I made an improvement to the FACE MILL MACRO, please see previous post.

I got asked at work if I knew how to probe a flat surface and have the control figure out the adjustment to update the axis offset so the surface is flat. I understand the basic concept of how to achieve this, but I lack the experience to wrap my head around the logic that needs to be written for something like this. This is for a NMV to allow us to prove the A-axis flat instead of indicate the surfaces while setting up the part. Any help or general direction someone can point me to would be great. I don't run this machine, but it's a good opportunity to start learning it.

Usually when you have a probe it will come with macros already built into it to square up A axis. For instance here at work we use a O9917 which is custom for our use. If you want to write your own macro you could use this general guide and this would be for a horizontal:

1st probe hit Z: X+ direction and then store position into variable #600

2nd probe hit Z: X- direction and then store position into variable #601

Run Macro:

#602=[#601-#600]/2.

#603=ATAN[#602]/[width of X total distance divided by 2.]

IF[#603GT180.]THEN#603=#603-360.

(Update G54 A)

#5224=#5224+#603

Note: If A goes the wrong direction subtract #603 from #5224

#5224 is the system variable for G54 A on a Fanuc and Haas controls.

I updated the rough square pocket program with cutter comp and fixed the error in the face mill macro. See previous posts for these changes.

OK, it was driving me crazy not being able to figure this out on my own so I downloaded the trial version of NC PLOT and I have to say it's awesome. I have been writing these macros the hard way for many years. With this tool It only took me about 15 min to find out where most of my errors were. I still have I think only one bug to work out. I just wanted to apologize if my programs have caused any unwanted frustration to those of you who are trying to use them. It is only my intent to make certain machining applications easier through the use of macros for you guys. Thanks, James.

Just downloaded NC PLOT trial version on my vacay, I will give it a try.

Has anyone ever used them in cast Inconel 718? I was able to see one run in steel and it looked impressive but that's steel. Book shows up to 164 sfm. Far better than anything else I have found for this material. Would like to hear from someone with experience with them in this material before deciding.

We have had great luck with Titex drills. You will get the best results with through coolant.

 

I tried your new program, motion takes place in the first depth, after  do one step  by X and Y  one step, and then goes to the next depth, and the program ends

 

I promise the next thing I post will be a proven program, I just need more time. James.

Not criticizing, just asking a question and trying to help you out.

Don't worry. Won't do that again.

It's all yours.

Sorry, I did not mean to get so defensive. I appreciate any criticism or new ideas and I appologize for being "snippy". I would just like to see people fix the problem if they know that there is one or come up with a new solution. I mean we are all here to help each other out, or at least that is my opinion.

Your logic for the Z top of stock position is flawed.

It doesn't permit Z0.

 

You still have conditional branching issues.

 

 

Why don't you use #3000 for actual alarm messages?

Look, I'm giving this my best shot at what I have available. If anyone can make it better please do and repost. I am just trying to help a guy out and I know I am not perfect. I did not cut anything at Z0 because you would be just cutting air or very small amount of material so the first Z cut is below Z0 by the Q amount. I did not use #3000 because I am not sure if it would work for his particular control and wanted a message that could be seen by any control.

Sorry, It's obvious I rushed through this. It's a work in progress. I will try to get a copy of NCPlot. I have never used it and am used to just proving out macros I write at the machines.

O3334(ROUGH POCKET)
(ABSOLUTE MACRO)
(MUST HAVE START HOLE IN CENTER)
(UNPROVEN)

(FORMAT G65/G66 XYQSTRZEF)
(X = #24 - X DIMENSION)
(Y = #25 - Y DIMENSION)
(Q = #17 - STEPOVER IN Z/ DOC)
(S = #19 - STEPOVER IN XY/ PERCENTAGE)
(T = #20 - TOOL DIAMETER)
(R = #18 - R PLANE)
(Z = #26 - Z START/ TOP OF STOCK)
(E = #8 - END OF POCKET IN Z)
(F = #9 - FEEDRATE)
(*********************************)

