[drdroopy]

Hello my shop just recently got an ingersoll with a fanuc oi-tc controller, this machine has a C axis and its something i have never used, what im trying to do is mill a large hex using the C axis, below is a post of what i have, but the C-Axis dosnt look like i believe it should, take a look and tell me what you think. Now when i try to run the machine tries to take off way further then allowed

O0009(POLAR MILL)
G54G97G99G0G40G18
G13.1
G98(IPM)
T0606
M50
G28H0.
S1000M23
G0X5.0Z.1C-114.018
G12.1(POLAR MILL)
G1G41X5.25C-114.018F10.
M54
Z.1
G98 G1 Z-.3775 F6.41
X2.5992 C-116.1 F10.68
X2.572 C-116.726 F12.27
X2.5498 C-117.45 F14.20
X2.5335 C-118.253 F15.77
X2.5234 C-119.112 F16.86
X2.52 C-120. F17.42
X2.5242 C-123.295
X2.5366 C-126.57
X2.5574 C-129.811
X2.5863 C-133.001 F16.81
X2.6232 C-136.127 F16.39
X2.668 C-139.177 F15.88
X2.7169 C-141.95 F15.34
X2.772 C-144.618 F14.76
X2.7944 C-145.774
X2.8115 C-146.959 F15.1
X2.8229 C-148.166
X2.8286 C-149.387 F15.54
C-150.611
X2.8229 C-151.831
X2.8114 C-153.039
X2.7944 C-154.224 F15.10
X2.772 C-155.382 F14.72
X2.7123 C-158.295
X2.6605 C-161.299 F15.41
X2.6166 C-164.386 F15.97
X2.5808 C-167.543 F16.46
X2.5531 C-170.759 F16.87
X2.5338 C-174.018 F17.19
X2.5228 C-177.305
X2.5201 C-180.603 F17.49
X2.5258 C-183.895
X2.5398 C-187.166
X2.5621 C-190.398 F17.08
X2.5924 C-193.577 F16.74
X2.6308 C-196.69 F16.30
X2.6771 C-199.725 F15.78
X2.722 C-202.214 F15.25
X2.772 C-204.618 F14.73
X2.7945 C-205.775
X2.8116 C-206.961 F15.10
X2.823 C-208.168
X2.8287 C-209.389 F15.54
C-210.613
X2.823 C-211.834
X2.8116 C-213.041
X2.7945 C-214.227 F15.10
X2.772 C-215.382 F14.70
X2.7123 C-218.295
X2.6605 C-221.299 F15.41
X2.6166 C-224.386 F15.97
X2.5808 C-227.543 F16.46
X2.5532 C-230.759 F16.87
X2.5338 C-234.018 F17.19
X2.5228 C-237.305
X2.5202 C-240.603 F17.49
X2.5259 C-243.895
X2.5399 C-247.166
X2.5621 C-250.398 F17.08
X2.5925 C-253.577 F16.7
X2.6309 C-256.69 F16.30
X2.6772 C-259.725 F15.78
X2.7221 C-262.214 F15.25
X2.772 C-264.618 F14.74
X2.7945 C-265.773
X2.8116 C-266.959 F15.10
X2.823 C-268.167
X2.8287 C-269.388 F15.54
C-270.612
X2.823 C-271.833
X2.8116 C-273.041
X2.7945 C-274.227 F15.10
X2.772 C-275.382 F14.70
X2.7123 C-278.295
X2.6604 C-281.299 F15.41
X2.6165 C-284.386 F15.97
X2.5807 C-287.543 F16.46
X2.5531 C-290.759 F16.87
X2.5338 C-294.018 F17.19
X2.5228 C-297.305
X2.5201 C-300.603 F17.5
X2.5258 C-303.895
X2.5398 C-307.166
X2.562 C-310.398 F17.1
X2.5924 C-313.577 F16.74
X2.6308 C-316.69 F16.30
X2.677 C-319.725 F15.78
X2.722 C-322.215 F15.25
X2.772 C-324.618 F14.73
X2.7944 C-325.774
X2.8115 C-326.959 F15.1
X2.8229 C-328.166
X2.8286 C-329.387 F15.54
C-330.611
X2.8229 C-331.831
X2.8114 C-333.039
X2.7944 C-334.224 F15.10
X2.772 C-335.382 F14.72
X2.7123 C-338.295
X2.6605 C-341.299 F15.41
X2.6166 C-344.386 F15.97
X2.5808 C-347.543 F16.46
X2.5531 C-350.759 F16.87
X2.5338 C-354.018 F17.19
X2.5228 C-357.305
X2.5201 C-360.603 F17.49
X2.5258 C-363.895
X2.5398 C-367.166
X2.5621 C-370.398 F17.08
X2.5924 C-373.577 F16.74
X2.6308 C-376.69 F16.30
X2.6771 C-379.725 F15.78
X2.722 C-382.214 F15.25
X2.772 C-384.618 F14.73
X2.7945 C-385.775
X2.8116 C-386.961 F15.10
X2.823 C-388.168
X2.8287 C-389.389 F15.54
C-390.613
X2.823 C-391.834
X2.8116 C-393.041
X2.7945 C-394.227 F15.10
X2.772 C-395.382 F14.70
X2.7123 C-398.295
X2.6605 C-401.299 F15.41
X2.6166 C-404.386 F15.97
X2.5808 C-407.543 F16.46
X2.5532 C-410.759 F16.87
X2.5338 C-414.018 F17.19
X2.5228 C-417.305
X2.5202 C-420.603 F17.49
X2.5259 C-423.895
X2.5399 C-427.166
X2.5621 C-430.398 F17.08
X2.5925 C-433.577 F16.7
X2.6309 C-436.69 F16.30
X2.6772 C-439.725 F15.78
X2.7221 C-442.214 F15.25
X2.772 C-444.618 F14.74
X2.7945 C-445.773
X2.8116 C-446.959 F15.10
X2.823 C-448.167
X2.8287 C-449.388 F15.54
G13.1
M55
G0U5.W3.
M25
M51
G99
M01
M30

