CNC Inlay

Facundus Cues

Facundus Cues

AzB Silver Member
Silver Member
When cutting a pocket for an inlay on the cue do you typically:
Have a fixture that shims up either the headstock or tailstock to level out the cue?
Cut the pocket into an unleveled cue where the inlay will end up being thicker on one end than the other? If so I guess you will be cutting air on part of the first couple passes.
Also what size cutter do you typically need for a finish cut to hide rounded corners to the average eye? I see DZ using .020 but I also see cutter down to even .005. I have never seen one in person but I cannot imagine how tiny it is and how many could could snap off in about 30 minutes of playing.
I haven't made it this far yet but I do have the equipment and will start playing around with it soon. Just starting to try and work all of this out in my head.
 
When cutting inlays both methods (shimmed and not shimmed) are used depending on the individual cuemaker's preference. I would say that a .031 cutter is the usual size for cutting most inlay, but the small the cutter the more precision the inlay work that can be done. Also as a rule of thumb the smaller the cutter, the more expensive it is, and easier to break. My suggestion is not to use any cutters smaller than .031 until you have dialed in your technique, as it is quite easy to break these small end mills. You didn't mention if you were going to be using CNC or a manual pantograph. Both can give exceptional results once you get used to the machinery.

Just my thoughts,
Alan

Phelps Custom Cues
 
dafunkdawg said:
When cutting a pocket for an inlay on the cue do you typically:
Have a fixture that shims up either the headstock or tailstock to level out the cue?
Cut the pocket into an unleveled cue where the inlay will end up being thicker on one end than the other? If so I guess you will be cutting air on part of the first couple passes.
Also what size cutter do you typically need for a finish cut to hide rounded corners to the average eye? I see DZ using .020 but I also see cutter down to even .005. I have never seen one in person but I cannot imagine how tiny it is and how many could could snap off in about 30 minutes of playing.
I haven't made it this far yet but I do have the equipment and will start playing around with it soon. Just starting to try and work all of this out in my head.
Click to expand...

I believe that end mills go as small as .002 but, of coarse no one uses them as they are way to expensive, break way to easily and the depth of cut is very minimal. .016 is usually as small as most cuemakers go. Any smaller is not cost effective between the slow speeds needed and the breakage. I usually go no smaller than .032 myself. I design all my inlays around this size.

Dick
 
BIG key is the smaller the cutter the faster and more accurate your spindle and must be. To minimize breakage, a good guide is .031 (18-24,000rpm) .020 (30,000rpm) .015 (36,000rpm) .010 (40,000rpm) .005 and smaller (45,000-80,000rpm)... Also the smaller the cutter the less material (depth) you can take with each pass. When using cutters below .020, taking off a depth of material equal to the cutter diameter per pass is a good rule of thumb. Another good practice is to "hog" out the bulk of the design with a bigger cutter, say .031, and finish the corners by chipping away at the size you require for the inlay.
 
Thanks for the info. I have a cnc router parts pro series 4'x4' machine with a porter cable router that is using the precise bits collets. I have not measures runout but I am afraid that they will not be as good as I need so I may invest in a small spindle like the Wolfgang to mount off to the side. I just finished building a rotary axis for it based on a taig bed and then read about people shimming one end. I figured that a flat cut would work. Next hurdle will be software. In the past I have used vectric software for everything but I do not believe it will do the 4th axis and from what I have read if you are not rotating while cutting that you will end up with the side wall of your inlay pocket not being a true 90 degree in relation to the cue. So looks like I am going to have to learn this Bobcad unless anyone can offer a better solution.
 
Chip load dictates everything. Your game better be tight when your talking about small endmills. .030 is pretty forgiving and you can really have shitty chip load and get decent results while only burning up the endmills. Other than spindle backlash, machine backlash will snap tiny endmills. Your machine and spindle should allow for success with as small .015. Fortunately it has low backlash but crappy resolution. It's motion would be considered jerky/rough if you asked an endmill smaller than 15
 
skins said:
BIG key is the smaller the cutter the faster and more accurate your spindle and must be. To minimize breakage, a good guide is .031 (18-24,000rpm) .020 (30,000rpm) .015 (36,000rpm) .010 (40,000rpm) .005 and smaller (45,000-80,000rpm)... Also the smaller the cutter the less material (depth) you can take with each pass. When using cutters below .020, taking off a depth of material equal to the cutter diameter per pass is a good rule of thumb. Another good practice is to "hog" out the bulk of the design with a bigger cutter, say .031, and finish the corners by chipping away at the size you require for the inlay.
Click to expand...

