Haas reads past macro argument in m98 sub call

I am using a Haas 2009 vf3 mill with a DS30-SSY

I'm having an issues where the macro argument reads past the Z level argument to end last z move. It will not move the next line of code, and continues to go back to the N100 line. This code is embedded in a sub call. I have written many helical milling macros much like the one below all on Fanuc based machines and had no issues. On a HAAS is there conflict with using M98 P#### calls being it may want to loop back with the look ahead?
%
O7001(HELICAL MILL+CBORE)


#640= 0.927 (PIN HOLE SIZE)
#641= -1.36 (COMPRESSION DISTANCE VALUE)
#642= 3.917 (PISTON MAJOR O.D. VALUE)
#643= 2.865 (LOCK RING DISTANCE)
#644= 0.073 (LOCK RING TOOL WIDTH)
#645= 1.007 (LOCK RING DIAMETER)
#646= 1.250 (PIN BOSS SPACING)
#647= 2.75 (PIN LENGTH)
#648= 3.130 (OUTSIDE PIN BOSS)

N778
#630= [ [ #642 / 2 ] + 0.1 ] (Z CLEARANCE PLANE)
#631= [ #642 / 2 ] (Z INITIAL CUT)
#632= [ [ #643 / 2 ] - #644 ] (1RST LOCK RING Z VALUE)
#633= [ #643 / 2 ] (2ND LOCK RING Z VALUE)
#634= [ [ #645 - #638 ] / 2 ] (LOCK RING DIA. VALUE)
#635= [ [ #643 / 2 ] + 0.09 ] (Z VALUE FOR CONTOUR BORES)
#636= [ [ COS[ 45 ] ] * [ #640 / 2 ] ] (LOCATION FOR THE REMOVAL NOTCH)
#637= [ [ #643 / 2 ] - 0.0937 ] (Z VALUE FOR NOTCH TOOL)
(#638-DIAMETER ARGUMENT FOR LOCKRING DIAMETERS)

#604=[[#648-#647]/2]]
#606=#640-#605
#607=#606/2
#611=[#604+.05]

N1000
X#601Y#602
G1Z#630F25.0
N100
G1Y#607 D23 F50.0
G2J-#607 Z#631
#631=[#631-.03]
IF[#631GE#604]GOTO100
G1Y#602
G00Z#630

IF[#651EQ0]GOTO2100

N2000
X#601Y#602
G1Z#630F25.0
N200
G1Y[#607-.005] D23 F50.0
G2J-[#607-.005] Z#635
#631=[#631-.03]
IF[#631GE#635]GOTO200
G1Y#602
G00Z#630

N2100
M99
%

I add a G103 P1 to limit the look ahead while I run the macro, then a G103 after the macro but before the machining to reset the look ahead.

Would this be the right approach adding it in the sub


%
O07001 (HELICAL MILL)
#640= 0.927 (PIN HOLE SIZE)
#641= -1.36 (COMPRESSION DISTANCE VALUE)
#642= 3.917 (PISTON MAJOR O.D. VALUE)
#643= 2.865 (LOCK RING DISTANCE)
#644= 0.073 (LOCK RING TOOL WIDTH)
#645= 1.007 (LOCK RING DIAMETER)
#646= 1.250 (PIN BOSS SPACING)
#647= 2.75 (PIN LENGTH)
#648= 3.130 (OUTSIDE PIN BOSS)

N778
#630= [ [ #642 / 2 ] + 0.1 ] (Z CLEARANCE PLANE)
#631= [ #642 / 2 ] (Z INITIAL CUT)
#632= [ [ #643 / 2 ] - #644 ] (1RST LOCK RING Z VALUE)
#633= [ #643 / 2 ] (2ND LOCK RING Z VALUE)
#634= [ [ #645 - #638 ] / 2 ] (LOCK RING DIA. VALUE)
#635= [ [ #643 / 2 ] + 0.09 ] (Z VALUE FOR CONTOUR BORES)
#636= [ [ COS[ 45 ] ] * [ #640 / 2 ] ] (LOCATION FOR THE REMOVAL NOTCH)
#637= [ [ #643 / 2 ] - 0.0937 ] (Z VALUE FOR NOTCH TOOL)
(#638-DIAMETER ARGUMENT FOR LOCKRING DIAMETERS)

#631=ROUND[#631]

#629=#631

#604= [ [ #648 - #647 ] / 2 ]
#606= #640 - #605
#607= #606 / 2
#611= [ #604 + 0.05 ]
#651=1

G103P1(TURN LOOK AHEAD OFF)

G01 Z#630
N10
X#601 Y#602
G01 Z#631 F25.
G01 Y#607 F50.

N100
G02 J - #607 Z#631
#631= [ #631 - 0.03 ]
IF [ #631 LT #611 ] GOTO200
IF [ #631 GE #611 ] GOTO100
N200 G02 J - #607 Z#611

G01 Y#602
G00 Z#630

IF [ #651 EQ 0 ] GOTO2100

N20
X#601 Y#602
G01 Z#630 F25.
N200
Z#635
G01 Y [ #607 + 0.0025 ] F50.
G02 J - [ #607 + 0.0025 ]
G02 J - [ #607 + 0.0025 ]
G01 Y#602
G00 Z#630

N2100
G103(TURN LOOK AHEAD ON)

M99
%

Here's a sample from the last one I did.

I did the G103 P1 right where the program enters the macro, and turned it off once it got to machining

Wherever your program enters the sub, I would have the G103 P1 be the first thing it reads.