Problem- Helical Milling

[mikepaubuchon]

I am trying to do helical milling on Citizens (without the h-mill option). I use a macro programs all the time but this one has me a little stumped. The holes come out nice (size,finish) but the program runs very slow. I freed up as much memory as I could, thinking maybe that might help, but it is still slow. I am not sure, but it seems to be waiting to recalculate before each move? If I try using G2/G3 I get alarm(no option). Do I need to RND or use different formula? If any has done helical milling I would appreciate some tips. I will paste copy below.Thanks.

O0006 (HELICAL-MILL)

(SAVE POSITION OF X-Y-Z)
(X) #141=#5041
(Z) #142=#5042
(Y) #143=#5043

(PROGRAM-RADIUS-COMP)
#110=[#7-#20]/2

(X-MOVEMENT-1-DEG)
#104=[#1/360]*2

(X-END-POINT)
#114=#24-[#2*2]

G50Y0Z0
G1 G98 Y0. Z0. X#24+.02 F#9

(LOOP-TO-BOTTOM)
#124=#24
#105=1
WHILE[#124GE#114]DO1
#125=#110*COS[#105]
#126=#110*SIN[#105]
G1 Y[#125 * #13] Z#126 X#124 F#9
#105=#105+1.(INC.-DEG.)
#124=#124-#104
END1

(FULL-REVOLUTION-BOTTOM)
WHILE[#105LE[#105+360.]]DO2
#125=#110*COS[#105]
#126=#110*SIN[#105]
G1 Y[#125*#13] Z#126
#105=#105+1.(INC.-DEG.)
END2

(ARC-OFF-BOTTOM)
WHILE[#105LE[#105+90.]]DO3
#125=#110*COS[#105]
#126=#110*SIN[#105]
G1 Y[#125*#13] Z#126
#105=#105+1.(INC.-DEG.)
END3

G1Y0Z0 F#9
G0X#24+.1

(SET-BACK-TO-ORIGINAL)
G50X#141Z#142Y#143
M99

(!!!-X=DIAM-VALUE-!!!)
(!!!-A,B=RAD.-VALUE-!!!)
(X- START-DIAMETER)
(A- DEPTH-PER-REVOLUTION-X)
(B- DEPTH-OF-HOLE)
(D- DIAM-OF-HOLE)
(F- FEED-IPM)
(T- TOOL-DIAMETER)
(M1- FOR-Y-RADIUS-MACHINES)
(M2- FOR-Y-DIAMETER-MACHINES)

(#105=PROGRAM-COUNTER-DEGREES)
(#110=PROGRAM-TOOL-RADIUS-COMP)

(#104=X-MOVE-1-DEGREE)
(#114=X-DIAM-AT-BOTTOM-OF-HOLE)

(#124=PROGRAM-X-COORDINATE)
(#125=PROGRAM-Y-COORDINATE)
(#126=PROGRAM-Z-COORDINATE)

(#141=X CURRENT POSITION)
(#142=Z CURRENT POSITION)
(#143=Y CURRENT POSITION)

[zooloader]

Hi, I assume RND stands for rounding off.
That sounds like a good option, the less number crunching the better, I guess. As long as you don't lose your size/finish!
With a Citizen machine, I again assume that you are working with rather small dimensions.
I noticed recently while milling a tapered bore, that the machine had a momentary dwell at the end/start of it's arc on/arc off movements. These rad's were small relative to the bore dia, and making them bigger changed this behaviour, and gave a flawless surface finish.
We have a couple of Tornos machines, though we have not tried any helical milling using a macro style such as yours, as we can use G02/G03 with a depth move, so I can't offer any direct solution unfortunately.
Unless you are being hounded to get the parts out quick smart, I'd leave well enough alone. Some things just take time

[MikeMc]

Depending on the age of the machine, and how good a relationship you have with your Citizen dealer, you may be able to get all the options turned on for free. ( Maybe the price of a service call). If you have a Mitsubishi control, most service techs can do it without a phone call.

[beege]

Those calculations take time, each and every time. If you could use a sub that only gets activated once after the machine gets turned on, and do all the calculations then, but not every time, then bypass the calculations for every part after that one, you might save some time.

Hardinge had a drilling sub that required 2 programs, one to do all the calcs, then one to do all the drilling. A block delete on the calcs sub allowed you the option to NOT calc every cycle.

Let us know what works for you!

[ProProcess]

Check the Control Parameter "Macro Single"
If this is on, all macro will execute one block at a time, this is for diagnostics.
If this is off, as it should be, all macro will execute more quickly.

Example...

Originally Posted by mikepaubuchon .... (SAVE POSITION OF X-Y-Z) (X) #141=#5041 (Z) #142=#5042 (Y) #143=#5043 (PROGRAM-RADIUS-COMP) #110=[#7-#20]/2 (X-MOVEMENT-1-DEG) #104=[#1/360]*2 (X-END-POINT) #114=#24-[#2*2]

With Macro single off these blocks would execute as if they were one block.
With Macro Single on, they execute one block at a time (slower).

HTH and good luck.