need some help figuring out some tool paths

[tnik]

Hey all, was wondering if you could give some tips/tricks on this part.

Just trying to do a simple chamfer on the 19" edge, and I know I can do it by manually creating the contour lines for the tool and using a 2d cut option, but I'm sure there's a way to do it in 3d and get the same results with less work.

What I'm trying to accomplish is for the tool to start roughing at the top outside of the material, with a step over of least .5 , and a Z depth change of .2 (moving towards the flat at Z0.) leaving around .03 for a finish pass.

Then the finish pass I want to start at Z0. and work my way down the part.

The chamfer tool I'm using is a 2 flute inserted chamfer cutter, minor dia being 1.07, major being 1.75.

I tried using the 2d chamfer tool option, but it wont accept a bigger chamfer than what the tool can make.

Thanks in advance

[tnik]

well, think I figured it out, if there's a better way, please speak up

I ended up making a top geometry box that was the lxw of the chamfer (19x1.38) then extended the surface of the chamfer past the box. Used Z rough/Z finish to do it.

Extending out the surface past the ends kept my tool paths from trying to wrap around the part and do some funky things.

[moldcore]

I’m a little confused to what you’re trying to do but I’ll offer some suggestions. From the model, it looks like you want the 45 deg. surface cut? I wouldn’t call that a simple chamfer, but that’s a matter of semantics I guess. Assuming the cutter is 45 degrees (you don’t say) , in 2 axis, chain the top edge(s) and enter 1.07 as the tool diameter (you don’t need to pick a cutter from the library) and under the cut control tab, geometry is "top", enter 45 for the “taper angle”. The depth of cut is set in the In Z windows; 1.38 for the amount to remove and .2 for the rough spacing. Make sure you enter .03 for the stock to leave in the “on sides” window. To finish, repeat the above steps but set the “stock to leave” on the sides to zero. This is the simplest method I believe but others may have other ways. Using 3 Axis will also work but takes a little more effort.

To do it in 3 axis “cut” mode using the surfaces you’ll have to edit the surface to get the normals (arrows) at the top and pointing in the direction you want to cut. Pick the surface, set up your cutter information and then set your increment value to .200. You can cut this with your 45 deg cutter or any cutter in your arsenal but the increment value will have to adjust accordingly. There are multiple options to choose from when cutting this type of surface. With any cut like this you’ll have to consider roughing off the material and both 2 Axis and 3 Axis methods can accomplish this with 3 Axis offering a more automated way of doing it.

[tnik]

Thanks for the reply, sorry I didn't specify, yes it was a 45 degree cutter. I ended up doing it the 3 axis way, but will try out your 2 axis way later on. I know there's always multiple ways to skin a cat, I like to find out as many ways as possible for future reference.