Turn Milling on Integrex e-670H ii

Hopefully someone can help me out.

I have a regular job that involves removing a large amount of Inconel 625 Cladding on an OD which also has a large intermittent cut going over a cross hole.

Up till now we have been using forward approach CNMG`s to get through this which is costly in both time and inserts.

I spoke with my Sandvik Rep and he recommended changing our process to turn milling using a ceramic button tipped facemill, He showed me a video of a recent trial that he had done elsewhere on what was basically the same job and it was most impressive and a huge reduction in time (will save hrs potentially).

I have tooling and inserts now in place for the trial though unfortunately the Mazatrol Turn Milling cycle will not work as is recommended (It will not feed in on Y axis) and based on other reports from various forums I believe the only way round this is to write a manual program. This is where I am now lost in a sea of G codes ( I am fine with regular 3/4 axis programming but not had to do much with the integrex`s lock/unlock spindles etc)

Please can someone point me in the right direction with regards to a program for this.

What I want to do is

1) Move Milling tool into position (off in Y)
2) Feed into cut (lathe spindle stationary, milling spindle rotating)
3) Mill along dia (both lathe and milling spindle rotating)
4) stop lathe spindle and retract tool.

Any help/pointers will be greatly appreciated.

Best regards

Harry

This is the how you start the g-code program on the E670 with the detail explain of the code. Just input the turn mill program after appro move


N3 (milling)
g64 (cutting mode)
m200 (milling mode, c-axis connect)
g90 g20 g40 g80 g17 g95 (abs, inch, cutter comp cancel, canned cycle cancel, x/y plane, feed per rev.)
t15.1 t5 m6 (tool 15.1=15a, next tool=5, tool change)
g53g91g0x0. (dummy move for g30p3 command)
g91g30p3x0. (referance position for b-axis index reading x value in parameters m6, m7, and su10)
g97s800m3 (mill spindle cw @ 800rpm)
m108 (b-axis unclamp)
g53 g90 g0 b90. (position b-axis 90. Deg. With respect to machine coordinate system g53)
m107 (b-axis unclamp)
g10.9 x0 (radial input)
g90g54g0c0. (position to c-axis 0.)
g68x[23.3/2]y0z0i0j1k0r90. (coordinate rotation around Y now it like mill machine)
g0x-1.0y0. (approach move)
g0g43z.1 (approach move)
g1z-.1f.015 (feed @ .015ipr)
g95g1x1.0f.009 (feed @.009ipr)
g91g0z.1 (escape move)
g69 (corrdinate rotation cancel)
g10.9x0 (radial input)
g53g91g0x0. (dummy move for g30p3 command)
g91g30p3x0 (referance position for b-axis index reading x value in parameters m6, m7, and su10)
m5 (mill spindle stop)

And this the turn mill macro I wrote for the mill turn

G00 G40 G90 G80 G20 G17 G95
T02 M06
G91 G28 Z0.
G00 G90 G54 X-1.44 Y-1.24 A0.
S500 M03
G43 H2 Z3.0 M08
G01 Z.010
#100 = 1 ( set valve 100 = to 1)
WHILE [#100 LT 46] DO1 ( add untill it move 45 time)
G91 G01 X.2 A360. F.015 ( every revolution is .2 in X )
#100 = #100 + 1
END1
G91 G28 Z0.
M9
M05
M30

Perfect, Thank you. Will be running it this month and will update you on how I get on.