MAX232 - possibly because it is an old discussion from over a dozen years ago, it seems to be primarily about the MAX232, and (as you pointed) it is highly likely this problem is related to use of the unfortunately abundant fake versions of the MAX232 that are floating around.The current production MAX232ACPE+ (which uses 0.1uF capacitors in its charge pump circuitry) does not have this problem in the many applications I have used it. I buy them only from Mouser or Digikey, and yes they are expensive.

3. Ah - you want to be able to reset the adapter using the S100 reset signal. That was why I asked earlier whether it was important that initialization of the adapter had to be synced with initialization of the controller and/or the IDE drive. Have you ever encountered a need to manually reset the adapter during your testing? My reservation with allowing a user to reset the adapter when the system reset button is pushed is in the case where someone inadvertently hits the system reset button before the adapter finishes writing out its track buffer.

4. You make an excellent point re socketing the 7438s. I was thinking exactly the same thing... and I completely agree, it would be best to have all 7438s in DIP sockets.

[Aron Hoekstra]

Thanks I fixed the schematic for the 7438's

Here are the parts chosen, please review:

7438 - will remain through-hole/socketed

74F74 - https://jlcpcb.com/partdetail/TexasInstruments-SN74F74DR/C6805

74F138 - https://jlcpcb.com/partdetail/TexasInstruments-SN74F138DR/C354160

74F163 - https://jlcpcb.com/partdetail/TexasInstruments-SN74F163ADR/C2675415

74F04 - https://jlcpcb.com/partdetail/TexasInstruments-SN74F04DR/C7159

74F00 - https://jlcpcb.com/partdetail/TexasInstruments-SN74F00DR/C7158

74F08 - https://jlcpcb.com/partdetail/TexasInstruments-SN74F08DBR/C4469192

74HCT163 - https://jlcpcb.com/partdetail/TexasInstruments-CD74HCT163M96/C2866759

To view this discussion visit https://groups.google.com/d/msgid/cromemco/3c43c953-b11b-4ce3-b2a0-74d739df5e9dn%40googlegroups.com.

[Mike Arnold]

Aron, those parts look ok. 

Peter, those with itchy reset fingers should not solder in the pRESET diode :-)

[Peter Higgins]

The SMT parts look okay to me also.

I've started looking at sourcing the 20MHz Z80. Unfortunately eBay is basically the only way to go. Within all the listings I've looked at I wouldn't be surprised if half the sellers are listing rebadged parts that may not be what the chip markings say they are. This is not going to be easy.

[curt mayer]

I have bought a lot of 20 MHz marked cmos z80 from eBay Chinese sellers, and at most 10% were legit.  The dead giveaways: they smelled like fresh paint, had identical top markings, date codes, etc, but the bottom mold marks were all different.  Be careful out there 

one of the crossbeams has gone out of skew on the treadle

To view this discussion visit https://groups.google.com/d/msgid/cromemco/48428be2-e45b-444c-b233-6f812e477482n%40googlegroups.com.

[Peter Higgins]

I looked a bit further into the issue Mike previously encountered with MAX232 chips that would "lock up" and then go into meltdown.

The problem seems to be entirely related to use of "fake" MAX232 chips. I was surprised by how big an issue this is with the MAX232 when I did a search on the words "fake MAX232".

[Mike Arnold]

Curt, thanks for the warning. I have an idea! Aron, would it be possible to also put an SMD pad layout on the board for the Z80 so that if we cannot source the DIP then we could manually solder (!!!) a QFP/PLCC in? Maybe that is a daft idea. I actually have a couple of spare 20MHz parts which I could pass on if desperate. Also, I think that the 10MHz part would work if clocked at 10MHz but I/O would be a bit slower. Not tested this.

Aron/Peter, I have tested the 28C256-150 and it works fine.

For information, the -5V supply draws 35mA which means the 7905 will dissipate less than 0.5W so does not need too much copper for a heatsink.

Mike

[Peter Higgins]

On Monday, July 21, 2025 at 7:54:52 AM UTC-7 Mike Arnold wrote:

Curt, thanks for the warning. I have an idea! Aron, would it be possible to also put an SMD pad layout on the board for the Z80 so that if we cannot source the DIP then we could manually solder (!!!) a QFP/PLCC in?

The problem is not being able to source the 20MHz DIP version (there are seemingly many available on eBay)  rather it is in sourcing parts that are not fake/rebadged. Unfortunately the 44 pin PLCC and LQFP versions are also afflicted by the same fake/rebadge problem. This has gotten to the point where one needs to buy a Z80 tester (there are several inexpensive versions available) that can help sort out the "likely okay" from the rebadged parts.

If there is room on the board, I suppose Aron could add a place to solder in a 44 pin PLCC socket. As an alternative, anyone interested in using the PLCC version could build this adapter specifically designed to plug the 44 pin PLCC version of the Z80 into a 40 pin DIP socket:

https://www.martenelectric.cz/z80cpu_plcc44_dip40_adapter.html

[Aron Hoekstra]

7.  The oscillator data sheet does show 0.01uF, should I stick with that?

https://lcsc.com/datasheet/lcsc_datasheet_2410311228_CTS-Electronic-Components-CB3-3C-3M686400_C1851439.pdf

9. Does it matter which pin / lead has the resistor?

10. Can you share a little schematic of how this should be set up?

To view this discussion visit https://groups.google.com/d/msgid/cromemco/05fc31bf-647f-4c16-bf82-e910168d5fe6n%40googlegroups.com.

[Aron Hoekstra]

Also I don't think I've added the external power headers to the schematic yet. What should I add inputs for: +8V, -16V, and GND?

[Peter Higgins]

My interpretation of the oscillator circuit diagram provided in the datasheet is that it merely indicates the parameters under which the manufacturer tests the device. For production use, I suggest using a standard 0.1uF capacitor, same as used for bypass of all the other logic ICs.

The resistor in series with the piezo sounder can be attached to either lead.

[Peter Higgins]

On Monday, July 21, 2025 at 7:28:01 PM UTC-7 Aron Hoekstra wrote:

Also I don't think I've added the external power headers to the schematic yet. What should I add inputs for: +8V, -16V, and GND?

Good question.... Mike designed his prototype stand-alone board for a regulated power input of +5V, -5V, and GND. For those using this as a standalone board, would they prefer:

- providing regulated power (as Mike has done)

- providing unregulated power allowing for a wider range of power input (minimum +/- 8V)

My guess is most would prefer the unregulated power option, in which case you can parallel the external power inputs with the S-100 bus power inputs to the board.

Re Mike's suggestion for a manual reset circuit:

- have a pair of solder pads with 0.3" spacing

- one solder pad connects to U45 pin 1, and the other solder pad connects to S-100 bus pin 75 (which is /RESET)

- user can decide whether to implement this option, by manually soldering a IN4148 diode to the pads

[Aron Hoekstra]

sounds good yeah I'll go with unregulated input since we'll have at least the smd 7905 already on there

To view this discussion visit https://groups.google.com/d/msgid/cromemco/dbe78322-7344-47d4-a344-808d9be4bb1bn%40googlegroups.com.