Here's a (probably daft) question...

If you only had an endmill and a slotdrill (say both are 10mm dia) which would you use for facing a small block of alu?

I'm asking because I recently read in a book that endmills aren't well suited for facing surfaces - they are designed to cut on their sides. At the moment I only own a few metric endmills. :p

Aside... I was mowing the lawn the other day and could help but think that the mower was just like a vertical mill... Tried both conventional cutting and climb milling but the finish was equally disappointing, too much moss and weeds.

A slot drill is essentially just a 2 flute endmill. I have found that if your machine is trammed in well, endmills work pretty decent at facing as long as you arent too worried about the finish (cut marks).

They both should work about the same.

If you hone the edges of the end mill you can get a great finish. A .015 to .025 Radius with the proper feeds and speeds will work fine.

But is a slotdrill really just a 2 flute endmill? One difference for example is that it can be plunged into the work piece. Surely it's cutting edges are quite different?

The book that I was reading is "Model Engineer's Handbook" by Tubal Cain (3rd edition). The interesting bit is in 5.12 Milling - "If an endmill is used as a facing cutter, even with a very light depth of cut, then the corner may break down and rubbing will result. It is preferable to stone a 45 deg bevel or chamfer on the sharp corner, ensuring that clearance or relief is maintained, and to employ a depth of cut not less than 0.006" even in finishing; more is better."

Later on he mentions that endmills are not suitable for cutting full width slots and that a slot drill should be used.

[Aside - found a similar thread asking what the difference is between these two types of milling cutters: http://www.cnczone.com/forums/showthread.php?t=9088]

Here's the book I'm referring to...

The Radii that I mention are in Inches. Also your book is correct but honing a small Radius is a lot easier than honing a 45 Deg.;)

End mill, slot drill is a lot like kerosene and paraffin

In the states they are all end mills, they are then sub divided into center cutting, non center cutting, each of which can have any number of flutes.

In the UK, maybe elsewhere they seem to separate out 2 flute center cutting end mills into a separate class called slot drills.

Ok, although you did say hone the edge with a radius and he said chamfer the corner... :)

Just to add to the confusion the set of 7 milling cutters that I have are all 2 flute so they could infact be slotdrills rather than endmills but... the receipt definately says endmills! :confused:

Ah Andre' B - just saw your post - that makes sense I guess.

That just leaves the corner thing - why does that need to be rounded and why does that help? I really don't understand how it ends up rubbing instead of cutting when used for facing... :confused:

The prettiest facing finishes usually come from having a cutter wide enough to face in a single pass. For most, that means a flycutter.

You'll get a decent finish out of an endmill. Slot or otherwise won't matter, because a facing job cuts the entire surface, you won't plunge, you will cut from the sides.

For surfacing, I like more flutes as they equate to more "effective" rpm for a given spindle rpm and feedrate. When surfacing, chip clearance is usually not a problem the way it is when you're down in a hole, so you can use 4 or more flutes.

I've heard elsewhere that a slight radius honed into place with a stone will improve the finish. No matter what, you're going to see tracks the width of your cutter, which is usually what people object to cosmetically.

One last point--tram is really important to your surface finish when facing.

Cheers,

BW

Ah Andre' B - just saw your post - that makes sense I guess.

That just leaves the corner thing - why does that need to be rounded and why does that help? I really don't understand how it ends up rubbing instead of cutting when used for facing... :confused:

Look at the End of the End Mill. You will see what appears to be a 90 degree angle which is actually concave if you were to cut it in half.

Here is a pic of an Bull Nose End Mill for reference. This is the edge you will be slightly honing. It is designated with an "R".

Thanks alot for that info, everyone!

My cutters and definately slotdrills, they cutting edges join up in the middle so it would appear to be centre cutting (although never tried it!)

Found a neat pic showing both styles of cutters - mine are like the ones 2nd row down and bottom row.

http://www.finelinehair.com/home/End_mill_set_20.jpg

I've been googling around looking for machining info and found a few websites to share:

http://machine-tools.netfirms.com/index.htm

http://www.frets.com/HomeShopTech/hstpages.html

http://www.finelinehair.com/home/index.htm

BW - your website's one of my faves too! :)

http://www.cnccookbook.com/

That just leaves the corner thing - why does that need to be rounded and why does that help? I really don't understand how it ends up rubbing instead of cutting when used for facing... :confused:

If you think of the theoretically perfect sharp corner it is just one atom of material with very little support. when it starts cutting it wears away very quickly. If you put a corner radius on the end mill then the cutting edge looks more like a knife and there is a lot more support for that edge so it holds up better. Also the heat created by the cut can flow into the body of the end mill faster so the very cutting edge runs a bit cooler. With HSS the hotter the edge the faster it will wear, this is not always true of modern coated carbide, some of those coating need to be run hot before the chemistry starts working.

