Carving 3d with single pass small cutter

[Eagle55]

I am kind of directing this at Joe, but decided to put it out for even wider coverage of expertise. I read somewhere, and thought it was Joe that might have told me, that they used a small cutter with very small step over rate to do the finish cut pass on 3d figures rather than a roughing cut pass and final finish cut pass. I wanted to verify this and to get a feeling of the results before I break off a 1/16" tapered ball nose bit. LOL I finally got around to setting up some custom tools in my V-Carve database and one of them was the tapered carving bit used on the CarveWright. The task wasn't as hard as I thought it was going to be. I used the following bit specs:

.0625 tip radius
7.13* single side angle
40 inch/min feed rate
10 inch/min plunge rate
8% stepover rate (ie cutting about .010 inch per pass)
1/2" pass depth

I may get enough nerve and desire to try this before I get an answer but would still like to hear of any comparative bit settings and results.

Roger

[sk8nmike]

I've used at 1/16" Taperd ball carving 3/4" of oak and 1/2 in Coran with out a problem.

[GARYR6]

I use an 1/8 ball nose for a single cut on 3d stuff no issues. Remember speed kills. slow it down a bit (75)

[Bob]

I've used at 1/16" Taperd ball carving 3/4" of oak and 1/2 in Coran with out a problem.

With no roughing pass?
If I can get away with it on carvings, I'll give it a try.
Bob

[meb]

I have cut 3d with a 1/16" bit without a roughing pass if the depth of cut is not to great. If the depth of cut is deep you heat up the bit and it will have a tendency the lose it's temper, thus dulling the bit quicker. Also do slow down on the feed rate so the bit has a chance to cut the wood without undue pressure on the bit. Most of the time I do use a roughing pass even though it will not take much waste away just so it is easier on the smaller bit. I have noticed in softer wood that I get a better finish cut if I use a roughing cut first. In harder woods I do not notice any difference.

[sk8nmike]

Cut with a 1/16' tapered bit in 1/2" Coran, No rough cut..

[jeb2cav]

I choose to use a roughing pass on my (wood) projects. I have passed on this if the depth of the carving is minimal, or I'm willing to back off on the speed. I also am experimenting using a larger BN at a higher speed, but setting the Z0 about 0.1 above the 'true' Z0 and running it fast - using a 1/4" BN. Then the 'final cutter' is only running against 0.1 worth of material. For this type of 'roughing' I'm also using a stepover of 20-25%. The whole intent is to do a fast roughing pass.

I've met folks who don't use any roughing pass even on a deep carving. However, they all say that the first pass is the most critical - as the bit is cutting the entire depth and width of the tool. They use the FRO to influence this and crank it down to 30% for example, until a few passes have been made and then return it to the desired speed. Also in this case they are using a small 8-10% stepover.

I think early in your use it's not a bad idea to definitely use a roughing pass - it may help overcome any other sins you may be committing as you learn. In the end, it is what you are comfortable with and know will work - good outcome and undamaged bits.

[sk8nmike]

"Damn the torpedo's Full speed ahead!"

No I agree with Joe, just because it can be done doesn't mean it's always a good idea. Unless you're short of time using a larger bit to rough out is a good idea.

[TDA]

While it is possible to cut full depth it is not recommend for multiple reasons.

First it's easier to break your tooling or in trying to prevent that cutting too slow and missing the sweet spot for your material.

Possibly more important is tool deflection. The deeper you cut per pass the more stress you put on the tool and the machine. This can actually bend the tool and/or the machine deflecting the tool. You can see this in some cases where you plunge or extract the tool (When the machine's not moving the tool is relaxed and in a non-deflected position). Now with varying height and feedrate you get varying deflection which basically causes position of the tip of the tool to shift destroying details or causing misalignment of your carving. The more stress (feed, depth of cut, material, ect) the more deflection.

One easy way of thinking of this (though not completely correct) is as the flute is trying to remove the material it's is being pulled into the material. The deeper the cut the longer the material can "pull" on each flute.