[deanmachine]

Hi,
We have a takasawa slant bed with a fanuc 6t we are teaching ourselves to program and run.
The issue is we have a contour to run in the id/face of the part it is cut using a boring bar.I use
mastercam x4 just to get my path then plug my path into my program by hand
We use G50s in the start and end at tool change. We need to
take many cuts so I used a G72 line and a G70 for my fin pass with path from mastercam between.
All runs well as far as the numbers but we cannot get to take more than 1 rough and 1 fin no matter
what we put in to the G72 D value. This is where we are out of ideas tryed a lot of things just cant get
it to multipass correctly. We dont have an issue with G71 when turning Why now??? This is a sample
of our program any thoughts guys?? Also the shape is just a golf disk top for a mold .

M41
G50 X11. Z5.
G97 S650 M3 T1010
G0X8.4466 Z.01
G72 P10 Q20 U.003 W.003 F.01 D500
N10 G1 Z-.0369
G3 X8.3981 Z-.0866 R.0844
X8.371 Z-.0949 R.0344
X6.5371 Z-.2799 R3.9844
X.0313 Z-.4124 R39.9844
G1 X-.015
N20 Z.01
G70 P10 Q20 F.008
G40 G0 X11. Z5. T1000
M30

Thanks
Dmachine

[angelw]

Hi,

M41
G50 X11. Z5.
G97 S650 M3 T1010
G0X8.4466 Z.01
G72 P10 Q20 U.003 W.003 F.01 D500
N10 G1 Z-.0369
G3 X8.3981 Z-.0866 R.0844
X8.371 Z-.0949 R.0344
X6.5371 Z-.2799 R3.9844
X.0313 Z-.4124 R39.9844
G1 X-.015
N20 Z.01
G70 P10 Q20 F.008
G40 G0 X11. Z5. T1000
M30

Thanks
Dmachine

Your problem is that you're using the G72 Cycle incorrectly. The action of this Cycle where a Bore is concerned, shallow as it may be, is for the the tool to be parked at or less than the smallest diameter of the profile in X and clear of the workpiece in Z. The "P" referenced block, N10 in your case, would be a move to the last Z coordinate in the part profile description. The tool would move the depth of cut set via "D" from the Start Z location of the tool, then feed in an X + direction to take the cut.

Four cutting patterns are considered as shown in the following attached picture. The pattern that applies to your profile is that shown in the 2nd quadrant of the picture. The tool path between A and A’ is specified in the block with sequence number referenced by the "P" address in the G72 Cycle Block. The part profile from the "P" to the "Q" referenced block is described from A through A' to B in that order.

Attachment 229158

The following is the program that will theoretically work, but physically can't because of the profile of your work, and the interference of the Boring Bar and Workpiece resulting from where the boring bar start location must be to be able to achieve the profile description shown in your example program.

M41
G50 X11. Z5.
G97 S650 M3 T1010
G00 X-.015 Z.01
G72 P10 Q20 U.000 W.003 F.01 D500
N10 G01 Z-.4124
G01 X.0313
G02 X6.5371 Z-.2799 R39.9844
X8.371 Z-.0949 R3.9844
X8.3981 Z-.0866 R.0344
X8.4466 Z-.0369 R.0844
N20 G01 Z0.01
G70 P10 Q20 F.008
G40 G0 X11. Z5. T1000
M30

What you will have to do is create a rough, flat bottomed bore large enough to give clearance on the Boring Bar, and use the G72 cycle to rough the profile to the limits of the bore. Then, depending on the style of boring bar you're using, you may be able to rough the remainder with long hand code.

You could use a G73 cycle (Pattern Repeat) to rough right to the centre, but there would be a fair amount of fresh air cutting involved.

Regards,

Bill

[fordav11]

btw don't use U positive when roughing a face shape otherwise your tool will cut into the finish profile on the rough passes.
If anything you want U- but U0 and W positive will work just fine for your profile.

You can't machine that profile with a regular (*) boring bar. To machine that profile correctly without destroying the tool requires a neutral OD turning tool set in the facing position (90 degrees to the part)
Something like a PDPNN turning tool will work just fine.

