EDA > General PCB/EDA/CAD Discussions

Standard drill size?

(1/3) > >>

tppc:
Hi there,
I just finished the design of my first PCB on JLCPCB's website.
before placing the order, I was just wondering if there is a standard drill size for
- Through hole 0.25W resistors ?
- Through hole DIP8 sockets ?

what puzzles me, is that available footprints on EasyEDA use strange drill sizes like 0.711mm or 0.914 mm for example.
Does a 0.711 mm drill even exist?

What will happen if I order a PCB with 0.711 mm holes? Will they round it to the next standard size?
BTW, is there a list of standard / recommended hole sizes for classic through hole components?

Thanks for your help.
Kind Regards.

evb149:
Keep in mind what shows up in the part library footprint for a pad is NOT the drill bit size.
It is the finished hole size desired in the pad.  For plated holes that will be slightly smaller (due to the plating thickness)
than the drill bit used to make the hole itself. 
So you'd be expecting them to support either metric or english standard drill bit sizes probably among those listed in the articles cited below, and to have finished holes available within their  tolerance range slightly smaller than the given bit sizes.

https://en.wikipedia.org/wiki/Drill_bit_sizes
https://en.wikipedia.org/wiki/List_of_drill_and_tap_sizes

https://jlcpcb.com/capabilities/Capabilities

As you'rel asking what's a common size for those kinds of through hole part leads, I suggest you check some
old texas instruments data sheets or similar from old NXP / Philips parts in DIP to see what they quote the
minimum / nominal / maximum size of DIP pins are for common chips and also what their suggested footprint is.

Once upon a time NXP had a good set of suggested footprints available for most of their packages as PDF files.
Now it seems to be less well organized / maintained, but last I saw you could still search for some package types / names
under their "packaging" menu somewhere in their quality web page or something like that.

Ultimately the resistor and DIP IC footprints and packages should correspond to JEDEC standards for those kinds of components.
So if you find the JEDEC package standard reference number for a 1/4 W axial resistor or 8-DIP or something you may be able
to find the "definitive" JEDEC specification for the cross-vendor package dimensions and lead tolerances.

There are also programs like the following that can help you calculate the IPC compliant dimensions of packages given
their datasheet derived types and tolerances e.g.:
https://www.pcblibraries.com/libraryexpert/pro/





--- Quote ---Drill Hole Size (Mechanical)    0.20mm- 6.30mm    
Min. drill size is 0.20mm. Max. drill size is 6.30mm.

Drill Hole Size Tolerance    +0.13/-0.08mm    e.g. for the 0.6mm hole size, the finished hole size between 0.52mm to 0.73mm is acceptable.

--- End quote ---


--- Quote from: tppc on June 15, 2021, 08:24:42 am ---Hi there,
I just finished the design of my first PCB on JLCPCB's website.
before placing the order, I was just wondering if there is a standard drill size for
- Through hole 0.25W resistors ?
- Through hole DIP8 sockets ?

what puzzles me, is that available footprints on EasyEDA use strange drill sizes like 0.711mm or 0.914 mm for example.
Does a 0.711 mm drill even exist?

What will happen if I order a PCB with 0.711 mm holes? Will they round it to the next standard size?
BTW, is there a list of standard hole sizes for classic through hole components?

Thanks for your help.
Kind Regards.

--- End quote ---

evb149:
Here's an example of a land pattern generator for a 8-PDIP IC device and its associated package drawing pdf:
https://www.ti.com/lit/pdf/mpdi001b
https://vendor.ultralibrarian.com/TI/embedded/?gpn=LM311&package=P&pin=8&sid=lit9a25d3409a25d3409a25d34060752a402bc9ca01&c=1

Here's an example of a DIP-8 socket, its drawing (including a suggested land pattern drawing), and its example machine readable generated land pattern:
https://www.digikey.com/en/products/detail/te-connectivity-amp-connectors/1-2199298-2/5022039
https://www.te.com/commerce/DocumentDelivery/DDEController?Action=srchrtrv&DocNm=2199298&DocType=Customer+Drawing&DocLang=English
https://app.ultralibrarian.com/details/012CB939-103F-11E9-AB3A-0A3560A4CCCC/TE-Connectivity/1-2199298-2?ref=digikey


tppc:
Hi evb149,

Thank you very much for this very precise and detailed answer.  :-+

hey hey, I found the 0.711 mm & 0.914 mm drill bits from your wikipedia links  ;D



Again, thank you very much for your time.
I am already reading the information on the links you indicated.   ;D

As per the pdf drawing they suggest simply 1 mm holes.

In the case of my first PCB, hole sizes are not critical, I just wanted to use hole sizes that make sense.

Kind regards
 :-+

dunkemhigh:
You might find this article useful:

https://www.pcb-3d.com/tutorials/how-to-calculate-pth-hole-and-pad-diameter-sizes-according-to-ipc-7251-ipc-2222-and-ipc-2221-standards/

Navigation

[0] Message Index

[#] Next page

There was an error while thanking
Thanking...
Go to full version