[louieatienza]

I don't think there's a thread like this anywhere, so I'm starting one. I use a wide assortment of router bits and endmills on my machine, for a variety of tasks. While some bits can be used for different material and purposes, they work optimally when used for the process and materials they were designed for.

Before I begin, here's how I currently sort them all. The packages below show all the spares I keep on hand. These are mostly the smaller bits which get used frequently and are susceptible to breakage.

[louieatienza]

These are not presented in any particular order other than from my larger to smaller bits. These are all 1/2" shank:

First bit is my single flute mortise compression spiral. I use this for most profiling tasks in hardwoods. Having a single flute allows me to run higher spindle speeds, and allow easier chip evacuation. These are called mortise compression because the upcut section is smaller, allowing downcut action on mortises, grooves and dadoes, etc. LMT/Onsrud

Next we have a PCD rougher/finisher. PCD stands for PolyCrystalline Diamond. The edge is serrated, allowing it to break up fibrous and fiber-reinforced material such as G10 Garolite. these bits can last up to 100 times as long as carbide in such material. Normally super expensive, you can find them at deep discount on eBay. LMT/Onsrud (retail: $615(!), ebay: $49)

Third bit is a 2-flute downcut rougher/finishser. The downcut keeps a nice finish on the top surface, and the serrated flutes break up the chips, allowing the bit to cut without excessive force (or allowing higher feedrates). These can also be used for pocketing and mortising, and I use these normally on hardwood and hardwood plywood.

Fourth bit is a wide mortise bit. I use this as a spoilboard surfacing bit, as a dedicated one can run upwards of $200-$400. This cost under $50. Amana

Fifth bit is an insert V-bit, 90 degree. The idea is that since the carbide is not brazed, it can be made of a harder compound, and thus can stay sharper longer. The carbide is also reversible and sharpenable on the flat. As unwieldy as it looks, this bit is actually well-balanced and leaves an excellent finish. And unlike many tipped V-bits, this one comes to an exact point. Amana

Sixth bit is a 1" core-box bit. I use this for general carving and shaping of smooth curvevd surfaces, as this leaves smaller scallops than a smaller bit.

[louieatienza]

On to the smaller bits and endmills:

First group are single-"O"-flute endmills used mainly for aluminum roughing. What's nice about these endmills is that they can be run at higher spindle speeds which could cause multi-flute bits to gall. The two spiral-"O"-flute bits are used mainly for harder aluminum alloys and cast aluminum plate. The slow spiral-"o" flute is used for soft aluminum; the low helix angle allows a chip to form and break off, which helps with normally stringy metals. It is also coated to help prevent edge build-up. The Spiral-O's really get chips out of the way, and are a big help in profile cutting. They leave a good finish, but not as good as a multi-flute bit. There are different types; one with a sharp tip, and one with a "sweeper" tip that leaves a better pocket floor finish. These also work well with brass and plastics. They also cut hardwoods extrememly well, and I use a 1/16" regularly for guitar work. All bits LMT/Onsrud

Next bit is a 1/4" 3-flute aluminum rougher. Like the wood roughers above, the flutes are serrated, which breaks up chips and reduces cutting forces. Destiny Tool

Third bit is a fiberglass burr/router bit. Unlike a conventional burr that abrades, these are actually cross-hatched flutes (14 in all) that cut. Again, for tough material like fiberglass-reinforced Garolite, these chew through the material and wear better than a conventional straight bit. LMT/Onsrud

Fourth pic is a .024" 2-flute endmill that I use for slotting guitar fingerboards. Don't let the delicate look fool you; I run these at 1XD at 60-70ipm! This is actually an aluminum endmill, but the larger flutes normally associated with aluminum endmills makes them work on hardwoods well. Kodiak Cutting Tools

Fifth pic shows two 3-flute aluminum cutting endmills. The left pic is a WIDIA Hanita, and the right is a Niagara. While the Niagara cuts well and leaves a very good finish, the Hanita outperforms it, due to the very highly polished flutes, and asymmetrical flute geometry makes it run smoother. I use 3-flute mainly for finish passes, though they can work well for roughing. I reduce my spindle speed about 30% compared to a 2-flute endmill.

[louieatienza]

This is Amana's InGroove insert signmaking set. Like the V-Bit above, the inserts are a harder carbde grade and can be honed. A nice feature is that when switching cutters, no re-zeroing is necessary. I have quarter round, flat, V, and a couple engraving cutters. They leave crisp edges, even in melamine and plywood. You can engrave aluminum with the V and engraving inserts, but you are depth limited to .005".

[louieatienza]

Two 1/2" straight bit, two purposes. The left is an MDF bit by Onsrud. The right is a general purpose bit by Bosch. As you can see, the Onsrud bit has larger flutes less tip rake, and a larger center clearance area between flutes. The Bosch, made mainly for handheld applications, has smaller clearances which help with kickback. These bits should be ramped or helixed in.

[louieatienza]

The left pic is a 90 degree drill-mill. These can be used for drilling, edging, chamfering, and I use this with OneCNC's hole recognition wizard to drill and chamfer in one step.


On the right, I have 10 Kyocera 1/8" spiral-"O"-flute endmills. These are designed mainly for plastics, but I think they should work for aluminum as well. I got these 10 for $29 on eBay; that's about the cost of a single one from Onsrud.

