circular interpolation description

[tom bryant]

Hello,
I have a supermax 40 mill w/ an Anilam crusader M control. I'm having a problem with getting a round bore using Anilams canned cycle. The program calls out the center of the bore X0Y0 and drops z to depth then feeds out at about a 30 degee angle to about 1 o'clock then goes counter clockwise around the hole past 1 o'clock to about 11 o'clock then back to center. The
resulting hole because of the extra overlap makes the hole out of tolerance. Is there someone out there that has run this control and can tell me if there is a different way to program this? I'm not that great on the mill yet I've been programming cnc lathes for about 23 years and have puchased three of these supermax's about a year ago. What does the term "interpolate" mean in lamens terms. Is it possible to hold .0007 in a bore or should I go back to the boring head? THANKS

[Eurisko]

Interpolation, in machining terms, is generating a path that connects data points. Close to the ideal path, but constrained by the control limits.

The proper way to cut a circle is to ramp into the circle (using a smaller radius), cut 360 degrees at the proper radius, then ramp out (using a smaller radius).

This ensures that there is no overlap.

Unfortunately, it would take an EXTREMELY accurate machine to hold .0007 tolerance interpolating a bore. If the machine itself is accurate to .0002 positioning, you've already used up over half of your tolerance!

When you add in other factors such as tool wear and deflection, material hardness, temperature, etc., you're really pushing the limit.

[Mazaholic]

Check the backlash on the machine.
We have three supermaxes..one of them looses about .02 in 6 inches.
.0007 i'd probably use a good boring head.

[tom bryant]

Mazaholic,
Does any of your machines have anilam controls on them. Also how do you tell if you have linear scales on a machine. My "programing manual " says I have backlash compensation. Is that the same as lost motion?

[HuFlungDung]

Using a slow feedrate on a light cut allows the cutter to do its very best at removing all the material that it can. Thus, there is nothing left to be cut on a 'spring pass'. If you still recut when going over the same path twice, then your tool is not sharp enough, the amount to finish was excessive, or your feedrate was too high.

When attempting to interpolate a bore to roundness, use a sharp tool reserved for the finish cut. Use a seperate profiling operation (with tool radius compensation) to take the finish cut, rather than a machine cycle. Use the machine cycles to rough and semi-finish with, that is what they are for.

My suggestion is that you reserve maybe .002" for a finish cut. Tool deflection during heavier cuts will easily cause the 'overcut' effect in any areas where the tool traverses twice (as in your overlap zone).

Slow the feed down considerably when attempting to interpolate bores very accurately. I found I could get very good interpolated roundness on my Haas if interpolating at about 10 ipm (in aluminum)ie, approx .0002 variation.

[Mitsui Seiki]

Originally Posted by Eurisko The proper way to cut a circle is to ramp into the circle (using a smaller radius), cut 360 degrees at the proper radius, then ramp out (using a smaller radius). This ensures that there is no overlap.

This is what it can look like:

g0g90g54x0y0
g1z-10f100
g2x0y12.5i0j6.25f200
i0j-25
x0y0i0j-6.25

[Mazaholic]

Originally Posted by tom bryant Mazaholic, Does any of your machines have anilam controls on them. Also how do you tell if you have linear scales on a machine. My "programing manual " says I have backlash compensation. Is that the same as lost motion?

Ours are Fanuc.
I just recomended a backlash check so you can remove it from your list of possible problems.
.0007 will not allow for much if any backlash.
Backlash is the total amount of (for lack of a better word) slop in your leadscrews.
Your machine probably already has some factory compensation for it but the amount will change due to wear and tear.
Just make sure you use a quality indicator that reads at least .0001 increments,you adjustment will only be as good as the indicator.
Interpolation with small tollerances can be a pain if your backlash isn't adjusted properly since your using two axis....you can imagine it wouldn't take much to create a square hole.