Will this PCB design work okay?

[djulien]

Does the PCB layout shown below look like it would work okay in terms of component layout, and being able to be fabricated by a PCB house? I used ExpressPCB to draw this. I have never had a PCB made, so I don't know what works or doesn't in terms of size of holes or how close they can be to the edge, etc. I guess I'm more concerned about the layout of parts, traces and holes, and not so much about the silk screen layer at this time (since I haven't labelled parts yet), although tips in that area would also be welcome.

I am wanting to make a single-sided board, so that maybe it could be home etched if I ever try that. I would also like to use this board as-is, or be able to cut it up into 8 sections that could be used individually, so I left a little clearance between each copy (but I didn't know how much space I should actually leave). I read over David Jones' excellent PCB design tutorial, and it was helpful but it seems to be more oriented towards "normal" boards (not the 1-sided, 8-up thing I'm trying to do).

I am also wanting to accomodate 14-pin or 20-pin PICs, so I put them in the same place and will use jumpers to connect the varying pins to their traces. The red lines show all the possible jumpers, but only half of them would be used for any given configuration (or less if ZC or ext clock were not needed). I bent a couple of the jumpers only so they did not hide the trace from view (they would be straight in actual practice). There are also a couple of jumpers that are there in lieu of a second side, so those ones are not optional.

For the ZC and power areas at the bottom, I really didn't know how to handle that in the smallest possible space, so I would be interested in any suggestions on that area also. I want to be able to use it several different ways:
- 120 VAC connected at bottom left to drive a regular H11AA1-based ZC circuit, with 5 VDC connected separately at bottom right
- ~ 12 VAC connected at the bottom left to supply ZC and if a diode bridge is populated then it can also be used to supply the regulator and caps in the bottom right
- connect either a filtered 5 VDC supply to the bottom right and bypass the regulator and caps, or an unfiltered 5 - 12 VDC supply and then use the regulator and caps to turn it into a filtered power supply on-board
- accomodate a half-size or full-size ext clock near the center in the bottom right (again just the standard Renard circuit)

thanks

don

[P. Short]

I don't have to much to add at the moment, other than you may have difficulties because of the lack of a ground connection on the RJ45 connectors, and that the cap on the input to the regulator might want to be exchanged with the cap that you now have on the output of the regulator. Also, you want to allow for physically larger resistors on the H11AA1 input, and you probably want to turn the input diodes around.

[budude]

Don - I don't believe jumper headers/shunts will fit in the "default" hole size of .056/029 - I'm not sure of the best size myself - perhaps someone can chime in here? I know MTA100 connecters don't fit and I think they are the same pin size - I had to drill out my pretty new boards to make them go in... I'm guessing a .075/.040 would be OK...

[n1ist]

An 0.025 square post has a diagonal of 0.0354. Amp recommends a 0.040 hole for their mates for the MTA100; I would use the same for a 2-pin "snap off" jumper. The 3M 2500 series wants a 0.035 hole, so I'm guessing the tails are a reduced size there.
/mike

[djulien]

Thank you for the info about hole sizes. That is very helpful.

Is there some kind of reference chart somewhere about which sizes to use for various types of parts or leads? I often see physical dimensions on spec sheets, but that doesn't really tell me how much "extra" clearance to leave.


you may have difficulties because of the lack of a ground connection on the RJ45 connectors

If I am charlie- or chipi-plexing the SSRs so that one of the I/O lines would be acting as ground, would a true ground still be needed for other purposes such as to reduce interference or to balance the twisted pairs?


the cap on the input to the regulator might want to be exchanged with the cap that you now have on the output of the regulator

Is that due to their sizes/shapes, or that the actual layout order with respect to direction of current flow is important?


allow for physically larger resistors on the H11AA1 input

Is it safe/acceptable to turn these resistors "on end" to take less space, or should they always be parallel to the board surface?

thanks

don

[aussiephil]

Re reference charts, nearly all spec sheets should list the hole size that is the finished plated hole, if they show a .040 hole and you place a .040 hole then it should be correct when you get the finshed board back.
If only the lead size is shown or i measure one then i add .006 to that dimension to get the hole size. I usually try and keep as few drill sizes as possible.

As for the ZC resistors i would stand them on end by default as this is good cooling orientation.

