through hole components pad and hole sizes

[POTL]

Hello
I erased several boards created in DipTrace and realized that my macros had the wrong sizes.
SMD components I fixed on technical documentation from datasheets
But for through hole of components this information is not available
all components have a diameter of 0.8mm/32mils (capacitors) of 0.9mm/35mils - 1mm/40mils (diodes)
toggle switches 0,8mm/32mils x 2mm/79mils
What do I need hole sizes and pad sizes

[Rixen]

are you making/drilling the boards yourself or at a fab ?

[POTL]

are you making/drilling the boards yourself or at a fab ?

I do it myself

what is the difference between self-made and factory

[Marcos - Munky]

I use 0.8mm for almost anything but 1N400X diodes, which I use a 1mm drill.

[GGBB]

what is the difference between self-made and factory

Factory can drill any size you want, so you can optimize for each component type. Therefore the best answer would be something like 6-12mils larger than the component lead.

To drill your own, you need drills, and you probably only want to buy 2 or 3 drill sizes, so you need to make sure the sizes you choose will cover all your needs effectively. So the right answer might be something like 35mils for most things, 50mils for larger component leads.

[POTL]

Drills are not a problem
Modern China = good quality and ridiculously low price
My friend ordered a set of drills (if I remember correctly 10 sizes of 2 copies) at a price of about two dollars
For various tests, about 6 boards were manufactured in each order of 30 holes, no drills had broken yet =)
Today a soldering iron with a temperature adjustment for $ 6 came to me, it works great
Instantly heats up and has about 8 replaceable stings (I did not exactly count).



It turns out that I drilled the correct holes.
But the pads seem too thin
With a hole of 0.9mm / 35mils I did a pad of 1.9mm / 75mils
I look at the boards of different manufacturers and it seems to me that they use a pad of 2.5mm / 98mils or 3mm / 118mils

[POTL]

what size should i do pads?

[ElectricDruid]

For my boards I do everything with 1mm hole and a 2mm pad, except for pots, obviously. That's a loose fit on some components, but it doesn't matter. The big hole and the big pad make life easy for DIY. The holes are through-plated on manufactured boards so don't finish up quite that big.

I generally aim to reduce the number of different holes sizes to the minimum (2 or 3, often) because some board manufacturers charge you for the number of drill changes required. This is slow for the machine, and means your board uses up more time on their production line - you pay for the time.

Doing it myself, I'd do everything with a 1mm bit because that used to be the only size I could get!!

HTH,
Tom

[yanng45]

For the pads, i personally used EAGLE's "auto" setting which is drill + 0.7mm. So for example mine are :

Resistor :
Drill 0.4mm
Pad 1.1mm

Capacitors :
Drill 0.6mm
Pad 1.3mm

DO41 Diodes :
Drill 0.7mm
Pad 1.4mm

Pots (16mm alphas) :
Drill 1.1mm
Pad 1.8mm

I initially thought a pad that small would be a pain to solder but it's really not, and it's easy to layout with. I should mention that i don't make my boards myself and use a Chinese manufacturer, it's really cheap (5$ for 10 boards). I'd also never bother with that if i had to drill myself !

[POTL]

Thanks for answers

[GGBB]

I look at the boards of different manufacturers and it seems to me that they use a pad of 2.5mm / 98mils or 3mm / 118mils

I don't know where those sizes come from, but they don't seem right to me. Many components such as ICs and some radial capacitors are based on a 0.1" (100mils) pin/lead spacing. Pads of 98mils (let alone 118mils) simply would not work since the space between adjacent pads would then be 2mils - far less than the minimum required spacing for fabs I know about. And I would also think that 2mils is less than the precision that most DIYers could achieve with their toner transfers and etches.

Pad size choices depend not only on component types and hole sizes, but also on layout goals. Do you want to align components to a specific grid spacing? Do you want to be able to run traces between horizontally or vertically adjacent pads on the grid? Or diagonally adjacent pads? Or multiple traces between double or triple spaced pads? So in the end everything is related - layout design, pad sizes, hole sizes, and trace widths. Too small can be a problem, but bigger is not necessarily better.

