How big is big enough for PCB patterns?

[R.G.]

In doing some of the updates on the Neovibe I mentioned in another thread, I did the up-front work to get it into a modern PCB system, so now I can pretty much enlarge/shrink, etc as needed and get newer versions with relatively little effort. One of these was that I took the 'first update' of the Neo to all 0.062" pads and 0.030 holes with 0.025" traces.

Then for grins I just changed all the pads to 0.085" and told it to find me where there were shorts. It worked fine, and I fixed the half-dozen places which were too close easily enough. Then I decided to put all the component pins on 0.100" centers so one could use a piece of perfboard as a drilling template. Then I re-ran the traces 0.050" wide. It got a little bigger, but not too bad. This last was 3.0" by 4.0". I have done versions in the past that were as small as 1.5" by 2.8" by standing stuff on end, etc.

This brought up the question in my mind - how do I know where to stop making pads, traces and spaces fatter? There is a certain maximum size for pads, because you cannot get most ICs with pins on spacings bigger than 0.1". That limits pad size to about 0.085" max. If you use transistors, you can bend the leads wider, but this gets to looking silly when you get them too big. And the board size to hold spraddled components goes up, so it's hard to find a box it will fit in, and that's **expensive**.

So I'm left with the philosophical question - how big is big enough? Easy to draw on copper clad with a crayon? nail polish brush? Toner transfer's 0.025 trace/0.012" space? Does it matter? Will most PCBs be bought, done by photo techniques?

Where does the obvious tradeoff of easy to hack and etch/solder start giving you boards that are too big for boxes? Does this matter? Will the generic "you" ever actually box the stuff up?

Agh, philosophy, the hardest soft science! 

[sean k]

I'd just like to mention that most of the rest of the world has gone to metrics and using hundreths of an inch is going to have most of us going for the calculator or doing guesstimates about the sizings you mention.

But as for your question I think you'd be safe to assume that most people who don't do there own artwork will be using photo methods.

I use an 0.7 sized clutch pencil with a 2B lead and the line would be 0.3mm then I use a sharpie to cover those and thicken things up so my limit, with this method is about 1-1.2mm for a trace which is... 100th of an inch is .25mm so I'm looking at say 1.25mm/ .25mm so it's 5 x 100th". Is that .05" for a trace?

If it is then a .025" trace is about .6mm and thats far too fine for sharpies or anything handheld unless we move into magnifying glasses so those sizes have to be photo.

[Skruffyhound]

Ah yes, where to draw the line, and how thick should it be?
Similar problem to what Taylor is contending with in the new Echo Base design thread. That one has split into the newb's board and the "I don't care how big, I'll rack mount it if I have to - just give me everything" camps.
Seems like the only solution to keep everyone happy is to provide the three options, Prof boards for sale (everyone can use them if necessary), small traces for the UV folks (seems like a growing segment) and a dorking great press 'n' peel board, for which the price is a huge enclosure.
When it gets to a certain level of complexity though, I would think even the hardcore toner transfer guys have got to rationalize that it's cheaper to buy a PCB than make/buy a monster enclosure. Could be wrong though, some are really successful even with tiny traces. Not me, never liked it and now I am a UV convert
Nice idea perf as drilling template.

[Mark Hammer]

I've purchased some PnP sheets in past, but most of my PCBs these days are done with photo paper.  It's cheap, works reasonably well with a certain degree of predictability, but it needs two things: space and "traction".



Since it is often difficutl for people to tell when a toner pattern has transferred to a board from photopaper, they often lift up the paper perhaps prematurely.  Without enough surface area covered to assure sufficient "grip" on the copper, the pattern may lift off clean from the copper and linger behind on the paper.  So thicker traces provide the sort of "traction" that lets a trace grip the copper and dislodge from the paper, rather than retreat with it.

The space part is a reflection of the larger particle size that the photoemulsion on the paper breaks off in.  The edge of lines and pads is rarely as crisp and clean on photopaper-made boards as it is on PnP.  It's like the difference between regular perforated and "clean edge" fanfold paper in the old days.  And those frayed (or micro-frayed) edges lends themselves to tiny solder bridges.

