Circle Contour Not Initiating

[TS656577]

Hey everyone! I'm a senior mechanical engineering student. I am trying to get a circle contour for the part in the picture attached. We have a Haas TM2 and I have used the macros to do the bolt pattern and the 2 pockets. The TM2 (at least ours) doesn't have an easy macro for circles. I don't want it to go all of the way through the part, just most of the way (i.e, it's 0.25" thick and I want the circle contour to go 0.24" for instance). I have tried to hand write g-code and have attached the program that I have been working with. It has the bolt pattern and pockets in there which I have tested using wood. The 4th section is my issue. It gets to the line after the N100 line and goes down the -0.08" and does not move. It just stays in that spot (i.e, doesn't make a circle). Can anyone help me? If anyone is curious, this is for our senior design project for FSAE. Thanks in advance for help!

%
O33333

(CIRCLE BOLT PATTERN)

(DRILL)
T1 M06
G00 G90 G54 X0. Y0.
S1070 M03
G43 H01 Z0.2
G83 G98 Z-0.7 F3.5663 Q0.05 L0
G70 I1.315 J30. L6
G00 G80 Z0.2 M09
M05
G28 G91 Z0
G00 G90 G54 X0 Y0
M01



(COUNTER-CLOCKWISE CIRCULAR POCKET)

(END MILL)
T3 M06
G00 G90 G54 X0. Y0.
S267 M03
G43 H03 Z0.2
G01 Z0. F1.335
N100 G13 G91 G01 Z-0.0406 I0.35 K1.125 Q0.2 F1.335 L2 D03
G00 G90 Z0.2 M09
G28 G91 Z0 M05
G00 G90 G54 X0 Y0
M01



(COUNTER-CLOCKWISE CIRCULAR POCKET)

(END MILL)
T3 M06
G00 G90 G54 X0. Y0.
S267 M03
G43 H03 Z0.2
G01 Z0. F1.335
N100 G13 G91 G01 Z-0.13 I0.35 K1. Q0.2 F1.335 L2 D03
G00 G90 Z0.2 M09
G28 G91 Z0 M05
G00 G90 G54 X0 Y0
M01


(COUNTER-CLOCKWISE CIRCLE CONTOUR)

(END MILL)
G20 T3 M06
G00 G90 G54 X0 Y0
S267 M03
G43 H03 Z0.2
G00 X-1.875 Y0
G01 Z-0.08 F1.335
N100 G17 G90 F5
G03 X-1.875 Y0 I1.875 J0 Z-0.08
G00 X-1.875 Y0
G01 Z-0.16 F5
G17 F5
G03 X-1.875 Y0 I1.875 J0 Z-0.16
G00 X-1.875 Y0
G01 Z-0.24 F5
G17 F5
G03 X-1.875 Y0 I1.875 J0 Z-0.24
G00 Z0.2 M05
G00 G90 G54 X0 Y0
M01
%

[angelw]

The 4th section is my issue. It gets to the line after the N100 line and goes down the -0.08" and does not move. It just stays in that spot (i.e, doesn't make a circle). Can anyone help me? If anyone is curious, this is for our senior design project for FSAE. Thanks in advance for help!

(COUNTER-CLOCKWISE CIRCLE CONTOUR)

(END MILL)
G20 T3 M06
G00 G90 G54 X0 Y0
S267 M03
G43 H03 Z0.2
G00 X-1.875 Y0
G01 Z-0.08 F1.335
N100 G17 G90 F5
G03 X-1.875 Y0 I1.875 J0 Z-0.08
G00 X-1.875 Y0
G01 Z-0.16 F5
G17 F5
G03 X-1.875 Y0 I1.875 J0 Z-0.16
G00 X-1.875 Y0
G01 Z-0.24 F5
G17 F5
G03 X-1.875 Y0 I1.875 J0 Z-0.24
G00 Z0.2 M05
G00 G90 G54 X0 Y0
M01
%

1. Your program uses Absolute Mode G90 (shown in Blue)
2. The Tool is positioned at Absolute Z-0.08 in the the 1st G01 block
3. You have programmed the tool to go to the same Absolute Z-0.08 in the block following the N100 block.

I'm a little surprised that a circular move was not made without a Z Move (Z already satisfied before the Helical block is launched). I'm assuming programming a Z coordinate in the Helical Interpolation block, that is the same as the current block, to be your problem, as the remainder of the block is correct.

Its not good practice to be Rapid Traversing in X Y at what would be the end of a Z move into the Workpiece, without lifting off the final Z point. In the case of your program there would not have been an issue, as had the Helical Move completed as it should have, the tool would have finished at the same X,Y coordinates as those specified in G00 X-1.875 Y0. Accordingly, this block is superfluous in your program.

Regards,

Bill

[fordav11]

remove the Z on the G03 lines

i.e.
G03 X-1.875 Y0 I1.875 J0

The non-movement is probably V-E-R-Y S-L-O-W feedrate.
Change F5 (without a decimal this means F0.0005 ) to something larger with a decimal point like F5.0 or delete it entirely and it'll use F1.335 from the line above.