How to program a taper mill

[Pilot Plant Supervisor]

I have been struggling with using a taper mill on a 2D contour toolpath. If I define the tool with a 10 deg. angle and .062 full radius tip and use wear comp, it comps the toolpath to the .062 regardless of what depth I use. I have to keep playing with the stock to leave to get the profile to come out right. What is the proper way to use a taper mill? It seems like when the tool is defined, it should adjust the comp at a given depth so the profile would be correct.

[Rotary Ninja]

Are you setting the tool up to be .062 diameter? Because whatever diameter you set for the tool diameter is where it comps to.

 

If you are driving around the OD of a part for example, pick the bottom chain. In your toolpath parameters on the linking page set the Depth to use Incremental. In the depth field enter -.031. That should get you there.

[Rotary Ninja]

[Pilot Plant Supervisor]

Thanks, I'll play with it some more.

[Pilot Plant Supervisor]

Yep, that works. Now, what if I want to change the depth to -.1 (incremental) so I'm not cutting with the tip so much? Do I have to figure the diameter to enter at that depth or is there an easy way?

[Rotary Ninja]

You could trig out the values and add them to the fields on the cut parameters tab for stock to leave on walls and floors. But yeah, if you find the diameter at the desired cut depth and comp to that you should be golden.

[Rotary Ninja]

Or another option, set the tool up as a spot drill. Touch off the tool and raise it in the control to place the length offset at the theoretical point of the tool. Create a chamfer toolpath and set the chamfer size to the actual perpendicular distance from the bottom to the top of the contour. Then you can use the Depth value on the Cut Parameters page to offset the tip. If this doesn't make sense let me know and I will try to get you another example when i get home.

[Pilot Plant Supervisor]

I usually draw up the tool and find the diameter at the depth and offset with stock to leave. I was just hoping there was a better way.

[Tony35]

set the chain at the bottom of the feature for incremental

turn on depth cuts with your taper angle filled in ( make sure the depth cut is deeper than the feature you are cutting)

then set depth to incremental and put in what ever value past your chain you need

[Pilot Plant Supervisor]

That's it! Thanks Tony35!!!

[Rotary Ninja]

Ok, that is sweet. Thanks Tony.

[kunfuzed]

Is a Taper Mill definition and contour set to 2d chamfer compatible? Works with the tool defined as a chamfermill, but not as a taper mill, for a 15 deg chamfer...