Official Luthiers Forum!

Wondering if anyone has a CAM program that will link profile cuts and the ability to remove the entry/exit moves between linked curves so that feed speeds can be changed while retaining movement continuity. I have BC and RhinoCAM and haven't been able to figure out how to to it. I have gone in to the code and manually changed the speeds but it seems like there should be a way to do this. I am trying to slow things down on corner neck/headstock cuts to avoid blowout.
Thanks,
Mike

My controller has acceleration control features that slow it down for corners. Not sure what you are using but perhaps take a look in the controller.

Interesting toolpath with the loopies, not sure I like that. I only profile the headstock sides and the tenon/heel area, the important vertical stuff, and let surfacing take care of the rest. Certainly not going for speed. YMMV

Slowing down at the corners won't necessarily prevent blowouts. What I do which has served me well is to do exactly what you'd do if you were using hand tools - Climb cut any end grain features first and then go back and climb cut long grain. In the end it will add a bit of time but you can pretty much eliminate any chance of blowout this way.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Thanks for the information, I am climb cutting but not addressing the end grain first, I will try that. I am using Mach maybe a CV setting would slow things on any moves greater or less a certain angle, will look.

Where are you having the tearout ? As Andy says splitting it up into separate ops is good. My headstock end is G style, perpendicular to the face, so it can't be final cut via profile. I use a z-level (waterline, horizontal - whatever yours is called) finish surfacing strategy to finally pick that up, last of 7 ops to slowly whittle it down.

I have struggled for the most part at the end of the headstock. I have worked it out with slow successive light climb passes around the headstock working my way in, but wanted to figure out a different way on a new neck shape. Wondering what style flute you all may be using for this portion of your work. I have been using a ball end spiral up-cut but wondering about straight and down cut and also flat vs. round. Thanks again for the information.

What Andy said is good advice, I used that exact approach for avoiding chipping on ebony fretboards in product and also use it on things like headstocks with points.

If you're having substantial top-edge blowout then you can mitigate it by using a ball and doing a few passes successively rolling over the edge. It's a good way to keep sharp corners, and it avoids having to use other options like down-spiral cutters which necessitate more tool changes and stocking more tools. On the plus side, it takes forever and a day to wear out a carbide tool if you're only cutting wood, so it's not like you'll ever have to replace them unless you're running a production shop.

I never used any tools except standard carbide endmills on production on necks until I was using custom insert cutters. I can see how a left hand spiral cutter could help on some operations if you have a tool changer. There was always something else that could be done to mitigate problems without using special tooling.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

One of my necks is similar to yours except for the headstock shape and tenon. It looks like your headstock end is the same angle as your headstock so you are profiling this ? Like a PRS, not like a G ? I like Andy's suggestion of climb cutting across that while you still have some extra stock on the sides for support, before profiling the sides.

My order of operations on the face down is:
1 Planar rough (.5" roughing end mill) set it aside to do the wild thing. True up or toss if excessive
2 Profile the sides of the headstock. Rough then finish cut. (.5" BM uses the sides not the end of the bit)
3 Planar finish the horizontal surface features (.5" BM)
4 Planar finish the more vertical areas of the neck shaft with smaller stepover (.5" BM)
5 Planar finish the headstock blend area smaller stepover different angle of attack (.5" BM)
6 Z-Level finish the headstock end (.25" BM due to minimum radius)

Again my headstock end is perpendicular to the headstock face. I do it last because of the tool change. I used to do what I could with the .5 BM but with the z-finish, tearout wasn't a problem so I eliminated that.

Your work looks good!

We approach the toolpathing a lot different. We use regions for defining the various operations. We typically will draw the regions below the part as shown in our attachments and usually set this for 1/2 of the ball nose that we use. Most times we only use 2 to 3 tools total. We have a large cnc and it is capable of cutting at 1200 IPM but for small parts we usually set it with the ball nose for 600 ipm...... the idea is that it can't accelerate or decelerate anywhere close to these speeds in short distances but we let the machine work all this out. This neck shown usually takes about 30 minutes from start to finish once setup..... but note the time that the software says.

Hope this helps need more information contact us off-site. www.waldronmusic.com

Blessings,

Kevin

There is a setting in Mach 3 on the general config page - something like stop CV on angles > "X" or something like that. I believe I have mine set at 80˚. This will cause the machine to switch to exact stop on a trajectory change in angle of 80˚ or more. i.e., if you set it for 45˚ the angle cut in the part is 135˚.

This also keeps it from rounding corners if your machine has high feedrates but only so so acceleration (like mine does). I can cut at 400ipm but my accel on my X is only 35

But, this still won't solve your problem. Cutting the end grain first will.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

One method of eliminating tearout at the end of a cut is to drill a hole at that location prior to milling the contour. For example, when cutting fretboards, I use the same 1/4" endmill to plunge a hole at the two opposite corners of the fretboard prior to milling the perimeter with the same tool.

I tried a 1/4" compression spiral on headstock end grain recently. The assumption being that a smaller diameter cutter would spend less time cutting perpendicular to the grain. I used 2 or 3 full depth passes with a stopover of .25 mm. It worked pretty well.

Thanks for all the information.

I always suspected the compression cutters might make a mess in the middle, but nice to hear they do an alright job. Totally true about the smaller cutters; you can get a smoother cut overall with larger cutters due to the edge speed but smaller cutters are way less likely to chip out. Before I started ordering my cuts strategically, I used a 1/8" cutter for everything dangerous.



Ain't that the truth! I wasn't expecting such a big difference since it look liked your machine had really high accel for a router in the video I saw. The Fadal (AFTER retrofit) was running a 14 minute program in 15-16 minutes with a programmed feed of 400 IPM, but the pre-retrofit acceleration was less than a third what it was running post-retro. My new machine, a mid-90s industrial router (6000lbs), has a max feed of 300 IPM but the motors are specced so close that it takes the thing a 8-12 inches of run-up to hit that speed! It took 6 hours to run a reported 50 minute program at 120IPM because it was all small features! Can't wait to get some free time to put the linear motors on and see what terrifyingly fast looks like, it's been quite awhile since I've seen regular fast!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob,

We can crank up the accerleration about 3 time faster but cuts/tearouts, tearing the neck off the fixture, and sanding increase ........... easier to let the machine do the work than us sand it manually or have to compensate for extra material especially when we are cutting the 4" tall guitar heels. One problem on the tall hills is breaking the vacuum when the heel height increases and the speed is increased ...... probably double the speed on a low profile neck.... we haven't cut to many electric necks....we've tried to stay out of this market..... to competitive for our liking. (Our machine weighs over 10,000 lbs..... so it takes a lot to move, stop, and start things rolling)

Blessings,

Kevin