6128 Plus video output distribution amplifier (splitting)

Started by Cwiiis, 17:44, 20 August 21

Previous topic - Next topic

0 Members and 1 Guest are viewing this topic.

Bryce

The 100µf C1 and RetroCPC's C6 perform the same function. The position on the layout is good too, so just decide which value you want to use (I think 100µf would be sufficient). The smaller C5 should be in parallel to your C1 and also close to the power socket.

Bryce.

RetroCPC

Chris,

To make your life easier, (and if you cared about interchannel Crosstalk - not so much an issue with the "Lo-Fi" CPC audio quality...)  then I suggest having one Dual opamp for the Left Channel and the second Dual Oamp for the Right Channel - this will make your Schematic, PCB layout & Life :) much easier.

When you layout the PCB, you want the PCB tracks between (R22,R30,R31,R23) & (R24, R25, R32, R35) and there connections paths to there respective +in / -in on the opamp as as short as possible (so the shortest PCB track from this end of the resistors to the opamp (+in / -in inputs).

"C6 postion" on my schematic can be place in parrellel with your C11 & C10...

WRT the potentional "Hum / Buzz" issue - I was refering to the fact you have the Left Audio input physically next to the Video Sync pin on the input header, as they are so physically close to each other, the high impedance audio input from the CPC could pick up the Sync signal which is physically one pin over (which could result in Hum / Buzz)... So my suggestion is to have the Audio inputs on a seperate pin header, physically spaced away from the Video pin header...

Also, good practice to layout the Audio input header "Left input, Ground, Right input"- with the center Ground pin now offering some isolation between the Left & Right channels (improving interchannel Crosstalk).

A lot of this is "Too much quality" for the CPC, but its more about learning - if your going to the effort :)

Bryce

Yup, you're giving some really excellent best practice audio design tips, but for a very Lo-Fi signal source :D It's a bit like giving tips on what 8K 75in OLED TV would be best for watching VHS video on. But it's all good information which can (and should) be used on "real" audio projects.

Bryce.

Cwiiis

Quote from: RetroCPC on 15:20, 02 September 21Chris,


To make your life easier, (and if you cared about interchannel Crosstalk - not so much an issue with the "Lo-Fi" CPC audio quality...)  then I suggest having one Dual opamp for the Left Channel and the second Dual Oamp for the Right Channel - this will make your Schematic, PCB layout & Life :) much easier.


When you layout the PCB, you want the PCB tracks between (R22,R30,R31,R23) & (R24, R25, R32, R35) and there connections paths to there respective +in / -in on the opamp as as short as possible (so the shortest PCB track from this end of the resistors to the opamp (+in / -in inputs).


"C6 postion" on my schematic can be place in parrellel with your C11 & C10...


WRT the potentional "Hum / Buzz" issue - I was refering to the fact you have the Left Audio input physically next to the Video Sync pin on the input header, as they are so physically close to each other, the high impedance audio input from the CPC could pick up the Sync signal which is physically one pin over (which could result in Hum / Buzz)... So my suggestion is to have the Audio inputs on a seperate pin header, physically spaced away from the Video pin header...


Also, good practice to layout the Audio input header "Left input, Ground, Right input"- with the center Ground pin now offering some isolation between the Left & Right channels (improving interchannel Crosstalk).


A lot of this is "Too much quality" for the CPC, but its more about learning - if your going to the effort :)

Ok, here we go, let's hope this is a revision good enough to go to the printers! I'll wait for feedback, as it seems pretty likely I may have made mistakes... I've attached the updated circuit diagram and PCB layouts. My previous layout really didn't have enough room left for all the audio circuitry, so I started from scratch and its ended up quite a bit smaller (90x108mm now). Once again, thanks for all of this guidance, there is zero chance I could have done any of this without help...

RetroCPC

Chris,

WOW your quick (That's what she said)... to spin a PCB! your welcome to came and help me out with my PCB designs!!!

Almost there:

Shield should be connected to Ground - I'd just just bringing the Ground plane all the way to the bottom of the PCB (on both layer) - also, your Video input header should have a Video Ground signal - so you will have two Grounds coming from the CPC - one for Audio, and one for Video... (is the CPC+ Shield connected to Ground on the CPC side? I'm presuming it is...)

