Problem- Machining a Parabola Fanuc 10T

[Steve Preece]

Good morning

I have a Puma 6 HS with Fanuc 10TF control.

I need to machine a stud, which has a parabolic curve profile.

Does anyone have an example program that I could reverse engineer and apply to the dimensions that I require to produce my final component.

I am aware of 'custom Macro' for Fanuc, but do I have to access machine parameters and change anything?

My thanks in advance

Steve

[Dan Fritz]

A parabola can be machined with a small macro, but the nature of the curve has to be defined mathematically. Generally, parabolas are curves where one axis (Z in this case) is a function of X squared. There can be other factors in the equation too, such as :

Z = X * X
Z = 1.5 * (X * X)
Z = 2 * (X * X)

Each one of these parabolas has a "tighter" curve, which is controlled by that multiplication factor.

When you write the macro, you need to first set the LIMITs of the curve (say from Z6.00 to Z5.0), then you start at X0.0 and "step" the X axis with some increment (say .002 per step). At each new X dimension, calculate the proper Z using your formua, then move in G01 to that new position. The macro "loops" until you get to the target location in Z.

Example:

Start point = Z6.00, End point = Z5.00, simple parabola: Z = X * X
Cutting starts at CL in X. As X goes from 0 to 1.0, Z goes from 6.0 to 5.0 along the curve.

#101=0 (START POINT IN X)
#102=0
#103=.002 (INCREMENT IN X)
#104=6.0 (START POINT IN Z)
#105=5.0 (END POINT IN Z)
WHILE[#102LE[#104-#105]]DO1
#101=#101+#103
#102=#101*#101
G01X#101Z#104-#102
END1


You can put code like this in your main program, or you can make a separate little macro and call it with an M98Pxxxx command. If you want to call the macro and pass the variables to it, you can use a G65Pxxxx command to call the macro and pass varibles using X, Z, I, K, etc. If this is a "one-time" job, try to keep it simple.

[sinha_nsit]

Dan,
I guess this program is for a turning centre.
The program will of course machine a parabola, but the initial depth of cut will be too large, and hence, machining would not be possible, if the workpiece is of uniform diameter.
The generated profile will have to be inserted between P and Q blocks of G71.

[Dan Fritz]

I was assuming that you would rough-turn it first. This macro is just the finish cut.

[Steve Preece]

Hi to both Dan and sinha_nsit,

Thank you both for your posts, I need to finalise my drawings, then apply the dimensions to the job.

Yes, it will be performed on a turning centre, and I have noted the need for a roughing cycle.

Thank you both again, I will keep you posted

Regards

Steve Preece