If you need assistance, please send an email to forum at 4hv dot org. To ensure your email is not marked as spam, please include the phrase "4hv help" in the subject line. You can also find assistance via IRC, at irc.shadowworld.net, room #hvcomm.
Support 4hv.org!
Donate:
4hv.org is hosted on a dedicated server. Unfortunately, this server costs and we rely on the help of site members to keep 4hv.org running. Please consider donating. We will place your name on the thanks list and you'll be helping to keep 4hv.org alive and free for everyone. Members whose names appear in red bold have donated recently. Green bold denotes those who have recently donated to keep the server carbon neutral.
Special Thanks To:
Aaron Holmes
Aaron Wheeler
Adam Horden
Alan Scrimgeour
Andre
Andrew Haynes
Anonymous000
asabase
Austin Weil
barney
Barry
Bert Hickman
Bill Kukowski
Blitzorn
Brandon Paradelas
Bruce Bowling
BubeeMike
Byong Park
Cesiumsponge
Chris F.
Chris Hooper
Corey Worthington
Derek Woodroffe
Dalus
Dan Strother
Daniel Davis
Daniel Uhrenholt
datasheetarchive
Dave Billington
Dave Marshall
David F.
Dennis Rogers
drelectrix
Dr. John Gudenas
Dr. Spark
E.TexasTesla
eastvoltresearch
Eirik Taylor
Erik Dyakov
Erlend^SE
Finn Hammer
Firebug24k
GalliumMan
Gary Peterson
George Slade
GhostNull
Gordon Mcknight
Graham Armitage
Grant
GreySoul
Henry H
IamSmooth
In memory of Leo Powning
Jacob Cash
James Howells
James Pawson
Jeff Greenfield
Jeff Thomas
Jesse Frost
Jim Mitchell
jlr134
Joe Mastroianni
John Forcina
John Oberg
John Willcutt
Jon Newcomb
klugesmith
Leslie Wright
Lutz Hoffman
Mads Barnkob
Martin King
Mats Karlsson
Matt Gibson
Matthew Guidry
mbd
Michael D'Angelo
Mikkel
mileswaldron
mister_rf
Neil Foster
Nick de Smith
Nick Soroka
nicklenorp
Nik
Norman Stanley
Patrick Coleman
Paul Brodie
Paul Jordan
Paul Montgomery
Ped
Peter Krogen
Peter Terren
PhilGood
Richard Feldman
Robert Bush
Royce Bailey
Scott Fusare
Scott Newman
smiffy
Stella
Steven Busic
Steve Conner
Steve Jones
Steve Ward
Sulaiman
Thomas Coyle
Thomas A. Wallace
Thomas W
Timo
Torch
Ulf Jonsson
vasil
Vaxian
vladi mazzilli
wastehl
Weston
William Kim
William N.
William Stehl
Wesley Venis
The aforementioned have contributed financially to the continuing triumph of 4hv.org. They are deserving of my most heartfelt thanks.
Registered Member #538
Joined: Sun Feb 18 2007, 08:33PM
Location: Finland
Posts: 181
I just finished designing the PCB for my next induction heater control circuit, and I was wondering about the use of a big groundplane in the toplayer. I know a big groundplane can be a very good thing or a very bad thing, depending on lots of factors. I'm pretty sure it wont matter that much in such a low frequency (20-100kHz) circuit like this but I want to learn how to do it properly. What are the things I should look out for when using a groundfill? When should I use groundfill? Should I use groundfill in my induction heater control board?
The toplayer (red) is for GND + VCC (there a few other traces on the toplayer but GND + VCC mainly) and the bottom layer is for everything else (some GND + VCC traces to components that cant be soldered on the toplayer like filter lytics).
No groundfill: Groundfill: Heres (most of) the circuit: then theres the SG3524 VCO + couple gate driver chips.
Please give advice in the groundfill matter or the PCB design in general (if you can spot something wrong with it).
Then to my other question, what would be a good finish/coating for a homemade PCB? I've heard some diffrent techniques:
Protective lacquer which functions as a flux too. Sounds expensive, but kinda handy. Chemical tinning which involves soaking the board in some chemical for a few minutes and it gives a tincoat. Sound very nice and my chemist friend said it wouldnt be too expensive/hard to make the stuff (I cant find the commercial stuff from anywhere in here). Then theres one option where you "paint" the board with tin paste and melt it in a hot oven or with a hot air blower. Sounds interesting and pretty inexpensive but not sure how well this works.
Registered Member #56
Joined: Thu Feb 09 2006, 05:02AM
Location: Southern Califorina, USA
Posts: 2445
As to the ground plane, I would throw it in. Some of the RF nuts might have some better advice, but for stuff like this they generally don't hurt.
As to the tinning, I have had good luck with a nice fat soldering iron and some solder. Just take a flux pen (or any type of flux for that matter, I like the pens) and flux up the board nice and good, take a nice beefy soldering iron (I use a 50w temp regulated weller for everything I do...) and melt solder down everywhere. A q-tip soaked in flux can help even it out for the really big areas. But really, you don't need to worry about it at all, the boards work just fine with bare copper exposed (although rework can be a pain if it gets too corroded)
Registered Member #63
Joined: Thu Feb 09 2006, 06:18AM
Location:
Posts: 1425
It probably won't matter too much, but I think your traces are a little thin... especially if you're going to homemake the board -- you may have some issues with the pad ripping off when you try to drill a hole in it... which makes things particularly difficult if you want double-sided boards -- if you've done it before though, you'll know from experience.