My cutters and definately slotdrills, they cutting edges join up in the middle so it would appear to be centre cutting (although never tried it!)

BW - your website's one of my faves too! :)



Those are 2 and 4 Flute EndMills, not Slot Drills, LOL.:)

There is one type of endmill that is called a MillDrill. You can find them in this link. They are not to be used for drilling steel but you can Slot, Groove, Drill, and Mill with them.
http://www.harveytool.com/products/product_detail.php?product_id=15400-C3&category_id=1&product_family=Drill%2FEnd+Mills

BTW: Who's website are you referring too?:confused:

[QUOTE=tobyaxis;616333]Those are 2 and 4 Flute EndMills, not Slot Drills, LOL.:)

Hey Tobe,
Down-under, and the UK use the term "Slot Drill"

Priciple behind it is they slot and they do drill ( hard to believe someone came up with that one )
and the difference in slotting is the cutting flute is deeper to allow chip evacuation when doing full width cuts. BUT they only run 1/2 the feedrate of a 4 flute

you guys use the 2 flute endmill term

[QUOTE=tobyaxis;616333]Those are 2 and 4 Flute EndMills, not Slot Drills, LOL.:)

Hey Tobe,
Down-under, and the UK use the term "Slot Drill"

Priciple behind it is they slot and they do drill ( hard to believe someone came up with that one )
and the difference in slotting is the cutting flute is deeper to allow chip evacuation when doing full width cuts. BUT they only run 1/2 the feedrate of a 4 flute

you guys use the 2 flute endmill term

LOL, that explains it. Different terms in different parts of the world. I will try to keep this in mind.

Thanks:)

I'm getting the hang of this - you say potato, i say tomato... :argue:

tobyaxis - I was referring to BobWarfield's website - http://www.cnccookbook.com

I follow your explanation that a rounded corner is better suited for facing as it won't wear down so quick...

Thinking some more - I guess if used for facing the endmill corner would spend 1/2 of it's revolution rubbing and the other 1/2 cutting (if cutting full diameter) but normally the endmill corner doing it's day job of profiling (as per it's job spec) it would spend 1/6 of a rev rubbing and 1/6 cutting, the remainder 2/3 are spent cutting air (if cutting 1/4 diameter as per the book's suggestion) so it's not likely to be getting too hot.

I had a look at the cutter you linked - looks interesting but noticed they don't recommend it for drilling...

http://www.harveytool.com/uploads/products/images/15400-C3_pic.jpg

http://www.harveytool.com/uploads/products/detail_graphics/drillmill_endview_15400_copy2.jpg

I'm getting the hang of this - you say potato, i say tomato... :argue:

tobyaxis - I was referring to BobWarfield's website - http://www.cnccookbook.com

I follow your explanation that a rounded corner is better suited for facing as it won't wear down so quick...

Thinking some more - I guess if used for facing the endmill corner would spend 1/2 of it's revolution rubbing and the other 1/2 cutting (if cutting full diameter) but normally the endmill corner doing it's day job of profiling (as per it's job spec) it would spend 1/6 of a rev rubbing and 1/6 cutting, the remainder 2/3 are spent cutting air (if cutting 1/4 diameter as per the book's suggestion) so it's not likely to be getting too hot.

I had a look at the cutter you linked - looks interesting but noticed they don't recommend it for drilling...



LOL, a 60 degree drill isn't the best for actual drilling, but a 90 degree Mill Drill I drive at 48 IPM @ 8000 RPM for Spot Locations all day. Then call it again for breaking edges. The goal is to make $$$$;)

OK, you guys want to know how the big boys do it ?

To get great facing finishes, think what a sharp corner cutter would give when facing ( to get a good finish F=0.01/0.02mm per tooth - slow huh ), now use the same speed/feed for a cutter with R8 on the corners ( the surface would be a mirror ), now speed this cutter up to get the same good finish as the sharp cutter- you are now looking at a feedrate up around the 0.5 to 1mm per tooth----if you were the boss, what one would he pick.

