[jack.depasquale]

I am new to parametric programming and so have a lot of questions. I saw your macro for the spiral hole, and saw you had several versions. Can you post them also? Can you supply a sketch showing the input variables I am not sure what the 1st one is q= zpick?


Appreciate any help possible,
Jack D.
[email protected]

[gbowne1]

I was wondering if G33 was similar (nobody posted to my thread about G33 that I am using).

Will these programs run on the 15M?

[sinha_nsit]

Some properties of a null variable:
In conditional expressions, except for EQ (equal to) and NE (not equal to), a null variable is same as 0.
In arithmetic expressions, it is always same as 0.
It it appears in an address, that particular word is ignored (e.g., G00 X#1 Z100 is same as G00 Z100, if #1 is null)

[stevo1]

Will these programs run on the 15M?

The macro I posted in post #10 I wrote for my 15series Fanuc controls so yes it will work in yours. Obviously do some investigating on your control before just running. You want to make sure that the variables I am using in the program are not already being used in your control for something else.

Stevo

[samu]

in this Thread, helical milling seems to be confused with spiral milling. Take a look a this thread that is more about spiral milling.
http://www.cnczone.com/forums/showthread.php?t=110522

[ajithashankar]

Hi...
I want to do spiral milling(constant depth) in my HMC machine (Fanuc contol) Could anyone please help for doing macro for this.

[samu]

if you follow the link i gave in my previous post, you'll find a lot of interesting stuff about spiral milling. I realy like the way i explain with the 2 center spiral cause it's simple and efficient and don't need a lot of calculation.

[msantaji1]

i will come back on this matter very soon
plz provide drawing details what you really want

[ajithashankar]

Dear Samu,

Thanks for the reply.The macro programme you given is working. But if i want to starting diameter of spiral is around dia 250, for that what i have to change ,could you please help.

[samu]

starting diameter is function of the step over. The tool plunge at the true center and arc 180 deg to the first "False" center. False centers are 1/4*stepover appart the true center. So the first move is a 180deg arc with a diameter of stepover/4 having its center at stepover/8 from the true center.

I'm very happy that you have tried it. If you need more explaination or have suggestion to improve it, don't hesitate.

[ajithashankar]

Hi..

Good morning,

Sir i understood the formula of the macro you given ,but the problem we are facing is to avoid the idle passes.In our component we need face serration having the step diameter from 250MM minor diameter and 400mm major diameter, but in macro starting diameter is step over/4 so we need to change the starting diameter to our component minor diameter.

[samu]

I think that the simpliest way is to begin at the start of the half turn that reach the start diameter. That way, you always have less than an half turn cutting the air. You have to determine if tis an odd or even half turn in order to know if the value are positive or negative. Nothing has been tested.

G65 P9013 Axx Bxx CXX Dxx Fxx Hxx Rxx Xxx Yxx Zxx
A=STEP OVER (#1)
B=TOOL DIAMETER (#2)
C=START DIAMETER(#3)
D=FINAL DIAMETER (#7)
F=X-Y FEED (#9)
H=Z FEED (#11)
R=RETRACT PLANE (#18)
X=X CENTER OF SPIRAL (#24)
Y=Y CENTER OF SPIRAL (#25)
Z=Z COORDINATE AT THE BOTTOM OF TOOLPATH (#26)

%
O9013(SPIRAL MACRO)
#7=#7-#2 (FINAL DIAMETER-TOOL DIAMETER)
#100=FUP[#7/#1+.5] (NUMBER OF HALF TURN NEEDED TO REACH FINAL DIAM)
#101=[#7/[#100-.5]] (CORRECTED STEP OVER )
IF[#3 NE #0] GOTO5 (IF THERE IS A START DIAMETER INPUTED)
#102=1 (HALF TURN COUNTER)
#103=[#101/4] (CURRENT DIAMETER)
G0 G90 X#24 Y#25 (RAPID TO CENTER)
Z#18 (RAPID TO RETRACT PLANE)
G01 Z#26 F#11
G91
G03 X#103 I[#103/2] F#9 (CUT THE FIRST ARC)
#102=#102+1 (INCREMENT COUNTER)
GOTO7
N5 #102=FIX[#3/#101]+1
#104=[#101*[#102-1]/2] (DISTANCE FROM START POINT TO CENTER)
#105=#102 AND 1
IF [#105 EQ 1] GOTO 6 (IF THE START HALF TURN IS AN EVEN HALF TURN)
G0 G90 X[#24+#104] Y#25 (RAPID TO START POINT)
Z#18 (RAPID TO RETRACT PLANE)
G01 Z#26 F#11
G91
#103=#101*[#102-1]
G03 X#103 I[#103/2] F#9
#102=#102+1
IF[#102 GT #100] GOTO10
GOTO 7
N6 G0 G90 X[#24-#104] Y#25 (RAPID TO START POINT)
Z#18 (RAPID TO RETRACT PLANE)
G01 Z#26 F#11
G91
N7 DO1 (CUT THE SPIRAL)
#103=#101*[#102-1] (CURRENT DIAMETER)
G03 X-#103 I[-#103/2] 
#102=#102+1
IF[#102GT#100] GOTO15
#103=#101*[#102-1]
G03 X#103 I[#103/2] F#9
#102=#102+1
IF[#102 GT #100] GOTO10
END1
N10 G03 I-[#7/2] (ENTIRE CIRCLE AT FINAL DIAMETER)
GOTO20
N15 G03 I[#7/2] (ENTIRE CIRCLE AT FINAL DIAMETER)
N20 G0 G90 Z#18
M99
%

[ajithashankar]

Hi!!!!

