circuit board creation.....

[orange_glow_fan]

Hi Guys,

 First off let me say that I know little about porting a circuit design into a workable PC board  design.. I could probably do this using perf board and point to point wiring, but I'd prefer something more reliable (and probably better looking)

Having said that, can someone tell me how to do exactly that with the pictured circuit?? This needs to be as compact as possible.

It is a replacement for the old 67 1/2 volt 'B' battery used in vintage AC/DC tube radios. The transformer is pricey too!  I've tried contacting the author, but there has been no response. The article was written back in 2003, by a radio collector in Australia and I'm not sure if he still 'around'

Thanks for your input..

Kerry

[Terry S]

Kerry, you are asking a very LARGE question.

I've been designing circuit boards for over 25 years. Well over in fact. And there is no one quick easy answer on how to do it. It's an art and a science. But first off, I would comment that there are much better ways to generate the B battery voltage than that old oscillator/transformer circuit. Again, topic for much discussion I'm sure.

There are a plethora of free PCB design packages -- but before you dive in, check out some possible purchased solutions. I'm sure some of the supplies offered for nixie clocks could be filtered and regulated down to provide 67.5 volts for a B+ supply.

Terry

[Paul Andrews]

The problem with a lot of solutions is EMF from the power supply messing up the radio. I would recommend a couple of things:

1. Post on antiqueradios.com
2. Take a look at this article: http://www.dos4ever.com/battery/battery.html

[Tomasz Kowalczyk]

A boost converter will be also a lot smaller, even with a big LC filter, which is recommended to keep your B+ free of converter noise. 

Also, efficiency will be much higher (80% is very realistic).

Are you able to determine current drawn from B+? Is the circuit drawing constant amount of current (class A operation, which is very probable)?

When it comes to PCB making, I think you should go with KiCAD or Altium CircuitMaker (I barely used the second one, but it offers limited capability of Altium Designer, which I use at work - unfortunately, license cost is out of private use reach).

67,5V is not very high, but you should use wider spacing between tracks than the standard 10mil.

Also, if it is possible, avoid designing a boost converter on the PCB yourself and buy a ready module - half of success of a converter is the PCB layout, which can be really tricky to achieve.

[JohnK]

Consider asking on

http://groups.yahoo.com/group/Oz-Wireless

 

John K

--
You received this message because you are subscribed to the Google Groups "neonixie-l" group.
To unsubscribe from this group and stop receiving emails from it, send an email to neonixie-l+...@googlegroups.com.
To post to this group, send email to neoni...@googlegroups.com.
To view this discussion on the web, visit https://groups.google.com/d/msgid/neonixie-l/61b99c68-4707-4b4c-b548-a0bbadeddb3d%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

[NeonJohn]

Hi Kerry,

If you just want something close to 67.5 volts, snap 8 9 volt batteries
together. That will produce 72 volts open circuit but will pull down a
few volts under load.

If you plan on using it a lot, then you might want to use these batteries

https://www.amazon.com/gp/product/B01M2Z442X/ref=oh_aui_detailpage_o00_s00?ie=UTF8&psc=1

There are two kinds of lithium "9 volt" lithium batteries. Those that
use 2 conventional LiPoly cells and only produce about 7.2 volts, and
these that use 3 LiPo cells and produce almost exactly 9 volts. The
beauty of these cells is that they are recharged using a micro-USB
cable. An excellent use for all those old phone chargers laying around.

Back to your question. That is a bad circuit. He's running at low
frequency so the transformer is huge. It is not resonant so the output
is a square wave. Lots of harmonics. They'll go through the bridge and
appear on the output. He has no filtering to speak of.

I'd use a resonant Royer oscillator running at high frequency. This is
the basis of our company's induction heaters. Here is the open source one.

http://www.neon-john.com/Induction/Roy/Roy.htm

This one runs at about 80kHz. It outputs a sine wave so there is little
output noise. The transformer will be tiny at the power you'll be
operating. You will wind the transformer on a bobbin core. The primary
will be something like 5 turns of Litz wire and the secondary will be
something like 9 or 10 turns.

