1. ## Angular interpolation

Hi.
My Fanuc 18i control offers me the opportunity to interpolate angular very simple.
Ex.
G0 x0 z0
g1x10.
,a32.x20.
etc.

We have a CL-20 (not sure which version control), in the shop, which doesn't allow the ,a input.
The chamfer and rounding option is available, like X20. R2., are there some other command I can try on the CL-20?

2. You need to use Right Angle Trig. to find your X,Z axis start and end points.

If you want just a 45 Deg cham and you have the option turned on in the contol, You can use the C word.

X.750,C.100

This will make a 45 Deg. Cham .100 wide.

Other degrees, say, 30 Deg. You must find the start point on the diameter X and the end point of Z. and just program like such:

X0.0Z0.0
G1X.6346F.005(START POINT)
X.750Z-.100 (30 DEG ANGLE)

Without the A word option, you must figure the start and end points for angles. Remember to use TNRC or your angles will be wrong. Use a right angle trig calculator or do it long hand. You can also get a pocket hand book for Right Angle Trig. Companies used to give these books out like Decimal equivilant charts. Not sure if they still do. Mine are from the 1950's and 1960's

Jake

3. Carr Lane still offers this book. \$1.00 USD

http://www.carrlane.com/books/Books_03.gif

Nobody wants books anymore!

Jake

4. Since cl20s could have yasnac lx3, fanuc ot, fanuc 21t etc, kinda need more info.

5. 1st post says Fanuc 18i.......

as a general guide for an OD chamfer if you move 3mm in X and 1.5mm in Z with a 1.2 radius insert you will get a 0.5mm chamfer. tool nose radius comp is not so important on a chamfer. just add a bit more or take a bit off to get the required chamfer.

otherwise work it out by hand with trig or use cam software to generate the whole part thus saving you time and brain work

6. Originally Posted by fordav11
1st post says Fanuc 18i.......
No, his 18i works, his CL20 doesnt. In fact, I don't remember ANY Cl20 coming with an i control. By the time the i control came out, think it was only Cl15's and Cl25's, and in fact the CL15 may have changed to the CL150 with the touch screen Mits on it by then.

7. Ah yes. It looked like he had an 18 at first glance. But actually it does not matter which Fanuc control he has, the programming code is the same regardless

I have not heard or read of angular interpolation nor seen in any text the use of an A or C to cut a chamfer.

If we're talking about Auto-chamfer/radius, that is enabled with one of those top secret option parameters that we can't talk about due to admins having no balls

However if auto-radius works as stated, auto-chamfer should also work because its the same option parameter, meaning the option is enabled.

Auto-chamfering is programmed with an I or K depending on which axis is moving first. If moving in X use K, if moving in Z use I.
The chamfer is formed at the end of the cut. I and K is incremental from the programmed end position and can be positive or negative depending on which direction you want the chamfer to go.
This is clearly explained in any Fanuc programming manual. The auto-chamfering method has been around since 6T. I know because I used it back in 1987 on a Wasino LJ3-3 with 6T control using I and K for the chamfer.

See example from Fanuc 16/18/21 manual below.....

8. Originally Posted by fordav11
1st post says Fanuc 18i.......

as a general guide for an OD chamfer if you move 3mm in X and 1.5mm in Z with a 1.2 radius insert you will get a 0.5mm chamfer. tool nose radius comp is not so important on a chamfer. just add a bit more or take a bit off to get the required chamfer.

otherwise work it out by hand with trig or use cam software to generate the whole part thus saving you time and brain work
Yes,

However, TNRC is so easy to use on an 18T that I ask why not use it?

PLUS, as the radius wears a bit you can just increase the R value and be done with it.

Also when pre-turning diameters for NPT you don't have to use any of the "bump math" you speak of to comp for the tool nose radius. Yes I know many do it this way. But I like to Blueprint program. Not math festival program. And when the job repeats 8 months later, I am not scratching my head about weird looking numbers in the program.

Another huge reason to use TNRC: If you truly want to machine a full radius (180 Deg.) on the end of tube face using two tools. (for ex.)
You will have blending problems if the toolpath is not 100% correct and precision compensation for the tool nose radius is not factored in. You will chase it around until maybe, if you're lucky get it right. With TNRC active, just program to the print and know your exact radius and quadrant of your insert and - perfection. I have made thousands of these types of parts that required a 10 Ra or better finish in 316SST using this method with supurb results. So many people do not know how to use TNRC because they let a computer write their code. Day one at Hardinge all those years ago was TNRC and Quadrant education. Priority 1.

But yes,

For +/- .005 jobs you can fudge it like some do.

Jake

9. All CAM-generated programs have weird numbers. I rarely use TNRC because I have more efficient alternatives. Not saying it's good or bad, just more convenient for me when I have FAPT/CAPS/MasterCAM available and my profiles are infinitely more complex than a simple shaft with chamfers or 90 degrees arcs.

We don't use TNRC at my work to avoid potential problems with unskilled operators. We have 80% unskilled (or lacking the required skill level) so potential is high to forget to set the correct values in the correct places so all programs already incorporate TNRC and cutter compensation on mills into the coordinates. Unskilled couldn't care less if program numbers are to the drawing or not. Actually unskilled don't care if the machined parts are correct to the drawing or not either!

On a mill if a size has a tolerance we still use G41/G42 but quite often the first part is scrap because the operator does not set the required D value in the offsets.

After it is written and running the numbers are forgotten because I know they are right. I frequently call up programs years later, put in the tooling listed in the program comments, set workshift/geometry and press start. Not had a problem yet in 22 years using my methods.

It all depends on what you are used to doing and how you are doing it. If it works continue as-is but it does not hurt to take note of alternatives