IF[[#24*#25*#17*#19*#20*#18*#26*#8*#9]EQ0]GOTO1000
(CALCULATE DOC IN Z)
#100=ABS[#26]-ABS[#8]
#100=ABS[#100]
IF[[#26*#8]GE0]GOTO1
#100=ABS[#26]+ABS[#8]
N1#101=ROUND[#100/#17]
#102=#100/#101
IF[#102GT[#100/2.]]THEN#102=#100
(CALCULATE DOC IN X)
#103=[#19*.01]*#20
#104=[#24/2.]-[#20/2.]
#105=ROUND[#104/#103]
#106=#104/#105
IF[#106GT[#104/2.]]THEN#106=#104
(CALCULATE DOC IN Y)
#107=[#19*.01]*#20
#108=[#25/2.]-[#20/2.]
#109=ROUND[#108/#107]
#110=#108/#109
IF[#110GT[#108/2.]]THEN#110=#108
(STORE POSTIONS AND GO TO Z START)
#111=#5001
#112=#5002
#114=#112
#115=#111
#116=#112
#117=#111
G0G90X#111Y#112
Z[#26+.1]
G1Z#26F#9
#113=#5003-#102
#120=#106
IF[#120LT#110]THEN#120=#110
WHILE[#101GE1.]DO1
IF[#101EQ0]GOTO10
#101=#101-1.
G90G1Z#113F#9
WHILE[#120GT0]DO2
IF[#120LT0]GOTO100
#120=#120-1.
(CALCULATE TOOL PATH)
IF[#109EQ0]GOTO20
#114=#114+#110
N20
IF[#105EQ0]GOTO30
#115=#115-#106
N30
IF[#109EQ0]GOTO40
#116=#116-#110
N40
IF[#105EQ0]GOTO50
#117=#117+#106
N50
(CUT POCKET)
G1G90Y#114F#9
X#115
Y#116
X#117
X#111
(DOWN COUNT)
#105=#105-1.
#109=#109-1.
END2
N100
X#111Y#112
#113=#113-#102
END1
N10
X#111Y#112
Z#18
M99
N1000
M00(DATA LACKING)

1

 

Hello Cncchipmaker ! I tried the program on the machine, but the tool path is wrong, it can be seen in the photo

37475.jpg

the transition to the next depth, it comes on the z and then follows retract and end

 

and i find 1 error

#120=#106

#IF[#120LT#110]THEN#120=#110     

WHILE[#101GT0]DO1

 

I am sorry that it did not work the 1st time, sometimes the macros take a while to debug. I will continue to look at it for you. Without being in front of a machine it might take me a little more while to figure it out. Yes we need to remove the # sign just before the IF, good catch. I will update it.

I need to take a string of digits (say 12345 for example) and then break that number down so that each digit goes into a different common varriable. Anybody have any ideas on how to acomplish this?

Here is an example of how you can pull the digits:

O8116( SIX DIGIT S/N MACRO)

( USE OFFSET 98 FOR SERIAL # )

( 00.0001 WILL ENGRAVE 1 )

( 1ST NUMBER )

#138=[#2098*.1]

#140=FIX[#138]

#141=#140+8100.

( 2ND NUMBER )

#138=[#140*10]

#139=FIX[#2098]

#140=#139-#138

#142=#140+8100.

( 3RD NUMBER )

#138=[#139*10]

#139=FIX[#2098*10]

#140=#139-#138

#143=#140+8100.

( 4TH NUMBER )

#138=[#139*10]

#139=FIX[#2098*100]

#140=#139-#138

#144=#140+8100.

( 5TH NUMBER )

#138=[#139*10]

#139=FIX[#2098*1000]

#140=#139-#138

#145=#140+8100.

( 6TH NUMBER )

#138=[#139*10]

#139=FIX[#2098*10000]

#140=#139-#138

#146=#140+8100.

( ARGUMENT )

IF[#141GT8100.]GOTO1

IF[#142GT8100.]GOTO2

IF[#143GT8100.]GOTO3

IF[#144GT8100.]GOTO4

IF[#145GT8100.]GOTO5

IF[#146GT8100.]GOTO6

GOTO100

N1M198P#141

N2M198P#142

N3M198P#143

N4M198P#144

N5M198P#145

N6M198P#146

N100M99

OK fixed it, thank you!

