[Gem1]

i am attempting to machine a groove in a part using an endmill. i want the X and Y to move in a repeating circular motion and have the Z feed down into the part. the kicker is i want the Z to feed at a different feedrate than the circular interpolation movement. fadal support said it cannot be done but it seems to be a fairly straight forward application. any thoughts? thanks.

[Neal]

If you are doing a helical motion then XY & Z appear on the same line. Any feed rate applied will be applied to the complete line. The software can not apply multiple feeds to different axis on the same line.

Neal

[cadman]

If you want constantly changing feedrates you will need to convert the helical path into a splined path. Depending on your post processor, this can be done in the post.

[fpworks]

It can be done (even without cam...keep reading), but you control this with your ramp angle, which will in turn give you a xy component feedrate and z component feedrate from your resultant (input) feed rate.

EXAMPLE
Say you want to use a 3 degree ramp while circular interpolating. Let's say you specify a feed rate of 45 inches per minute(ipm). Your lateral feed rate will be 44.94 ipm and your vertical feed rate will be 2.36 ipm.

45ipm*cos(3 deg) = 44.94 ipm
45ipm*sin(3 deg) = 2.36 ipm

---------------------------------------------------------------

...but all that really doesn't matter. Here is what you really need to know:

PROGRAM
Helical mill a 1.5" diameter hole at the location X=2, Y=5 through 0.75" stock with a 0.5" endmill.

The endmill will trace a 1" diameter circle to create a hole that is 1.5" diameter. The distance it will travel in one lap around the hole is 3.1415" (just taking the perimeter of a 1" diameter circle = pi (3.1415) * diameter)

tan(3 deg) = delta z/3.1415, so
delta z = 3.1415*tan(3 deg)
delta z = 0.1646" (this is the value you want the z axis to feed into the workpiece while making a 360 degree circular interpolation.

Now, write a program:

T2M6
M3 S5000
G54
G90 (absolute mode)
G0 X2. Y5. (location of hole center)
G0 Z0.1 H2 M8
G91 (incremental mode)
G0 X0.5 (offset the radius of your TOOLPATH)
G3 Z-0.1646 I-0.5 F45. L7 (do this 7 times to go feed 1.1522" in z)
G1 X-0.5
...etc, now get the endmill back out of the hole (and go back to absolute mode)


You don't have to figure out the vertical/horizontal feedrate individually, all you need is your ramp angle and a horizontal feedrate.

Good luck,
Justin
(hope I didn't make any mistakes...I did this kind of quick)

P.S. In all reality, I rarely use this since my CAM software can do it faster than I can. (but with a lot more code) I do like the above technique since it is very little code and can be changed very quickly.

[Gem1]

thanks to all who replied. your insight helped a ton.

enjoy the holiday.

[Gem1]

you were a big help. got it running in one setup (i changed the ramp angle to 30 sec). we set a grinding pin in our VMC to grind the groove (eliminated another setup and freed up a machine) and we needed to control the feedrate as to not burn up the pin.

have a great holiday.

[fpworks]

Glad that worked out for you. Take care.

[osomaker]

HI EVERY ONE
IM NEW IN THE COMMUNITY. SO I HOPE ITS THE RIGHT WAY TO POST A QUESTION.
SO..I HAVE BEEN ATTEMPTED TO MILLING AN ARRAY OF CIRCLES, IN THE POCKET MODE AND IN THE CONTOUR MODE, WHIT THE MC8.1 AND WHIT THE MC9, AND THE RESULTS ARE THE SAME MY FADAL VMC40 , MAKES STRANGE FORMS LIKE SQUARES OR ROMBOIDS, INSTEAD THE DESIRED CIRCLES.
ANY ONE CAN HELP ME?
TANKS
[[email protected]]