Official Luthiers Forum!

Y'all,

In the course of making my guitar bodies, I need to "hog out" a lot of material.


Inside of the front body-half of the Heresy 2 acoustic.

In the interest of optimizing this process (i.e., minimizing machining time, while not jeopardizing cutter life), just wondering what some of your thoughts are.

The image below tries to capture the key ingredients of the issue, at least as I see it.



In essence, the key issue is the purple area, the "area of engagement" of the cutter, as it plows into un-machined wood... multiplied by the speed at which you plow.

On one hand, for a given RPM, you could maximize the feed rate (the speed at which the cutter is moving), but cut back on say, the depth of cut and / or step over. On the other (for example) you could go with a monstrous depth of cut, medium step over, and very slow feed rate.
Yes, you can calculate out which approach will take the least time, but I also don't want to abuse the spindle nor the cutter.

Part of me feels that, in order to get the most use out of your cutter, you should use "fairly deep" depth of cuts, so that you're actually using a good portion of the tool, and not just wearing out the bottom tip.

Also, what are your thoughts about "roughing cutters" vs. standard end mills (for massive hogging-out ops.)


Roughing cutters

Looking forward to your thoughts and opinions.

Thanks a ton,

Jeff
KOZM Guitars
http://kozmguitars.com/index.html

Long time tool & die maker here.... you're going to burn up your cutters, if you ask me. You're going to have to come back with a 2 fluter for a clean-up cut anyway after using these. I mean, is it really taking you so long to do your hog out with a 2 flute end mill? How much time do you need to save? Are you making such a buttload of these that you need to cut production time per unit to make money?

_________________
"Act your age, not your shoe size" - Prince

I personally would probably use a spoil board bit or a large rabbet/dado bit if I were hogging material ..... then the finish bits for the places I couldn't go....

Here is one of the cheaper companies bits...... http://www.amanatool.com/cncroutingdetails/rc-2252.html but Guhdo, Onsrud and a host of others make these bits. (Personally like the ones with more than two inserts. ) Here would be an example of a dado/planer bit. http://www.mikestools.com/852-504-11-CM ... shank.aspx

These bits will cut a lot of material fairly quickly and there are all kinds of configurations...... not sure the size of your router..... If you look around you can possibly find some of these bits on closeout. The thing with the inserts..... cost is low after the initial purchase of the tool. ( you do need fairly good extraction for dust in using these bits and your hold down may have to be changed..... to hold the material... a lot of push on the material itself.... )

Blessings,

Kevin

I use the Vortex roughers (lower helix than what you have pictured) for solid body chambering, roughing hard maple carved tops, and for mahogany necks. On my lighter duty machine they cut like butter at a lower RPM, are very quiet running so I don't have to wear hearing protectors, and in the case of the necks the cut is so aggressive it eliminated some tearout issues without having to specifically pre-cut areas. Their chipbreaker bits also rock and leave an excellent finish.

I also have CAM HSM features which helps a lot with the deep pockets. Generally with HSM I'll start at 2xdiameter doc and nearly max cut feed. I've played around a lot (without HSM which can't be used in some situations) with feeds, speeds, doc and cutter overlap and generally end up with doc=radius, 50% overlap, and feeds per the chipload recommendation. On my little machine the deeper traditional cuts don't sound right even when reducing the feed accordingly. Your Shopsabre should be a much more capable machine so things may be quite different. I think this esoteric stuff has it's place with the lower end machines but I'm not sure it would make sense with a real mill or commercial quality router.

I'll be happy to do an HSM toolpath of your deep chamber if you'd like to see how that looks. Not sure what posting issues might crop up.

This question is covered in detail over on www.cnccookbook.com . There's a lot to consider, heat, tool deflection, horse power, rigidity etc. Cycle time as Chris suggests can be of lower importance if your machine isn't running near full capacity.

Rand I typically don't go deeper than 1X diameter for fear of increasing tear out. Are you cutting a 2X with non-HSM toolpaths too or is this just another benefit of HSM?

This question is covered in detail over on www.cnccookbook.com . There's a lot to consider, heat, tool deflection, horse power, rigidity etc. Cycle time as Chris suggests can be of lower importance if your machine isn't running near full capacity.

Rand I typically don't go deeper than 1X diameter for fear of increasing tear out. Are you cutting a 2X with non-HSM toolpaths too or is this just another benefit of HSM?

Sheldon: The 2x diameter would be HSM only. The sweeping arc movements make the difference. I could go even deeper but usually I need to make 2 passes anyway so I go heavier on the first and lighter on the second. Even after ripping through a deep pocket the bit feels like body temp. You've got a big powerful rigid machine and I'm sure your world is much different.

Using carbide and a full depth cut will maximize tool life, but it takes forever to wear a tool out in wood; it's almost a non-consideration. Two flutes- you don't need any more unless you're cutting steel, though three is nice for slotting in aluminum. Weird edge geometries have no advantage in wood, you just want the edges sharp.