So what if I don't have spindle that goes 80k
 
I have cut parallel to the center of the cue. Parallel to the surface and even skewed to where I was parallel to nothing on the cue. Have used everything from .125" to .0157".
I am probably the least experienced , most CNC illiterate person on this forum. I have messed up a lot of wood and bits. I even have plans for cues where I am cutting from the inside of the cue out. A CNC is a powerful tool, but unleashing your imagination is the most power tool you have.

I have no Bobcad experience, but if I remember correctly, it doesn't do 4th axis. Unless you buy a very expensive add on.

Larry
 
dafunkdawg said:
Thanks for the info. I have a cnc router parts pro series 4'x4' machine with a porter cable router that is using the precise bits collets. I have not measures runout but I am afraid that they will not be as good as I need so I may invest in a small spindle like the Wolfgang to mount off to the side. I just finished building a rotary axis for it based on a taig bed and then read about people shimming one end. I figured that a flat cut would work. Next hurdle will be software. In the past I have used vectric software for everything but I do not believe it will do the 4th axis and from what I have read if you are not rotating while cutting that you will end up with the side wall of your inlay pocket not being a true 90 degree in relation to the cue. So looks like I am going to have to learn this Bobcad unless anyone can offer a better solution.
Click to expand...

Instead of shimming the end you can buy a offset dead center from Chris Hightower its used in his manual inlay machines and works well,,,I have the Wofgang spindle and it does work well.
 
LGSM3 said:
Chip load dictates everything. Your game better be tight when your talking about small endmills. .030 is pretty forgiving and you can really have shitty chip load and get decent results while only burning up the endmills. Other than spindle backlash, machine backlash will snap tiny endmills. Your machine and spindle should allow for success with as small .015. Fortunately it has low backlash but crappy resolution. It's motion would be considered jerky/rough if you asked an endmill smaller than 15
Click to expand...

An issue I've run into is getting the cutter to take "chips" in certain types of materials. Gummy woods mostly. The nominal speeds and feed rates are not standard in these types of circumstances and have had to "play around" for a useful solution which is not easily obtained.

Any thoughts on that Jake?
 
Yeah I know feeds and speeds are critical and are a lot easier with metals when you have a good starting point that you can find online. Even with that you can go through some bits. It cost me at least $100 to learn how to cut aluminum on my cnc before I realized that the material that I had was garbage and turned into the equivalent of goo no matter how I seemed to cut it. It turned out to be some 50 something series. I bought some 6061 and 6065 and it did not take long after that. I consider it tuition. I am having some serious doubts whether my machine will be up to standards on repeatability and resolution. The advertised resolution is .0015. I have it torn down right now redoing the spoilboard and painting the sides of the gear rack to keep surface rust off. Good old Louisiana is like a rainforest at times.
 
I am now using an offset to approximately level the cue, but sometimes have to do cues that the offset won't fit and I also did them for quite a while with no offset. You can safely cut pockets up to .5 inches wide and still have enough of a side wall on the outside edge to capture the inlay without rotating the cue while cutting. Zero out your Z-axis in the middle of the inlay, and as long as it's not too long (like 5-6" or more), you should be okay (your maximum depth of cut will be determined by the cutting length of the bit you're using). If you go too deep, the shank of the bit will start pushing the cue around. Not good. One end will be shallower than the other, so just cut your inlay to be thicker than the deep end of the pocket. The offset is definitely worth it. Don't worry about tapering the inlay if you can taper the whole thing after the inlays are glued in.

I usually use a 1/16" bit which works for most stuff but have done quite a few with the 1/32" bit. Not as much cutting depth, so I don't go as wide. Mostly small inlays in ringwork and initials/inscriptions.

Bobcad. I've been using 21 which doesn't do 4th axis. It was pretty easy to learn after being shown a few things that weren't very intuitive. We recently upgraded to 28 and it's a total bafflement to me. Very little of the 21 stuff works the same. I'm still trying to wrap my head around varying diameter curves on the bottom of the inlays. It's way more than is needed for what we do. Now I just need to find a tutor for an hour or two to save me weeks of trial and error... If you need any help, need sample programs to play with, or have any questions, feel free to PM.
 
