There must be BILLIONS (or maybe even a googolplex) of DIP chips that have been placed on boards over the years. It follows that there MUST be some sort of “standard” for the drill bit size; as well as a standard for the through hole plating for the finished size.
Now, I realize that technology over time has changed. So, in addition to the original question, if time matters please include that in the reply. I can very easily believe that this value has gotten smaller over time.
If you don’t have an “answer” I’d still appreciate a reply with the value that “you use”.
There is no one answer, especially if you use sockets. Turned pin socket pin diameters vary between 0.46mm and 0.71mm nominal for different models from just one manufacturer. Stamped pins are generally at the wider end of the scale
I didn’t mention sockets, I stated, “chips”, meaning Integrated Circuits (I simply didn’t want to type all the extra letters that I am now typing even more letters to explain that I wanted to type fewer letters … ) in the common Dual In-line Package.
What finished hole size do you most commonly request in your PCB designs for DIP “parts” not “sockets”?
If there is any use for packages like this in my realm it’s during prototyping on proto boards.
Their holes are such, that a 1.05 mm drill still fits while a 1.10 mm drill doesn’t.
During assembly the pins get bent a bit anyway to keep the device from falling out or the angle of the pins in those rows is such that they do this automatically during insertion, so the hole size can be larger than that even.
Well, here’s a board from early 2015, containing a LM3915 in DIP16 package . . . . the holes are . . . . ummm . . . . 35 mils (about 0.9 mm). And here’s on from summer of 2016 . . . with a LT1495 in DIP8 . . . . and the holes are . . . . (drum roll) . . . .35 mils.
THIS JUST IN . . . . A dispatch from the archeological expedition . . . . via Morse code . . . a treasure trove of ancient manuscripts uncovered . . . . a cryptic inscription appears to be “intel data catalog 1976” . . . . obviously pre-dating the invention of upper-case letters . . . a sketch labeled “16-lead plastic dual in-lone package type p” . . . . must await authentication by comparison to drawings on cave walls . . . . seems to specify pins with max material condition of 23 mils by 15 mils at the tips . . . which would fit into a 28 mil hole (0.7 mm) . . . . but the pin tapers to 32 mils at the seating plane . . . which would require a 36 mil hole (0.9 mm).
I remember having two versions of a board for different assembly processes. At the time DIL auto-insertion required much bigger holes than were ideal for parts hand inserted and then wave soldered.
If you take a 74HC14 from TI the pin diameter is 14 to 26 mils or 0.36 to 0.66 mm, a big variation. With 0.1 pin spacing you can use 32mil finish hole and a 50mil pad. Our board supplier Labo Circuits has a ±3mill hole tolerance so 32mil finish + 3mil tol + plating = drill size and round out to the nearest standard drill size. You should have room left between the pads for a trace or two. You should check all the component dimensions on the datasheets, Kicad will check the traces, opens and shorts but cannot guess you have correct footprint. You should also consider the placement machine tolerances if the chips are to be inserted by a pick&place machine. One last note, if the hole is small repair is more difficult.
The KiCad PTH output is assumed to be finished hole size, not drill size, unless your PCB fab specifically says that they want drill size. Most fabs don’t give the information on plating, so it is the only way to go.
Oversize holes gives dry joints, but fortunately those thin TI chip pins have a wider shoulder that sits on the top of the hole
the fab is likely to substitute a reasonably close drill size when they plan the drilling of your holes along with the hundreds/thousands of other holes in the larger panel, so you may not be able to dictate the hole size you get back over and above the fab’s usual tolerance.
The general rule of thumb for DIP and other small component PTH size is pin/lead diameter + 6 mils. For rectangular pins use the diagonal + 6 mils. Therefore most DIP packages will fit a 31 mil hole size. As always consult the manufacturer’s datasheet.
In practice slightly larger holes are often preferred as larger holes allow the solder to more easily wick to the other side and they also allow for easier desoldering.
Edit: “Slightly” larger would be in the range of 35 - 40 mils and 38 mils has already been mentioned. Again, consult your datasheets and, as previously mentioned, it will depend on the standard sizes your fab has available.
This topic seems to appear every few months. The most common practice is to call out the FINISHED hole size. Poke around the fabricator’s web site (or contact him directly) to find out what he provides as “standard” hole sizes, and how he handles hole sizes that don’t exactly match his “standard” sizes.
Like many have said before, 35 - 40 mil is good. Another CAD program I use called PCAD-2001 (which came out in 2001, obviously ) defaults to pads which are 60/38 (60 mils for the pad, 38 mils for the drill) which works great for many ICs, resistors, transistors, etc.
(For those using mm, 1 mil = 0.0254 mm.)
Looking at this from the manufacturing side, the drill size you call out is taken to mean the final size you want after plating (assuming it is plated) and is usually assumed to have a +/- 3 mil tolerance. The PCB shop will drill the hole in the PCB slightly bigger than the specified number, but when the plating is added, the diameter shrinks down to your target size. The tolerance also gives the PCB shop a chance to use a common drill bit size if you have two holes with almost the same diameter or if you call out a weird hole size that they don’t have the exact drill bit for.
Now, you can specify the tolerance you would like them to use if +/- .003 is not acceptable. For instance, if for some reason you have a hole that you absolutely don’t want any bigger, but don’t mind if it gets smaller (like a certain type of via perhaps?) you can specify in the drill table that this drill has a tolerance of +0/-.006 or something. This is not typical, so you likely won’t have to worry about specifying anything, but you could. If you don’t specify anything, the PCB shop will assume they you don’t mind whatever default tolerances they use (which they should advertise), and is usually fine for most projects because PCB shops generally know what they are doing.
I hope this helps you understand the humble pcb through hole and what flexibility you have as a designer
Thanks for this! Along with other information I have seen online, this gives me some assurance that I won’t end up paying extra for different houses to have to purchase a new bulk order of drill bits.
As a follow up, the tolerances used by online prototype shops might have wider tolerances to keep the costs down, while production-oriented shops might have tighter ones. It is a really good idea to take a look at the manufacturing specs of whatever service you plan on using.
Also keep in mind that while the Note Table and Drill Table on a PCB file is the designer’s way of communicating tolerance and other design requirements to the PCB shop, many online prototype services explicitly do not read or follow those notes. They use an automated workflow which will follow their published manufacturer specs, so be doubly sure that you check those specs when using such services.
In the “good old days” (formerly known as “these difficult times”) the “Notes” communicated specific, detailed requirements. One drawback was that boards were sometimes over-specified because Notes were either simply copied from one drawing to another, or else Notes were standardized by a management bureaucracy that didn’t understand their meaning or significance.
Today the information formerly communicated by the Notes is often entered by clicky-clicking on a web page. Rather than over-specifying a board I think there is a temptation to under-specify, as you search out the most favorable price and delivery options. More disturbing to me is that there are significantly fewer choices available from the web-based ordering pages. I may have never had actual requirements for, say, high-temperature substrates or abrasion-resistant soldermask, but the options were always available in the Notes.
) defaults to pads which are 60/38 (60 mils for the pad, 38 mils for the drill) which works great for many ICs, resistors, transistors, etc.