[ALEXCOMO]

Where is the code for activate the milling function?
Is g13.1?
I can send you a example tommorow.

[drdroopy]

not sure what the 13.1 is or what turns on the milling, but the endmill does turn on


EDIT: the 13.1 is to end milling cycle, 12.1 to start

[fordav11]

G12.1 is Polar Coordinate Interpolation and can be used when a lathe has live tooling but does not have a Y axis.
It has limited uses and the accuracy of the machined profile is questionable and even noted by Fanuc.
Programming using G12.1 can get quite complicated.
If you want to know more read the Polar Coordinate Interpolation section of any Fanuc Lathe manual.
See simple example below....

[ALEXCOMO]

Ok , I think the program is not in polar coordinates....
when g12.1 is used is like to program a milling machine whit x axes programmed double(because is a lathe) and C sobstitute Y.

[fordav11]

it looks like the post has done all the complicated work so polar coordinates are not needed. try removing G12.1 and G13.1
not sure though because C should be between -360 and +360 (for degrees) and your program has C values up to -449?
exactly how big is your hex?

are you sure the program is correct or the method used to create it is correct? generally an auto-generated program like that should work if the post is configured correctly.

[angelw]

G12.1 is Polar Coordinate Interpolation and can be used when a lathe has live tooling but does not have a Y axis.
It has limited uses and the accuracy of the machined profile is questionable and even noted by Fanuc.
Programming using G12.1 can get quite complicated.
If you want to know more read the Polar Coordinate Interpolation section of any Fanuc Lathe manual.
See simple example below....

Either Polar Interpolation, or X coordinate and C angular moves would be used with a part such as the one shown in your attached picture irrespective of whether the lathe had a Y axis or not. To machine such a profile using X and Y would require the tool to cross over the center line of the machine into -X. There is seldom much travel past center line for a live tool mounted parallel to the Z axis.

The only limitation I know of with Polar Interpolation is that the C axis feed rate may exceed the maximum feed rate set in parameters for the C axis, if the tool gets close to the center line in X. This is because the C axis component of the X C feed becomes greater as the tool approaches the center. In this case an alarm is raised. I have clients that routinely use Polar Interpolation on relatively complex profiles that have to be true to form, with no more difficulty than if the part were machined on a VMC. Could you post the comments made by Fanuc on the subject, or the Fanuc manual they appear in.

Stevo might like to chime in and give his take on Polar Interpolation he used on a recent project.

drdroopy
As ALEXCOMO stated, the coordinates in your program indicates that Polar Interpolation is not being used. The C moves are clearly angular moves and Polar Interpolation is programmed using Cartesian coordinates.

In your program you've executed a Reference Return in C and then moved to Absolute C-114.018. Unless you have a reason to start at that angle, its a strange place to start. The fact that you have C angles less than -360.000 is doable. If for example you needed the 4th axis to complete two rotations, you can program C720.000 from C0.0 to achieve that.