I run 0.015" endmills quite regularly on my Gorton pantograph without breakage. It only goes 18000 rpm. At work I have run 0.010" endmills on a cnc with only 6300 rpm spindle.
It is as Jake said it is all based on chip load. For example 0.0002" chip load at 80000 rpm and 2 flute cutter is 32 inches per min but at 10000 you are only going 4 IPM. Wood is quite forgiving when it comes to spindle speed if you are using sharp positive rake cutters you can actually run quite slow spindle speeds. Just think of a hand plane vs router bit they both can do a very nice job of cutting wood but if you calculate the the actual cutting speed of the material passing over the cutting edge they are drastically different.
 
skins said:
An issue I've run into is getting the cutter to take "chips" in certain types of materials. Gummy woods mostly. The nominal speeds and feed rates are not standard in these types of circumstances and have had to "play around" for a useful solution which is not easily obtained.

Any thoughts on that Jake?
Click to expand...

good question.....actually the same answer with regards to very small cutters. My experience was kind of trial and error, but in general i like to use high feedrates with multiple drops. Ive had much better, cleaner results with making multiple, very shallow cuts. Another trick when doing gummy woods is to program and additional profile reverse of the intial cleanup pass. This will usually either burnish the sidewall or drag the sticky's back inside the pocket. I have seen where guys will do a full drop with a 020-030 endmill when roughing a pocket. The thought of doing that never really occurred to me. I guess it would work fine as long as your feeds and speeds and direction are correct. If there not then i would imagine the endmill is burning up and also pushing the cue around all over the place.

The smaller endmills will work fine at 20-30k rpm but with much slower feedrates and less extreme acceleration. Also like to ramp in if possible as a straight plunge followed by linear move almost always breaks .010 due to no chip clearance.

P.S. i guess you know i was just fukn with you on the 80k spindle
 
Canadian cue said:
I run 0.015" endmills quite regularly on my Gorton pantograph without breakage. It only goes 18000 rpm. At work I have run 0.010" endmills on a cnc with only 6300 rpm spindle.
It is as Jake said it is all based on chip load. For example 0.0002" chip load at 80000 rpm and 2 flute cutter is 32 inches per min but at 10000 you are only going 4 IPM. Wood is quite forgiving when it comes to spindle speed if you are using sharp positive rake cutters you can actually run quite slow spindle speeds. Just think of a hand plane vs router bit they both can do a very nice job of cutting wood but if you calculate the the actual cutting speed of the material passing over the cutting edge they are drastically different.
Click to expand...

i bet thats like watching paint dry...just a cleanup pass i hope? What would that be like 2 ipm with almost invisible engagement!
 
LGSM3 said:
i bet thats like watching paint dry...just a cleanup pass i hope? What would that be like 2 ipm with almost invisible engagement!
Click to expand...

The stuff we do at work is usually into thin shim stock, alum and brass. We have recently invested in a 80000 rpm spindle to speed things up. With the machine spindle at only 6300 rpm I would sometimes let the machine go over night.
 
LGSM3 said:
good question.....actually the same answer with regards to very small cutters. My experience was kind of trial and error, but in general i like to use high feedrates with multiple drops. Ive had much better, cleaner results with making multiple, very shallow cuts. Another trick when doing gummy woods is to program and additional profile reverse of the intial cleanup pass. This will usually either burnish the sidewall or drag the sticky's back inside the pocket. I have seen where guys will do a full drop with a 020-030 endmill when roughing a pocket. The thought of doing that never really occurred to me. I guess it would work fine as long as your feeds and speeds and direction are correct. If there not then i would imagine the endmill is burning up and also pushing the cue around all over the place.

The smaller endmills will work fine at 20-30k rpm but with much slower feedrates and less extreme acceleration. Also like to ramp in if possible as a straight plunge followed by linear move almost always breaks .010 due to no chip clearance.
Click to expand...

With a .031 I usually do passes at .070 deep but have gone single pass in the past with good results but I just like the two passes. It works well even though I know Im putting double dutty on the bottom half of the cutter. I recently had a lot of issues with .020 mills even at, .030 passes, slow feed rates ( 5 ipm ), and 24000rpm... Ramping sounds like a good route to take.

LGSM3 said:
P.S. i guess you know i was just fukn with you on the 80k spindle
Click to expand...

Absolutely.... I deserve it though..:wink:
 
Guys,
This has been one of the most informative threads here in a while.
Thanks very much and keep it coming!
Gary
 
I'm guessing that a standard router isn't getting the job done with these .015 endmills...Tommy D.
 
You must log in or register to reply here.
Back
Top