3/4" bowl bit?

[scottp55]

Anyone got a good starting point for a 3/4" SEtools bowl bit? Never used one and all of a sudden tomorrow will probably be doing a bunch in a rush and I only have the one bit. Quality of cut most important. Cutting profile online a 1" right triangle in a vacuum/heat treated ash(torrefied) which cut clean with NO fuzzies because the fibers are so brittle. Feeds,speeds, pass depth suggestions welcome. Was thinking 1.1,.5,14K at .2 depth but guessing. Was going to make it the first toolpath as its on the corner of a pocket and I'm worried about tearout if I cut it second. Going .4" down total

[Brady Watson]

I'm not sure I understand the bit you already have...Is it a 3/4" dia bowl bit, or do you need a 3/4" radius in the bottom edges, or is that 3/4" dia with 3/8" radius at the bottom edges?

If you need a super clean cut, I would do it in several step downs with allowance (like .02-04) and then come back full depth (make it step down fully in one pass) to give everything a nice clean finish with no stepdown/waterline marks.

-B

[scottp55]

Sorry Brady, 3/4" Diameter bowl/tray bit from Southeast tools. Thanks for 2 toolpaths. Not good with anything over 1/4" diameter yet:)

[Brady Watson]

Here's what I would do, if I determined that the bowl bit was not up to the task. I looked at the specs on that bit & it says it has a 1/4" radius. I don't really like tools with brazed on flutes and avoid them if I can use solid carbide. I would be inclined to offset the pocket vector inside 1/4", and hog it out with a 1/2" end mill. That will give you a nice flat bottom, without violating the bottom radiused corners. Then, create 2 inside profile toolpaths using my original vector (not the offset one): One that steps down with a 1/2" ball with .02" allowance, stepping down .19" per pass. Then a cleanup pass, where you set the pass depth on the tool to .4 and clean up that edge in one nice clean pass. This will eliminate any waterline/stepdown marks on the edges & give you that radius at the bottom.

It is *critical* that you Zzero in the exact same spot when you change tools to minimize any chance of a step between the hog out pass with the 2-flute square solid carbide end mill (upcut spiral) and the radiused bottom and edge with the 1/2" 2-flute ball end mill.

If you find the top edges wanting to tear out, start the cut with a downcut, then switch to an upcut. Most downcuts don't give a smooth bottom in some materials, so that is why I suggest the upcut. BUT...I would at the very least try the bowl bit first in a similar material and see how it performs. You may find that if you ramp it in and keep your cut depths shallow, you could get away with 2 pocket toolpaths. The first with .02-.03 allowance, and the 2nd with zero allowance stepping down in one pass .4" deep to clean it all up.

Take that bit and make yourself a 'test area' in the scrap pocket area that is going to be machined away anyway - and use that to gauge if the tool is going to tear out and see how it performs. If it looks OK, carry on with that bit. If it is tearing out at the top, you know you need to run a downcut say .1" deep first, before running that bowl bit. Like any new material, sometimes you have to 'sneak up' on your settings and listen to what the tool and material are telling you. Then adjust as necessary.

-B

[scottp55]

Thanks for all your trouble Brady, will try today. Good idea to try in pocket area 1'st, will save time. Need to try a 1/2" Ballend for a different project soon anyways so will order today. Much appreciation for the detailed toolpathing advice. Ouch! 3:30 and just started planning layout in my head to maximize wood---WITHOUT COFFEE!:eek:

[srwtlc]

Scott,

I use 1-1/4 bowl and tray bits a lot (once it a while the 3/4). I use it for hollowing out covers of badge and gun boxes mostly. I get bottoms that are clean/flat and need very little sanding (usually sized large enough to drop a 1/4 sheet PC sander into). The thing to watch out for with these bits is to find a brand that cuts a flat bottom. I've had some that actually cut a very shallow 'V' and it next to impossible to sand the bottom out on those. I've had very good results with Infinity (http://www.infinitytools.com/Bowl-Tray-Router-Bits/products/1008/) and CMT (http://www.amazon.com/CMT-851-502-11-Router-Cutting-Diameter/dp/B000P4LQ7W/ref=sr_1_2?ie=UTF8&qid=1391618175&sr=8-2&keywords=cmt+851.502.11) (wrong picture). I have them resharpened as needed and they're always right on. I prefer the 1-1/4 diameter ones because the pass overlap or cut width is larger and leaves that much better of a bottom (less pass marks to sand clean).

