You can open the Orcad design file (probably the .MAX file for the PCB) in the (free, downloadable) viewer and look at the mounting hole coordinates. Or use Orcad itself if you have it installed. Click on one of the pads, then open the spreadsheet for 'footprints' and you will see something like this (the one you clicked should be at the top and highlighted):
If you want to use Brian's method, the default Orcad Excellon file name is a text file named THRUHOLE.TAP and the relevant section would look something like this:
This is tool 12 (T12), diameter (in inches in this case) of 0.138 with some more-or-less random downfeed rate (200 inches per minute) and spindle RPM (100,000)- those numbers will be replaced by the PCB manufacturer most likely anyway. The tools are in sequence from T1 onward, not necessarily sorted by size. This file was (as usual) done with absolute coordinates, not incremental, and the holes are at coordinates (in inches). The number of digits may vary, as may the units, but inches are still most common.
In inches, the coordinates are as follows:
(0.1, 0.275),(0.1, 2.275),(2.6,0.275),(2.6,2.275)
If you are trying to align connectors, I suggest using the pad locations rather than the component locations.
This is a big pain, especially when switching EDA systems. Recently I saw hundreds of boards scrapped because the designer misaligned a couple mounting holes by a bit over 1mm. Not much, but enough. Fortunately, it was caught before the boards were populated. So I suggest listing and double/triple checking all the critical alignment coordinates. Comparing the Gerbers might be worthwile.