[LouF]

This is Amana's InGroove insert signmaking set. Like the V-Bit above, the inserts are a harder carbde grade and can be honed. A nice feature is that when switching cutters, no re-zeroing is necessary. I have quarter round, flat, V, and a couple engraving cutters. They leave crisp edges, even in melamine and plywood. You can engrave aluminum with the V and engraving inserts, but you are depth limited to .005".

Louie so you give the thumbs up on the InGroove signmaking set?


Lou

[louieatienza]

Louie so you give the thumbs up on the InGroove signmaking set?


Lou

I am happy with mine, and would recommend it with the caveat that you should find use with all the included inserts. Otherwise it might be better to buy the shank and bits separately.

[aarggh]

Wow! I just saw this thread and what a great load of useful posts! I have a habit of destroying almost anything with a sharp edge, so the helpful and descriptive real life use and comparisons will greatly benefit me! :wave:

cheers,
Ian

[Alleykat]

Thanks for the info,do you have a preference on were to purchase end mills?

[louieatienza]

Thanks for the info,do you have a preference on were to purchase end mills?

For wood I prefer Amana and Onsrud. I will be testing some BamCarbide bits soon. Scour eBay for deals; don't even bother buying Chinese crap. You can find USA and high end import stuff for close to the same price.

For endmills, my favorite supplier for inexpensive ones is Kodiak Cutting Tools, as you can see by the sea of red bit containers. I'm always experimenting on the finish end, and SGS and Hanita seem to give me some of the nicest cuts. You can get SGS (S-Carb) from MSC and Hanita (AluSurf) from Fastenal.

You should keep in mind that while typical bits made for handheld use work fine for CNC, they are rdoc-limited, and cannot (and should not) be fed more aggressively than a CNC bit.

[TrickyCNC]

Thanks for posting Louie

It's a very informative thread for newbies like me !

[mmonti]

Excellent, this is good stuff. Make it a sticky

[TrickyCNC]

this link was posted on another forum... It might be of interest here ...

http://www.vortextool.com/images/chipLoadChart.pdf

[louieatienza]

this link was posted on another forum... It might be of interest here ...

http://www.vortextool.com/images/chipLoadChart.pdf

Pretty good resource. For many DIY machines, it may not be possible to achieve the reccomended feedrates and spindle speeds due to certain factors, but you could still get pretty close to the recommended chipload.

Usually however the chipload is known, and then the feedrate could be calculated for a given spindle speed, derived from the chipload formula:

feedrate = spindle speed X chipload X number of flutes
chipload = feedrate / (spindle speed X number of flutes)

The other useful formula is for SFM, or Surface Feet per Minute. Some manufacturers will list their tooling's capacity in this way, calculated as:

SFM = 3.1416 X RPM X bit diameter / 12

Yet another one is the MRR, or Material Removal Rate, but you'd need the IPT, or Inch Per Tooth feedrate to calculate it:

IPT = feedrate / spindle speed (rpm) / number of flutes

MRR = spindle speed X depth of cut X width of cut x IPT x number of flutes

So for example, in the BMX chain sprocket video above, pocketing the openings between the spokes, my parameters are:

72IPM, .125"aDOC, .035"rDOC, 13,000rpm

My chipload is .0027, SFM = 850, IPT = .0027 and MRR = .315in^3/min

[louieatienza]

Found this online calculator which makes it easier...

Milling Formula Calculator

[Bunbun]

Pretty good resource. For many DIY machines, it may not be possible to achieve the reccomended feedrates and spindle speeds due to certain factors, but you could still get pretty close to the recommended chipload.

Usually however the chipload is known, and then the feedrate could be calculated for a given spindle speed, derived from the chipload formula:

feedrate = spindle speed X chipload X number of flutes
chipload = feedrate / (spindle speed X number of flutes)

The other useful formula is for SFM, or Surface Feet per Minute. Some manufacturers will list their tooling's capacity in this way, calculated as:

SFM = 3.1416 X RPM X bit diameter / 12

Yet another one is the MRR, or Material Removal Rate, but you'd need the IPT, or Inch Per Tooth feedrate to calculate it:

IPT = feedrate / spindle speed (rpm) / number of flutes

MRR = spindle speed X depth of cut X width of cut x IPT x number of flutes

So for example, in the BMX chain sprocket video above, pocketing the openings between the spokes, my parameters are:

72IPM, .125"aDOC, .035"rDOC, 13,000rpm

My chipload is .0027, SFM = 850, IPT = .0027 and MRR = .315in^3/min

Hi I'm quite new with this and trying to play with wood cutting speed and feed.
Per above calculation and Vortex Chipload Chart,
1) What is chip load unit? Is it IPT or unitless?
2) I didn't see DOC in chipload formular. What is suitable DOC? Let say I cut hard wood with 1/4" 2F 12Krpm.

Please advice and thanks in advance.

[louieatienza]

Hi I'm quite new with this and trying to play with wood cutting speed and feed.
Per above calculation and Vortex Chipload Chart,
1) What is chip load unit? Is it IPT or unitless?
2) I didn't see DOC in chipload formular. What is suitable DOC? Let say I cut hard wood with 1/4" 2F 12Krpm.

Please advice and thanks in advance.

Chipload is in inches. DOC is typically 1XD, the diameter of the tool used.

[bimmer525i]

This is some good stuff. thanks guys! should be stickied for sure so i dont have to search the forums again =P

[skylanehku]

Wow thats the best info I've seen for us newbies, thank you for taking the time to post all this info and pictures. I too think it definately should be a "sticky".
Thanks again
Terry