Old PADS-PCB Orcad Project

Help Support GroupDIY:

spoontex

Well-known member
Joined
Jun 14, 2019
Messages
45
Hi,

I want to build this tube based headphone amplifier. But It seems that the pcb files are made with an old version of PADS-PCB and orcad, the same with the gerber files. Anyone can help me to open this files or convert to standard Gerber for me?

Thanks.

 

Streamliner

New member
Joined
Jul 31, 2015
Messages
4
I just looked at the gerbers w/ CAM350...they are not exactly aligned. You need to point this out to your fabricator so they can correct it. I used to use PADS PCB & Perform (now using PADS VX) and this was typical. But the gerbers are good.
I converted his Orcad schematic to PADS Logic (but he has a pdf there).
I looked at the dxf and dwg files, and they are empty and disabled. But it would be easy to replicate in Solidworks from the pictures and dxf export of gerbers alone.

IF....IF you are going to use JLCPCB or any of those offshore fab houses....MAKE SURE THEY UNDERSTAND THAT THE GERBERS ARE NOT ALL ALIGNED. Talk to them first.
 
Last edited:

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
197
Hi,

I want to build this tube based headphone amplifier. But It seems that the pcb files are made with an old version of PADS-PCB and orcad, the same with the gerber files. Anyone can help me to open this files or convert to standard Gerber for me?

Thanks.

I would hold-off on building this headphone amplifier from the supplied GERBER and N/C Drill files for just a little while. Similar to "Streamliner", I also have the CAM350 program and after I had imported all of the data files from the supplied ZIP-file and reviewed everything, in my opinion everything is at least "slightly hosed" and I wouldn't trust it to actually build something from!!!

As "Streamliner" has pointed out, not only are none of the GERBER files in alignment with one another, but none of the GERBER files are in alignment with the N/C Drill data files!!! Now..........since it is the job of the PCB fabricator to provide you with "GOOD" PCBs, they will have to spend the time to correct and fix everything that is messed up in order to get you a "GOOD" PCB!!! And.....time is money!!! So, it's very possible that your "Setup Charge" many end up being higher because of the amount of time spent fixing stuff.

Now.....since I am an "Official Old Fart" that sits here staring at my 34" curved monitor while collecting vintage dust, I have already gone ahead and aligned all of the data files together so they all have the same "0/0" origin point. Then, I saw some items within the SILKSCREEN Layer that bothered me, as it could create some confusion, so I am cleaning some of those items up as well.

The N/C Drill file is like way out-of-line from anything I would consider "NORMAL" in its format structure, so I will be tackling that next and then my CAM350 will output a better and newer N/C Drill Data output file for your PCB fabricator to use. Then, after I get that accomplished, I will check over the SOLDERMASK Layer and see if that needs any attention. I am certain that it will as well.

So.....HANG ON THERE!!!.....for a short while as I struggle through trying to get everything straightened out here with these files.

/

By the way, "Streamliner".....which version of CAM350 are you using? How often do you use it?

/
 

Streamliner

New member
Joined
Jul 31, 2015
Messages
4
I would hold-off on building this headphone amplifier from the supplied GERBER and N/C Drill files for just a little while. Similar to "Streamliner", I also have the CAM350 program and after I had imported all of the data files from the supplied ZIP-file and reviewed everything, in my opinion everything is at least "slightly hosed" and I wouldn't trust it to actually build something from!!!

As "Streamliner" has pointed out, not only are none of the GERBER files in alignment with one another, but none of the GERBER files are in alignment with the N/C Drill data files!!! Now..........since it is the job of the PCB fabricator to provide you with "GOOD" PCBs, they will have to spend the time to correct and fix everything that is messed up in order to get you a "GOOD" PCB!!! And.....time is money!!! So, it's very possible that your "Setup Charge" many end up being higher because of the amount of time spent fixing stuff.

Now.....since I am an "Official Old Fart" that sits here staring at my 34" curved monitor while collecting vintage dust, I have already gone ahead and aligned all of the data files together so they all have the same "0/0" origin point. Then, I saw some items within the SILKSCREEN Layer that bothered me, as it could create some confusion, so I am cleaning some of those items up as well.