These are for facing or floor finishing methods

All roughing tooling tends to be Al inserts ( extra sharp and uncoated )
Endmills Roughing---R3mm corner radius, max RPM, F.2/tooth,DOC=3mm leave 0.2mm sidesand 0.5mm floors ( use "slotdrill" type cutters in deep pockets to get chips out ) ( there's that bloody "2 flute center cutting endmill" again )
Endmills Finishing floors---R1.5mm minimum ( aerospace spec. ) benefits are extra security in keeping the corner, improved surface finishes, if zig-zagging across the face any mis-matches because of cutter flex or machine sloppiness is blended out

Facing
Roughing Large Faces---80mm Base dia. Octo Facemill-6 tip-Al inserts- S6000, F0.15mm/tooth(F5400.), DOC=2mm, step over 60% -80%, leave 0.5mm for finishing
Finishing Large Faces---same cutter, S6000, F.10/tooth (F3600.), DOC=0.5, step over 50%
80mm Iscar Octo Facemill (http://www.iscar.com/Ecat/familyHDR.asp/r/I/relation/TI/cat/3101045/fnum/132/mapp/ML/app/60/GFSTYP/M/tool/I/type/2/lang/EN)
using smaller tools---50mm, 32mm or 25mm with R3 tips, max RPM, F.1/tooth, DOC 2mm > 80% width of cut, DOC up to 6mm < 30% width of cut
50mm iscar (http://www.iscar.com/Ecat/familyhdr.asp/r/I/relation/TI/fnum/2684/mapp/ML/app/61/GFSTYP/M/tool/I/type/4/lang/EN)

Benefits for using octo facemill - 45 degree cutting edge, the cutting forces are transmitted 90 degrees to the cutting angle, so instead of pushing the cutter back towards the start of cut bending the tool out of the spindle , the forces now go up the Z-axis towards the taper spindle forcing the tool to seat harder---result= less horsepower needed to drive the tool, more stable and faster cutting action, deeper DOC is permitted.

Thanks Superman - one day I might understand what you just said... the picture told me what I needed though - they look expensive! :D

I'm not keen on fly cutters - I don't think they do the spindle gears much good so I'll carry on with the slotdrill/endmill thing for facing and perhaps eventually splash out some dough for a facemill, perhaps like one of these:

http://www.chronos.ltd.uk/acatalog/Glanze_Gace_Mill_Cutter_System.html

If anyone has an ideas for face cutting without spending big money, please share! :)

Rough off to within a few thou of the finished surface using an endmill (or slot drill :)) then finish with a flycutter taking off a very small cut. Don't worry about it being hard on the gears it will be working at a very low load.

NN, those Glanze facemills don't look too bad. At least they're not using those crappy TPG inserts. The knock off imports keep getting better it looks like, which is great for the budget!

I like the APKT inserts. There are now razor sharp versions for aluminum. I just picked up an Iscar HM90 (Helimill) face mill that uses the same APKT insert size as my 5/8" Helimill indexable endmill.

The main thing on these facemills is that they use a good insert type like APKT and they have plenty of positive rake. It's really hard to tell what's going on with something like the Glanze's--they don't tell you much. For example, it looks to my eye like the 50mm on that page has more positive rake than the 63mm, but its probably just the picture. This rake I refer to is how far laid back the insert is. If it stands vertically, it has 0 rake.

With the name brands like Iscar, you can just read the specs and choose the cutters that are intended for small mills. They'll even tell you how much rake the cutter has, typically.

Such cutters are expensive to buy new from suppliers, but you can always find deals on eBay in my experience and get them for half price. At that point they're very close to what you pay for the knock offs.

Trying to figure out the zillion different inserts is a real pain. I look at 3 things:

- Do I see these inserts used by a lot of different brands? My first face mill was great, but used expensive inserts proprietary to that brand. What seemed a great deal on eBay was expensive to keep in inserts!

- Are they available cheaply on eBay from lots of suppliers? BTW, there are knock off inserts too. Most are lousy. You want name brands in the grades (i.e. intended for the materials you want to cut) you need.

- Last is I prefer if every cutter doesn't use a different insert type. Hence I bought a facemill that matches my endmill's cutters.

With all that said, the fly cutter will leave a finer finish if set up properly. Use the facemill to get down to nearly the right depth and then finish it with a flycutter if the finish matters.

I've got one of Widgitmaster's mini-routers and it is a gleaming work of art because of his flycutter work. Don't be afraid it'll harm you mill's gears as Geof says.

Cheers,

BW

Thanks folks - your advice appreciated. :)

Good info given about fly cutting - so they're cheap, give a good finish and don't wreck your mill if used for shallow cuts - sounds like my next purchase!

BobW - your comment about tools that use well made and commonly available inserts makes plenty sense. I guess I'll hold off buying index tooling until I've learnt something about the variety of inserts...