Finally, while many component types, like TO-92 trannies, 1/4w resistors, silicon diodes, and op-amps, have highly standardized footprints, the range of component sizes for caps is vast.  I often find myself having to drill holes a little off from what the PCB mask shows, in order to accommodate a cap, or find myself bending stuff this way and that just to make room for a cap, or to find space to tilt a tall one over a bit so that it doesn't crowd a toggle or pot directly above it.

So there you go: space and traction....largely for photopaper-based etches.

As an aside, with so many folks using either 1590BB or 125-sized boxes, and with the relatively standard size of both stompswitches and jacks, it can often be possible to expand the surface area required of a PCB, without precluding use of phone jacks, stompswitch, battery and power jack.

[bean]

Based on my experience, I get the best results with PnP as follows: 82mil pads, 35 mil holes and 32mil traces. When the trace run parallel I take them down to 24mil. I also fillet all 90deg angles and now I'm bring out a 66mil tab from the pads as another fillet. Ecthing results are great! Also, a 24mil grounding plane with 32mil isolation.

Here's an example from a Mosfet Booster layout I did:


Drilling with a #64 carbide bit is pretty much like knife/butter...very hard to miss the hole. Also, if the transfer leaves smudged areas they are pretty easy to get in there with an Exacto knife before etching.

[R.G.]

I'd just like to mention that most of the rest of the world has gone to metrics and using hundreths of an inch is going to have most of us going for the calculator or doing guesstimates about the sizings you mention.

Yes, thank you - I'd heard there was a different measurement system somewhere, but had no clue that people really used it.  

You might also want to read some of my postings - I commonly, although not always, put dimensions in both systems. Check it out.

One other reason I use mils (1/1000 of an inch, a milli-inch) is that the mil has been the common basis for PCB layout for decades. This is only now changing as parts become available in so-called "hard metric" sizes. At the bottom of things, if you do PCB layout, it will be another decade or so before you can quit worrying about inches as a unit. But I digress. I tend to use both systems, and have just gotten used to using a calculator to do divide-by or multiply-by 25.4 as needed.

But as for your question I think you'd be safe to assume that most people who don't do there own artwork will be using photo methods.

That would be nice. How about that old "it's too small to solder" issue? How small is too small to solder?

My thoughts are that if you can't solder IC pins, you can't do much real electronics soldering, so 0.062" (that's 1.57mm for the inch-impaired  " on 0.100" centers (that's 2.54mm...) is as coarse as needed. Is that wrong?  Show of hands, please...  yes - any you, and you... OK, that's- uh, lessee, carry the two...  

I use an 0.7 sized clutch pencil with a 2B lead and the line would be 0.3mm then I use a sharpie to cover those and thicken things up so my limit, with this method is about 1-1.2mm for a trace which is... 100th of an inch is .25mm so I'm looking at say 1.25mm/ .25mm so it's 5 x 100th". Is that .05" for a trace?

25.4 mm/inch. To get inches, divide millimeters by 2.54. To get mm from inches, multiply by 25.4. 1mm is 0.03937", 1.2mm is 1.2/25.4 = 0.0472". Yes, 0.050" is close.

If it is then a .025" trace is about .6mm

0.025" * 25.4 = 0.625mm. Close enough.

and thats far too fine for sharpies or anything handheld unless we move into magnifying glasses so those sizes have to be photo.

OK. What's the smallest (a) hand held, (b) toner transfer, and (c ) photo traces the larger You will bother etching?

Ah yes, where to draw the line, and how thick should it be?
Similar problem to what Taylor is contending with in the new Echo Base design thread. That one has split into the newb's board and the "I don't care how big, I'll rack mount it if I have to - just give me everything" camps.
Seems like the only solution to keep everyone happy is to provide the three options, Prof boards for sale (everyone can use them if necessary), small traces for the UV folks (seems like a growing segment) and a dorking great press 'n' peel board, for which the price is a huge enclosure.
When it gets to a certain level of complexity though, I would think even the hardcore toner transfer guys have got to rationalize that it's cheaper to buy a PCB than make/buy a monster enclosure. Could be wrong though, some are really successful even with tiny traces. Not me, never liked it and now I am a UV convert
Nice idea perf as drilling template.

