Feeds and speeds for very small Router bits

This section is for useful tips and tricks for Aspire
Wallycarve
Posts: 14
Joined: Wed Aug 13, 2014 5:12 am
Model of CNC Machine: Shark HD 2.0

Feeds and speeds for very small Router bits

Post by Wallycarve »

Recently I purchased some very small bits for my Shark 2.0 HD from Rockler, I called Rockler Customer Service to get some idea of factory recommended feeds and RPM but they were of no help.
I realized that these bits (0.25mm and 0.5mm) resembled dental drills, and dental drills run 250,000 to 420,000 RPM !!!
I want to use these bits for a very fine detail on Basswood and Oak.
I found one website, toolstoday.com and using their information/calculations for wood and
Solid Carbite bits I'm getting unrealistically high RPMs.
For example, 1/32" or 0.313" comes to 262,140 RPM
I sure could use some help understanding this.
What would the proper RPM and Feed rate be so I can enter in the Tool Database for use with these tiny router bits ?
Any practical approach to this would be appreciated.
Wally

User avatar
Adrian
Vectric Archimage
Posts: 10466
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Feeds and speeds for very small Router bits

Post by Adrian »

Personally for bits that small I would start shallow and slow and just experiment as most figures I've seen are for 1/8" and upwards bits. Even with a set of chipload figures it doesn't mean that they would be right for your machine/bit/material combination.

To be honest I'm not sure if you'll get anywhere with bits that small in wood. I've used them in composite plastic materials without problems but I'm not so sure they'll work ok in wood.

Hopefully someone who has direct experience will chime in but I'd still be careful as all machines are different.

Wallycarve
Posts: 14
Joined: Wed Aug 13, 2014 5:12 am
Model of CNC Machine: Shark HD 2.0

Re: Feeds and speeds for very small Router bits

Post by Wallycarve »

Thank you Adrian,
I know what you mean about using these tiny bits on wood.
I'm hoping that with oak there will be a noticeable difference especially around the eyes.
I'm trying to carve portraits of my grandkids.
Wally

User avatar
IslaWW
Vectric Wizard
Posts: 1298
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: The Ultimate Woodworking Machine
Location: Marquette, MI, USA

Re: Feeds and speeds for very small Router bits

Post by IslaWW »

Wally...
Bits that size will require extremely small chipload, my guess would be sub .001"

Lets try for half a thousandth. 2 flute bit @ 15K rpm @ 15ipm = .0005" chipload.
Also... 2 Flute bit @ 20K rpm @ 20ipm also equals .0005 chipload.

That should give you some starting points. You may have to convert feed units to the one you use.
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com

User avatar
Leo
Vectric Wizard
Posts: 3056
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Feeds and speeds for very small Router bits

Post by Leo »

Wally,

I am not the most diplomatic person here - and I say it as I see it - please don't be offended.

In wood - it's not likely that the .25 (.009) cutter is going to do anything for you. You are just going to break it, so - just do it. Doesn't really matter, the speeds and feeds.

In Oak - which is a really course grained wood - bits that small will not really yield anything that fine in detail any way - even if you do get it to work.

If you invest in a 1/32 tapered ball nosed end mill you will get something closer to what you want with a stout and strong tool. Yes they are expensive. BUT - you will be able to do what you want to do - and get results -vs- a less expensive cutter that does nothing for you.

Try the 15 IPM @ 15,000 RPM - maybe it will work - I do not have better advise there except to get the 1/32 tapered ball nosed end mill. I have found them for around $35 each
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

John Murphy
Vectric Wizard
Posts: 676
Joined: Thu Jan 15, 2009 1:08 am
Model of CNC Machine: AXYZ 5010
Location: Maryhill Ontario Canada
Contact:

Re: Feeds and speeds for very small Router bits

Post by John Murphy »

I engrave 304 stainless with a 1/32 solid carbide 4-flute FB stub end at 12000 rpm, 6-ipm and .002 depth of cut. You will have much better tool life if you can ramp into the material. I use a .100" ramp distance. I can get the same endmill (except a ball end) for about $7.00 per cutter. This is a regular end mill and not a tapered.

john

User avatar
Leo
Vectric Wizard
Posts: 3056
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Feeds and speeds for very small Router bits

Post by Leo »

John, I agree with you. When I worked at a very popular and prominent medical manufacturer, we engraved text in 17-4 PH all day long with a 1/32 ball end mill at 15,000 RPM and 5 IPM @ .005 DOC on a horizontal machining center, and we plunged in. I ran the same cutter on a mill-turn machine engraving the same 17-4 at 5,000 RPM and 5 IPM @ .005 DOC and plunge in. The 17-4 is a little tougher to cut than 304. We engraved miles of text that way - so I don't doubt for one minute what you are saying.

In my home shop with my little CNC router that is no where as rigid, I have been successful sometimes and broken many 1/32 straight end mills. I have never had any issue with a 1/32 taper. It is a very strong cutter and well adapter to the home shop and wood cutting. You get the detail of the 1/32 ball nose and the strength of a 1/4 end mill while being able to increase feedrate. I can run over 100 IPM without worry of breaking a delicate tool. At 6 or 20 IPM - 3D cutting of a surface can easily rack up hours of cutting - and still break the cutter.

