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
%

[KenFoulks]

You are missing the decimal in your feed rates.

[obiwon]

You are missing the decimal point on your feed of 5(.) in your example, the machine will assume a feed of .005

Sorry got the I & J mixed up in my original post... My memory is not so good from home ):

Try this program
G00 G90 G54 G43 H3 D3 X0 Y0(center of your part.. use tool radius in tool 3 offsets )
S267 F5.
G00 Z0.2
M03
G00X-1.5 Y-1.5
G41(cutter comp left)
G01 X-.975 Y-1.3
G01 Z-0.08 F1.335
F5.
G02 J1.3 I.975
G01 Z-0.16
G02 J1.3 I.975
G01Z-.240
G02 J1.3 I.975
G00 Z0.2
M05
G40
X-1.5
G00 G90 G54 X0 Y0
M01
%

[TS656577]

Hmm thank you for your help! Doesn't G17 need to be initialized somewhere?

[gizmo_454]

G17 is the default when the machine is powered on. It stays on until you call G18 or G19.

Mike

P.S. That pesky decimal gets me every time!

[TS656577]

obiwon, I'm curious as to why the i and j values are what they are since I am trying to cut around the outside (with a diameter of 3.25").

[Matt@RFR]

You also will want to get out of the habit of using the same N# multiple times. If you start writing macros or subroutines, this practice could get you in trouble. It doesn't make sense anyway.

[Machineit]

obiwon, I'm curious as to why the i and j values are what they are since I am trying to cut around the outside (with a diameter of 3.25").

I's and J's are the distance from the starting point of the arc to the center of the arc. So if you are starting on the left or right of an arc, the I could be a positive or a negative number.

If it confuses you try drawing it quickly on paper and it will be easier to visualize. That makes it easier when programing by hand.

Mike

[obiwon]

R x.6=I and neg X start point
R x.8=J and neg Y start point
Programing with no R will cut a full circle and I always use cutter comp as its easier to figure out and you can adjust your finish diameter with your tool radius instead of changing your program...Hope that helps