Re: gEDA-user: Verifying footprints

[DJ Delorie <dj@xxxxxxxxxxx>]

> Pad[-3543 -393   -3543 393   5118   2000 5718 "1" "1" "square"]
> Pad[ 3543 -393    3543 393   5118   2000 5718 "2" "2" "square"]
> 	
> According to the gEDA how to create footprints document the dimensions for
> the 0805 are (these values are taken from the IPC-SM-782A Standard):

Note that PCB has at least 10 0805 footprints, in at least six
different sizes, depending on whether you have a resistor, capacitor,
or inductor, and whether your process needs the most, least, or normal
amount of copper.  The plain "0805" is approximately (silk differs)
the CAP2012N footprint.

Also, if you read our library sources, you'll see that we follow
IPC-7351.

>   C      X     Y     Z      G       Grid
> 74.8   59.1  51.2  126.0  23.6  157.5 x 315.0
> 
> So from the document the pad sizes as follows:
> 
> Calculated dimensions:
> C = 3543 * 2 = 7086 = 70.86 mils

Ok.

> X = 5118 = 51.18 mils

X = 5118 + (393 - -393) = 59.04 mils

> Y = 393 * 2 + thickness = 5904 = 59.04 mils

Y = 5118 + (3543 - 3543) = 51.18 mils

You have X and Y swapped in your figure relative to PCB's X and Y
axes, so confused the dX and dY addends.

> G = C - thickness = 7086 - 5118 = 1968 = 19.68 mils

Ok.

> Z = C + thickness + clearance = 7086 + 5118 + 2000 = 14204 = 142.04 mils

Ok.


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user