[djulien]

I found this note on the ExpressPCB site:
You should leave a .020 space from the fab edge of the board to the nearest copper elements to prevent traces from being cut off and possible mask peeling and exposed copper.

Is it safe/acceptable/good practice for the traces to go that close to the edge? That would save over .5" on this board if I did that, but would it make it harder to home-etch in future?


I usually try and keep as few drill sizes as possible.

Would it be better to make some holes a little larger than needed (say, up to 50% larger?) and then need extra solder to fill them, in order to reduce the number of hole sizes? For example, on this PCB there are several holes for jumper wires that I made smaller than the default sizes on pre-defined components because those seemed too large, but maybe I should just use that same size for the jumper holes also?

don

[P. Short]

If I am charlie- or chipi-plexing the SSRs so that one of the I/O lines would be acting as ground, would a true ground still be needed for other purposes such as to reduce interference or to balance the twisted pairs?

I wasn't considering that you were using charlie-plexing, so the grounds are not needed from a functional point of view. They are not needed for balancing the twisted pairs, especially since charlie-plexing doesn't drive the wires in a paired fashion. And for reducing interference, I don't know, since nobody here does any systematic testing for interference.


Is that due to their sizes/shapes, or that the actual layout order with respect to direction of current flow is important?

(Referring to the caps by the regulator). It appeared to me that you wanted the option of powering the board from a low-voltage AC source, based on the full-wave bridge rectifier circuit. If so, you need a big enough cap on the input to the regulator to ensure that the input voltage to the regulator does not dip below the regulator's dropout voltage. If you are always using a DC power source then this is not a consideration.


Is it safe/acceptable to turn these resistors "on end" to take less space, or should they always be parallel to the board surface?

This doesn't matter, in my opinion. Way back when the design rules called for the resistors to be flat on the board so that they could be automatically inserted with the equipment in use at the time. Since the resistors are going to be hand-inserted, I don't think it matters if they are "on end" or not, unless you are worried about accidental damage later on.

[djulien]

(Referring to the caps by the regulator). It appeared to me that you wanted the option of powering the board from a low-voltage AC source, based on the full-wave bridge rectifier circuit. If so, you need a big enough cap on the input to the regulator to ensure that the input voltage to the regulator does not dip below the regulator's dropout voltage.

Whoops. Yes, I forgot to add a big capacitor to smooth out the rectified AC. Those caps are usually pretty big, so I guess I need to move stuff around. Maybe I can squeeze it in just after the diodes. Does it matter how close it is to the regulator?

don

[P. Short]

That should be OK.

[David_AVD]

Does it matter how close it is to the regulator?

Regulator manufacturers usually recommend the filter cap be within 1" (track distance) of the Vin terminal. If not, add a 100n (0.1uF) bypass capacitor right at the Vin terminal. Also, don't skimp on the track size between the filter capacitor and Vin.

[djulien]

Thank you all for the additional tips. The overall PCB design concepts seemed fairly simple, but there are so many of these extra little details to consider that make it a much bigger task.


Regulator manufacturers usually recommend the filter cap be within 1" (track distance) of the Vin terminal. If not, add a 100n (0.1uF) bypass capacitor right at the Vin terminal.

Is there a threshold current or power under which this is not critical, or should it always be done?


Also, don't skimp on the track size between the filter capacitor and Vin.

I've seen some formulas for trace width vs. current for a given copper thickness, but do holes affect that? For example, if I use the recommended trace width for a given amperage but that trace also has a via or unpopulated hole along it, does the trace width around the hole matter? Using simple geometry the effective trace width at the hole would be (outer diameter - inner diameter), but is it necessary to do that extra calculation for each hole along the trace?

thanks

don

[David_AVD]

Holes in the trace shouldn't have much an effect if that hole is filled. (with a component leg or just solder) Don't forget that plated through holes will add to the effective area too via the inside hole edge.

The reason for keeping the filter cap close to the regulator and using thick traces is to lower the source impedance for the regulator's Vin pin. This helps keep them stable. The 0.1uF capacitor trick is for when you just can't get the filter cap close enough - often due to heatsink placement.

I follow these rules no matter what the power draw. It's just good design practice. Why skimp on a 15c (retail) capacitor and have potential problems with power? Without stable power, nothing else can be guaranteed.