[Rob Strand]

There are design rules from the old days and they are very different to what you see today.  This is where a lot of confusion comes from.  If you follow the "rules" you will find they never specify any dimensional constraints.  The reasons is they are all based on manufacturing tolerances.   The manufacturing tolerances depend on the manufacturer and these tolerance are now much smaller then they used to be.   So the manufacturer says what they can do.  An old colleague of mine worked for a large (and expensive) PCB manufacturer He wrote what was to become more or less the standard for PCBs in au.   It's all based on tolerances.   The telecom industry, when they used to make stuff here, had their own set of standards.  The would impose minimums on some dimensions which were more to do with not damaging the PCB down the track if someone had to rework the boards.

For through-hole boards it was common to use the 0.8mm/0.9mm and 1mm holes; rarely smaller.  For connectors where you wanted it to sit nicely and not lift up or not mount crooked you might use something more specific.    People kept the number of holes sizes to a minimum as this would increase the price of the PCB.  It was quite common to see:

normal pad: 100mil
small pad: 80mil
wired pad:  120mil
larger items: 160mil
IC pad:  100mil x 80mil  ()
Tracks were often 20mil and 50mil.

These are certainly problem free sizes for a home made PCB.

Nowadays things have moved on.  As far as manufacturers go you will find some still recommend the old sizes for single layer boards. You won't have any problems with these because the large sizes make it bullet proof against anything.  However these days companies regularly make boards with tiny features.  The problem with making things too small or close is you run the risk of solder balls and solder whiskers shorting things.

[Edit: For plated through boards  62mil pads and 0.8mm holes were pretty common.    You might use 50mil pads and 0.7mm holes for ICs

Here you go,
http://hairyraho.com/component-lead-sizes/
https://en.wikibooks.org/wiki/Practical_Electronics/PCB_Layout
]

[Rixen]

the issue with when making boards yourself is if the pads are small, most of it disappears when you drill, especially so if the drill wanders off centre. So I usually make the pads bigger than they need to be without getting stupid. 70 x 100 mil is my norm for IC pads, unless I need to squeeze a track through between them, and drill 0.6 or 0.7mm (sorry for swapping units).

resistors etc I would do with 70 to 100 mil and drill 0.7 or 0.8mm (again, sorry...), and only go below that if really pushed for space.

don't discount the usefulness of oblong pads to get parts closer and still put enough surface area to make a good joint.

Of course I've gone much smaller, but only when I need to, and a pedal is rarely that.

A fab house can be a lot more accurate with everything, so 62mil pads would be my norm for most of the above. 0.3mm with 0.15mm hole (done it again..) for vias. Plated through holes have most of the strength inside the hole so less copper needed on layer.

[ElectricDruid]

"Do you want tracks between 0.1" spaced pins?" is a good question raised above.

I've done this on manufactured boards that I've had done, and with modern tolerances, it's no problem. But I wouldn't do it on a board that I intended to etch or drill myself, and I wouldn't do it on a board that I was manufacturing with a view to having other people DIY it. Too error prone. Thin tracks like that lift easily if you overheat them. I like to keep everything nice and big and solid and widely-spaced. It makes it much harder to screw up the PCB, and much harder to short adjacent tracks. The only downside is that you probably need a bit more PCB, and you have to think a *lot* more to lay the bl**dy thing out!!

Tom

[GGBB]

"Do you want tracks between 0.1" spaced pins?" is a good question raised above.

I've done this on manufactured boards that I've had done, and with modern tolerances, it's no problem. But I wouldn't do it on a board that I intended to etch or drill myself, and I wouldn't do it on a board that I was manufacturing with a view to having other people DIY it. Too error prone. Thin tracks like that lift easily if you overheat them. I like to keep everything nice and big and solid and widely-spaced. It makes it much harder to screw up the PCB, and much harder to short adjacent tracks. The only downside is that you probably need a bit more PCB, and you have to think a *lot* more to lay the bl**dy thing out!!

Tom

I couldn't agree more. I personally wouldn't ever try to DIY traces between 0.1" spaced pads. But between diagonally adjacent pads on a 0.1" grid is achievable although I've never tried that either. What I have done is three traces between 0.3" spaced pads for routing underneath opamps. That wasn't too difficult except for the fact that I did the layout using Inkscape.