tuning and live tooling

[fjd]

This is new for me needing to cut 2 slots 180 apart with 1/4 inch ball end mill shaft OD 4.753 diam at the finish slot depth 4.41 .
this is being done on a fanuc control. I am curius what the code should look like.

[Jayhawk]

On our Mori's I would do something like this.

N5 G0 T0505
M45 (ACTIVATE C AXIS)
G0 C0
G98 X4.853 Z0.225
G1 X4.41 F50.
Z-1. F5.
G0 X4.853
Z0.225
C180.
G1X4.41 F50.
Z-1. F5.
G0 X4.853
M5
M46
G99
G28 U0 W0
M1

[fjd]

Jayhawk

the way i read the code you are cutting the slot from the end
of shaft back Z-1.
If thats correct I am wanting to cut across the shaft.
if that makes sence.

[Jayhawk]

I wondered about that after I had posted. If you have Y axis you can do it like this.

N5 G0 T0505
M45 (ACTIVATE C AXIS)
G0 C0
G98 X4.853 Z-1.
Y-1.
G1 X4.41 F50.
Y1. F5.
G0 X4.853
C180. Y-1.
G1X4.41 F50.
Y1. F5.
G0 X4.853
Y0
M5
M46
G99
G28 U0 W0
M1

[fjd]

the guy that owns this machine says that he should be able to
feed in and out in X with while spindle rotates some amount.
I dont thinks it has Y.

Thanks

[Murf]

The best way to visualize the math involved is this:
Draw a circle 4.753" in diameter and draw the flat 2.205 above centerline of the circle. Extend the line representing the flat beyond the circle. Next draw a circle .25" in diameter tangent to the 4.753" circle and the "flat line". Now draw a .25" circle on the flat vertically from the centerline of the part. Now draw a .25" in between the two .25" circles. Now you have a drawing of your cutter path half way through the part. Draw a line vertically from the centerline of the part to the center of the cutter, label it "a". Next draw a line horizontally from the center of that cutter to the one that is tangent to the bar and the flat, label it "b". Now draw a diagonal line from that cutter back to center line of the 4.753" circle and label it "c". Now a=2.205+.125, c=2.3765+.125. Your start point will be angle"B" (The angle formed by the intersection of a and b.) B=ATAN(b/a) b=SQRT(c^2-a^2) . Now dive length b by the distance you want to travel in each move. The more moves you make the flatter your flat will be. You can adjust your C-axis starting point so it will relate to othe features on the part, then program the "B" angles as "H" (incremental moves). The program should look like this. (Programming from the center of the cutter)


X5.0030 C68.661 F393.33 (initial position)
G98G1X4.9770 H0.781 F393.33
X4.9519 H0.789 F397.39
X4.9277 H0.797 F401.36
X4.9045 H0.805 F405.24
X4.8823 H0.812 F409.01
X4.8611 H0.819 F412.66
X4.8408 H0.826 F416.2
X4.8216 H0.833 F419.6
X4.8035 H0.84 F422.87
X4.7863 H0.846 F425.99
X4.7702 H0.852 F428.96
X4.7552 H0.857 F431.77
X4.7412 H0.862 F434.41
X4.7283 H0.867 F436.87
X4.7166 H0.872 F439.16
X4.7059 H0.876 F441.26
X4.6963 H0.88 F443.16
X4.6878 H0.883 F444.87
X4.6804 H0.886 F446.37
X4.6742 H0.889 F447.67
X4.6691 H0.891 F448.76
X4.6651 H0.893 F449.63
X4.6623 H0.894 F450.29
X4.6606 H0.895 F450.73
X4.6600 H0.895 F450.95
X4.6606 H0.895 F450.95
X4.6623 H0.895 F450.73
X4.6651 H0.894 F450.29
X4.6691 H0.893 F449.63
X4.6742 H0.891 F448.76
X4.6804 H0.889 F447.67
X4.6878 H0.886 F446.37
X4.6963 H0.883 F444.87
X4.7059 H0.88 F443.16
X4.7166 H0.876 F441.26
X4.7283 H0.872 F439.16
X4.7412 H0.867 F436.87
X4.7552 H0.862 F434.41
X4.7702 H0.857 F431.77
X4.7863 H0.852 F428.96
X4.8035 H0.846 F425.99
X4.8216 H0.84 F422.87
X4.8408 H0.833 F419.6
X4.8611 H0.826 F416.2
X4.8823 H0.819 F412.66
X4.9045 H0.812 F409.01
X4.9277 H0.805 F405.24
X4.9519 H0.797 F401.36
X4.9770 H0.789 F397.39
X5.0030 H0.781 F393.33

Feed rates must be converted to degrees per minute! Feed rate is based on 18.34 IPM. Index 180 degrees from your start point and repeat.

Good luck,
Dan

[fjd]

Thanks Murf

Thats what i was thinking it would look somthing like.
Now all i got to do is figure out how to get Gibbscam to do whats needed then find the correct post for it thanks again.

fjd

[Murf]

fjd,
I have an excel spreadsheet I'm working on to generate the code. It's a little rough at the moment but it seem to work. I also have one for calculating tangency points and right angle trig. I'm new here so I'm wondering if it's possible to post an XLT or XLS file here?

Dan

[M@T]

Originally posted by Jayhawk On our Mori's I would do something like this. N5 G0 T0505 M45 (ACTIVATE C AXIS) G0 C0 G98 X4.853 Z0.225 G1 X4.41 F50. Z-1. F5. G0 X4.853 Z0.225 C180. G1X4.41 F50. Z-1. F5. G0 X4.853 M5 M46 G99 G28 U0 W0 M1

Imperial Programming using G98 Feed Per Minute

Everything is Metric using G99 Feed Per Rev over here in England. I'd go insane trying to program like you lot.

Mind you, i'm working with a guy now and his last place programmed everything in Incremental and they refused to use canned/stock removal cycles so everything had to be roughed out long-hand. No way could I work like that

And count yourself lucky you get to use Mori Seiki's, they are good solid machines. Unlike the pile of junk Yam machines i'm on at the moment

[rr1021ab]

How do i mill a hex on a puma 240 lathe using a half inch end mill siz of hex is 2.4mm i dont have mastercam i need the code using c,x and z

[CNCRim]

Originally Posted by rr1021ab How do i mill a hex on a puma 240 lathe using a half inch end mill siz of hex is 2.4mm i dont have mastercam i need the code using c,x and z

Not tried to be rude/ anything but the post is back 2003, it's 7 years old. since you already check ...... the post way back. check some of the post last year. There was one program match your spec. I think the title was something "hex with live tool"