[djulien]

I'm wanting to be able to use either cat5 or ribbon cable wires for jumpers and connections. For hole and pad sizes, are the following choices correct?

- cat5 is typically 24 AWG, and I found a chart that says its outer diameter is .0201" (.51054 mm)
- ribbon cable is typically 28 AWG, which the chart said was .0126" diameter (.32004 mm)
- I'll just use the larger of these two (.0201" outer diameter) for the remaining calculations.

In the software I used (ExpressPCB), a hole size of .020" +.003/-.005 is available, but with the +/- tolerance it is likely to end up being too small. The next larger hole size is .025" +/- .004", so that should work okay. An even larger hole size of .029 +/- .004 is available, but it has a minimum pad size of .056", which is getting rather large for areas where I would like to place the holes only .05" apart. So it seems like the .025" size is my best option - is that correct?

Based on that, if I went with the .025" hole size and also wanted a .01" effective trace width (but I didn't want to fill in unused holes in case I needed them later), I would need to use a pad size of at least .025+.01 = .035" - is that also correct?

One further question: If I am making a 1-sided board, can I use "round vias" (which have sizes that are slightly closer to what I want) and a PCB manufacturer would typically convert them just to holes and pads, or must I explicitly stick with the "pad with hole" type?

don

[n1ist]

You can create custom pad sizes. Select the "place a pad" icon, then click on "Create new pad" in the upper right corner. You can specify any of the standard drill sizes, and any size annular ring that is at least 0.017" larger in diameter than the hole. Just make sure you leave enough copper around the pad to solder to.

As for vias vs. holes, there's no difference as far as ExpressPCB is considered, so you can use the already-existing 0.029 via with an 0.050 pad.

/mike

[djulien]

As for vias vs. holes, there's no difference as far as ExpressPCB is considered, so you can use the already-existing 0.029 via with an 0.050 pad.

I noticed that the vias vs. plated-thru holes looked the same within ExpressPCB, but I didn't know what a board fabricator would do with those if I order a single-sided board - would they convert it (possibly automatically), or would the hole/via be dropped since the order would be single-sided but the via was a double-sided feature?

I tried to incorporate everyone's recommended changes and I played around with the PCB layout some more. I got the board size down to about what I had on stripboard, so I think I'm happy with it. Here is what I came up with.

One further question - is it considered bad practice to use the ring around a hole as a trace? When I compressed the PCB layout, a mounting hole fell on top of a trace, but if there's copper around the hole anyway, I figured I might as well make use of that copper (ExpressPCB didn't have an option for a hole without a pad around it).

thanks

don

[n1ist]

One thing to check - I don't have any expressPCB boards handy right now, but as for other vendors, the main difference between a via and pth is that the via usually ends up with solder mask on the pad, so you can't solder to it. I think ExpressPCB doesn't do this; certainly on the maskless boards, its a non-issue.

As for using the hole as a trace, electrically that's fine. The problem is that your mounting screw is now connected to the trace, and that may be a problem. If your case is metal, it will connect all of those mounting screws together. Also, I wouldn't do that on a high-voltage or high-frequency trace. The proper way to do this is to not connect the mounting holes to anything, or connect them to circuit ground if that is appropriate for your design. You also need to keep other traces or vias far enough away from the mounting hole so they don't get shorted together by the screw head. Been there, and it's a pain to debug the problem since it will only show up when the board is mounted in the case :-) For example, the one on your zc/rect board would likely short (or allow an arc) the 110v input.

/mike

[djulien]

As for using the hole as a trace, electrically that's fine. The problem is that your mounting screw is now connected to the trace, and that may be a problem. If your case is metal, it will connect all of those mounting screws together.

Hmmm, sort of a second layer without jumpers. :)

I hadn't considered a metal housing; I was thinking of plastic or wood mounting initially. Looking it over again, it looks like most of the mounting holes would be okay if they were connected (via metal housing). The only problem area would be the little "extra" strip along the bottom. I think I would need to enlarge it or use smaller holes because there is not much clearance in that area.

Is it poor style to require a "non-metalic housing", or some kind of insulation on the mounts?