(*) you can get a boring bar especially for ball-turning with front clearance angle that is near to 45 degrees and using a 35/55 degrees insert you could take cuts like you want to

Attachment 229146

it's far easier to use a PDPNN turning tool at 90 degrees.

[deanmachine]

Hi,
We are useing the proper tool identical to your pick
We are a little confused with this you say :

"btw don't use U positive when roughing a face shape otherwise your tool will cut into the finish profile on the rough passes.
If anything you want U- but U0 and W positive will work just fine for your profile."

Do you mean write my path from the center out? we tryed that and it just runs our fin path and did not step in we even
made our z 0 at the bottom of bore instead of face of part will not step ???

Many Thanks,
dmachine

[deanmachine]

THANKS!! To you guys We got it figured out!! BTW we have to keep putting to the machine back to uo wo before we
start by handle is there a faster way to MDI back to that position we tryed to do it but it wont go there??

[angelw]

Hi,
We are useing the proper tool identical to your pick
We are a little confused with this you say :

"btw don't use U positive when roughing a face shape otherwise your tool will cut into the finish profile on the rough passes.
If anything you want U- but U0 and W positive will work just fine for your profile."

Do you mean write my path from the center out? we tryed that and it just runs our fin path and did not step in we even
made our z 0 at the bottom of bore instead of face of part will not step ???

Many Thanks,
dmachine

Your profile is effectively a bore (Internal Profile). Accordingly, a U+ finishing allowance is going to cause over cutting, particularly at the larger diameter area of your profile. The attached picture in Post #2 shows the respective directions of U and W for the four cutting patterns available. Your profile relates to the pattern shown in the second quadrant of the picture. and as can be seen, the U is minus and the W plus.

THANKS!! To you guys We got it figured out!! BTW we have to keep putting to the machine back to uo wo before we
start by handle is there a faster way to MDI back to that position we tryed to do it but it wont go there??

What did you find to be the problem? It helps others following these Thread to know what the issue and resolve was. Post a copy of your successful program for others to see the solution.

What do you mean by "putting to the machine back to uo wo". Are you referring to the Reference Return Position in X and Z? If so, either via MDI or included in your program, the following command can be executed:

G28 U0.0 W0.0

Regards,

Bill

[deanmachine]

Bill,
We were trying to run your program but had wrong value in the u thats what we did wrong and that was the confusion.
As soon as we put it back to u0 just as you guys tried to explain to us problem solved THANK YOU!! As for the u0 w0 it always goes back in a program
no problem, but if I move it around off u0 w0 and want to put back fast without handle and try to MDI to u0w0 wont work. So do I use gode G28 u0 w0 ?
Thats the only thing I havent tried G0 u0 w0 dosent work. Thanks again for helping a couple of dummies this is the example program we ran .
M41
G50 X11. Z5.
G97 S650 M3 T1010
G00 X-.015 Z.01
G72 P10 Q20 U.000 W.003 F.01 D500
N10 G01 Z-.4124
G01 X.0313
G02 X6.5371 Z-.2799 R39.9844
X8.371 Z-.0949 R3.9844
X8.3981 Z-.0866 R.0344
X8.4466 Z-.0369 R.0844
N20 G01 Z0.01
G70 P10 Q20 F.008
G40 G0 X11. Z5. T1000
M30

dmachine

[angelw]

Bill,
We were trying to run your program but had wrong value in the u thats what we did wrong and that was the confusion.
As soon as we put it back to u0 just as you guys tried to explain to us problem solved THANK YOU!! As for the u0 w0 it always goes back in a program
no problem, but if I move it around off u0 w0 and want to put back fast without handle and try to MDI to u0w0 wont work. So do I use gode G28 u0 w0 ?
Thats the only thing I havent tried G0 u0 w0 dosent work. Thanks again for helping a couple of dummies this is the example program we ran .
M41
G50 X11. Z5.
G97 S650 M3 T1010
G00 X-.015 Z.01
G72 P10 Q20 U.000 W.003 F.01 D500
N10 G01 Z-.4124
G01 X.0313
G02 X6.5371 Z-.2799 R39.9844
X8.371 Z-.0949 R3.9844
X8.3981 Z-.0866 R.0344
X8.4466 Z-.0369 R.0844
N20 G01 Z0.01
G70 P10 Q20 F.008
G40 G0 X11. Z5. T1000
M30

dmachine

The U and W addresses are the Incremental equivalents of the Absolute, respective X and Z addresses. Accordingly, by commanding G00 U0 W0, or G01 U0 W0, the X, Z slides move Zero Distance from the current location.