The circuit board package to use these days is KiCAD. It's a
professional quality program, is FOSS and it's development is mostly
funded by CERN. Eagle used to be the go-to package but since they
started renting their software and not selling it, most of the open
hardware community had moved to KiCAD.

Going from schematic to PCB is fairly straightforward. Each part must
have an outline for the schematic and a footprint of the physical part
for the PCB layout.

You would draw the schematic editor and do a design rule check. This
catches things such as lines close but not quite connected to a pin.

When you're finished with the schematic, you fire up the PCB layout
portion of the program. All your components' footprints will be there
in one blob. You move them around the board, the dimensions of which
you've already specified. The components are connected by "air wires".
The layout is usually quite similar to the schematic layout. You route
traces between components, switching from front to back as needed until
all the air wires are gone.

You'll run another design rule check which will catch things like
crossed traces, connections not quite made, traces too close together
and things like that.

When you're satisfied with the layout, have the program produce Gerber
files. These files contain the actual photoplotter instructions and are
what you send to the board house. You MUST inspect these closely with a
Gerber visualization program. You will frequently find mistakes that
all the preceding steps did not. In the Linux world where I work, the
program gerbv is the best. No idea about other environments.

The last step is to prepare a specification document. It will specify
the board size, what kind of board to use, how thick the copper should
be in ounces, etc. And most importantly what each Gerber file is.
Incredibly there is no convention on naming files. Most folks follow
the Pcad (very expensive board layout program) protocol.

Finally, you bundle the Gerbers up with the specification file into a
zip. After having made arrangements with the board house you select,
you email that zip (or sometimes upload onto a web page designated for
that purpose), pay them and wait for your boards to return.

Before you start any board work, I strongly suggest you download LTSpice
and simulate your circuit. LTSpice is free and it works very well,
especially if you enter all the characteristics for each part. ESR for
capacitors, for example.

I hope that's enough to get you started.

John

--
John DeArmond
Tellico Plains, Occupied TN
http://www.tnduction.com <-- THE source for induction heaters
http://www.neon-john.com <-- email from here
http://www.johndearmond.com <-- Best damned Blog on the net
PGP key: wwwkeys.pgp.net: BCB68D77

[gregebert]

Some other useful tips I can pass along:

1. Make sure you have all of the unique parts so you can visualize how they will fit together. This is especially true for connectors, switches, pots, heat-sinked devices. Mechanical drawings in the datasheet are very helpful, but nothing beats having the part in your hands.

2. When you make your footprints, print them out 1:1 scale and make sure they match your parts. I've found a few errors this way before sending a board out for fab, and as a result every PCB I've made accommodated the parts the first time.

3. Be careful about pin diameters; it's very easy to make PCB holes too small for the device. I use a digital caliper to measure pin diameters. Also be aware that PCB manufacturers have specific drill-sizes, and the hole-plating process makes the holes slightly smaller. A good PCB house will provide specs on their hole tolerances.

4. Dont forget to add mounting holes. I usually lay those down first, because they block traces.

5. Dont go with minimum tracewidth/separation over the entire board. The tightest pad-pitch I've dealt with is 0.5mm, which is about 10 mils. Most PCB houses are doing 6-8mils.

6. Be aware that PCB traces are not perfect conductors. There is a handy tool (Saturn) available for free download that helps you understand resistance/voltage-drop, spacing for higher voltages, etc.

7. Dont be afraid of surface-mount devices. 0805 size components are very cheap and take up minimal board area. They are easy to solder by hand with a pair of tweezers

[Robert L]

Hi Kerry,

I'm also a KiCad fan... I've switched to it and most of the engineers at work have followed along for our non-product boards - test fixtures and such.

You will find loads of decent on-line support via YouTube videos and such. The package includes a pcb trace calculator as Greg recommends, as well as a decent Gerber file viewer.

Enjoy the process... it can be loads of fun.

Bob