through hole components pad and hole sizes

Frequently asked question on the subject of designing, creating, producing printed boards, veroboards or perfboads and on point-to-point construction techniques.
Post Reply
User avatar
POTL
Resistor Ronker
Information
Posts: 335
Joined: 26 Sep 2016, 03:11
Has thanked: 58 times
Been thanked: 67 times

Post by 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

User avatar
Zokk
Resistor Ronker
Information
Posts: 287
Joined: 05 Jul 2010, 20:00
Location: tantalum shortcut area
Has thanked: 211 times
Been thanked: 68 times

Post by Zokk »

Hi
usually I draw patterns for resistors, small signal diodes, and capacitors with these parameters:
type: through hole
shape: Oval
width: 1.65mm
height: 1.65mm

Hole
shape: Round
diameter: 1mm

This is pretty standard and works fine with most component, even the Vishay military resistors will fit these holes.
For 1N400x diodes I use a slightly larger pad and hole diameter is 1.2mm.
For electrolytics capacitors, rating between 10 to 63V, I like hole size to be 0.75mm.

Toggle switches:
type: through hole
shape: oval
width 2.2mm
height: 3.2mm

Hole:
shape: oval
width: 1.4mm
height: 2.4mm

This is a pretty tight fit but every toggle switch will go in with no friction.
I've tried larger pads and hole for these switches but this size is the best compromise between mechanical resistance, and space used on the pcb.
Of course if I use these pads/holes on a single layer pcb, I would enlarge a bit the pads size as it's not soldered on both sides (it may be weaker than on a double sided pcb).

Cheers.

User avatar
Dirk_Hendrik
Old Solderhand
Information
Posts: 4193
Joined: 03 Jul 2007, 08:44
Location: Old Amsterdam
Has thanked: 232 times
Been thanked: 887 times
Contact:

Post by Dirk_Hendrik »

For pads the hole size is the actual size that is defined by the designer. If you state a hole size to be 0.8 mm the manufacturer of the board will ensure the end result is 0.8mm. The drilled hole at the start of the board manufacturing process will be bigger. However, if the component is stated to have a lead diameter of, sau. 0.8 mm, better make that hole a little bigger. 0.9mm or so.
For via's the hole size is the drill size. If the designer states 0.8mm the hole will be drilled at 0.8mm. The final result will therefore be smaller than this 0.8mm.

Above is common practice for PCB fabbers.
Sorry. Plain out of planes.

http://www.dirk-hendrik.com

User avatar
Dirk_Hendrik
Old Solderhand
Information
Posts: 4193
Joined: 03 Jul 2007, 08:44
Location: Old Amsterdam
Has thanked: 232 times
Been thanked: 887 times
Contact:

Post by Dirk_Hendrik »

Browse for IPC-2221 and then read chapter 9
Sorry. Plain out of planes.

http://www.dirk-hendrik.com

Post Reply