3
\$\begingroup\$

I am using some standard 5mm screw terminal blocks for a simple design at low voltages (less than 20V).

The datasheet does not have a standard footprint for the device.

The pin itself has a diameter of 1.3mm, so I was thinking a hole size of 1.5mm, with a solder pad surrounding the hole of 1mm.

There's no real science in choosing these dimensions. What considerations should be given to choosing the pad size? If so, what pad size is best?

\$\endgroup\$
2
  • \$\begingroup\$ What amount of current will you need to support? Then, consider the minimum cross section of copper that the current will be passing through. There are calculators online that allow you to determine minimum trace thickness and width for the amount of current you need to support. \$\endgroup\$
    – TDL
    Jul 27, 2013 at 15:22
  • \$\begingroup\$ @TDL: good point, and it has made me realise that my question was not precise enough. I was looking more for mechanical requirements, and any flow-on (no pun intended) effects that will impact on the manufacture of the boards. In this instance, I was going to hand solder them myself (they're for my Dad's train set!) but I'm guessing something like this will affect how it gets assembled by a CM. \$\endgroup\$
    – Damien
    Jul 28, 2013 at 0:28

2 Answers 2

Reset to default
1
\$\begingroup\$

According to IPC-7251, IPC-2222 and IPC-2221 standards:

Minimum Hole Size is calculated according to equations below:

Minimum Hole Size = Maximum Lead Diameter + 0.25mm (for Level A of IPC-2222)

Minimum Hole Size = Maximum Lead Diameter + 0.20mm (for Level B of IPC-2222)

Minimum Hole Size = Maximum Lead Diameter + 0.15mm (for Level C of IPC-2222)

note:

http://www.pcb-3d.com/wordpress/wp-content/uploads/p/pth-dimensions/P1_Maximum_Lead_Diameter.JPG

Minimum Pad Diameter is calculated according to equations below:

Pad Diameter = Minimum Hole Size + Minimum Annular Ring X 2 + Minimum Fabrication Allowance

Minimum Annular Ring is 0.05mm (50um).

Pad Diameter = Minimum Hole Size + 0.1mm + 0.60mm (for Level A of IPC-2221)

Pad Diameter = Minimum Hole Size + 0.1mm + 0.50mm (for Level B of IPC-2221)

Pad Diameter = Minimum Hole Size + 0.1mm + 0.40mm (for Level C of IPC-2221)

Density Level A is used for General Design Producibility. It is a Preferred Level. Level A is used for the Low component density. In this case, footprint geometry is ‘Maximum’. This method is applied to the most robust producibility.

Density Level B is used for Moderate Design Producibility. It is a Standard Level. Level B conditions are suitable for re?ow, wave, drag or dip soldering. In this case, footprint geometry is ‘Median’. This method provides a robust solder attachment conditions.

Density Level C is used for High Design Producibility. It is a Reduced Level. Level C is used for the High component density. In this case footprint geometry is ‘Minimum’. This method is applied to a hand-held and portable appliances.

\$\endgroup\$
1
  • \$\begingroup\$ Accepted because of the explicit reference to a standard. Thank you. \$\endgroup\$
    – Damien
    Oct 30, 2017 at 3:36
1
\$\begingroup\$

What I always done in this case is put the pad size the double of diameter of the hole.

For example if the hole of the connector is with 1.3mm, the hole I put with 2.6mm of diameter.

enter image description here

If you put put a very large pad, you will have problems to solder the connector and could have cold solder too.

If you put a very thin pad the connector can be easily pulled, even when you're screwing a cable in conector.

So I recomend the double of the hole diameter when the datasheet doesn't gives you the pad size.

\$\endgroup\$
3
  • \$\begingroup\$ double the hole size makes for huge pads IMO. Most vendors will have a recommended footprint in their datasheet. \$\endgroup\$
    – akohlsmith
    Sep 4, 2013 at 14:13
  • \$\begingroup\$ double the hole size makes for huge pads IMO. In your example, a 2.6mm dia pad means that a 5mm pitch component would have its pins shorted to each other. Most vendors will have a recommended footprint in their datasheet. In the question it is stated that this is not the case and some quick googling has not helped get a definitive answer. I'll keep looking and post an answer. \$\endgroup\$
    – akohlsmith
    Sep 4, 2013 at 14:20
  • \$\begingroup\$ @akohlsmith I know that almost every manufacture should put this info in the datasheets, but if they dont put I try to use this rule. And it won't short circuit the pads, because the radius of the pad is 1.3mm (2.6 / 2), so if the distance between the pads are 5mm, 5 - 1.3 - 1.3 = 2.4mm between the pads. \$\endgroup\$
    – Butzke
    Sep 4, 2013 at 14:37

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.