The N/C Drill file is like way out-of-line from anything I would consider "NORMAL" in its format structure, so I will be tackling that next and then my CAM350 will output a better and newer N/C Drill Data output file for your PCB fabricator to use. Then, after I get that accomplished, I will check over the SOLDERMASK Layer and see if that needs any attention. I am certain that it will as well.

So.....HANG ON THERE!!!.....for a short while as I struggle through trying to get everything straightened out here with these files.

/

By the way, "Streamliner".....which version of CAM350 are you using? How often do you use it?

/
V12.1....and not very often any more. I saw some of the silkscreen stuff you mentioned, and agree. Some of the cap polarity markings make for some ambiguous and dangerous assembly lol.
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
197
Hi,

I want to build this tube based headphone amplifier. But It seems that the pcb files are made with an old version of PADS-PCB and orcad, the same with the gerber files. Anyone can help me to open this files or convert to standard Gerber for me?

Thanks.

[convert to standard Gerber for me?] -- Well.....The GERBER files that are available for this project and/or are within the ZIP file are already "standard" GERBER files, they are just a very, very, very, very old version of GERBER files!!! Personally, I haven't used this type of version of GERBER files since 1993. This version of GERBER files is called "RS274-D". What you -- REALLY -- want to use as a minimum is called "RS274-X" and ideally in today's CAD-design world, you would be better off using the new "ODB++" file format.

Attached to this message you will find three (3) PDF files detailing the GERBER data files concerning this project of yours. The first PDF file is titled, "HA1 -- Original Screwed-Up PCB Data Files" and it shows you how all of the various data files are "non-aligned" with one another. As I have already written previously, "YES!!!" you can send these files out to a PCB fabricator, but then before they are able to fabricate a working PCB for you, -- THEY -- have to make sense out of all of this mess in order for them to create the films, program their drilling machines, etc., etc. and come up with a PCB that will work for you.

The second PDF file is titled, "Headphone Amplifier -- Separate Gerber Files" and, although you cannot "see" it as this PDF file visually presents this data to you, all of the GERBER and N/C Drill data files are in alignment with one another, but are displayed individually one-by-one. This allows for you to easily see what is on each layer and how things are within each individual layer.

The third PDF file is titled, "Headphone Amplifier -- Composite Gerber Files" and here, not only are you able to see that now all of the files are in alignment with one another, but you can also see that each layer is displayed as a different color, which makes it somewhat easier to differentiate one layer from another. My being able to align the layers with one another was done by using my CAM350 "GERBER Editor" program. Not too many people at home have this software as it is like "way pricey"!!!

Now.....while I am somewhat familiar with the design engineering work of Mr. Millett, who had originally designed this circuit and I have the utmost and highest regard and respect for him as a "Circuit Designer", but as a "PCB Designer" however, I would rate this layout to be between a > C- < and a > D < due to all of the "phoo-pahs" that are evident within this PCB design. Which only goes to prove a long-standing point.....Just because you may be the "King of Circuit Design".....it doesn't automatically also make you the "King of PCB Design"!!! I am in no way, shape or form putting Mr. Millett down in any manner. I am merely commenting that he has done things within this PCB layout that -- IF -- I had done any of the same things while designing a PCB for any of the companies that I have worked with.....I would have been immediately "shown the door" and escorted out of the building!!! There are -- JUST SOME THINGS THAT YOU JUST DON'T DO -- in PCB design work!!! I am only guessing that since his layouts are for hobbyists and DIY'ers, that he simply let certain things slide-by and considered these items to be unimportant and NO BIG DEAL.

The one main item of contention within this set of PCB fabrication files is the fact that Mr. Millett is showing that there needs to be two different drill-size hits in four different locations, yet this additional drill-hit information does -- NOT -- appear within the N/C Drill Data file or in the Drill Report File. It is only merely mentioned somewhere in one of the GERBER files with a line pointing to a single location. In other words.....it's easy to miss this. UN-COOL!!!