G28 is a programmable Reference Return command through an intermediate position. Lets say that the current location of the tool is X2.0 Z0.5. If you were to execute the following command:

G28 X6.0 Z1.0,

the Tool would go to X6.0 Z1.0 first and then directly to the Reference Return position. G28 is a two part command, and if you execute the G28 command in single block you can see this, as the axis slides will go to the Intermediate Position at the press of the Cycle Start button, and a second press of the button is required for the G28 command to complete.

G28 can also be used with Incremental addresses U and W. If the following command were to be executed:

G28 U0.0 W2.0

the axes slides would move Zero distance in X and plus 2.0 in Z, before moving directly to the X,Z Reference Return position. Therefore, if you want the axes slides to go directly home from the current position, execute G28 U0.0 W0.0 and the slides will go to the machine's Reference Return position, through the Intermediate point Zero distance away from their current location. G00 does not have to be programmed with G28; G28 executes in rapid traverse speed.

G28 is not a Modal command. If you wanted the X slide to move to the Reference Return position in X first, say to avoid hitting the Tail Stock, then the following could be executed:
G28 U0.0
G28 W0.0

Note that G28 has to be included in both blocks.

Regards,

Bill

[fordav11]

the correct way to machine that profile is by feeding in the X minus direction when facing. if you feed the other way you are plunging into the material at X0 which is not good for longevity of the insert.

you should always start and finish at the zero return position. each tool does not need to go back home but certainly the start and end should. that is done as a safety measure to ensure that if the slide is moved manually the machine automatically goes home before applying the first G50.

another way to avoid going home each time is to use a G30. A simple parameter change can enable it and another two set the X and Z 2nd Reference Return position.

[deanmachine]

Bill,

The way we set up our lathe is as follows:
turn on and home out machine
set orgin uo wo
move u-1. w-10. by hand
reset orgin u0 w0
this is where we tool change and start stop program from so
stays away from tailstock and less travel to part all works well
will run all day
However while we are setting up and proving out program and moving
it around what is the command to bring it back to this spot we
picked and set orgin u0 w0 to? Can this be done or are we setting this
up wrong? better way? g28 just sends it to ref return 0 0 (that we call machine home)
Thanks,
DMACHINE

[fordav11]

as you say, you're setting it wrong. it's really not as complicated as all of the chatter above would suggest.

G28 U0 W0
G0 U-1.0 W-10.0
M41
G50 X11.0 Z5.0 S1000
G0 T1010 M8
G96 S350 M3
....
.....
.....
.....
G0 X11. Z5. M9
T1000 M5
M1
G28 U0 W0
M30

[angelw]

Bill,

The way we set up our lathe is as follows:
turn on and home out machine
set orgin uo wo
move u-1. w-10. by hand
reset orgin u0 w0
this is where we tool change and start stop program from so
stays away from tailstock and less travel to part all works well
will run all day
However while we are setting up and proving out program and moving
it around what is the command to bring it back to this spot we
picked and set orgin u0 w0 to? Can this be done or are we setting this
up wrong? better way? g28 just sends it to ref return 0 0 (that we call machine home)
Thanks,
DMACHINE

Either via MDI, or included in the program under block delete, you execute the following:

G28 U0.0 Y0.0
G00 U-1.0 W-10.0

As suggested by ford11, 2nd reference Return Option, G30 can also be used,

Regards,

Bill

[deanmachine]