Personally, if your control has Polar Interpolation, not all do as it is an option, I would use that feature for sure. You could replace the relatively long program you have now, with not much more than a dozen blocks, and that would include small debur rads on the points of the Hex. You would create the tool path in the same way you would for a three axis machining center with C being output as the second virtual axis. If your control didn't raise an illegal G code alarm when it read the G12.1 in your program, then your control will have the option.


Regards,

Bill

[drdroopy]

well after messing around quite a bit i managed to get it to cut the hex, i did have to remove the 12.1 and 13.1, also forgot to mention this machine does not have a Y axis, as for the C values, they are angular and the reason it started at 114 is because of the start position i chose in mastercam but the values keep growing in C axis well past 360 the program i have ends at around 1200 but it does work.

Our machine does have Polar Interpolation but mastercam outputs in Cartesian

heres a sample of what i had to do, this is only half the program as its rather large


G0 T0404
G18
S1200 M23
G0 G54 X2.9937 Z.25C111.168
G1G41X2.9937 Z.25C111.168F20.
M8
G97
Z.1
M54
G98 G1 Z-.3775 F6.41
X2.8683 C113.022 F235.83
X2.7486 C115. F256.86
X2.6583 C116.655 F277.14
X2.5703 C118.424 F296.2
X2.5575 C118.755 F338.46
X2.5479 C119.139 F392.1
X2.542 C119.56 F429.42
X2.54 C120. F448.54
X2.5442 C123.281
X2.5566 C126.543
X2.5774 C129.77
X2.6062 C132.947 F433.47
X2.6431 C136.061 F422.68
X2.6879 C139.1 F409.82
X2.7361 C141.825 F395.87
X2.7901 C144.447 F381.31
X2.8113 C145.518
X2.8279 C146.616
X2.8398 C147.733 F395.27
X2.847 C148.863
X2.8494 C149.999
X2.847 C151.134
X2.8398 C152.264
X2.8279 C153.381
X2.8113 C154.479
X2.7901 C155.553 F379.51
X2.7307 C158.459
X2.6791 C161.455 F397.97
X2.6355 C164.532 F412.37
X2.5999 C167.679 F424.95
X2.5725 C170.883 F435.36
X2.5534 C174.13
X2.5426 C177.403 F448.5
X2.5402 C180.687
X2.5461 C183.965
X2.5603 C187.221
X2.5827 C190.439
X2.6133 C193.604 F431.39
X2.6519 C196.703 F420.14
X2.6983 C199.725 F406.89
X2.7419 C202.126 F393.48
X2.7901 C204.447 F380.53
X2.8114 C205.521
X2.8279 C206.619
X2.8399 C207.736 F395.26
X2.847 C208.866
X2.8495 C210.001
X2.8471 C211.137
X2.8399 C212.267
X2.828 C213.384
X2.8114 C214.482
X2.7901 C215.553 F379.17
X2.7307 C218.459
X2.6791 C221.455 F397.97
X2.6354 C224.532 F412.37
X2.5999 C227.679 F424.95
X2.5725 C230.883 F435.36
X2.5534 C234.13
X2.5426 C237.403 F448.51
X2.5401 C240.687
X2.546 C243.965
X2.5603 C247.221
X2.5827 C250.439
X2.6133 C253.604 F431.41
X2.6518 C256.704 F420.15
X2.6983 C259.726 F406.9
X2.7418 C262.125 F393.5
X2.7901 C264.447 F380.42
X2.8113 C265.519
X2.8278 C266.617
X2.8398 C267.734 F395.27
X2.847 C268.864
X2.8494 C270.
X2.847 C271.136
X2.8398 C272.266
X2.8278 C273.383
X2.8113 C274.481
X2.7901 C275.553 F379.53
X2.7307 C278.459
X2.6791 C281.455 F397.98
X2.6355 C284.532 F412.37
X2.5999 C287.68 F424.95
X2.5725 C290.883 F435.35
X2.5534 C294.13
X2.5427 C297.403 F448.5
X2.5402 C300.687
X2.5461 C303.965
X2.5604 C307.221
X2.5828 C310.439
X2.6134 C313.604 F431.38
X2.652 C316.703 F420.12
X2.6984 C319.725 F406.87
X2.742 C322.124 F393.47
X2.7901 C324.447 F380.63
X2.8113 C325.518
X2.8279 C326.616
X2.8398 C327.733 F395.27
X2.847 C328.863
X2.8494 C329.999
X2.847 C331.134
X2.8398 C332.264
X2.8279 C333.381
X2.8113 C334.479
X2.7901 C335.553 F379.51
X2.7307 C338.459
X2.6791 C341.455 F397.97
X2.6355 C344.532 F412.37
X2.5999 C347.679 F424.95
X2.5725 C350.883 F435.36
X2.5534 C354.13
X2.5426 C357.403 F448.5
X2.5402 C360.687
X2.5461 C363.965
X2.5603 C367.221
X2.5827 C370.439
X2.6133 C373.604 F431.39
X2.6519 C376.703 F420.14
X2.6983 C379.725 F406.89
X2.7419 C382.126 F393.48
X2.7901 C384.447 F380.53
X2.8114 C385.521
X2.8279 C386.619
X2.8399 C387.736 F395.26
X2.847 C388.866
X2.8495 C390.001
X2.8471 C391.137
X2.8399 C392.267
X2.828 C393.384
X2.8114 C394.482
X2.7901 C395.553 F379.17
X2.7307 C398.459
X2.6791 C401.455 F397.97
X2.6354 C404.532 F412.37
X2.5999 C407.679 F424.95
X2.5725 C410.883 F435.36
X2.5534 C414.13
X2.5426 C417.403 F448.51
X2.5401 C420.687
X2.546 C423.965
X2.5603 C427.221
X2.5827 C430.439
X2.6133 C433.604 F431.41
X2.6518 C436.704 F420.15
X2.6983 C439.726 F406.9
X2.7418 C442.125 F393.5
X2.7901 C444.447 F380.42
X2.8113 C445.519
X2.8278 C446.617
X2.8398 C447.734 F395.27
X2.847 C448.864
X2.8494 C450.
X2.847 C451.136
X2.8398 C452.266
X2.8278 C453.383
X2.8113 C454.481
X2.7901 C455.553 F379.53
X2.7307 C458.459
X2.6791 C461.455 F397.99
X2.6355 C464.533 F412.38
X2.5999 C467.68 F424.95
X2.5726 C470.884 F435.35
X2.5535 C474.13
X2.5435 C477.058 F448.32
X2.54 C480.
X2.542 C482.255
X2.5479 C484.502
X2.5515 C484.934
X2.5588 C485.341 F415.84
X2.5696 C485.705 F372.14
X2.5835 C486.015 F314.8
X2.6991 C487.976 F267.23
X2.8201 C489.809 F244.81
X2.9246 C491.241 F225.92
X3.0308 C492.57 F209.76
X3.0004 C489.623 F372.88
X2.9781 C486.637
X2.9641 C483.626 F384.14
X2.9583 C480.601
X2.9608 C477.575
X2.9715 C474.562
X2.9813 C472.858
X2.9937 C471.168
Z-.755 F6.41
X2.8631 C473.103 F236.26
X2.7383 C475.182 F258.3
X2.6533 C476.752 F278.72
X2.5703 C478.424 F296.75
X2.5575 C478.755 F338.46
X2.5479 C479.139 F392.1
X2.542 C479.56 F429.42
X2.54 C480. F448.54
X2.5446 C483.464
X2.5585 C486.905
X2.5816 C490.304
X2.6137 C493.642 F431.53
X2.6547 C496.903 F419.65
X2.7042 C500.073 F405.59
X2.7452 C502.294 F392.14

