The question is related to the datasheet for LED part number MHT151WDT. It is manufactured by Lianyungang Meihua Electronics Technology Co. Ltd. The datasheet can be found here.

The pg. 2 in this datasheet gives this drawing as guide to create the PCB footprint:

enter image description here

There are two issues:

  1. What is really point of having a pad size containing 4 decimal places? This is mind boggling.
  2. Why is there a circle drawn in the drawing where the pad copper must be exlucded?

This leads to one question:

  1. How does one design a PCB footprint for this package in Altium designer? It is not clear how to cut out copper as per the circle diagram shown.

Note (on page 2):

All dimensions are in millimeters. (inches)

Tolerance is ±0.10mm(0.004") unless otherwise specified.

  • 3
    \$\begingroup\$ My guess is they just calculated the pad length from the carve-out and then didn't round whatever the result was, so you end up with a ludicrous number of decimal places. I'll just mention that the pad-terminal overlap in that dimension only needs to be 75% to satisfy IPC-A-610 inspection criteria for class 3 and 50% for class 1 and 2. You could also request a footprint from e.g. SnapEDA and make it their problem but results may vary. \$\endgroup\$
    – vir
    Apr 27, 2023 at 20:09
  • \$\begingroup\$ The SnapEDA does not appear to have the 2D model and 3D model for this part. \$\endgroup\$
    – quantum231
    Apr 27, 2023 at 20:23
  • \$\begingroup\$ What exactly is IPC-A-610? \$\endgroup\$
    – quantum231
    Apr 27, 2023 at 20:23
  • \$\begingroup\$ You can request the big online libraries to make a footprint for you from a part number, provided that the datasheet has dimensions for it. IPC-A-610 is an international standard for acceptability criteria for electronic assemblies. \$\endgroup\$
    – vir
    Apr 27, 2023 at 20:33
  • 1
    \$\begingroup\$ According to my calculations, the rectangle width is exactly 5/30 of an inch. Then 25.4 * (5 / 30) / 2 - sqrt(1.15^2 - (1.25/2)^2) = 1.1513 mm. \$\endgroup\$
    – rodrigo
    Apr 28, 2023 at 11:41

2 Answers 2


This is called a reverse entry type. The LED is designed to project through the PCB to the bottom side to allow viewing from the bottom. I would use a rectangular pad with a small clearance from the hole. The connections remain on the top side.

The part is still technically on the top side to keep assembly on one side only.

  • \$\begingroup\$ Are there other components that are of "reverse entry type"? I have never heard of this before. \$\endgroup\$
    – quantum231
    Apr 28, 2023 at 1:24
  • \$\begingroup\$ @quantum231: I haven't seen any, perhaps some connectors. It is a way to avoid having to put parts on two sides. It is more expensive to assemble. It is fairly common for LED indicators. \$\endgroup\$
    – RussellH
    Apr 28, 2023 at 1:28
  • 1
    \$\begingroup\$ @quantum231 Photodiodes can come as reverse. I think some buttons do too. \$\endgroup\$
    – DKNguyen
    Apr 28, 2023 at 1:35
  • 1
    \$\begingroup\$ @quantum231 I've seen some reverse entry pin headers, and a handful of sensors. It's not common, but it's not rare either. \$\endgroup\$
    – Hearth
    Apr 28, 2023 at 1:36
  • 1
    \$\begingroup\$ Some microphones do this. Good ones too, you see them in smartphones! \$\endgroup\$ Apr 28, 2023 at 15:01

Create the outline with lines and arcs, convert outline to region, and place a pad entirely within the region.

They likely don’t want the copper right up against the hole because you could get a rogue sliver of copper that could cause shorts elsewhere on the PCB. Especially with an unplated hole.

  • \$\begingroup\$ I will give it a try and let you know. \$\endgroup\$
    – quantum231
    Apr 27, 2023 at 22:53

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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