Taper offset compensation

[elaganis]

Does anyone here successfully use the taper compensation column in the offset menu? What units is it in? Example, is it total taper compensation per linear move or per inch?

such as +/-.005 per inch of z travel? or total over the 13" of my part? I'm not sure what to enter.

-Thanks
-Ed

[Demon Precision]

i have used it on the tl3 i run at work , it,s hit and miss for the most part , you take the taper amount and divide it the length to be turned and this gives you the value you type into the machine

eg. .004"(amount of taper) divided by 6.250"( Z travel ) = 0.00064 this is the amount you type in , you may need to add a - depending on the direction of taper .

to correct taper i have been adjusting the X dia at Z zero and the X dia at Z finish this works way better , if all goes well i may not have to do any taper adjustments now , the guys from HAAS where in today and aligned the headstock and tailstock today , the head stock was out .004" .

[CNCRim]

Lathe or mill?

[elaganis]

thanks demon!
I tried it today...and you're right it's hit or miss. In this one case it did NOT work well. Like you said it's better to taper compensate in your program than at your controller offset. I just had no choice but to use quick code since my MasterCAM PC was down. Also, I think my tailstock and headstock is out.

For me, the best result to date on long pieces was to take a dia. measurement every one inch over a long lenght such as 16". Enter those as points in MasterCAM and draw a line thru points. I would program and finish to that new curve shape. This would take care of my bow and taper problem and get me within tenths.
YES I NEED A STEADY REST! Anyone know of a good one for my TL lathe?

-Thanks
-Ed

[SeymourDumore]

For one-offs or short runs it is a hit or miss.
If your tailstock is out though, it should be right on once you figured out the amount of compensation needed.
For production runs, there is no way I'd write it into the code itself.
Most often the reason for the taper is push or whobble with large length to diameter ratios, which results in either over or under cutting.
As your tool wears, this taper changes. You replace the tool, the taper changes, you get softer/harder stock, this taper changes, your roughing tool wears, this taper changes. Monkeying with the code to compensate for each of these reasons is just not my cup of tea.
This obviously applies to production runs, but you can do absolutely amazing things with it.
Fanuc's alternative is to change the offset register between Block A and B. That is more precise to measure and does make a much more controllable method to be written into the control. Haas can also use the offset register switcheroo, so if you're not comfortable with the taper register may want to look into using that method. The program remain unchanged and only the offset value is adjusted to hit your target.
The downside is that you need to keep stuff in order and switch back and forth as required. Not the case with the Haas taper register, as it is always applied for that tool depending where it is in Z.