it keeps going like that till it has completly rotated

thanks for the help guys advice deff saved me some time

[angelw]

Our machine does have Polar Interpolation but mastercam outputs in Cartesian

To create a program using Polar Interpolation you need the output to be in Cartesian Coordinates. Your example program is not Cartesian Coordinate output.

Following is a sample program snippet using Polar Interpolation to machine a 100mm AF hex with 0.5 debur rads on points. The attached picture is a Z view of the tool path with the C axis rotating Counter Clockwise.

Regards,

Bill


T0101
----
----
----
G00 X140.0 C0 Z10.000 Positioning to start position
G01 Z1.000 F2000
G01 Z-10.000
G12.1 Start of polar coordinate interpolation
G41 G01 X140.000 C20.000 F __
G03 X100.000 C0.000 I0.000 J-20.000
G01 X100.000 C-28.579
G02 X99.500 C-29.012 I-0.500 J0.000
G01 X0.500 C-57.591
G02 X-0.500 C-57.591 I-0.250 J0.433
G01 X-99.500 C-29.012
G02 X-100.000 C-28.579 I0.250 J0.433
G01 X-100.000 C28.579
G02 X-99.500 C29.012 I0.500 J0.000
G01 X-0.500 C57.591
G02 X0.500 C57.591 I0.250 J-0.433
G01 X99.500 C29.012
G02 X100.000 C28.579 I-0.250 J-0.433
G01 X100.000 C0.000
G03 X140.000 C-20.000 I20.000 J0.000
G40 G01 X140.000 C0.000
G13.1 Cancellation of polar coordinate interpolation
G00 Z10.000
G00 X __C __
----
----
----
M30
%

[fordav11]

Either Polar Interpolation, or X coordinate and C angular moves would be used with a part such as the one shown in your attached picture irrespective of whether the lathe had a Y axis or not.

