Best CNC bit for smooth finish for pocketing

Post Reply
mrorange
Posts: 19
Joined: Tue Aug 31, 2021 1:34 pm
Model of CNC Machine: Axiom

Best CNC bit for smooth finish for pocketing

Post by mrorange »

I have about 100 pieces I am about to start making that require a circular, 6" diameter, .5" deep pocket with sharp (not rounded) interior edge. For each one of these my main goal is to limit sanding and obviously get the job done fast.

I have used 1/4" and a 1/2" end mill spiral upcut. Each work ok, but don't give me the same glassy finish I can get with a dish bit (but this has sharp inside edges, so a bowl bit won't work.

Is there something I am missing? would one of these be better?

https://www.toolstoday.com/v-11847-rc-2 ... -4QAvD_BwE

User avatar
AboveCreations
Posts: 32
Joined: Wed Sep 01, 2021 8:56 pm
Model of CNC Machine: Chinese 6040
Location: NC

Re: Best CNC bit for smooth finish for pocketing

Post by AboveCreations »

Without knowing what each tool settings are, I might assume that your pass depth and/or your stepover might be too much for each of the endmill tools you are trying. You could try reducing the pass depth and see if that helps. Another technique I've used is to set the DOC to something like .480 and then either create a finish toolpath with a start depth .480 and the .5 DOC;, or lower the Z0 by .02 and rerun the same toolpath. That Amanda tool bit is mainly for surfacing, which I would only use very small amounts of DOC. Another factor is the type of wood you are carving/cutting. Softer wood like pine will easily create fuzzies and burrs. Again, you could try to reduce the pass depth, or run a finish carve over the last the carve. And what I mean by that is, after the toolpath is done with the .5 DOC, rerun that toolpath with a start depth of .5 and a zero DOC. It should be enough to shave off any fuzzies. Otherwise we would need more information of what you are trying to do. The vcarve file would also really help.

User avatar
adze_cnc
Vectric Apprentice
Posts: 1868
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Best CNC bit for smooth finish for pocketing

Post by adze_cnc »

AboveCreations wrote:
Wed Sep 22, 2021 10:04 am
set the DOC to something like .480 and then either create a finish toolpath with a start depth .480 and the .5 DOC
To original poster: if you use this technique, the start depth is 0.480 but the cut depth should be 0.02 for a total of 0.50 not 0.980 as the above will do.

GEdward
Vectric Craftsman
Posts: 198
Joined: Wed Jul 05, 2017 9:13 pm
Model of CNC Machine: 24 X 36 3 Axis
Location: Ipswich, South Dakota

Re: Best CNC bit for smooth finish for pocketing

Post by GEdward »

Be advised that the cutter you referenced from Toolstoday will not work for plunge cutting. The ramp recommendation for that tool seems a bit long in order to be efficient for pocketing without using a clearance tool first.
Sometimes climb cutting the walls works better because the cutting edge is pulling the fibers into the wall creating shear support. You might also try an end mill with a lower helix angle or down cut end mill.
Also, sharpness is king. I love solid carbide and coated end mills for their longevity, especially in demanding cutting conditions, but bright uncoated HSS wins the day for potential in the sharpness department IMHO. To be fair, I have not experimented with every kind of coating on every available substrate but HSS can be ground very sharp.

If all else fails you could leave enough material for a light cleanup pass, coat the pocket with a quick drying product like shellac or Minwax wood hardener then a final finish pass.

Ed

mrorange
Posts: 19
Joined: Tue Aug 31, 2021 1:34 pm
Model of CNC Machine: Axiom

Re: Best CNC bit for smooth finish for pocketing

Post by mrorange »

Thanks for the replies. I am unfamiliar with HSS bits, I have always just gone with Whiteside carbide bits. I will have to check that out.

I have a few questions:

-I feel like I set everything to climb cut. I know not to do that with a free hand router or on the router table, but why not just always climb cut with CNC.