Now, I know that you have a desktop and can't run as aggressive as I do, but what I've found to give the best finish is to make the pocket with a conventional raster strategy and do the profile pass first with a 0.015-0.020 allowance for a slower higher rpm profile clean up pass. An offset strategy will leave to many cross grain markings and won't sand out as easy. Be sure to ramp in (about 1" works good with the 1-1/4" bit) as these bowl bits can't be plunged straight down much if any at all. With ramping in, I generally cut 0.125" - 0.25 deep per pass at 12000-14000 rpm and 4-5 in/sec (in walnut, maple, cherry, oak). I'll follow this up with a normal profile pass to clean up the edge and apply a shallow curved approach/overlap to the wall. Depending on your final depth, you may have to make the profile pass in two down steps due to the cutting edge length and the tip radius. I generally run this at 1"/sec and 15000-16000 rpm. Gives a nice clean wall. If you have any outside corners in your pocket, be mindful of the grain at that corner and give it a radius if possible.

A warning about hogging the pocket with an endmill first and then doing the wall with the bowl bit, you'll risk large splinters coming off the long grain edges. That's why I do the profile pass first and then raster the pocket. You could do a climb cut, but that won't give as nice of a cut (can get fuzzy depending on material).

[scottp55]

Thanks Brady, Full depth skin pass worked a charm. Scott, You mean THIS groove? Also you see I got the raster info too late- But the good thing is I have to go a hair deeper and will redo toolpaths. Another nice thing is I was just profiling on a line with the bowl bit so it hides any discrepancies in height from pocket to curve and fits the item exactly(Looks like I did it on purpose:) ). Thanks

[Burkhardt]

Please excuse my ignorance...what is the difference between a bowl bit and a corebox bit? Or is it the same thing?

[scottp55]

G. , Brady said mine had 1/4" radius but the bit is 3/4" diameter so it has a flat (SUPPOSED to be:)) bottom and can go much larger stepover. Mine had a little nib dead center-looks like brazing-Like Scott W. said.

[srwtlc]

Yup, poor grind quality (geometry) will do that. Try one of the Infinity ones.

[scottp55]

Thanks Scott, saves me searching and surprises(of the wrong kind),good thing I've got wet diamond wheels from gem carving.

[Brady Watson]

It still irks me with what these tool grinders get away with these days...and many of these bits are not cheap. "Stupid Woodworkers" must be the mantra. Like when they sock it to you when you buy an 'upcut spiral' router bit - stupid woodworkers will pay 3x more than an identically ground solid micrograin carbide end mill.

I'm still ticked that none of these manufacturers have stepped up to the plate with a guaranteed ground angle on 2-flute (or greater) v-bits over 1" in diameter. If anyone of them did that, the money would pour in...

-B

[scottp55]

OK, Thanks to Brady and Scott I tweaked the toolpaths for the bowl bit and the pocketing toolpaths and got an acceptable cut in hard maple, but sadly lacking in larger diameter bits as we don't use them much. Got 1/2" up/down/straights coming from carbide processors just to try out and have on hand for prototyping, BUT if this goes into production the bottleneck is the pocket where it has to meet the bowl profile and cut 2/3's of the pocket with a clean 90 Degree at the bottom. Had to do protos with 1/4" bits as it's all I had on hand. Had tiny tearouts that 3M Bristle discs took out, but it affects the tiny fonts in bottom of pocket.
Gary B. took a VERY preliminary look and said MAYBE a chipbreaker/finisher would be the answer. I looked at the 1/2" prices:eek: Scary to me and don't want experiment at those prices. I also saw Low Helix Finishers which intrigue me, but I don't know ANYTHING about these 2 types of bits.
It's only a Desktop with spindle so not sure how much time this would save me as batches small. Pocket is only 2X3.5X.4" but is half the run time.
Does anyone have pics of sidewall and pocket bottoms done with either an Onsrud 1/2" Chipbreaker/Finisher or a Low Helix/Finisher in a hard maple or similar? What kinds of feed speeds does the finisher like in Maple say?
Don't want to bother Mr. Beckwith until I know more. Sticker shock an 1/2" ballnoses also!:eek:

[Burkhardt]

.....Sticker shock an 1/2" ballnoses also!:eek:

You can get HTC stub length 1/2" ball nose bits (http://www.the-carbide-end-mill-store.com/m5/105-2500--1-2-ball-nose-end-mill-stub-length-htc-105-2500-2-flute-gp-30-uncoated.html) for about $25 and standard length for $32. Obviously more than some of the usual smaller bits but I find it not too bad. End mills about the same price.

[scottp55]

Thanks G., got an inexpensive 3" from MillMonster as it's just for a concept cut for a wood carver who's letting us run the second desktop in a room in his shop. He teaches Acadian style carving classes and seminars and wants to know if we can hog out (1/2" up) and Ball nose (1/2") the majority of the waste so his students can spend the majority of the time developing their detail work.
Like I said concept- may not be what he has in his minds eye. Basswood for that one.