Siemens 840d Automated Tool Length Setting

setup_tools.mpf

; Automated tool length measurement 
; Siemens 840d (Tested on DMU50)

; This program will call every tool into the main spindle and run a blum
; laser measuring cycle designed to record the tool length offset of the tool
; I've included citations of the manual pages I referenced to find the pieces 
; of data used in the program

; See the manual SINUMERIK 840D sl / 828D Job Planning for information on the 
; high-level nc language

DEF INT _i
DEF INT _t

; $P_TOOLNT     a count of the number of tools defined in NCK   [1]
; $A_TOOLMN[n]  magazine number of tool n                       [2]
; $TC_DP1[c,t]  code representing tool type (mill,drill,        [3]
;               probe,etc) of cutting edge c on tool t
; $TC_TP2[t]    tool identifier string                          [4]

FOR _i = 1 to $P_TOOLNT
    ; store tool number 
    _t = $P_TOOLT[_i]
    ; if the tool is located in any magazine
    IF $A_TOOLMN[_t] > 0
        ; if the tool type is NOT any kind of probe or aux 
        IF $TC_DP1[_t, 1] < 710
            ; load tool by identifier
            T=$TC_TP2[_t] M6
            ; turn spindle slowly
            S1200 M3
            ; laser measuring cycle
            BL9902(3,0.002,0,3,0.0004)
        ENDIF
    ENDIF
ENDFOR

M30

; 1. SINUMERIK 840D sl Tool Management, sec. 5.8.46, pp. 336
; 2. SINUMERIK 840D sl Tool Management, sec. 5.8.36, pp. 325
; 3. SINUMERIK 840D sl Tool Management, sec. 5.3.2, pp. 239
; 4. SINUMERIK 840D sl Tool Management, sec. 5.2.2, pp. 232

Why do you use line 27: $TC_DP1[_t, 1] < 710, to determine if the tool type is not a probe or aux? What does the number 710 have to do with this?