djulien wrote: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.
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.
David_AVD wrote: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?
David_AVD wrote: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
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.
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
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
