# Thread: How to programme an ellipse?

1. ## How to programme an ellipse?

Hello, boys and girls.
I really need help here.

We have a Dah-Lih lathe with fanuc manual 0-MC software.
How is the best way to program an elliptic toolpath? Is there a function for this, or can i use a mathematical expression? Or do i simply have to use a CAM-software for this?

Best regards
Daniel

2. there is no built-in function. cam software is easiest as it can give you multiple tangential arcs.
it can also be done using macro.
I wrote a 20 or 30 line macro to do an ellipse on a mill years ago.

3. If the control has the optional macro B this bit of code will do it.
Code:
```#100= 2    (X AXIS RADIUS)
#101= 0.25  (Y SCALE, 1.0 FOR A CIRCLE)
#102= 1    (STEP ANGLE)
(----------------------)

#103= 0    (CURRENT ANGLE)
G1X[#100*COS[0]]Y[#101*#100*SIN[0]]

WHILE [#103 LT 360] DO1
G1X[#100*COS[#103]]Y[#101*#100*SIN[#103]]F10.0
#103=#103+#102
END1
G1X[#100*COS[360]]Y[#101*#100*SIN[360]]
G0X0.0Y0.0```

4. that's for a mill. it won't really help on a lathe though
I've turned many ellipses on lathes. the easiest way is with cam software.

5. Ops, missed the lathe part.

6. It should be possible to convert Andre' B's macro to generate an elliptical toolpath by swapping Y for Z, yes?

7. without cam, macro is a good way to do it. But an ellipse approximated with line of a constant angular increment won't have the same tolerance all along the profile, especially if there is a big difference between X and Y radius. I wrote a macro trying to solve that using an increment inversely proportional to the distance from the center to the current point on the ellipse. It's a mill macro but like Geof said, it is not to hard to convert in lathe macro. More detail here:
http://www.cnczone.com/forums/508047-post9.html (macro programing)

8. I'm sorry guys, my english got mixed up a bit there, I ment that it's a mill. So i'm going to try what Andre' B suggests.

Thanks! This was really helpfull since i'm really new to all this!
Have a nice day!

9. Using a scale factor for y-axis does not make it exact ellipse, though it would look like one. If a mathematically true ellipse is to be made, one has to use its mathematical equation.

10. You are right, only the center of the tool is moving in an ellipse, disregarding the cord error.
The part that is cut will be distorted some by the radius of the tool.
Turning on radius compensation should take care of that.

But keep the end mill small relative to the minor diameter and for many jobs it is not going to make a measurable difference.

11. An ellipse is one of those curves you can't really 'measure' so it's not usually that important if it's not perfect as long as it is smooth.
Our hacky programmers in the office don't have a clue and draw an ellipse in Autocad then manually best-fit 3 or 4 curves per quadrant with close-enough tangents then dimension the start/end points and center points to get the coordinates then use that data to program the part.
Depending on how knowledgeable your quality control people are that method can normally be used with impunity.

12. In manual drawing also (isometric projection), an ellipse is drawn using four-center method, consisting of four arcs. It looks pretty good. The method is explained in all engineering-drawing books.

Page 1 of 2 12 Last

1. ###### Thread How to programme an ellipse? | CNCzone.com-The Ultimate Machinist Community | BoardReader
05-08-2012, 02:23 PM