Need Help!- Turning a Thin part and Getting a Bad taper

[JWB_Machining]

Hey,

Ok so i'm gonna explain my set up and problem and hopefully someone will have that obvious solution I'm just not seeing.

I'm using a 5C collet with a collet stop to hold a 3/8 dowel of aluminium 7075. The dowel is 3" long and has been faced and centerdrilled on both ends. about 2.2" of the dowel hangs out past the collet. I have a live center in my tail stock, the tail stock is tighten down into it's spot and I applied good pressure going into the part and then locked down the live center. I then use a 35 degree cutting tool to turn down the dowel to a Diam. of 0.26" Then on the half closer to my collet I have to turn down a reduced diameter an inch long. It takes a radius going into and out of this reduced diameter. Right where the radii end the diameter of the part is supposed to be 0.160 and they taper to the middle of the reduced diam. to a diam of 0.159. My problem however is that the side closer to my tail stock is .160 but the end closer to my collet is .157. I've reduced my feed and depth of cut on the finishing pass to 0.001 in/rev and .001. My machine is a haas TL-1 so the spindle is running at 2000 RPM. Is there anyway to over come this problem and possibly make my set up more rigid or is AL 7075 just too soft and i have to modify my program so that it's actually cutting thte part oversized but with bending it will be correct diam? Sorry if this isn't clear just ask me about anything and I can clarify it for you.

[beege]

I always try to compensate for tapers "in-program". I know there'll be one, even if its only a few tenths. I was trained to do it one way, using 2 offsets for the same tool, activating the second offset during the long cut. Micro adjustments are possible then. Now, I do it a different way, using variables:

X[.160+#500]Z0
X.160Z-1.

If I need the Z zero end to be .001 smaller, I put .001 in variable #500

This would be on a Fanuc, YMMV

[Geof]

Check that your tool is cutting on center or a few thou below; if it is above center you get more rubbing pressure which can easily deflect thin parts.

You mention 'good pressure' on the center; wrong technique, your are tending to buckle your skinny little cylinder with a large compressive load. The center should be just firm enough to remove any chatter but not really tight.

Even so you may need to play with compensating for the taper by programming an opposite taper.

Good luck; sorting out these annoying little things can sometimes be an exercise in frustration.

[Haas_Apps]

Originally Posted by JWB_Machining Hey, Ok so i'm gonna explain my set up and problem and hopefully someone will have that obvious solution I'm just not seeing. I'm using a 5C collet with a collet stop to hold a 3/8 dowel of aluminium 7075. The dowel is 3" long and has been faced and centerdrilled on both ends. about 2.2" of the dowel hangs out past the collet. I have a live center in my tail stock, the tail stock is tighten down into it's spot and I applied good pressure going into the part and then locked down the live center. I then use a 35 degree cutting tool to turn down the dowel to a Diam. of 0.26" Then on the half closer to my collet I have to turn down a reduced diameter an inch long. It takes a radius going into and out of this reduced diameter. Right where the radii end the diameter of the part is supposed to be 0.160 and they taper to the middle of the reduced diam. to a diam of 0.159. My problem however is that the side closer to my tail stock is .160 but the end closer to my collet is .157. I've reduced my feed and depth of cut on the finishing pass to 0.001 in/rev and .001. My machine is a haas TL-1 so the spindle is running at 2000 RPM. Is there anyway to over come this problem and possibly make my set up more rigid or is AL 7075 just too soft and i have to modify my program so that it's actually cutting thte part oversized but with bending it will be correct diam? Sorry if this isn't clear just ask me about anything and I can clarify it for you.

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.

[Geof]

Originally Posted by Haas_Apps In the tool offset pages there is a column to adjust taper for deflection. ....

He's right!!!

Look in the index and there it is Taper Compensation page 39.


I guess even before all else fails READ THE MANUAL. Hoist by my own petard.