As I was working on cleaning up and fixing this set of GERBER and N/C Drill Data files for you, I ended up having to chuckle to myself, as I discovered that I had already downloaded the exact same set of files from somewhere about a year and a half ago and I had forgotten that I had done so!!! Then, I remembered that I had wanted to build a "Vacuum-Tube Based Headphone Amplifier" for a friend of mine who is really into tubes and their "sound", but I just forgot that I already had this circuit!!! WOW!!!

Looking around on my hard-drive, I saw that I had also downloaded the "original" schematic that was created using the OrCAD Schematic software and since I also have the entire platform or "suite" of CADENCE/OrCAD "PCB Editor" Release 17.4 software, I then remembered that I was going to use Mr. Millett's OrCAD schematic and then I was going to create my own OrCAD PCB layout of this "Headphone Amplifier" which would eliminate all of the various layout, soldermask, silkscreen and fabrication errors that are inherent within this particular layout. I also remembered that I was going to go ahead and build a second "Headphone Amplifier" for myself, so I could listen to The MOODY BLUES and PINK FLOYD here in my "Official Old Fart" vintage-audio days of life with a swirling haze of "Mother Nature" wafting about above me!!! AAAAAHHHHHH.......GRO-O-O-O-OOOVY!!!

Anyway.....back to reality.....it will still take me a bit of time to continue going through these PCB data files and straightening things out within them. When I finally get them done.....I will let you know, OK??? Sound like a plan???

/
 

Attachments

  • HA1 -- Original Screwed-Up PCB Data Files.pdf
    149 KB · Views: 5
  • Headphone Amplifier -- Separate Gerber Files.pdf
    117.9 KB · Views: 3
  • Headphone Amplifier -- Composite Gerber Files.pdf
    116.9 KB · Views: 3

ruffrecords

Well-known member
Joined
Nov 10, 2006
Messages
14,553
Location
Norfolk - UK
I designed an 'improved' version pf Pete Millet's tube headphone amplifier. It incorporates some negative feedback to reduce the distortion in the outpu stage. I had some PCBs made and built one into my very first mixer. The remaining PCBs I sold over the years. However, I have open sourced the Gerbers which you can find under the DIY rab of my web site:

Custom Tube Consoles - DIY

Just scroll down and click on the the OpenSourcePCBs folder. The file you want, if interested, is ECC99pone.zip

Cheers

Ian
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
197
I designed an 'improved' version pf Pete Millet's tube headphone amplifier. It incorporates some negative feedback to reduce the distortion in the outpu stage. I had some PCBs made and built one into my very first mixer. The remaining PCBs I sold over the years. However, I have open sourced the Gerbers which you can find under the DIY rab of my web site:

Custom Tube Consoles - DIY

Just scroll down and click on the the OpenSourcePCBs folder. The file you want, if interested, is ECC99pone.zip

Cheers

Ian
THANKS, Ian!!! I will certainly look them over!!!

I was wondering about a couple of things on your "improved" circuit". 1) Would you possibly have a KiCAD schematic of your new design? That would be a rather neat thing to have!!! 2) Is there a "Power Supply" schematic that would go along with this circuit? Would one of your existing "Power Supply" designs work with this circuit? 3) Apparently due to the age of your BOM file, the links that you have included now go to "Discontinued" parts. Updating that may be something to do during on a Saturday afternoon while enjoying a cup of tea!!!

While I have no idea of what the technical capabilities are that Spoontex may possess, I get the impression that they may not have the ability to redraw your hand-drawn schematics into a CAD-design program, let alone layout a PCB. But, I could be completely wrong with my assumption!!! Should you not have a KiCAD schematic, I can do that both for myself and Spoontex, as well. But, a power-supply schematic will also be needed anyway.

I was going to work from an OrCAD schematic that Mr. Millett had originally provided because I also have that software. But, I know that you are a fan of KiCAD, so if I were to redraw your hand-schematic, I would go that route "just because".

And, if I may say so.....I personally and truly admire and respect all of your vacuum-tube knowledge to the utmost!!! I am merely a "builder" of electronic equipment and I only have a rudimentary knowledge of actual electronics. So, my knowing someone such as yourself who knows all about "biasing" and "how to load impedances" and knows about "negative feedback" and all of that, well.....I cannot help myself but to -- "bow down" -- to someone who knows all of that stuff!!! THANK YOU FOR JUST BEING!!!

