What's new
What's new

Fanuc polar mode close to X0

SRF

Plastic
Joined
Sep 26, 2020
I'm sure this isn't a new problem, I've found a few threads about it but I haven't found any real solutions apart from don't do it...I can program around it but I'm wondering if there is a better way because it gets really annoying at times.

Machine has a 0iTC control, and the post outputs pretty much everything in polar mode. All of our parts have holes in the center, so there is no live tooling work near the X0 point, the problem is during positioning moves. The way the post outputs it indexes to C0, enters G12.1, then heads over to the start of the feature. However if the feature is at C180 (or somewhere close to) it tries to pass through X0 and it alarms out due to the infinite C axis speed required to maintain X feed.

#1 - is it possible to make the control ignore the programmed feedrate of X and move the C at rapid while the X creeps along? It seems odd to me that this isn't how it behaves by default, it isn't an ideal cutting situation but it seems to me it would be better than not being able to do it all.

#2 - This is sort of related, but are the different parameters for the C axis rapid (G0) speed and the C0 interpolated speed (G1 in G12.1)? Reason I ask, this is a big vertical lathe, 57" chuck. When the X gets close to the centerline of of the chuck in G12.1 it will spin MUCH faster than a G0C_ move. The inertia in the chuck is huge and the geartrain makes a heck of a noise when it starts accelerating that fast. I'm not sure if this is normal behavior or if the mtb overlooked something here but I almost want to try and slow it down so it's not so hard on stuff
 
#1 - is it possible to make the control ignore the programmed feedrate of X and move the C at rapid while the X creeps along? It seems odd to me that this isn't how it behaves by default, it isn't an ideal cutting situation but it seems to me it would be better than not being able to do it all.

#2 - This is sort of related, but are the different parameters for the C axis rapid (G0) speed and the C0 interpolated speed (G1 in G12.1)? Reason I ask, this is a big vertical lathe, 57" chuck. When the X gets close to the centerline of of the chuck in G12.1 it will spin MUCH faster than a G0C_ move. The inertia in the chuck is huge and the geartrain makes a heck of a noise when it starts accelerating that fast. I'm not sure if this is normal behavior or if the mtb overlooked something here but I almost want to try and slow it down so it's not so hard on stuff

Hello SRF,
G00 can't be used inside Polar Interpolation. You get the alarm because the "C" axis component of the Feed Rate exceeds the value set in parameter 1422. If it won't harm the tool, you could set a larger value in 1422, or change the Feed Rate in your program.

Regards,

Bill
 
You can use an arc move to your next position to negate any big X movements.

I used to doo that when I had bigger sized flats to make.
The stuff that I mill flat in C these days doesn't really need that, so it's been quite a while since I have done the arc method (had a Y axis lathe for <20 yrs now) but I recall that working swell for not getting too jerky.

Another thought - I never start at X0 when I start G112.
I typically start at X2.000 or whatnot. (something clear of the part in X)


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

Think Snow Eh!
Ox
 
Hi Bill, thanks for the response.

Thought I changed that wording, I am aware that G0 doesn't work in polar mode. The post uses a G1 move with a higher feedrate for initial positioning that is what I meant. For instance this would alarm because it passes too close to X0:

/ N7 M33
N8 M1
N9 T1111
N10 M6
N11 G97 S2000 M3
N12 M13
N13 M16
N14 G90 G40 G80 G98 G94 G17 G54
N15 G0 X15.9 C0.
N16 Z0.85
N17 G12.1
N18 G1 X-15.8301 C0.7447 F59.055
N19 Z-0.42
N20 Z-0.6678 F20. M10
N21 X-15.8292 C0.7451
N22 C0.7457
N23 X-16.2855 C1.3205
N24 X-16.2863 C1.321

There are ways to program around this obviously, we do it every day, but it is an annoying problem to deal with consistently

Feedrates -

N01420 A1 P 15000 A2 P 12000 A3 P 720
N01421 A1 P 0 A2 P 0 A3 P 0
N01422 P 5000

I don't see how 1422 comes into it, I would think it would alarm based on 1420 A3 due to the programmed feedrate requiring a c axis speed greater than 2 rpm. But the interesting thing is, when programmed as it is above, I can get the chuck going wayy faster than 2 rpm momentarily when passing through small values of X in polar mode

I don't see why it couldn't move until C was as maximum rotational speed then decelerate X to maintain position. This would mean cutting at under programmed feerate in certain situations, but machine tools do this all the time anyways with acceleration curves in sharp corners anyways, it's just one of the realities

Cheers
Sam
 
You can use an arc move to your next position to negate any big X movements.

I used to doo that when I had bigger sized flats to make.
The stuff that I mill flat in C these days doesn't really need that, so it's been quite a while since I have done the arc method (had a Y axis lathe for <20 yrs now) but I recall that working swell for not getting too jerky.

Another thought - I never start at X0 when I start G112.
I typically start at X2.000 or whatnot. (something clear of the part in X)


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

Think Snow Eh!
Ox

Changing to an arc move, that is probably an easier solution than what I am doing, and I may actually be able to automate that since it's really only the initial positioning move I am having issues with at this point. Will have to take a look at the post.

It does always start G12.1 at the OD of the part. There isn't any cutting anywhere near X0, it is just the moves to the next feature that are causing the issues.

Thanks!
 








 
Back
Top