V10.5 Chamfer

[brrian]

I'm super excited to see the new Chamfer toolpath as part of V10.5. Question though - it looks like it only works with a ball end or vee mill. Is this correct? If so, any plans to (or why not) also allow a radiused end mill?

Reason I ask: I chamfer aluminum plate. I use a square end mill to clear out most of the material because a ball end mill doesn't do it well. Then I come back with a ball end mill & finish it. I'd like to replicate this in VCarve

Thanks...

[kstrauss]

I also work mostly in aluminum and apply a small 45-degree chamfer to the edges of most of my projects. Is there some reason why you can't use a normal chamfer mill with the appropriate angle? I've been doing it this way for years in Vcarve and see few advantages to the new chamfer toolpath. It is far faster than doing the work with a ball endmill or radiused endmill. What am I missing?

[mtylerfl]

I also work mostly in aluminum and apply a small 45-degree chamfer to the edges of most of my projects. Is there some reason why you can't use a normal chamfer mill with the appropriate angle? I've been doing it this way for years in Vcarve and see few advantages to the new chamfer toolpath. It is far faster than doing the work with a ball endmill or radiused endmill. What am I missing?

Hi,

One advantage is the ability to choose/create any chamfer angle, and not be limited to "stock" chamfer bit angles.

[AdamJ]

kstrauss, we are offering both options. Just using a V Shaped with the appropriate angle is fine, however depending on the geometry you have available then it might require a bit of trigonometry to work out offsets for your profile toolpath (obviously the 45 degree case isn't so bad) so we are just doing that bit of calculation for you.

brrian: We can certainly look at the radiused end mill option.

Cheers,
Adam

[kstrauss]

I understand the angle advantage; I mentioned the requirement for a chamfer mill with the appropriate angle in my original post.

My issue with the new chamfer toolpath is that it appears to position the tip of a v-shaped cutter ON the toolpath. This means that unless I create an offset toolpath I am cutting with the middle of my tool which cuts poorly/leaves a mark on the edge of my stock. (My usual tool is a 90-degree chamfer tool with 4 cutting edges.) It would be perfect if the options for a chamfer toolpath allowed one to specify an offset from the path selected. That would also mean that a circular leadin/leadout would work nicely.

[brrian]

Thank you Adam! For me, ideally I'd be able to use a square end mill to rough out the chamfer. that would result in a series of steps that are the depth of each pass, but it gets rid of most of the material & I can finish with the ball end mill. A radius end mill is a happy medium. In the meantime, as you suggest I may try to work out the offset so I can fake the rough passes with a ball or vee mill.

kstrauss - my chamfers are large, usually 1/4" to 3/8" deep.

Thanks!

[kstrauss]

brrian noted that "my chamfers are large, usually 1/4" to 3/8" deep."
Proper chamfer cutters are readily available in sizes that would cut a 3/8" chamfer in a single pass. Of course one might not have sufficient spindle power and chip clearance may be an issue.

A huge advantage of an angled cutter is the ability to cut in a single (or perhaps a few) pass. To cut a chamfer by roughing with an endmill followed by a ball mill with a small stepover will require many passes and significant time plus a tool change.

My only complaint about the new Vcarve capability is the lack of an easy way to to offset the V-tool's point from the edge of the work.

[dealguy11]

I haven't used this toolpath because I use either regular profile toolpaths (for v-bits) or moulding toolpaths (for round cutters) to do this. So take my comment with a grain of salt. It seems like a simple workaround to get the tip of the v-bit off the edge is to offset the outline vector by a small amount and increase the depth of cut appropriately. That's what I would do for either of the existing options for chamfers.

[kstrauss]

I completely agree and I have successfully used offsets to create chamfers on many projects. On a complicated project the offset toolpaths clutter the image (particularly for a double sided project) so it would be great if the offsets could be an integrated part of the setup for the chamfer. A further problem with explicitly created offsets is that I cannot use document variables to improve consistency between projects.

[brrian]

I'm on a WorkBee, cutting with a Dewalt router. I know about the large v bits, but they're not an option for me.

To rough out the chamfer I figure out the geometry needed to do it in shallow steps about .025" deep, then I use a series of profile cuts. It works fine but is a little tedious & I have to be very careful that I'm selecting the correct profiles.

The current state of the Chamfer tool gets me halfway there - I can't use a square or radius end mill to rough, but i can rough 'the hard way' then finish with a ball mill. It's a step in the right direction... I'll take it & cross my fingers that it gets some additional tool options later.

Thanks!

[dealguy11]

This really seems like a situation where a moulding toolpath might be a better choice. It will automatically generate the roughing pass(es) for you.

[brrian]

I had no idea that the moulding toolpath could do this. I just played with it and it looks like it'll work perfectly. Thank you!!!