/
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
197
I designed an 'improved' version pf Pete Millet's tube headphone amplifier. It incorporates some negative feedback to reduce the distortion in the outpu stage. I had some PCBs made and built one into my very first mixer. The remaining PCBs I sold over the years. However, I have open sourced the Gerbers which you can find under the DIY rab of my web site:

Custom Tube Consoles - DIY

Just scroll down and click on the the OpenSourcePCBs folder. The file you want, if interested, is ECC99pone.zip

Cheers

Ian
GREETINGS!!! --- I don't know if my last posting actually made it on here or not, but I was wondering if you happened to have a power-supply schematic for your "Improved Headphone Amplifier Schematic" that you had recently posted? Or, can you direct me to a power-supply schematic somewhere on this forum or anywhere on the Internet that would work just as well with your own "Improved" schematic? I am not a circuit designer, so I don't even know where to begin to design such a circuit, no matter how easy it may actually be. But, I can certainly take a completed schematic and turn it into a pretty nifty end product!!! (NOTE: I tend to prefer using all PCB-mounted components primarily to eliminate loose wiring within an enclosure and also having to use extra connectors to interface between externally mounted components and the PCB. Just saying.....). THANKS FOR EVERYTHING!!!

/
 

ruffrecords

Well-known member
Joined
Nov 10, 2006
Messages
14,553
Location
Norfolk - UK
The HT250 power supply would be fine for the HT. The heaters can just be 12V AC direct from a suitable transformer. Th HT350 schematic is attached.

Unfortunately I don't have a Kicad schematic for the improved headphones amp. The hand drawn one is the only one. When I first started doing my own PCB layout about 15 years ago, affordable PCB was hard to come by and I settles on FreePCB which as its name suggest is free. However it has no schematic capture although you can use TinyCAD to create net lists for it to import. Unfortunatelt TinyCAD is missing may of the schematic parts I wanted to use so I just drew the schematics by hand and used FreePCB to create PCB versions. Fortunately all my boards are quite simple so forward and back annotation takes place inside my head.

Cheers

Ian
 

Attachments

  • HT250schematic.png
    HT250schematic.png
    37.6 KB · Views: 9

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
197
The HT250 power supply would be fine for the HT. The heaters can just be 12V AC direct from a suitable transformer. Th HT350 schematic is attached.

Unfortunately I don't have a Kicad schematic for the improved headphones amp. The hand drawn one is the only one. When I first started doing my own PCB layout about 15 years ago, affordable PCB was hard to come by and I settles on FreePCB which as its name suggest is free. However it has no schematic capture although you can use TinyCAD to create net lists for it to import. Unfortunatelt TinyCAD is missing may of the schematic parts I wanted to use so I just drew the schematics by hand and used FreePCB to create PCB versions. Fortunately all my boards are quite simple so forward and back annotation takes place inside my head.

Cheers

Ian
THANK YOU SO MUCH!!! I really do appreciate the power-supply schematic that you have provided. THANKS!!!

Now.....what changes to the schematic values need to be made in order to work properly with a 120VAC input here on "the other side of the pond"? I have a few PCB-mounted 120VAC/120VAC @ 100 mA "Isolation Transformers" that should work for this I'm guessing. I also have a few PCB-mounted 120VAC/12.6VAC @ 2.85-Amp transformers that should be suitable for the tube heaters.

Your schematic shows an R4 as " 2 X33K 2W " ..... Does that mean there are - 2 - 33K 2W resistors in parallel? Or, series? I'm not sure. And, your headphone amplifier schematic shows the C5 and C6 symbols drawn with a small rectangle box at the top. Is that the
positive ( + ) side? I realize that you "Blimey's" over there do things a bit differently than us 'Merican's do over here, so I just want to make sure. I have seen some other European schematics where a small rectangle box shown on a capacitor symbol was actually the "NEGATIVE" side going to GND, so I need to have that clarified. THANKS!!!

