"Inverse time feedrate" is typically for coordinating combined linear
/rotary motion on milling machines:
http://www.google.com/search?hl=en&q únuc+g93&btnG=Search
--Basically, whenever the control is in this mode your F address represents
the amount of time you desire for the move to be completed within.
It's a modal command so don't forget to change back to G94 mode when it is
desired to go back to using the more usual (inch per minute) convention.

OK, so not being able to do this, and finding out that it runs the 4th
axis in degrees per min, not inches per min.. any idea how I can come up
with a formula to do a tangital arc segment movement, and find the
correct feedrate?
I came across This text, not sure what machine it is for, but looks like
it might work.. But I run into a problem..
<quote>
Feed Rate Calculation for Linear Interpolation with Rotary Axis
Caution concerning the feed rate must be applied when linear interpolation
between the rotary axis and the Z-axis is done. The tangential feed rate
along the
tool path becomes high when the arc length of the rotary axis move is
relatively
short in comparison to the travel distance along the Z-axis. The feed
rate must be
reduced, accordingly. It can be calculated as shown in the example, below.
Example: Machining is done on the OD of a 1.5Â” diameter part, rotating
the Caxis
Angle = 30Â° while moving the Z-axis minus 1Â”, at the same time.
The desired feed rate along the tool path F = 5Â”/minute.
Calculate the feed rate to be used for the interpolation command: G1G98 H60.
W-1.0 F___?
Steps for calculation of the tangential feed rate:
1. Calculate the length of the 30Â° arc segment on the periphery of a 1.5Â”
diameter circle: Arc length=2Rx /360x60=2x0.75x3.14/360x30=0.392Â”
2. Calculate the length of the tool path: L= Square root of
(0.392Â²+1Â²)=1.07Â”
F Â° per minute =F (IPM) x 57.296 / R
F Â° per revolution =F (IPR) x 57.296 / R
10
3. Calculate the time it should take for the 1.07Â” long cut, applying
the feed rate
of 5Â” per minute. Time = 60/5x1.07.84 seconds.
4. Calculate the feed rate in degrees per minute that is required for a
rotation of
30 degrees in12.8 seconds: F0/12.8*601 degrees per minute.
Or apply the following formula, where: F = feed rate in inches per minute,
A= C-axis rotation angle
L = Length of the tool path
F Â° per minute =F (IPM) x A / L
Feed rate in degrees per minute =5 x 30 / 1.071 degrees per minute
</quote>
So with the below snippet of code, and if I'm doing my math right, the
F?????? would be F1468.31.. and that just doesn't seem right.. Sounds
like a busted endmill to me..
<code>
G00 Y-0.2825 Z7.1678 A84.27
Z6.2678
G01 Z6.1678 F14.3250
X0 Y-0.2805
Y-0.28
X-7.6313 Y-0.28
X-7.6518 Y-0.2794 A84.268 F??????
</code>

tell
it
convention.
interpolation
below.
1.5"
minute,
once
I cant vouch for the accuracy of the options table that can be found here :
http://www.control.com/thread/977589453
But it looks like probly parameter 1 bit zero is what allows feedrate coding
to be in I/T mode

tell
it
convention.
interpolation
below.
1.5"
minute,
once
Sorry my mistake no g93 is available on the fanuc 6
I have the operator manual publication # B54044E /02 here wherin rotary /
linear feed rate ( additional axis simultanious option enabled allowing
three axis combined ) ( as well as simultanious 4th axis control option
enabled where 4 combined axis moves can be combined ) is explained on pages
55 / 56
On pages 204 /205 the rapid only type index table is covered wherein rotary
moves will always be in rapid--attempting to combine a linear will result in
an alarm.
Anyways I may be able to scan these pages so if you don't have an operators
manual let me know....

Nope. That will work. But be careful when you switch to a move with a
linear axis and no rotary motion. Leaving the feed rate that high will
break the end mill.
You need to calculate a different degree per minute feed rate for every
move.

ok, thanks for that.. I'll try it and make sure that any linear movement
has the correct feedrate..
Damn Y axis motor took a crap on thursday, sounded like a bearing went..
Of course, it wasn't something that simple. One of the magnets
decided it was time to come loose.
Took it out to our motor repair guy, he fixed it up, but of course, now
the machine won't work for some stupid reason..
I'll keep this updated with what worked.
Thanks for all your responses.

With 16i/18i/160i/180i Fanuc, 2 parameters to set:
1408.0
Ex: N01408 A1 P 00000000 A2 P 00000000 A3 P 00000000 A4 P 00000001
(A4 = 4th axis)
1465 (Set Radius)
Ex: N01465 A1 P 0 A2 P 0 A3 P 0 A4 P 5575
(A4 P5575 = 4th axis with 5.575 either mm or in radius, no decimal)
Dinh.

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.