 

O3334(ROUGH POCKET)

(ABSOLUTE MACRO)

(MUST HAVE START HOLE IN CENTER)

(UNPROVEN)

(FORMAT G65/G66 XYQSTRZEF)

(X = #24 - X DIMENSION)

(Y = #25 - Y DIMENSION)

(Q = #17 - STEPOVER IN Z/ DOC)

(S = #19 - STEPOVER IN XY/ PERCENTAGE)

(T = #20 - TOOL DIAMETER)

(R = #18 - R PLANE)

(Z = #26 - Z START/ TOP OF STOCK)

(E = #8 - END OF POCKET IN Z)

(F = #9 - FEEDRATE)

(*********************************)

IF[[#24*#25*#17*#19*#20*#18*#26*#8*#9]EQ0]GOTO1000

(CALCULATE DOC IN Z)

#100=ABS[#26]-ABS[#8]

#100=ABS[#100]

IF[[#26*#8]GE0]GOTO1

#100=ABS[#26]+ABS[#8]

N1#101=ROUND[#100/#17]

#102=#100/#101

IF[#102GT[#100/2.]]THEN#102=#100

(CALCULATE DOC IN X)

#103=[#19*.01]*#20

#104=[#24/2.]-[#20/2.]

#105=ROUND[#104/#103]

#106=#104/#105

IF[#106GT[#104/2.]]THEN#106=#104

(CALCULATE DOC IN Y)

#107=[#19*.01]*#20

#108=[#25/2.]-[#20/2.]

#109=ROUND[#108/#107]

#110=#108/#109

IF[#110GT[#108/2.]]THEN#110=#108

(STORE POSTIONS AND GO TO Z START)

#111=#5001

#112=#5002

#114=#112

#115=#111

#116=#112

#117=#111

G0G90X#111Y#112

Z[#26+.1]

G1Z#26F#9

#113=#5003-#102

#120=#106

#IF[#120LT#110]THEN#120=#110

WHILE[#101GT0]DO1

IF[#101EQ0]GOTO10

#101=#101-1.

G90G1Z#113F#9

WHILE[#120GT0]DO2

IF[#120LT0]GOTO100

#120=#120-1.

(CALCULATE TOOL PATH)

IF[#109EQ0]GOTO20

#114=#114+#110

N20

IF[#105EQ0]GOTO30

#115=#115-#106

N30

IF[#109EQ0]GOTO40

#116=#116-#110

N40

IF[#105EQ0]GOTO50

#117=#117+#106

N50

(CUT POCKET)

G1G90Y#114F#9

X#115

Y#116

X#117

X#111

(DOWN COUNT)

#105=#105-1.

#109=#109-1.

END2

N100

X#111Y#112

#113=#113-#102

END1

N10

X#111Y#112

Z#18

M99

N1000=(DATA LACKING)

Thank you Cncchipmaker! Error in line and there is no number 50

IF[#105EQ0]TOTO50

1

I think we can remove the ( in front of that line :

 

(IF[[#24*#25*#17*#19*#20*#18*#26*#8*#9]EQ0]GOTO1000

 

 Nice macro cncchipmaker.

Yes, please remove it. I hope that is the only thing wrong. Can someone please let me know if it works out, I do not get a chance to prove out everything I write.

Hello Cncchipmaker! I Interested in how to do this with step by Z(step down) and use modal call (used as a cycle)

Hello Cncchipmaker! I Interested in how to do this with step by Z(step down) and use modal call (used as a cycle)

Yes, I already have the Z step down figured out, but not sure how to calcutlate the pocket yet. I will need some time to figure that out. This will be used as a G65 macro call. Ex: G65P0001T.5Q.2X5.Y6. where T is tool diameter, Q is stepover, X&Y are the dimensions of the pocket, and so on.

Hi Everyone! The question is how to create a rough pocket . I saw it on the machines "Hardinge/Fanuc System II - VMC Series II"  but it is used as a cycle G72

1.jpg

Maybe at somebody have this cycle,please share

Do you want this routine to also step down in Z or do u want to adjust it every time?

Does anyone have any questions yet about the macros I posted?

Looking for some help with thread milling 152 holes in 304 stainless. tap drill .300 deep max. 10-24 unc 2B .17 deep min. I have done some thread milling before. But not with anything this small. We only have one thread mill. So I am hoping to get it right from the start. The cutter is tiny and I am afraid of breaking it.Especially with it being 304. Wondering how many radial passes to make and what depths for each.

Roll tapping would be much more efficient than thread milling. We have had great luck in 304, must use oil though and make sure the minor diameter is free of coolant before tapping