Hey all, working on a HAAS TL lathe tonight turning some 3-2 internal acme threads. I started with .002 depth of cut per pass and it was running well until it got to about 2.9 major dia, then started getting pretty rough, which I kind of expected. Restarted the program with a d.o.c. at .001 per pass, however current commands shows it taking d.o.c. of .003 per pass. I did not look at what it was taking per pass when I had it set to .002 so I don't know what it was doing before I changed to .001. Any ideas why it's taking more than I tell it to?
Update: Changed it back to .002 per pass and it's still taking .003
View attachment 227391
Hello ADCSpecialtyMfg,
Setting 99 specifies the minimum DOC. This setting on your control must be currently set to 0.003".
The DOC is calculated using the following algorithm
DOC = First DOC x SQR(N)
Where N = the Nth number of Threading Pass, ie 1,2,3 etc
If the difference between the current Threading DOC, minus the DOC of the previous Threading Pass is less than the value set in Setting 99, the Setting 99 value will be used as the incremental DOC. Without this feature, the difference between the calculated current DOC and the previous DOC could become small to the point where the tool merely rubs.
On a Thread where the Thread Form is relatively deep you will end up with a lot of Threading Tool engagement if its allowed to cut on both the Leading and Trailing edge of the insert. An "A" address is available to specify the included angle of the Threading Tool and allow cutting to be performed by the Leading edge of the insert. If the "A" address is omitted, as in your program, A0 is assumed and the Thread cutting will be performed equally by the Leading and Trailing edge of the insert.
I'd suggest including an "A" address value of 29 and you should see an improvement in the Thread cutting.
Because the D address value is used in the algorithm for calculating the DOC, if the first DOC (address D) is very small, then each subsequent DOC will result in an even smaller incremental DOC until the value set in Setting 99 is reached. Rule of thumb, the first DOC should be as much as the Cutting Tool, Machine and Work setup will tolerate.
A "P" address is available in software ver. 6.05 on and provides four different cutting methods:
P1 = Cutting amount constant, single edge cutting.
P2 = Cutting amount constant, both edge cutting.
P3 = Cutting depth constant, single edge cutting.
P4 = Cutting depth constant, both edge cutting.
If the P address is omitted, P1 method is assumed. An angle needs to be specified with the A address to interact with the P1 to P4 methods.
Regards,
Bill