I guess everything just takes longer than I thought. When I started flogging the boards to use toner transfer, it was because the photo stuff was too hard to use. It just takes pushing long enough and the herd comes around, I guess. Photo stuff has made great strides from when I'd tray-develop and etch a 200mm (Hey Sean! I used millimeters!!  ) long board and then slice it into PCBs.

However, the ongoing slow motion crash of the USA electronics industry has made all the PCB houses add on low quantity Proto services that did not exist ten years ago. Today, you can get a FX sized board for as low as $40 each on a completely new design. That simply didn't exist back when. It's so good I don't even photo anymore, I just send in the Gerber files.

Finally, while many component types, like TO-92 trannies, 1/4w resistors, silicon diodes, and op-amps, have highly standardized footprints, the range of component sizes for caps is vast.  I often find myself having to drill holes a little off from what the PCB mask shows, in order to accommodate a cap, or find myself bending stuff this way and that just to make room for a cap, or to find space to tilt a tall one over a bit so that it doesn't crowd a toggle or pot directly above it.

That's why I don't do generic cap footprints any more. I find at least one part in Mouser's catalog that fits the space and is in stock.  But I'll take that as a vote for sized to fit 1/4W resistors and TO92s.

So there you go: space and traction....largely for photopaper-based etches.

So... can you give me an "inches" or "mm" size for that, and for soldering? Soldering was a recent issue, so I decided to explore it.

Based on my experience, I get the best results with PnP as follows: 82mil pads, 35 mil holes and 32mil traces. When the trace run parallel I take them down to 24mil. I also fillet all 90deg angles and now I'm bring out a 66mil tab from the pads as another fillet. Ecthing results are great! Also, a 24mil grounding plane with 32mil isolation.

Thanks. Good, concise answer.

Others?

[served]

My point of view.

I like to drill holes with 1mm drill. So I really need that i would not drill the copper off around the hole. That's my main problem with all the schematics, I just have to redraw them.
I'm using printing technique, so there is actually no limits to how wide the trace should be. Probably would manage to mark 0,2mm to the board also.
I don't know how much soldering space should be, never had a problem with it.

Hope it helped.

[R.G.]

I like to drill holes with 1mm drill. So I really need that i would not drill the copper off around the hole. That's my main problem with all the schematics, I just have to redraw them.

That's 0.03937", probably 0.040 with normally (slightly dull) bits. That's kinda big for most component leads, but works if you hand solder. The minimum hole you can use with that is 0.060" (1.524mm) and really you should use larger, 0.080"/2mm being about right.

I'm using printing technique, so there is actually no limits to how wide the trace should be. Probably would manage to mark 0,2mm to the board also.
I don't know how much soldering space should be, never had a problem with it.

Good, concise answer. Thank you.

[Boprikov]

I make traces and pads as large as possible. One benefit is, there is much less to etch, and that saves etchant.
And, more important, it is possible to de-solder and re-solder components without traces lifting. I hate lifting traces, i rather make my boards and enclosures oversize.

Edit: This pcb is not designed by me, but you get the idea.
http://www.electro-dan.co.uk/electronics/TDA2040pcb.gif

[R.G.]

I make traces and pads as large as possible. One benefit is, there is much less to etch, and that saves etchant.
And, more important, it is possible to de-solder and re-solder components without traces lifting. I hate lifting traces, i rather make my boards and enclosures oversize.