Also, I'd add some PCB vias evenly distributed across the PCB to tie the top and bottom Ground planes together for lowest Ground plane impedance - see attached image you can see the vias evenly spread around the Solid Ground plane to connect to different Ground layers  (Top / Bottom in your case).

Also, for shortest PCB track from Resistor Pad to Opamp +IN pad, I'd move resistors R30, R31, R32, R33 upwards towards the Top of the PCB, this will result in the short connection track to the +IN's on the Opamp.

Its always a good idea to add a HF bypass capacitor as close as possible to your power input jack - so I'd add an extra 100n Ceramic capacitor in the space in-between the DC input Jack and C1.

Last point, I'd thicken the PCB tracks where possible - with the power tracks as thick as you can go without going stupid (I typically use 40th to 100th for "thinner" power tracks) - with signal tracks from 10th to 30th depending (30th for audio / 10th for Video) :) thin PCB tracks are easy to break - ESPICALLY to connector pads - and larger unsupported stand up components (such as the transistors) - its common practice to use "tear-droping" to go from say a connector pad to a thinner PCB signal track (such as the video signal lines) - attached is an image of a pcb teardrop... (You just want to added extra Copper support to the thinner PCB tracks from component Pads that can be stressed).

My PCB software is rather old and does not automatically create teardrops - so l just manually step down the PCB track as it progresses from the component pad e.g.:

Connecter pad is 80th diameter, so I start from the connector pad with a short length of 80th PCB track (to create the "teardrop"), and then step down to say 10th track (for signals such as video) for the "proper track" that goes along the PCB...

Dont forget to add your name to your PCB :)

Cwiiis

Quote from: RetroCPC on 07:25, 03 September 21
Chris,

WOW your quick (That's what she said)... to spin a PCB! your welcome to came and help me out with my PCB designs!!!

Almost there:

Shield should be connected to Ground - I'd just just bringing the Ground plane all the way to the bottom of the PCB (on both layer) - also, your Video input header should have a Video Ground signal - so you will have two Grounds coming from the CPC - one for Audio, and one for Video... (is the CPC+ Shield connected to Ground on the CPC side? I'm presuming it is...)

Also, I'd add some PCB vias evenly distributed across the PCB to tie the top and bottom Ground planes together for lowest Ground plane impedance - see attached image you can see the vias evenly spread around the Solid Ground plane to connect to different Ground layers  (Top / Bottom in your case).

Also, for shortest PCB track from Resistor Pad to Opamp +IN pad, I'd move resistors R30, R31, R32, R33 upwards towards the Top of the PCB, this will result in the short connection track to the +IN's on the Opamp.

Its always a good idea to add a HF bypass capacitor as close as possible to your power input jack - so I'd add an extra 100n Ceramic capacitor in the space in-between the DC input Jack and C1.

Last point, I'd thicken the PCB tracks where possible - with the power tracks as thick as you can go without going stupid (I typically use 40th to 100th for "thinner" power tracks) - with signal tracks from 10th to 30th depending (30th for audio / 10th for Video) :) thin PCB tracks are easy to break - ESPICALLY to connector pads - and larger unsupported stand up components (such as the transistors) - its common practice to use "tear-droping" to go from say a connector pad to a thinner PCB signal track (such as the video signal lines) - attached is an image of a pcb teardrop... (You just want to added extra Copper support to the thinner PCB tracks from component Pads that can be stressed).

My PCB software is rather old and does not automatically create teardrops - so l just manually step down the PCB track as it progresses from the component pad e.g.:

Connecter pad is 80th diameter, so I start from the connector pad with a short length of 80th PCB track (to create the "teardrop"), and then step down to say 10th track (for signals such as video) for the "proper track" that goes along the PCB...

Dont forget to add your name to your PCB :)
Thanks, and so close now! Unfortunately I'm out for the day, but I got a little bit of time this morning to start on some of those changes - attaching a screenshot in case there was any misunderstanding; all my traces were previously 10mil, I've now added a bypass cap to the power input and bumped up those traces to 30mil, after C1 all power lines are now 20mil and I've started making all the audio traces 20mil too. When I get home later I'll finish off and teardrop all the through-hole pads, as well as add a bunch of vias :)

Re the shield/ground, I've tested a few cables and machines in the past and none seem to connect them to the same ground source... I'll avoid that in this board, with the presumption that if either side ties them together then that will do (unless you think otherwise?) - I'll double-check this specifically on the Plus when I get back later too :)

Cwiiis

And hopefully done! All the suggested changes made I think, bar the shield/ground tie. I'll let it cool off for a day or so, so any comments, please do let me know, but otherwise I'll take this to the printers and cross my fingers :)

RetroCPC

Chris,

:) Its getting there (have I said this before)? ...