If you had Y there would generally be no need to use G12.1 unless the part and tool path required was larger than the total Y axis travel. Especially if it was a multi-axis lathe/mill with almost no limitations like the Mori Seiki NT-series.

It would be a good project to see if a generic macro can be written to machine flats with G12.1 by simply providing the number of flats and the distance from center to the flat. It should be possible. I wouldn't be surprised if it has already been done.

To machine such a profile using X and Y would require the tool to cross over the center line of the machine into -X. There is seldom much travel past center line for a live tool mounted parallel to the Z axis.

It depends on the brand of machine and model. Many models do have travel into X- especially if they have a Y axis. Alternatively C can be rotated first so the machined face is on the X positive side of the part then Y is used after. This is shown below in the attached pic as '1. Side Milling'

Could you post the comments made by Fanuc on the subject, or the Fanuc manual they appear in.

Errors most likely only occur when machining internal profiles. See attached pic.

[angelw]

Errors most likely only occur when machining internal profiles. See attached pic.

With regards to the error shown in the bottom left most picture of the key way being cut, this error is not actually caused by the Polar Coordinate Interpolation function, but is due to a machine not having a Y axis. It will occur in any event when the C axis is rotated with a tool engaged along the X axis, irrespective of whether the program uses Cartesian, or Polar Coordinates. It seems to me that the term Polar Interpolation has been used generally in your attached document. The true reference to Polar Coordinate Interpolation by Fanuc is as follows in an extract from their manual. Note that reference is made to front surface cutting.

Fanuc have a different function called Cylindrical Interpolation (G07.1) for allowing programming of machining on the cylindrical surface of a workpiece and a tool engaged along the X axis, and as if the cylinder was unwrapped. However, even using Cylindrical Interpolation, a Y axis would be required to avoid the error that is shown in your picture.

It would be a good project to see if a generic macro can be written to machine flats with G12.1 by simply providing the number of flats and the distance from center to the flat. It should be possible. I wouldn't be surprised if it has already been done.

I have a Custom Macro program for machining hexagonal components with G12.1, based on the AF, virtually the same as distance from centre (AF/2), and the size of a corner radius. The cycle time to complete one complete circuit of the hex is quicker if a small radius is included, than if the intersection of the flats only are programmed. It would only be a small mod to this Macro to do the calcs for different number of sides. Macro statements and calls to Macro programs are allowed in G12.1

Regards,

Bill


Extract from Fanuc manual
Polar coordinate interpolation is a function that exercises contour control in converting a command programmed in a Cartesian coordinate system to the movement of a linear axis (movement of a tool) and the movement of a rotary axis (rotation of a workpiece). This method is useful in cutting a front surface and grinding a cam shaft on a lathe.

[drdroopy]

Polar Interpolation seems a much better system to use, a lot less clutter in the program. Any of you wouldn't happen to use mastercam and know if there is an option to turn this on?

[angelw]

Polar Interpolation seems a much better system to use, a lot less clutter in the program. Any of you wouldn't happen to use mastercam and know if there is an option to turn this on?

You could modify your post processor to output G12.1 and G13 as well as the profile in Cartesian Coordinates. You can do this yourself if you have a knowledge of writing posts, or you may know someone who can write it for you.

The example program of Polar Coordinate Interpolation I provided earlier, was generated via another CAM package that I wrote a Post Processor that included Polar Interpolation. Its doable with MasterCam.

Regards,

Bill

[Camfather]

before we had a solid mill turn post, we would post to a 3x mill, change Y to C, Double X and I inside of a G121 (polar mode) cycle and that worked ok (pasted the code in the lathe program)

In polar mode, your C should be the same as a Y on a mill.

Hope that helped.

[angelw]

before we had a solid mill turn post, we would post to a 3x mill, change Y to C, Double X and I inside of a G121 (polar mode) cycle and that worked ok (pasted the code in the lathe program)

In polar mode, your C should be the same as a Y on a mill.

Hope that helped.

Yes, that's a work around, but the I is not doubled. I is an incremental value to the centre of a radius whether used in a mill or lathe process.

Regards,

Bill

[Camfather]

Yes, that's a work around, but the I is not doubled. I is an incremental value to the centre of a radius whether used in a mill or lathe process.

Regards,

Bill

yes you are correct, it is late and I am tired.