-What would be a good recommendation for pocketing besides 1/4" and 1/2" end mills? Something like this?
https://www.toolstoday.com/v-5312-45566.html

User avatar
AboveCreations
Posts: 32
Joined: Wed Sep 01, 2021 8:56 pm
Model of CNC Machine: Chinese 6040
Location: NC

Re: Best CNC bit for smooth finish for pocketing

Post by AboveCreations »

adze_cnc wrote:
Wed Sep 22, 2021 3:05 pm
AboveCreations wrote:
Wed Sep 22, 2021 10:04 am
set the DOC to something like .480 and then either create a finish toolpath with a start depth .480 and the .5 DOC
To original poster: if you use this technique, the start depth is 0.480 but the cut depth should be 0.02 for a total of 0.50 not 0.980 as the above will do.
It was suppose to say Start Depth .480 and a DOC .02? Sorry for any confusion.

GEdward
Vectric Craftsman
Posts: 198
Joined: Wed Jul 05, 2017 9:13 pm
Model of CNC Machine: 24 X 36 3 Axis
Location: Ipswich, South Dakota

Re: Best CNC bit for smooth finish for pocketing

Post by GEdward »

The cutting recommendations for that, and the rest of the tools in that family, are that they are designed for very shallow broad cuts. Probably great for surfacing spoil board or as a finish tool to clean up a largely finished pocket.
HSS refers to high speed steel. Almost any manufacturer of end mills has a high speed steel line.
I do not own an Axiom machine but I certainly believe that for the money they are fairly rigid. With that said, 1 1/2 inch diameter tools can put a lot of stress on machines that size. If you wish to improve production times I would first recommend experimenting with your feed rates with tools no larger in diameter than your largest collet for pocket and profile work. I am guessing that you have the spindle option with an ER20 collet which gives you 1/2 in. A 1/2 in. end mill running a 100 inches per minute with the appropriate rpm and depth of cut for the material you are cutting can remove a lot of material in short order. If the machining times are too slow then I would suggest that you increase the cutting diameter incrementally until you get the production rate you desire without overloading your machine.
You may want to check out the Axiom forum for practical advise about how large a tool your machine can comfortably handle.

Ed

User avatar
Rcnewcomb
Vectric Wizard
Posts: 4768
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Best CNC bit for smooth finish for pocketing

Post by Rcnewcomb »

Centurion Tools has a series of FEM (Flat End Mill) bits that are designed for a good bottom finish.

The FEM (flat endmill end) is a cutter to use if you want good finish when cutting with the end of the bit. if you have dado's that require a good finish on the bottom, this is the cutter to use. you can still plunge with this bit, but not as aggressively as you can with a plunge end
- Randall Newcomb
10 fingers in, 10 fingers out
another good day in the shop

User avatar
scottp55
Vectric Wizard
Posts: 4456
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10.5**
Location: Kennebunkport, Maine, US

Re: Best CNC bit for smooth finish for pocketing

Post by scottp55 »

+1 on the Centurion Downshear FEMs.
CENTURION FEM DOWNCUTS 1.jpg

Way back when, my first design for sale was a biz card holder, and that size pocket was a PAIN to sand!!
On Shopbot forum got a recommendation for those bits, and sanding went to virtually zilch:)
Ivy League college was interested, BUT market is locked with extra middlemen:(
Biz card Cherry 1.jpg
I was still screwing material down then, and a newbie not set up for production!
biz card Maple and cherry2.jpg
Had an order from 2 people for 144 each for blanks, but couldn't meet their price point...
AND they were laser people and wanted a lacquer finish?
I barely have room for the wheelchair, never mind a spray room with exhaust...so that ended that.
BUT use those bits when called for...sanding pockets(or anything:) is one of my Least favorite things!!

STILL a Firm adherent to hog with an allowance for depth and size(.01-.02"), and then doing a full depth
smaller stepover skim pass to bring it to full depth and size!

Personal experience only, but ALWAYS ramp those bits into a cut!
Also they like to go fast, so start at much lower RPMs on test cuts, and then work your way up.
Also I had best luck with a conventional cut(and most downshears for that matter).

Test cut...check bit temp, test cut...check bit temp,etc. , and Then cut:)
scott
"When in doubt...Zero it out!"

No idea who, but first saying I learned the Hard Way
scott

Post Reply