Thank you very much samu its working...

[Mohak]

HI Samu,

I am very new to VMC Programming , more of a lathe guy. I have a problem with which i hope you can help me.

I have to make a hole of 43 mm in a Recatngle piece of steel, My X and Y 0 are the center of the stock and i am using an 11mm endmill . depth of the hole is 40 mm and i am planning to this in 2 passes of 20 mm each

I have predrilled a hole of 25 mm in the center and now i have to open it to the finish diameter of 43mm with a 0.5 mm step over. I am planning to use the macro that you have posted, can you please look at my code below to see if it will work fine?? Its an Old Mill with Fanuc Om

Thank you for any help you can give.
Mohak

G65 P9013 A0500 B11.0 C25.0 D43.0 F600 H100 R2 X0.0 Y0.0 Z-20.0
A=STEP OVER (#1)
B=TOOL DIAMETER (#2)
C=START DIAMETER(#3)
D=FINAL DIAMETER (#7)
F=X-Y FEED (#9)
H=Z FEED (#11)
R=RETRACT PLANE (#18)
X=X CENTER OF SPIRAL (#24)
Y=Y CENTER OF SPIRAL (#25)
Z=Z COORDINATE AT THE BOTTOM OF TOOLPATH (#26)

[Mohak]

HI Samu,

I am very new to VMC Programming , more of a lathe guy. I have a problem with which i hope you can help me.

I have to make a hole of 43 mm in a Recatngle piece of steel, My X and Y 0 are the center of the stock and i am using an 11mm endmill . depth of the hole is 40 mm and i am planning to this in 2 passes of 20 mm each

I have predrilled a hole of 25 mm in the center and now i have to open it to the finish diameter of 43mm with a 0.5 mm step over. I am planning to use the macro that you have posted, can you please look at my code below to see if it will work fine?? Its an Old Mill with Fanuc Om

Thank you for any help you can give.
Mohak

G65 P9013 A0500 B11.0 C25.0 D43.0 F600 H100 R2 X0.0 Y0.0 Z-20.0
A=STEP OVER (#1)
B=TOOL DIAMETER (#2)
C=START DIAMETER(#3)
D=FINAL DIAMETER (#7)
F=X-Y FEED (#9)
H=Z FEED (#11)
R=RETRACT PLANE (#18)
X=X CENTER OF SPIRAL (#24)
Y=Y CENTER OF SPIRAL (#25)
Z=Z COORDINATE AT THE BOTTOM OF TOOLPATH (#26)

[siskk]

Hi guys,
Here is something i worked on last few days. Works perfect on fanuc 32 milling center.
I did it on the most stupid way, It is not complicated at all. Simple but absolutely effective.

%
O7998(MAIN PROGRAM)

(X#24 X0)
(Y#25 Y0)
(Z#26 HOW DEEP)
(T#20 TOOL DIA)
(A#1 STP OVER)
(U#21 HOLE DIA)
(D#7 FINAL DIA)
(F#9 FEED)
(H#11 RETRACT)


T1M6
G54G40G80G90
(G52X...Y...)
G0X0Y0S3500M3
G43Z10H1M8
G65P7999X0Y0Z-20T15.96A.3U36.5D39.06F1000
G0Z100M15
G91G28Y0
M30

(-/-/-/-/-/-/-/-/-/-/-/-/-/-/-)

O7999(SpIral pocketing)

#1=#1/4
#20=#20/2(TOOL DIA TO Radius)
#21=#21/2(HOLE DIA TO Radius)
#28=[#21-#20](HOLE Radius minus TOOL Radius)
#7=#7/2(FINAL DIA TO Radius)
#7=#7-#20(FINAL Radius minus TOOL Radius)
G1Z#26
G1X#28
IF[#28GT[#7-[#1*2]]]GOTO2
N1G3X0Y[#28+#1]R[[[#28+#1]+#28]/2]
#28=[#28+#1]
IF[#28GT[#7-[#1*2]]]GOTO3
G3Y0X-[#28+#1]R[[[#28+#1]+#28]/2]
#28=[#28+#1]
IF[#28GT[#7-[#1*2]]]GOTO4
G3X0Y-[#28+#1]R[[[#28+#1]+#28]/2]
#28=[#28+#1]
IF[#28GT[#7-[#1*2]]]GOTO5
G3Y0X[#28+#1]R[[[#28+#1]+#28]/2]
#28=[#28+#1]
IF[#28GT[#7-[#1*2]]]GOTO6
GOTO1
N2G3Y0X-#7R[[#7+#28]/2]
I#7
Y0X[#7-#1]R[[[#7-#1]+#7]/2]
GOTO9
N3G3X0Y-#7R[[#7+#28]/2]
J#7
X0Y[#7-#1]R[[[#7-#1]+#7]/2]
GOTO9
N4G3Y0X#7R[[#7+#28]/2]
I-#7
Y0X-[#7-#1]R[[[#7-#1]+#7]/2]
GOTO9
N5G3X0Y#7R[[#7+#28]/2]
J-#7
X0Y-[#7-#1]R[[[#7-#1]+#7]/2]
GOTO9
N6G3Y0X-#7R[[#7+#28]/2]
I#7
Y0X[#7-#1]R[[[#7-#1]+#7]/2]
N9G0X0Y0Z10
M99
%