[bgmnn]

I am cutting 10 holes on a 6.599 bolt circle with a .625 end mill.
Using "Mill Circle" at .03 step down to .75 depth, the holes are .004 out of round.
I tried programming the holes using a single arc segment with the same results.

Would a circle programmed as 4 arc segments yield a rounder hole?

Thanks in advance,

Mike

[bloke]

Sounds like backlash. Have you measured it yet? Post it up and I'll tell you how to compensate it.

[job_it]

The rigidity of your machine can't handle the the size of your end mill your end mill or spindle is flexing about .002 thousands. or your x or y axis is moving or a combination of all.

One thing to help would be predrill the hole to about 9/16 to use endmill. endmills do not like plunge cuts

If on a cnc use a smaller endmill and ramp on plunge cuts but predrill always better.


If you are trying to create perfect round holes to size in the right location.

1. Use a center drill to start holes
2. Drill stepping up in sizes till .010 to .020 thousands smaller the finish size
3. Ream hole in a single fast motion.
4. Chamfer edge to about .005 thousands.

Remember the less stress on the metal the more accurate the hole.

Hope this helps

Jim

[bgmnn]

bloke

Not sure of the best way to do that. The indicator zeros to the axis display when moved then returned.


job_it


The hole was plunged with a 1" EM. The final size is 1.188.
The end mill is cutting, no more than, .015 " per side, stepping down .03".
I have recently cut a profile made up of 8 arc segments. It measured correctly.

[bloke]

Jog the axis in a positive direction only until zero on the dial gauge then zero the part setup. Continue to jog in a positive direction for a few thou then change to a negative only direction to bring the dial gauge back to zero.
If the gauge kicks on change of direction, it's over compensated for backlash.
If there is a slight delay on change of direction, it has backlash.
The figure on the machine display will tell you how much.

[job_it]

you need to check the count. The way you check it is clamp a long piece 12inches or longer of metal to the table. use a edge finder find the edge set "0" . only on the x axis Do not move the Y axis without stopping spindle jog to other side find edge. write the number down. now go back past "0" and come back and find the edge without looking at the reading look up and if "0" then axis good. do the same procedure for Y. you will probably find the "x" or "y" is different. by .002 thousands.

you could use your vise but for y clamp metal between jaws to eliminate play.

If it is out tighten your x y gibs or rails. then repeat to eliminate table

If servo your in-coder could be bad

Thats how the axis makes a out of round hole.

If not then the problem is the spindle or machining procedure.

Jim

[bloke]

The other way you could check for backlash is to cut a frame. The step size on the front of the frame where the cut starts and finishes will be the backlash / overcomp in a cutting condition.
Rotate the frame about centre to find the backlash / overcomp in X.

[bgmnn]

Bloke,

What is the procedure for backlash compensation?

Thanks in advance,

Mike

[underthetire]

Out of round in what direction, x,y, or at quadrants. If it's out in quadrants then you will need to tune the servos. X or y could be backlash, like bloke said. He is the hurco man!

[hurconotes]

I use a g code program to test it

Heres an example for X

Put indicator in vice and put the tip on left side of spindle
zero x y in part setup and z in tool setup for tool 1

no tool in spindle

program:

T1
G0 G90 X0 Y0 Z0 (MACHINE SHOULD NOT MOVE BECAUSE YOU ARE THERE)
G1X1.0F25.
X0
G4X4.0 (4 SECOND DWELL... LOOK AT INDICATOR IT SHOULD BE 0)
Z1.0
X-1.0
X0
Z0
M30 (LOOK AGAIN AT INDICATOR)

THEN I ADJUST AND REPEAT....
I USUSLY ADJUST THE REVERSE COMPENSATION....

HURCOGUY.COM