PCB Footprint Design Dimensions

I am trying to make a Eagle library for a Micro USB B connector. The library is unavailable and I decided to make one with the datasheet dimensions provided. But it is rather confusing.

The units are in mm

Please check the attached image.

1. The Dimensions are shown as subtracted from another. Like A-B I thought that was a tolerance. (Not sure though if it is a tolerance.)
I do not understand that notation. Looks like a huge error. Is it a good idea to design the footprint to the maximum error provided?

2. I have marked the rear pin in the following image within rectangles. As the top view the size of the pin is 4-1.00 But as Y the size is 2-2.00!!

I did a little research and as I understood

4-1.00 First view (marked as X) suggests that the dimension can be 4mm or 3mm.
2-2.00 Second view(marked as Y) suggests the dimension is 2mm

But it is for the same side of the same pin!!! Shouldn’t the dimensions be the same? Literally the pin is same. That is the width of the pin.

Please advice me how to read this dimensions in the datasheet.

Regardless of what the datasheet says I would want the actual part in front of me to check that the part actually fits on the PCB when its printed out at 1:1.

I always test new footprints in this way.

4-1.00 First view (marked as X) suggests that the dimension can be 4mm or 3mm.

You think so ?

Look at the plan, print it out large scale and check if you like.

If the distance between the little pins is 3.7mm, does it seem likley that the little pin could be 4mm wide ?

Just measuring in the screen suggests the pin is 1mm wide, check on the real connector.

you are misinterpreting the notation. I don't know what it's supposed to mean either, but where the measurement is preceded by a number and a dash, the number and dash are not part of the dimension in question.

I think that this is confusing notation!
The "dash" number probably means that
the dimension shown applies to more than
one location. We usually use "2 PLCS" or
"4 PLCS."
Herb

sahirudilan:
I am trying to make a Eagle library for a Micro USB B connector. The library is unavailable and I decided to make one with the datasheet dimensions provided. But it is rather confusing.

The units are in mm

Please check the attached image.

1. The Dimensions are shown as subtracted from another. Like A-B I thought that was a tolerance. (Not sure though if it is a tolerance.)

4--1.00 means 1.00mm, repeated four times

I do not understand that notation. Looks like a huge error. Is it a good idea to design the footprint to the maximum error provided?

2. I have marked the rear pin in the following image within rectangles. As the top view the size of the pin is 4-1.00 But as Y the size is 2-2.00!!

The soldermask size is 2mm, the hole size is 1.6mm and the metal tab is 1mm. The slop is bigger for rear tabs than the front ones, means the pick-and-place machine won't fail to drop the part into the holes(*) - this is an SMT part with through-hole as well.

I did a little research and as I understood

4-1.00 First view (marked as X) suggests that the dimension can be 4mm or 3mm.
2-2.00 Second view(marked as Y) suggests the dimension is 2mm

As I said 1mm tab, 2mm soldermask

(*) A heavy part like a metal connector will be picked up by its centre of mass by the pick-and-place, so the slop required for the holes depends on their distance from the centre of mass, as there is always some rotational error - with normal SMT pads the solder's surface tension corrects for minor misalignment, for dropping a peg in a hole you have to get that right every time or the production line is broken.

Where did you buy the part? Mouser and Digikey have the Eagle libraries for almost everything they make. And if they don't have it, they will make it on request. No purchase needed.