Wood doesn't have much real strategy required in roughing, you just run the cutter as fast and as deep as you can without burning or tearing the part off the fixture. If there's no smoke then you're still on the safe side. The fixture tends to be the issue on full-powered machines, and feed/speed limits are the issue on under-powered machines. The fancy toolpath strategies are there to mitigate issues wood doesn't have, mainly chip evacuation and spindle load balancing, though I suppose there are probably people using under-powered spindles who could benefit. Seems odd to fix the $1000 problem of an underpowered spindle with $15K of software, though!

Finishing is a different problem entirely since, unlike metal, wood cracks and tears.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob - I didn't pay anything additional for HSM, it came in their normal upgrade cycle about 5 years ago. It is their default strategy for pocketing and vertical roughing but it's their own implementation, not the big bucks 3rd party stuff and likely not as good. Makes cutting aluminum tolerable on my underpowered underwhelming machine

Jeff,

-what software are you using? -it makes a difference. what options does your software have?
-what kind of machine are your using? cnc machining center or homebrew router?
-try a coated 2 flute solid carbide. at least Tin/Ticn. a 3 flute will break up tool harmonics much better.
-try a tracing cut at say .062 deep to "pre-score" the pocket edges to help eliminate tearout.
-you've got too much radial engagement in the corners of your smaller pockets, and too much dwell time in them as well. use a smaller diameter cutter and generate the radii. avoid stabbing into the corners using no more then 90 deg of radial contact. it will eliminate chatter and burning. program the tool to get in and out of the corners swiftly. optimizing feedrates in the corners will help as well.

corn cobb roughing cutters:
pretty oldschool. when men in oily aprons sat down with Kerney and Trecker universal mills, sloped on pints of sulphurized oil with a paint brush smoking up the shop, and tried to look busy for the boss, these were in vogue. lots of surface area within those rippley teeth. they require a lot of power and force to get them going properly and leave ugly primary and secondary burrs. ime a lot of metal cutting geometry doesn't work so well with wood.

were this done with mastercam i'd have gone for one of the hsm pocketing routines. helix down to depth and rip it out with a small stepover (like say 10% of cutter dia to start) but constant cutter engagement (the routines are designed for this). as you know everything starts with chip load per tooth driving feedrate. (sfpm * 3.82 / cutter diameter = rpm) then (rpm * desired or mfg suggested chip load * number of cutter teeth) = feedrate in ipm. this will give you a ballpark starting number. i use as a general rule for deeper then 1x diameter in depth of cut, back off on the other parameters by 33%. current thought in the programming community is that full depth but lighter and faster is more effective then slow hogging. in nearly 30 years in the chips i would agree with this.

Most of my roughing is done with a two-flute, 1/2" or larger ball, a depth of 1/2" or more, 4000 rpm (that's max on the Haas TM-3) 80-150 ipm feed rate, and usually no less than 75% stepover. You want to ENGAGE carbide cutters...make big chips.

Those roughing cutters strike me as an unnecessary tool change...and that's about it.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

My general method's what Stuart's talking about. I had 10K RPM to work with last I was in production, so I'd run at 300-400IPM. It seemed like the 1/2" cutters may have been running into FPT issues at the top feeds, but they'd get through if the part was fixtured securely. I preferred the 1/2" cutters for roughing on wood even over my larger solid cutters because it was still way faster than it needed it to be, and if there was a problem with the fixture or the integrity of the blank then the 1/2" cutters didn't throw the debris nearly as hard as larger cutters.

Everything was a million times faster with the big honkin' insert cutter I bought later on, but I can't really recommend spending 500-700 on a cutter that's never going to pay for itself at the production rates most builders work with. Beautiful cuts, shiny even, with razor sharp inserts on cutters 1.5" diameter and up at 10K RPM.

On aluminum, I've gotten amazing removal rates from what Arie's describing- full depth, shallow horizontal engagement. I got the spindle on the Fadal up to full load with a 1/2" cutter on aluminum and only needed light mist coolant...the thing threw off big solid chips that looked like single, curled leaves an inch and a half long.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

What is this insert cutter that you speak of Bob? I've got a 3/4" Glacern but I'm not sure I'd use it for finishing.

It appears they no longer carry it, but my cutter was either 1.375 or 1.5". I sold it with the mill, since it had a shank too big for my new machine.

The 3.5" insert cutter was my pride and joy- it uses 3" tall solid carbide knives like a jointer, and I have shaped ones for special cuts. Also has a shank too big for my new machine, but I had it custom built so I wasn't giving it away!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

So this was a woodworking tool not a insert milling cutter.

This company will make about anything you want in a custom insert bit ...... we have a lot of their tooling and like them a lot...... great quality, most from Germany.

http://www.guhdo.com/router-tooling/cus ... rview.html

Blessings,

Kevin

The big one is a custom tool made for wood, yes. The inserts aren't OTS, they're made by the company that made the cutter (Vexor).

They do stuff similar to what Kevin just posted.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services