Need Help!- OiM cutting feedrate problem

[Purdue Guy]

I am relatively new to machining and am having problems getting with the programmed feed rate. If I post more than one tool such as a roughing pass and then a finishing pass the second tool (and all following tools if there are other sequences) runs at roughly 65 to 70% of the programmed feed rate. The control displays the called feedrate as it is programmed, but the actual feed rate is reduced just like you turned the feed override knob down. If anyone knows what needs cancelled or changed after the first tool sequence I would greatly appreciate the help! My control is a Fanuc OiM control and it is on a 2004 Hardinge VMC 1250II.

[christinandavid]

It sounds like your finishing tool paths are not being processed quickly enough and your controller is adjusting the feedrate to suit.

You need to look at what options you have purchased with the controller regarding 'look ahead' modes/commands.

Search this site for info on AICC or G5 or G8 settings/parameters.

You could also alter the tool path style off-line to improve feedrates.

DP

[gwarble]

at least from 0i-mC forward G8P1 is always available and AI APC (called with G5.1 Q1) is available without option purchase...

so you should have:

safety code
M6 toolchange
before g43, use:
G8P1
G5.1Q1R5 (the r is optional, depends if you have aicc or nano or...)
apply tool offset (g43)
work offset
start cutting

there are limitations as to what can and can't be used in AI APC mode, particularly not rigid tapping in most cases, but read around the forum there are lots of explanations

personally i have put g8 and g5.1 inside my toolchange macros (m6)... and disable them with my rigid tapping (m29) macro... and never run into issues on the newer i-series controls... so they are always on typically

- gwarble

[Purdue Guy]

Thanks for your replies. I finally found in the Fanuc book where the machine reduces the feedrate by the ratio of the cutter center path radius divided by the actual cut path radius. There is an override parameter 1710 that will allow a minium reduction % to be used. Thanks for your help!

[Leha_Blin]

In this case you should notice that when going around radius from the outer part the feedrate should increase. Not sure but in some cases machine can even increase RPM - it depends on settings.

[teabag]

Hi,

I having a similar problem too. The machine is working fine at the beginning until 1 month ago. The feed rate will reduce about 30% whenever there is module G41 and G42. We tried run the same program on other machine (with 0i-MD controller), but it is working fine. We also tried inserting a simple G41 program and test run, the feed rate doesn't reduce either!

So will override parameter 1710 or adding G8P1 help solve the problem ?

[sinha_nsit]

In radius compensation mode, the specified feedrate is maintained along the part boundary. It would be different from the speed of cutter's center.