Ok thanks
BTW In ref to our last few threads
We have our part programmed to cut inside to out now
and we can step it in fine with d but we have to drill a small hole
on center so not to chip the insert this works fine. When we program
it out to inside it wont step we have even tried moving our z0 to bottom of bore
and no luck there as well. From what your previous thread explains we should
be able to do it this way?? I am confused this is an example do you see the issue
or is this somthing a 6t control will not do?? It would be great to cut out a tool
change and run outside to inside if possible if not other way works fine also
just alittle bit longer and more setup.
Thanks,
DMACHINE

M41
G50 X11. Z5
G97 S500 M3 T1010
G0 X8.4466 Z.01
G72 P10 Q20 U0 W.003 F.05 D500
N10 G1 Z-.0369
G3 X8.3981 Z-.0866 R.0844
X8.371 Z-.0949 R.0344
X6.5371 Z-.2799 R3.9844
X.0313 Z-.4124 R39.9844
G1 X-.015
N10 G1 Z0
G70 P10 Q20 F.05
GO X11. Z5. T1000
M30

[angelw]

Ok thanks
BTW In ref to our last few threads
We have our part programmed to cut inside to out now
and we can step it in fine with d but we have to drill a small hole
on center so not to chip the insert this works fine. When we program
it out to inside it wont step we have even tried moving our z0 to bottom of bore
and no luck there as well. From what your previous thread explains we should
be able to do it this way?? I am confused this is an example do you see the issue
or is this somthing a 6t control will not do?? It would be great to cut out a tool
change and run outside to inside if possible if not other way works fine also
just alittle bit longer and more setup.
Thanks,
DMACHINE

M41
G50 X11. Z5
G97 S500 M3 T1010
G0 X8.4466 Z.01
G72 P10 Q20 U0 W.003 F.05 D500
N10 G1 Z-.0369
G3 X8.3981 Z-.0866 R.0844
X8.371 Z-.0949 R.0344
X6.5371 Z-.2799 R3.9844
X.0313 Z-.4124 R39.9844
G1 X-.015
N10 G1 Z0
G70 P10 Q20 F.05
GO X11. Z5. T1000
M30

It has nothing to do with it being a Series 6T control, but that you're using the G72 cycle. If you refer to Post #2 all is explained there. I stated there that the example program I listed would work in theory but would be impractical. The four cutting patterns shown in Post #2 are what are available with the G72 cycle, and show the Profile Description direction that has to be obeyed from A to B through A' in that order. Your part profile relates to pattern 2 shown in the 2nd quadrant of the picture. The G72 cycle is normally used in conjunction with a bore, when cutting patterns 1 and 2 in Post #2 are considered, allowing for the cutting action being from inside to out.

In that example program of Post #2, it shows the tool starting at X-0.015. In that case, part of the insert is on the negative side of X0.0 and accordingly, the workpiece material going in the wrong direction for that portion of the insert to cut. Further, using a set spindle speed of 500RPM, the surface speed at 0.15 diameter would only be in the order of 1.9635 f/min and Zero at the absolute centre, creating even more adverse cutting conditions for the insert.

When a turning operation is being executed, and particularly where there is a significant variation in the profile diameters, such as in your example, Constant Surface Speed Mode G96 should be used. The maximum Spindle RPM can be clamped by specifying the max revs with G50 as shown in the following example:
G50 S2500
The above code will limit the RPM to 2500 when the tool approaches X0.0.

If you wanted to continue using G72, you could do as suggested in #2, rough form a flat bottom bore to just short of full depth, so that the tool is not starting so close to X0.0, and then after the G72 has finished roughing from the rough bore to the outside, semi finish the section of rough bore from Outside toward Centre.

Regards,

Bill

[fordav11]

You said you have MasterCAM so why don't you just use the long hand G-Code generated by MasterCAM? Even with each cut separate your curved profile will fit in the modest memory that a 6T has. Then you can machine it any way you want without having the restrictions that a fixed cycle imposes. That would be the easiest way and you can machine it from large diameter to center taking the depth of cut you want to take and using a PDPNN tool with DNMG insert set at 90 degrees to the face.
Using fixed cycles is not always the best way to do something....

[vnn34d]

I Mycompany use fanuc 6m but a few day these error, can you share me fanuc 5,6m maintance

Thanks

My email: [email protected]