The line
#7=#2003
is going to set #7 to whatever the value of tool length offset 3 is, which depending on how your shop does offsets may be somthing like -5.236 etc..
If you are then doing H#7 the control is going to be confused.
You have 5 drills and 5 reamers so I would use offsets 1 thru 5 for the drills and 11 thru 15 for the reamers.
Assuming the tool changer on the machine can handle 15 tools then the tool number can be the same as the length offset.
You then just need some code at the top of your program to set which tools you want to use.
Code:
#1=3(DRILL TO USE)
#2=#1(REAMER TO USE)
(DO NOT EDIT BELOW THIS POINT)
G0G17G20G40G49G80G90G94
N1M1(DRILL)
T#1
M6
M1
T#2 (PRELOAD IF IT APPLIES TO YOUR MACHINE)
G0G90G54X0.0Y0.0
S500M3 (THIS IS WHERE YOU CAN GET FANCY )
(AND USE #1 TO GET A TOOL RADIUS/DIAMETER )
(AND CALCULATE THE RPM TO THE DESIRED SFM )
(WHICH COULD BE HARD CODED INTO THE )
(CALCULATION OR SET AS ANOUTHER VARIABLE )
(AT THE TOP OF THE PROGRAM)
G43Z1.0H#1
M8
G83Z-2.5R0.1Q0.2F6.0L0(NOTE FEED COULD ALSO BE CALCULATED)
.
.
.
G80
M9
G91G28Z0M5
N2M1(REAM)
(SEE DRILL JUST SWAP THE #1 AND #2)