This reminds me of the "minimum-etch" style, common back in the first days of PCB technology. The PCB connections were separated by thin lines of no-copper, perhaps 0.032" to 0.05" (1 to 1.3mm) wide. This was common back in the late 1950s through mid 1960s. The true minimum etch style evolved into the style for which you provide the illustration - very large, indistinct and combined pads, more just areas of copper. This is handy, and fits well with hand-drawn artwork well. It was evolved away from industry for a few reasons. The rise of donut pads and PCB tape to get higher speed in layout by eliminating hand-drawing of artwork; the need for consistent heating in automated soldering, and the rise of small pin-separation ICs and smaller components in general.

To heat pads for soldering, the pad has to absorb heat until it reaches solder-wetting temperature. The more surface area, the more copper to heat, and the longer this takes. For soldering automation, each pad needs to heat (ideally) at the same time; certainly within the minimum preheat time as the others. This criteria says that each pad should be identical, or at least similar.This is the exact reason that pads in ground planes are isolated from the plane and only connected with those little traces - it lets the pad heat more easily than the plane. The etched area around such pads are called thermal breaks or thermal reliefs.

Your suggestion is not bad if you draw your own artwork and are willing to hand solder them all. It does help with pad lifting, although I'm embarrassed to report that I ... have... lifted traces on such boards by my sloppy soldering back in the past.    But it helped me get better at soldering.  That which does not blister our fingers makes use stronger.

IC pads on 0.100"/2.54mm centers forces you back to the dilemma of how big can you stand it. Pads 0.100" will short DIP IC pads 100% of the time. So you're left with a minimum pad size of 0.100" minus whatever spacing you want between pads. This can be as small as 0.010"/0.254mm, but 0.015"/0.037mm is better for preventing solder shorts.

A tip on soldering - if you lift pads, your soldering iron is either not well tinned, or too cold, or both. The trick in soldering and re-soldering is to get in quickly with high heat, solder/unsolder quickly before the heat has a chance to travel far or to cause chemical/thermal changes in the surrounding parts. As I said, I have lifted even really fat pads in the past. But with long practice I can now unsolder/resolder 0.050"/1.27mm pads multiple times without losing them. It does take practice, though.

You make valid points. Thanks!

[Electron Tornado]

I make traces and pads as large as possible. One benefit is, there is much less to etch, and that saves etchant.
And, more important, it is possible to de-solder and re-solder components without traces lifting. I hate lifting traces, i rather make my boards and enclosures oversize.

Edit: This pcb is not designed by me, but you get the idea.
http://www.electro-dan.co.uk/electronics/TDA2040pcb.gif

I do the same. I have only etched a few boards, so I'm still new to it. Making pads as large as possible also gives me some room for error when drilling (I also use perf board as a template for ICs), and allows me some wiggle room with regard to placing components on the board.

[Ice-9]

How about that old "it's too small to solder" issue? How small is too small to solder?

For me that would be when the component drill hole is bigger than the pad its goes through.

but seriously, even though i have just started to wear glasses i can still solder these IC's with a normal soldering iron by hand AT49LV1614A. These are 48 pin TSOP packages and the pin spacing is 0.5mm 0.02inches

[space_ryerson]

This is the exact reason that pads in ground planes are isolated from the plane and only connected with those little traces - it lets the pad heat more easily than the plane. The etched area around such pads are called thermal breaks or thermal reliefs.

I was wondering about why they were there just the other day, and you preemptively answered my question. Thanks!

[kristopher612]

i usually use a .065" pad with a .035" hole for component leads, a .09" pad with a .043" hole for wires, and .03" or .04" traces.  these are all standard sizes in the ExpressPCB library, and the holes are just right for the #65 and #57 drill bit sizes.  I use the photo transfer method when i etch my boards, and have no trouble with these sizes. 

[bean]

This is the exact reason that pads in ground planes are isolated from the plane and only connected with those little traces - it lets the pad heat more easily than the plane. The etched area around such pads are called thermal breaks or thermal reliefs.

I was wondering about why they were there just the other day, and you preemptively answered my question. Thanks!

Yep, even with thermals it still takes longer than regular pads to get good heat transfer. But, ground planes greatly simplify the process of layouts (for me, at least).