cutter comp formula's for cnc lathe nose radius

[n***@gmail.com]

I want to know the formula for finding compensated value while doing radius.

[m***@telia.com]

Post by n***@gmail.com
I want to know the formula for finding compensated value while doing radius.

Inner corner you just subtract the noseradius from the radius you want to do. if negative number it can not be done. error occure

Outter corner you just add your noseradius to your radius you want to do.

and to calculate noseradius Z with ease in calculator use this:
Z = NR-((NR - cos(A) * NR) / Sin(A))
A is the angle you want to do. 0 and 90 does not need to compensate.
If calculate X just take 90-A and the formula above again. Double it and
you get the diameter value for X.
Also... if you got a cam nearby, compare your calculations with the
program the cam spits out. Calc correct, and both should be same.

[m***@gmail.com]

well, It took me a while but I finally committed these formulas to memory. No
more tables for different nose radius sizes for programming.
Compensation for x axis
2 [nose radius-(nose radius x sin (45 - angle / 2 ))]
1. divide angle by 2
2. subtract answer from 45
3. find sin of answer
4. multiply by nose radius
5. subtract this answer from nose radius
6. multiply by 2. this is comp value in x.
compensation for z axis
nose radius-(nose radius x sin ( angle / 2))
1. divide angle by 2.
2. find sin of answer
3. multiply by nose radius
4. subtract answer from nose radius. This is comp value for z axis.
good luck, hope it helps.

can u post a pictorial representation

[k***@gmail.com]

well, It took me a while but I finally committed these formulas to memory. No
more tables for different nose radius sizes for programming.

G42
G41
G40
Works just as well, too - and if I have to throw a diffeternt TNR insert in, I
don't have to change the program.
I know that there seems to be a bias against using TNR in turning, but unless
you're doing some weird turn, plunge, back-up moves, then it seems to make my
job easier.
Tom

g41,42,40 is a nice. but some shop with old and knuckle head machinist the g41,42,40 is not in their dictionary. and just because they work without those g code for 30 years, they not gonna use it. that why these formula come in handy.