What's new
What's new

Fanuc 18i OD taper groove programming advice wanted

BAR0710

Plastic
Joined
May 25, 2024
Location
United Kingdom
Hello,

I am looking for advice regarding programming a feature on Fanuc which I am having issues with.
This is the profile that I have been attempting to machine;
1716643774829.png
The tool is an internal grooving bar (clearance restriction) with a 2.5mm wide insert with 1.0mm rads on each edge.
initially I set the tool as type 3 and compensated the width manually with radius compensation on as suggested which threw up error 041 interference in NRC, I then removed the radius compensation which would allow the machine to run, however it (as expected) did not complete the profile to spec but gave me an idea on how it would turn out.

The part is correct on the G41 side of the program in Z- but bigger on X, on G42 it is correct in X but bigger in Z-. This gives me material to remove still.

Here is my "revised" program which I am unable to test until I am back at work;
T00L TYPE 9 - setting as a button tool
N1 T1010 M8 (2.5MM R1.0 OD GROOVE);
G97S500M3;
G0G40G54G80G99X73.0Z30.0;
Z2.0;
G1G42X72.0Z-2.682F0.1;
X71.0Z-3.182;
X64.974Z-4.279;
G2X63.0Z-5.688I66.0K-5.688R1.5F0.1;
G1Z-6.0;
G0X73.0;
G40Z2.0;
Z-7.0;
G1G41Z-8.0F0.1;
X68.0;
G3X63.0Z-5.5I66.0K-5.500R2.5F0.1;
G0X73.0;
G40Z30.0;
X270.0;
G28U0.0W0.0M9;
M5;
M01;

I have added 0.5mm to all Z faces on the G42 move to compensate for the fact it is not a button insert.
I am looking to know if this would potentially work as is and if not, why and what would be the correct approach?

The tool path would ideally stay split as the tool will not handle a back cut.

Thanks in advance,
Alex
 
I noticed a rapid (G0) move while comp was still on. I usually don't do that.
As much as I use Fanuc cutter comp, this may be one of those times where you're better off not.
 
One obvious problem is the insert. With or without TNRC it won't cut the profile. The flat from 5.188 to 5.5 is only .312 wide, but the insert flat is .5 wide. It won't fit in there.

Use a full radius insert with a smaller radius than the smallest profile radius for starters.
 
One obvious problem is the insert. With or without TNRC it won't cut the profile. The flat from 5.188 to 5.5 is only .312 wide, but the insert flat is .5 wide. It won't fit in there.

Use a full radius insert with a smaller radius than the smallest profile radius for starters.
Hi,

I explained this to my boss, He said this will be fine and to continue, I did also say that this would be so so much easier with a full radius insert however they had bought these inserts beforehand and are insisting they get used, I found one full radius insert which was dismissed when i suggested i use that instead. It's difficult for me to explain these things as I am still an apprentice and learning cnc and his experience is solely cnc milling and manual machining.

Looking past the geometric issues I'm looking to learn the programming for this kind of profile.

Thanks,
Alex
 
I find it much less confusing to program an undercut from both ends to the middle. All you need worry about then is the tool is not so wide that it undercuts on the opposite side.

If you want to make an od groove with a radius or chamfer at the top using TNRC, do this. Program the chamfer and proceed to the bottom of the groove. Then make a dummy move equal to 2X the TNR and then pull straight out. For example, if the tool nose radius is .010, and the bottom of the groove is at X1.000 Z-1.000, pull out of the groove at Z-1.020. The tool won't move, but will pull straight out, since the sense of the TNRC is still correct for the far side of the TNR. The groove will then equal the tool width.

For a face groove you've gotta move 4X the TNR, since X moves are on the diameter.
 








 
Back
Top