You added extra Vias :) , but they are isolated from the Grounds - so apart from adding extra holes to the PCB they currently serve no useful function :)

Also, for High Frequency signals, its recommended to avoid 90Deg sharp track angles - also avoid unnecessary track "details / undulations" - some examples:

The PCB track from the Emitter of Q6 to R10 has both (90Deg angles + some weird "pip undulation" on the track) - not good for HF signal intergrity nor my OCD...

The PCB track from the Emitter of Q10 to R17 could avoid the 90Deg transition if you just continued the 45Deg section.

The Transistor Base connections (middle pin) could just be run though the first transistor to the second transistor Base pad - no need for the "twisted" track length to the second transistor Base's....

I'd also move the whole transistor block (with input termination Resistors) down the PCB - as close as possible to the output DIN sockets - this reduces the PCB track lengths (Video is High Frequency signals).

Also, rotate R1, R2, R3, R4, R13 - so that the Resistor end that connects to the transistor Base is as close as possible to the transistor Base - also the Ground end of the Resistor is now as near as possible to input Ground (Best for signal termination).

Last point, if you move the Via closer to the Opamp Power pin (Pin 8) - this will allow a wider ground path under both Opamps - at the moment, the Ground path flowing under the Opamp is unnecessary restricted by the Power Via on Opamp Pin 8 placed so far away from the pin / pad.

When I design PCB's, I always tray to move tracks to minimise Ground plane restriction if possible (Such as keeping the Ground plane as wide as possible under the Opamp).

I'm still freaked out that there is only one Input Ground connection (shared fro both Video and Audio)... This would trigger my OCD and prevent me from sleeping at night!!! I'm dont recall if you mentioned you already have done this, but just confirm if the DIN shell is not connected to Ground at the CPC side.. if it is connected, then no need to seperate them on the Buffer PCB.

Personnaly, I would connect them together and have full Ground fill... The more solid Low impedance Ground - the better...


You make a better PCB designer then I could ever be a Musician - I'm so envious!!  :P

pelrun

The 90 degree track thing is a complete myth; it has nothing to do with EMI and everything to do with manufacturing process issues from decades ago that no longer apply. If you're etching your own boards it might help, but if you're getting a proper fab to make them it's irrelevant.
https://resources.altium.com/p/pcb-routing-angle-myths-45-degree-angle-versus-90-degree-angle
I'm still going to use them but only for aesthetic reasons :D

RetroCPC

For sure too much information for a our humble CPC designs, but as Chris is teaching himself PCB design (and doing very well), I'm just offering advice from my own 40+ years of experance of designing electronics & pcbs (I admittelty suffer from OCD).. :)

WRT the Altuim artical, I have to disagree as its very easy to see the reflections of 90Deg PCB traces with a TDR system - I'm afraid the Altuim article is too simplistic and therefore incorrect.

Using a TDR system, any variation along the signal path can clearly been seen, with a sharp 90Deg PCB edge being really messy.... A decent engineer never wants to needlessly compromise there design - so after ones first encounter with the effects observed on a TDR system - avoiding 90 Deg PCB angles becomes matter of fact...

In my lab I use TDR heads on extender cables to bring the TDR sampling system as close as possible to the PCB to aid measurement (probing) fidelity - when those idiots at Altuim show respective TDR measurements then things will become apparent to them.

Do 90deg tracks work - for sure yes, BUT they demonstrably impact HF signal integrity (confirmed by anyone using TDR) so WHY use them if they can be avoided?

Also - anyone who has to worked with Altuim PCB software will attest, Altuim software is truly terrible to use, PCB software designed by software engineers not working PCB designers !!! I have several Altuim perpetual license's as sometimes I have to work with Altuim files, but NOBODY in the lab wants to work with it - I'd rather shoot myself in the head, so I have laugh when I see such article's from Altuim!

As a side note, when I design High speed PCB's I embed TDR test tracks - where I place a rectangle kink (2x 90Deg transition) in the open-ended track length - (with a normally unpopulated SMA connector footprint at one end of the track to allow a controlled connection to the TDR system when needed for QC) - using this imbedded TDR test track(s) allows me to Quality control multilayer PCBs (inner layer stackup, PCB dielectric etc.)