I agree about the price of cutters and end mills - these tapered cutters are killer expensive. It took me some time to get over the cost part of it.

I don't mean to undermine what you are saying, or to be argumentative - this is just healthy bantering - please don't think of it as badgering
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

joeporter
Vectric Wizard
Posts: 503
Joined: Tue Jul 21, 2009 8:22 pm
Model of CNC Machine: ShopBot Buddy Standard
Location: Marietta, GA.

Re: Feeds and speeds for very small Router bits

Post by joeporter »

Wally, have you looked at Precise Bits? http://www.precisebits.com/products/car ... 250b4f.asp ...joe

John Murphy
Vectric Wizard
Posts: 676
Joined: Thu Jan 15, 2009 1:08 am
Model of CNC Machine: AXYZ 5010
Location: Maryhill Ontario Canada
Contact:

Re: Feeds and speeds for very small Router bits

Post by John Murphy »

Hi Leo.

No offence at all. I think we come from a vary similar background. I spent over 25 years in CNC metal machining, and I've learned that each individual machine has it's own sweet spot. I've seen one cutter work great on a horizontal mill, but be less than productive on a vertical mill. I engrave elevator panels from time to time, and I've found my sweet spot for my machine.

There are so many factors to consider when figuring out proper feeds and speeds, but the definitive numbers come from how well it's works on the machine in front of you.

John

User avatar
Leo
Vectric Wizard
Posts: 3056
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Feeds and speeds for very small Router bits

Post by Leo »

John - very true about the machines.

Yes I do have a substantial number of years in metal cutting, but that is only limited help in wood CNC router cutting.

This world of CNC routers and cutting of materials is one that has humbled me since I started in 2007. It's just not the same world I am used to in metals. Similar, yes - same, no. Slightly different rules apply.

Never-the-less, I am having fun doing stuff I dreamed about for so many years in machining.
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

User avatar
TReischl
Vectric Wizard
Posts: 3568
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Feeds and speeds for very small Router bits

Post by TReischl »

So there I was, owning a 400K dental carving tool with dental burrs and a CNC machine, what could go wrong using them in the CNC?

Not much really. I do not remember what feedrate I used, probably around 10 IPM or some such. The only problem I had was getting a collet that would keep them from creeping out.

I think all this works because those bits are designed to be used in hand held tools. I have had a lot of fun engraving in all sorts of wood with them. Never tried oak because the grain is so prominent carvings tend not to show up very well.
"If you see a good fight, get in it." Dr. Vernon Jones

Larry Stobbs
Vectric Craftsman
Posts: 100
Joined: Tue Apr 07, 2009 2:00 am
Model of CNC Machine: CNC Shark & Axiom
Location: St. Joseph, Missouri

Re: Feeds and speeds for very small Router bits

Post by Larry Stobbs »

I agree with the gentleman that said go to precisebits.com I have been using their small bits for years in my shark and I know somewhere on the site he had a write up on bit speeds and how to calculate. Most of what I make is law enforcement and military emblems but I agree with the person that said some of the really small bits are a waste of your money. The smallest I use is .0313 in diameter and I only use that bit on highly intricate carvings. I don't use oak very often, mainly walnut and cherry and I will tell you that you will find a certain amount of variance even when carving the same type of hard wood. I have had walnut that carved perfectly with one set up and once in a while I get some that is very hard and have to slow my feed rates down. You also don't want to go too slow as you will get heat build up that ruins your bits. Use the reference library at precisebits.com and I think you will find a good starting point. Good luck

User avatar
scottp55
Vectric Wizard
Posts: 3694
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10
Location: Kennebunkport, Maine, US

Re: Feeds and speeds for very small Router bits

Post by scottp55 »

I think Larry meant this article, probably the most helpful to understand I ever read when I started.
http://www.precisebits.com/tutorials/ca ... speeds.htm
scott

Wallycarve
Posts: 14
Joined: Wed Aug 13, 2014 5:12 am
Model of CNC Machine: Shark HD 2.0

Re: Feeds and speeds for very small Router bits

Post by Wallycarve »

Hello Scottp55
Thank you very much for pointing me to precisebits tutorial.
Exactly the kind of information I was looking for.
Wally

Wallycarve
Posts: 14
Joined: Wed Aug 13, 2014 5:12 am
Model of CNC Machine: Shark HD 2.0

Re: Feeds and speeds for very small Router bits

Post by Wallycarve »

Hello Scottp55
As I was reading the ColletCare part, I decided to measure my Bosch Palm/Collet run out
and to my amazement it was huge!
Right at the collet it was .004" and further down it was .010"
so now I know what was eating my small router bits!

Now that I know that, I was wondering if you might have some ideas how to change this?
New collet? New router ? or just forget using tiny bits?
What router/collets combos run truest?
Thank you for your help.
Wally

Post Reply