Chamfer cutting holes in steps

[gary adams]

I am trying to machine a chamfer at the top of a hole 10mm x 10mm my cutter has a 4mm x 4mm cutting edge,so I want to do it in series of steps.I tried contour path and tapered walls using a taper cutter at 45deg at knock off I still had the problem of getting the cutter to start at the hole centre at each step. I am hopeing someone has a procedure so first up tommorow I can hit the ground running.

Gary

[Mr. Wizzard]

Try contour. Chain your thru hole diameter. Use 2D Chamfer as contour type. Define your tool correctly. You may have to play with the tip offset and chamfer size, but it will work. Start with getting a 2mm x 2mm chamfer working correctly. Then, work your way up to -8mm stock to leave in X/Y (10mm - 2mm), with everything else the same. Then, set it back to zero and work your way up to -8mm stock to leave in Z.

 

I just tried it on a cylinder and it worked.

 

Hope this works for ya, i've done it before on parts where the chamfer is bigger than the cutter.

[gcode]

I use a custom chamfer tool with the defined diameter at the bottom of the chamfer tool.

Then chain the top of your hole, use contour

and define your angle and depth of cut on the Depth page..

It works great..

If you're in a hurry and don't want to make a custom tool, you can lie to Mastercam and use an endmill that's the same size as the bottom of your real life chamfer mill .

It won't look right in Verify or Backplot, but the code will work out on the machine.

[gary adams]

Many thanks off to work now armed with knowledge for once

Gary

[billet programmer]

I do it the same way as gcode & it works very well. Your results will be as acurate as your custom tool is defined.