I've attached a picture a 20GHz TDR head I use to measure signal integrity of the critical PCB tracks...

Cwiiis

Quote from: RetroCPC on 06:45, 04 September 21
Chris,

:) Its getting there (have I said this before)? ...

You added extra Vias :) , but they are isolated from the Grounds - so apart from adding extra holes to the PCB they currently serve no useful function :)

Also, for High Frequency signals, its recommended to avoid 90Deg sharp track angles - also avoid unnecessary track "details / undulations" - some examples:

The PCB track from the Emitter of Q6 to R10 has both (90Deg angles + some weird "pip undulation" on the track) - not good for HF signal intergrity nor my OCD...

The PCB track from the Emitter of Q10 to R17 could avoid the 90Deg transition if you just continued the 45Deg section.

The Transistor Base connections (middle pin) could just be run though the first transistor to the second transistor Base pad - no need for the "twisted" track length to the second transistor Base's....

I'd also move the whole transistor block (with input termination Resistors) down the PCB - as close as possible to the output DIN sockets - this reduces the PCB track lengths (Video is High Frequency signals).

Also, rotate R1, R2, R3, R4, R13 - so that the Resistor end that connects to the transistor Base is as close as possible to the transistor Base - also the Ground end of the Resistor is now as near as possible to input Ground (Best for signal termination).

Last point, if you move the Via closer to the Opamp Power pin (Pin 8) - this will allow a wider ground path under both Opamps - at the moment, the Ground path flowing under the Opamp is unnecessary restricted by the Power Via on Opamp Pin 8 placed so far away from the pin / pad.

When I design PCB's, I always tray to move tracks to minimise Ground plane restriction if possible (Such as keeping the Ground plane as wide as possible under the Opamp).

I'm still freaked out that there is only one Input Ground connection (shared fro both Video and Audio)... This would trigger my OCD and prevent me from sleeping at night!!! I'm dont recall if you mentioned you already have done this, but just confirm if the DIN shell is not connected to Ground at the CPC side.. if it is connected, then no need to seperate them on the Buffer PCB.

Personnaly, I would connect them together and have full Ground fill... The more solid Low impedance Ground - the better...


You make a better PCB designer then I could ever be a Musician - I'm so envious!!  :P
You might surprise yourself with the music, much like PCB design, everyone should give it a try! :)

So I've rejigged all the transistor routing/positions - I think that was one of the first bits I worked on, so it definitely needed a revisit - that weird routing instead of just connecting the centres was a hangover from when they were all in a row I think, and some of the wonky tracks and 90 degree angles similarly were side-effects from moving components around. I'm going to look a bit more carefully at the other routes as well in case there are more obvious deficiencies - of course, every change is getting more and more awkward at this point, so I might call it a day soon!

Re the vias, I guess I'm having a hard time seeing where the ground planes get separated - I suppose given it's mostly through-hole parts, every resistor or capacitor ground connection is also acting as a connection between planes? Maybe there's a tool for this that I've not found that'll make it trivial...

So I just tested sheild/ground on the Plus and I'm going to have to eat my words - they are connected. So I guess I can just treat the shield as another ground input and tie it to the ground planes. I feel a little weird doing it as I feel the splitter should act like a cable in some respect, but if it's tied at the Amstrad anyway, may as well take advantage of it. I'm going to open an Amstrad up and triple-check this later...

Bryce

Quote from: pelrun on 07:43, 04 September 21
The 90 degree track thing is a complete myth; it has nothing to do with EMI and everything to do with manufacturing process issues from decades ago that no longer apply. If you're etching your own boards it might help, but if you're getting a proper fab to make them it's irrelevant.
https://resources.altium.com/p/pcb-routing-angle-myths-45-degree-angle-versus-90-degree-angle
I'm still going to use them but only for aesthetic reasons :D

Not quite correct. Sharp points on the edge of tracks act as tiny antennas, however, this only happens when you get up to Gigahertz frequencies with high energy. This can be easily demonstrated with PCB trace spark gaps (great fun to experiment with). But for 99% of circuits it's totally irrelevant.

Bryce.

pelrun

The exceptions are in the linked article, but nobody is making a 10GHz design without actually knowing what they're doing. Not if they want it to work, anyway.