Did you autoroute the board? My suggestion would be to fatten up what traces you can... especially traces going to GDTs etc. Sure, it's no big deal, but it's good habit, I suppose. ^.^
A groundplane will make the board a little more difficult to solder (without commercial soldermasking, that is), but is usually worth it in the long run. Your signals will be cleaner, and everything feels better when you see it on the scope.
I've used chemical tinning, and as a person that dislikes the wet PCB process, it is a bit of a pain. Proper flux (yes, that acidic yellow goo, where the fumes burn the inside of your mouth and taste horrible) works miracles on copper boards you want to tin. If you flux the whole board with a tissue and use a hot iron, you'll get beautiful results.
Registered Member #79
Joined: Thu Feb 09 2006, 11:35AM
Location: Arkansas
Posts: 673
For a protective coating, I've started using spray polyurethane. Just spray it on the entire board, I usually do a couple thin coats. It burns right off when applying the solder (right up to the edge of the solder), seems to work quite nicely. However, I only started doing this about 2-3months ago, but I sure don't expect any problems long term
Here's a pic of my latest DRSSTC control...
Oh, and I'll also make a plug for wider traces. A groundplane will decrease the resistance, make the signals look better, and if you're doing the toner method for etching the board, it will made the process easier (the toner tends to stick better with more than just the traces.) If you want more info, I etch boards ALL the time, and as cheaply as possible. Just drop me a line and I'll give you all the details.
Registered Member #538
Joined: Sun Feb 18 2007, 08:33PM
Location: Finland
Posts: 181
BlackPlasma wrote ...
It probably won't matter too much, but I think your traces are a little thin... especially if you're going to homemake the board -- you may have some issues with the pad ripping off when you try to drill a hole in it... which makes things particularly difficult if you want double-sided boards -- if you've done it before though, you'll know from experience.
Did you autoroute the board? My suggestion would be to fatten up what traces you can... especially traces going to GDTs etc. Sure, it's no big deal, but it's good habit, I suppose. ^.^
A groundplane will make the board a little more difficult to solder (without commercial soldermasking, that is), but is usually worth it in the long run. Your signals will be cleaner, and everything feels better when you see it on the scope.
I've used chemical tinning, and as a person that dislikes the wet PCB process, it is a bit of a pain. Proper flux (yes, that acidic yellow goo, where the fumes burn the inside of your mouth and taste horrible) works miracles on copper boards you want to tin. If you flux the whole board with a tissue and use a hot iron, you'll get beautiful results.
Yeah thickening the traces is a good idea, but I'm pretty sure it wont really matter for drilling since I've done smaller SMD boards with vias with no problems ( some holes not matching up properly because the films moved when exposing).
Edit: fattened all the power carrying lines:
And no, no autoroute, I have never managed to make anything proper with it.
Aand groundplane shouldnt make the soldering that much more difficult because eagle leaves space around ALL pads in a groundfill so its easier to solder them.
But I'll prolly have to buy some tin paste and flux to try the diffrent coating methods.
Registered Member #505
Joined: Sun Nov 19 2006, 06:42PM
Location: Yorkshire!
Posts: 329
You could also put a ground plane on the bottom too. Make sure you name the plane GND in Eagle (or whatever you've called your circuit reference) Always select "thermals on" when pouring a plane - it makes soldering it much easier
Registered Member #72
Joined: Thu Feb 09 2006, 08:29AM
Location: UK St. Albans
Posts: 1659
Ground plane is good, but use automatic "groundfill" with caution.
Too many times I have seen designs where as the last step the engineer has said "and fill all the remaining gaps with ground plane". The problem is that it's the *remaining* gaps. If you have traces going all over the place, the ground might end up not being well connected. The last thing you want is a long thin bit of ground snaking its way from the main ground to a large, otherwise isolated, patch. The term we use is "ground lace curtain" instead of ground plane, where the hoped-for low impedance plane has been shredded by signal tracks carving their way through it.
What you must consider is the current flows in the ground to be every bit as important as current flows in your signal tracks. It's good practice to route explicit ground tracks, with adequate width, in low inductance pairs with all of your signal tracks. This ensures that you have thought about current loop area, ground current injection from one part to another etc etc. Now when you do the last ground fill, it should only make thing things better. As an aside, if you didn't know you had to consider ground currents or are unable to estimate where they might flow, you are at risk of being bitten by unexpected circuit behaviour, especially unintentional coupling between things that shouldn't.
If you have just routed the signal tracks and then done a fill, it's good practice to explicitly go look for ground connectivity problems. Look for isolated lands, look for long thin bits of ground, check especially in the area of any long signal tracks which cut across the ground plane, whether you were expecting any ground return current to flow across that slot. Usually all of these problems can be corrected by a few extra connections to repair the tears in the ground lace curtain, or to move a signal track so that it doesn't tear.
Registered Member #30
Joined: Fri Feb 03 2006, 10:52AM
Location: Glasgow, Scotland
Posts: 6706
I totally agree. I do all this stuff in my commercial board designs whenever I'm restricted to 2 layers for budget reasons. But you have to wonder whether the average hobbyist really wants to know.
The most foolproof form of construction for RF circuits is the "Manhattan" or "Dead Bug" style, where you make your circuit with squares of copperclad glued to an unbroken solid groundplane. It's hard to screw up an RF circuit if you build it in that style. You can screw it up, but you actually have to try.
This site is powered by e107, which is released under the GNU GPL License. All work on this site, except where otherwise noted, is licensed under a Creative Commons Attribution-ShareAlike 2.5 License. By submitting any information to this site, you agree that anything submitted will be so licensed. Please read our Disclaimer and Policies page for information on your rights and responsibilities regarding this site.
PCB design + PCB finishing/coating