Since I don't see any 75V terminal or usage within your headphone amplifier schematic, I am assuming that it is something that was leftover from whatever this schematic was originally designed for, correct? So, those parts can be deleted/eliminated, right? Come to think of it, if the 75V output is not needed, then wouldn't R4, R5 and C5 all be eliminated???

The HT250 schematic capacitor C6 that goes across the mains input is probably either a 0.1mF or a 0.01mF @ 400V capacitor?

And, I am also assuming that a rating of 1-Amp is sufficient for the HT250 schematic component DB1? I have a bunch of small 6.2mm X 8.5mm PCB-mount "Thru-Hole" diode bridge rectifiers. I also have several 3-Amp versions as well, just in case.

What value (audio-taper?) pot could be used on the input feeding V1/Pin-7 as a volume control? 50K?

I saw that the SOWTER 8665A transformers are in the neighborhood of 125-Euros each!!! Since I am an "Official Old Fart" and my hearing is nowhere nearly as good as it was when I was in my 20's (the old TV horizontal circuits at 15KHz used to drive me nuts!!!), is there a suitable and certainly less expensive type of PCB-mount output transformer that could be used instead? Maybe if you can just provide me with the suitable transformer characteristics (i.e. turns ratio/DC resistances/impedances/inductance/etc. and so forth), I could try to locate and source a transformer on my own. I realize that you have to be a busy person running your mixing console company and don't have the time for doing something like this. I'm not running a recording studio and my old hearing "ain't so good anymore", so I don't need any top-notch/high-end output transformers for what I will be using this for. I would just enjoy the overall "vacuum-tube sound" and let it go at that!!!

I >> THANK YOU!! << again for all of your assistance!!!

JBW

/
 

ruffrecords

Well-known member
Joined
Nov 10, 2006
Messages
14,553
Location
Norfolk - UK
Answers as follows:

You really need a mains transformer with a 240VAC secondary. Here is a groupDIY thread that lists some alternatives:

HT Transformers for Vacuum Tube Preamps

Your heater transformers should be fine.

2 x 33K means two 33K 1W resistors in series. These, combined with the 22K resistor divide the HT by exactly four. Because the pair of 33K resistors support three quarters of the HT voltage, they dissipate more heat than the 22K so I used a pair to share the heat (and 66K is not a standard value anyway)

The open rectangle of a capacitor does indeed represent the positive terminal. If you look at the HT250 schematic you will see it also uses them but includes a handy + sign as well just to be sure.

The 75V output is needed. The headphones amplifier uses what is called an SRPP output stage which has one triode sitting on top of another. The voltage on the cathode of the top one is therefore about half the HT voltage whereas the bottom one is close to analogue 0V. All tubes will only support a limited positive or negative voltage between their heaters and cathode. The heaters need to be referenced to analogue 0V somehow in order to prevent hum. If you connect one side of the heaters direct to analogue 0V then the top triode of the SRPP has half the HT voltage plus the signal on its cathode. This can come uncomfortably close to or exceed the tubes' spec for the allowed voltage between heater and cathode (known as Vhk). The solution is to "elevate the heaters". Instead of connecting one side of the heaters to anlalogue 0V you connected it to the 75V output which ists at one quarter of the HT voltage. The top cathode now is only 25% of the HT above its heater and the bottom cathode is 25% below it so both are within the Vhk spec.

C6 is 100nF which is 0.1 microFarads. If you write 0.1mF that really means milliFarads. The usual abbreviation for microFarads is uF. I normally use these:

https://uk.farnell.com/kemet/r46ki310000m1k1/cap-0-1-f-10-pp-radial/dp/2429367?st=100nf

For DB1 I use a DIL 1 AMP 100V part such as this one:

https://uk.farnell.com/vishay/df10m-e3-45/bridge-rectifier-1kv-1a-dip/dp/3373276

An audio taper pot is what you need. The value depends as much as anything on what you drive it with, but 50K will be fine for just about all sources.

The Sowter transformers are very good but very expensive. There used to be a much cheaper alternative available from Edcor on your side of the pond. It was one of their WSM series with a 32 ohm secondary but I do not see it listed on their web page. It is what I used in the prototype. It was a 4K8:32 type (12:1 turns ratio).

Cheers

Ian
 

Latest posts

Top