Quote from: RetroCPC on 11:13, 04 September 21WRT the Altuim artical, I have to disagree as its very easy to see the reflections of 90Deg PCB traces with a TDR system - I'm afraid the Altuim article is too simplistic and therefore incorrect. Using a TDR system, any variation along the signal path can clearly been seen, with a sharp 90Deg PCB edge being really messy....
Your TDR is necessarily throwing exactly the sort of ultra high frequency pulses down the line that 90 degree bends dislike to detect issues, but that doesn't mean the circuit itself is doing it in normal operation. After all, the TDR is intended for those high-end applications as well, but it's overkill for a low frequency one.

RetroCPC

pelrun,

People often confuse "operating frequency" with signal frequency content.

While the CPC operates at 4MHz (with a 16MHz Oscillator) - the typical edge speeds on the digital IC's are about 4nS - which equals 250MHz (and don't forget we are talking a squarewave - so signal content much MUCH higher then "4MHz" would suggest). With such edges speeds, you should really take care with characteristic track impedances etc... However, the CPC was design pre EMC days, when digital design was little understood in the consumer world - the introduction of EMC regulations forced designers to take more care with correct signal termination / Ground planes etc. - A cheap "fix" was to Series terminate digital lines with 33ohms to 100ohm resistors at the source...

With 4nS edge speeds, things get messy quickly when incorrectly terminated... and yes, YOU can see the "Ripple" caused by a 90Deg PCB bend even with a 500MHz scope (with correct probing), and things just get even uglier using a faster scope!

pelrun

And we're back to "I can see it when I use high-frequency test equipment". It's still something that will *not* affect the operation of *this* device. We're also not talking about trying to meet commercial radiative EMI standards, which are extremely rigorous and also extremely expensive, hardly something that's going to be required here.
Again, if you're working on a device that *actually* requires proper certification or operates at frequencies where these things actually matter, then there's a hell of a lot more to worry about than just the angle of the trace corners.
(we can argue the point and who has more real-world RF EE experience but it's really not worth the bother. For this design and for almost anything we're likely to see that's CPC related, 45 degree corners are entirely an aesthetic choice.)

Cwiiis

Now now, I think RetroCPC has been pretty clear - at least, as I understand it, while this may not affect this particular board, it is an issue that should be considered in more cases than you might be lead to believe and is good practice to consider, especially for someone like me that's learning. If it's a good habit, why not get into it now when the stakes are a bit lower and have fewer problems in the future?

Anyway, I think this is probably close to the final revision now as I'm getting a bit sick of looking at this  :D

I've moved the transistors down the board and flipped the terminating resistors - I've also re-routed most of those lines, so the video lines are shorter and have fewer kinks and no 90 degree turns. I also made the power line going to the audio section a bit shorter. I noticed that C2 and C4 were offset vertically, so moved those a little so that the traces are shorter and straighter and they're in line with C3 and C5 (I think this must've just been an oversight).

Shield is now tied to ground, so there are two grounds coming in at the top and 2-4 at the bottom, depending on the outputs connected.

I've removed the pointless vias - I'm pretty sure both copper pour layers are continuous (I can't see any disconnected sections) and given the number of through-hole ground pads, I don't understand where adding any vias would make sense. I'll definitely add some if someone can explain that to me though :)

I think at this point, this is probably good enough, but again I'll let it cool for a day in case anyone spots anything terrible, or anything easily implemented that's worth addressing now rather than in a later revision.

Bryce

Quote from: pelrun on 14:12, 04 September 21
And we're back to "I can see it when I use high-frequency test equipment". It's still something that will *not* affect the operation of *this* device. We're also not talking about trying to meet commercial radiative EMI standards, which are extremely rigorous and also extremely expensive, hardly something that's going to be required here.
Again, if you're working on a device that *actually* requires proper certification or operates at frequencies where these things actually matter, then there's a hell of a lot more to worry about than just the angle of the trace corners.
(we can argue the point and who has more real-world RF EE experience but it's really not worth the bother. For this design and for almost anything we're likely to see that's CPC related, 45 degree corners are entirely an aesthetic choice.)

Of course. All this discussion is just theory and completely unnecessary for the circuit in question, but for someone who's learning, it can be an interesting discussion. Even a hobbiest can end up getting into technical issues/trouble when you consider the harmonics that a modern devboard like an RPi can produce on its clock signal. Yes, RetroCPC is gold-plating the design, but it is important "best practice" methods that one should learn.