You also need to keep other traces or vias far enough away from the mounting hole so they don't get shorted together by the screw head. Been there, and it's a pain to debug the problem since it will only show up when the board is mounted in the case :-) For example, the one on your zc/rect board would likely short (or allow an arc) the 110v input.

Electrically, how much clearance should there be between 110VAC traces?

I was thinking that the parts and screw heads would all be on the "top" and the traces themselves would all be on the "bottom" of the PCB (single-sided), so the screw heads themselves could not short anything unless they actually touched some of the parts. So would this only be a problem if a single-sided PCB design was printed by a double-sided shop (so that holes ended up with copper on both sides of the board)?

Or, maybe I could just skip the mounts within the extra strip along the bottom. How much should a PCB "overhang" the mounting holes?

don

[David_AVD]

Is it poor style to require a "non-metalic housing", or some kind of insulation on the mounts?
IMO yes. Letting the mounting points become live (with any signal) and relying on the case material to isolate that point is not the way to go.

The only exceptions really are if your are intentionally connecting the mounting point to ground, or if the mounting method is inherently insulated. (nylon bolts or snap-in posts)

Signals on mounting holes is only asking for trouble. Is the board size critical? Can you make it a little bigger to allow for the track?

Even if the screw head was on the top and the pad in question was only on the bottom, you'd need to make sure the spacer between the PCB and case was non-metallic too. You'd also need to make sure the ID of the bottom pad was larger than the hole.

[aussiephil]

Hmmm, sort of a second layer without jumpers. :)


Electrically, how much clearance should there be between 110VAC traces?


don

In my opinion, if you have opto isolation onboard, in your case the ZC chip then all spacing from 110v to the low voltage traces should match the 0.300 spacing under that chip.

Actual spacing between high voltage traces is dependant on a number of things such as solder masks, board coatings etc and were a board may be home etched should be worked out for a oncoated copper board and the peak AC voltage plus a bit for safety.

at the bottom of the page in the link there is a table that is good to know
http://www.pcbwizards.com/faq.htm

Cheers

[djulien]

at the bottom of the page in the link there is a table that is good to know
http://www.pcbwizards.com/faq.htm


Thank you for that link; that table is helpful!


Can you make it a little bigger to allow for the track?

Yes, but then it costs more due to the larger surface area. :(


Even if the screw head was on the top and the pad in question was only on the bottom, you'd need to make sure the spacer between the PCB and case was non-metallic too. You'd also need to make sure the ID of the bottom pad was larger than the hole.

Are metal spacers common? I don't like those for other reasons (they could touch parts, etc).

I don't think ExpressPCB provides that option. Maybe I have exceeded its abilities and should use something else like Eagle.

don

[budude]

You might want to give PCB Artist (http://www.4pcb.com/index.php?load=content&page_id=46) a try also - it's simple to use like ExpressPCB. I absolutely hate Eagle - it must be the most non-intuitive program I think I've ever used (and yes I know the Eagle lovers will tell me I'm nuts...). You can have boards made through them (Advanced Circuits) also - I haven't used them myself however...

[David_AVD]

Yes, but then it costs more due to the larger surface area. :(
Cutting costs is often why designs are compromised. If you cram a design into a smaller space than normal design rules dictate, something has got to give.


Are metal spacers common?
Yes, but even with plastic spacers, the thread of the bolt will likely make contact with the edge of the "live" pad unless you make the pad ID larger than the hole. Relying on this for isolation is not a good design choice.

[n1ist]

ExpressPCB does not offer non-plated holes. Yes, you can drill them out, but I wouldn't count on remembering that, especially if you plan to sell/give the board to others.
/mike

[djulien]

ExpressPCB does not offer non-plated holes. Yes, you can drill them out

I do not plan to drill them out if they end up plated. I just didn't know what I would get if the PCB file shows them as plated thru-hole but I submit the order as a single-sided order.

don

[chilloutdocdoc]

Cutting costs is often why designs are compromised. If you cram a design into a smaller space than normal design rules dictate, something has got to give.


Yes, but even with plastic spacers, the thread of the bolt will likely make contact with the edge of the "live" pad unless you make the pad ID larger than the hole. Relying on this for isolation is not a good design choice.

Agreed. And often what will give is somebody or something's safety. You do NOT want any chance of an energized piece of metal sticking out of the board, exactly the same reason you don't want to have energized male plugs out on the board.