SL10 id bore taper?

[FUN4ME]

Hi all,
On a SL10 in the tool offsets which way does the taper value go?
We are boring about 3.00 inches deep and getting a .0004 taper smaller at z –3.00
Which way would I put the taper value?in the offset page .0004 or -.0004?

Thanks Erich

[Technical Ted]

.0004 You want to remove more material. Depending on the part you could just edit in an X dimension with the Z-3.000.

Ex. X2.0004 Z-3.000

[FUN4ME]

Thanks Ted,

I tried that (adding .0004 to the z-3. Line but the caned cycle didn’t like it)
So after some experimentation I ended up with -.00010 on the taper .
It seems backwards but it worked, also I think that the taper is calculated per inch

[WOLOG]

The Haas control will "Whig Out" in a canned cycle if there is a change in direction in X. This means that the canned cycle the machine wants only X values that go from small to larger for a OD and large to small for an ID. The .0004" added to X to remove the taper is a change in direction which equals an alarm. If you put the Z start position on the canned cyle line where first X is, it will clear up the alarm. I have to do this all of the time to do thread undercuts and such on both OD's and ID's.

(TNMG-432 RH OD)
G54
G00 G53 X0 Z0
T101
G50 S2000
G00 G96 S600 M03
G00 X2. Z.1 (Z START) M08
G71 P100 Q101 U0.030 W0 D.125 F0.015
N100 G00 X1.44 Z.1(Z START POSITION)
G01 G42 Z0 F.006
X1.5 Z-.03
Z-1.25
X1.44 Z-1.28(UNDERCUT)
Z-1.375
X1.94.........

To remove the taper, it works the same way.

[Geof]

This is copied from a post by Haas Apps in a thread about taper on a long thin part;

In the tool offset pages there is a column to adjust taper for deflection. The below text is from the manual - hope this helps:

Deflection of the part occurs if it is not supported precisely in the center, or if is too long and unsupported. This causes the cut to be too shallow so the resultant part is under-cut. This can apply to O.D and I.D cutting. Taper Compensation provides the ability to compensate by adding in a calculated value to the X movement based on the position of the Z cut. The zero point of the taper is defined to be the 0.0 of the work-zero coordinate of Z. The taper is entered on the tool shift page as a 5 place number and stored in an array indexed by tool, which is called “Taper” on the Tool Shift / Geometry page. The value entered should be the deflection in the X-axis divided by the length in the Z-axis, over which the deflection occurs.

[FUN4ME]

Originally Posted by Geof The value entered should be the deflection in the X-axis divided by the length in the Z-axis, over which the deflection occurs.

Thanks that helps, our book says

"The user can modify the taper at any time"

in place of what I quoted from you.
Thanks again
Erich