Bryce.

Cwiiis

Ok, update; I had the PCBs made and got them today - I had enough parts already to populate the video section, making it functionally the same as what I had on the breadboard. Good news: it works! Bad news: there's fringing and a red tint (visible even when the Amstrad is off but the monitor is on and plugged into the splitter) so I expect some of my soldering may have not been up to par or there's an issue with the design I missed. Neither issue were present on the breadboard. It isn't really visible in the photo, but it's very visible in real life.


The only circuit difference between this PCB and my breadboard prototype at this point are the added decoupling capacitors (I only tested with a smoothing cap on the breadboard). I also powered the breadboard via USB rather than barrel jack, but I don't see why that'd make a difference... I reckon either a ground short somewhere or a poor ground connection, based on how I felt about the soldering, but if you guys have any specific ideas of what to look for, I'm all ears :)

Re the design, if I was going to spin another board, there are two things I'd change:
- the input may as well be a DIN8 port - This would make the soldering a bit easier and you can buy DIN8-DIN8 cables, so it'd save making a custom one up. I don't know why I didn't think of this before  :picard: As it is, the cable will be integrated.
- The transistor footprints should have the pins spread out more... They're way too close together and I wouldn't be surprised if I had a short or two somewhere there... I should've checked the footprint more carefully, maybe I'd have noticed before this point. Lesson learned!

Otherwise, it went surprisingly well! Here's hoping I can fix that image degradation and then I'll design an enclosure for it.

Cwiiis

Found the mistake - R1 which is meant to be a 100 ohm resistor on the red line got mixed up at some point and is a 10K resistor - so that'll be that! Will fix tomorrow 🙂

RetroCPC

Wow that was Quick - and great to see professional quality PCBs :) Very nice work :)

Lets us know if the resistor swap resolves the issue :) Then you can be brave and try the Audio section :)

Cwiiis

Quote from: RetroCPC on 12:58, 11 September 21Wow that was Quick - and great to see professional quality PCBs :) Very nice work :) Lets us know if the resistor swap resolves the issue :) Then you can be brave and try the Audio section :)
So yes, I'd mixed up R1 (100 ohm) with R13 (10k). A not-so-quick (jeez, that ground plane really sinks heat...) swap and the video portion of the board performs perfectly! Even with the temporary cable I've put on that I used with the breadboard, the picture quality is bascially as good as plugging straight in - glad I followed all your advice :)

Still waiting for the opamps to be delivered, hopefully they'll come in the next week or two, then I'll put together that portion of the board and report back - fingers crossed! I dare say this is the first Amstrad Plus video amplifier in the world  :P I'll have to do a celebratory live-stream once it's finished!

RetroCPC

Yeh - pretty sure its the first (and only) CPC video splitter :)  I admire your determination and the end results  :)


Just a little worried about the Audio opamps input Bias current, you might need to change a couple of resistor values in the "Virtual Ground" circuit to compensate if it proves an issue... nothing complicated.

When you have the Audio section built, then measure the DC voltage on the opamps outputs and confirm its about 2.5V (before the output capacitors). It should be half the input power voltage so 5V/2.

Bryce

I've a CPC video splitter, but it's only video, no audio and it was made by (ugly) modding a VGA splitter, not an original design.

Bryce.

Cwiiis

Quote from: RetroCPC on 14:09, 11 September 21
Yeh - pretty sure its the first (and only) CPC video splitter :)  I admire your determination and the end results  :)


Just a little worried about the Audio opamps input Bias current, you might need to change a couple of resistor values in the "Virtual Ground" circuit to compensate if it proves an issue... nothing complicated.

When you have the Audio section built, then measure the DC voltage on the opamps outputs and confirm its about 2.5V (before the output capacitors). It should be half the input power voltage so 5V/2.
Just completed the board (got the chips in earlier this week and then discovered I was 1 capacitor and 1 resistor short, bloody typical! Just got those in this evening :)) - measuring the opamp outputs, it is indeed 2.5V (well, I measure 2.46, but this is on a 5V power supply under load, so I assume that's a normal reading). Is this what's expected? After your comments, I'm a bit cautious to just plug the monitor straight in, so I'll wait for your confirmation first in case!

RetroCPC


Powered by SMFPacks Menu Editor Mod