A while back I bought a set of (cheap) lathe tools with triangle carbide inserts, the cutting edge seem to chip easily - at this stage I'm not sure if they're cheap & nasty or if it's something I was doing wrong... am thinking of getting back to basics and trying to grind my own HSS tools. Have been reading "Tool and Cutter Sharpening", learning about rake and clearance angles - just need to get/make a grinding tool rest! :D

.... am thinking of getting back to basics and trying to grind my own HSS tools. Have been reading "Tool and Cutter Sharpening", learning about rake and clearance angles - just need to get/make a grinding tool rest! :D

Real men have strong fingers and stiff wrists and don't need a tool rest. :D

Seriously; develop the ability/technique to grind freehand and it will stand you in good stead. It is difficult to impossible to grind top rake on a tool for aluminum using a rest and sharpening drills is a hands only process.

A thing to remember about grinding tool bits is that you do not need to hog into, just have the tool float into the grinding wheel. You may need to do a bit of reading on what wheels to use and get hold of a wheel dresser so you can clean up a glazed wheel and square the periphery and corners; for this a rest is needed.

Those cheap triangular inserts that are commonly available are not too good. I like CCMT lathe tooling a lot better.

Best,

BW

Just found a thread about inserts - looks like a good place to start the quest: http://www.cnczone.com/forums/showthread.php?t=54153

The triangle inserts on my lathe tools don't seem to have any rake other than that formed by the channel (chip breaker?) running close and parallel to the cutting edge. Is that normal? The insert sides have relief though.

Meanwhile... no doubt you guys are gonna get fed up with me going on about what the various books say but... the author of the sharpening book suggests that attempting to grind freehand is totally inadequate but does say that sharp cutters with the wrong angles will do a much better job than blunt cutters with optimal angles. He must have weak fingers and wrists! :D

Talking of angles, why do boring bars with inserts seem to have negative rake?

Just a bit of side info on inserts

If you look at rotating cutting tools , observe the method that holds the insert in place 99.999% of all inserts have a screw mount

Lathe inserts are usable in milling cutters, but the available grades of carbide will differ, lathe use constant pressure on the tip, milling machine are intermittant cutting, they can handle the shock of entering / exiting the cut better

And for your safety ( general rule of thumb ) ( on open guarded machines )
never use tip tools where the insert is not secured by a screw thru it's guts

I've seen what damage a tip slipping out of a wedge or top-clamp style facemill, running at 8,000 RPM, can do.

Just found a thread about inserts - looks like a good place to start the quest: http://www.cnczone.com/forums/showthread.php?t=54153

The triangle inserts on my lathe tools don't seem to have any rake other than that formed by the channel (chip breaker?) running close and parallel to the cutting edge. Is that normal? The insert sides have relief though.

I have to second the CCMT insert for small hobby lathes, you can get many different grades and styes of inserts in that size.
I have a 6" Atlas/Craftsman lathe got tired of playing with the lantern style tool holder so I made up a tool block that mounts where the compound slide does and got a 7 piece set of 1/2 tools from Micro 100. http://www.micro100.com/ page 9 in the M100Dex pdf. Loose the compound but it was always in the way anyway and it only takes a few seconds to switch back.


Meanwhile... no doubt you guys are gonna get fed up with me going on about what the various books say but... the author of the sharpening book suggests that attempting to grind freehand is totally inadequate but does say that sharp cutters with the wrong angles will do a much better job than blunt cutters with optimal angles. He must have weak fingers and wrists! :D

Talking of angles, why do boring bars with inserts seem to have negative rake?

That author obvsley did not study under the same high school shop instructor I did.

Not sure if these are available on you side of the water but they have a nice selection of small boring bars look in the Everede Tool Co. catalog download is about 3 meg.
http://www.everede.net/literature.htm
The bars start about page 20.

....Talking of angles, why do boring bars with inserts seem to have negative rake?

Don't take any notice of people who write books; them that can, do; them that can't, write books. :)

Maybe not always correct but sometimes uncomfortably close. All I can say is I must have used a lot of 'inadequate' tools in my life.

To answer the boring bar question; negative rake cutters are be less prone to chatter than positive rake; important with a long skinny boring bar.

Don't take any notice of people who write books; them that can, do; them that can't, write books. :)

Maybe not always correct but sometimes uncomfortably close. All I can say is I must have used a lot of 'inadequate' tools in my life.

LOL that is the truth:D those that can't either write books or become critics.:)

Don't take any notice of people who write books; them that can, do; them that can't, write books. :)


LOL that is the truth:D those that can't either write books or become critics.:)

Oh, maybe a harsh judgement (nuts) but I'm not in a position to judge! Assume it's really just because there's so many different right ways to do the same thing and people's experiences and perceptions will differ. :)

I'll keep the suggestion of a writing career in my mind if this swarf making thing proves to be tricky! :)

Thanks for all the advice and links folks, will be taking a closer look at CCMT tools.

For the lathe I just need to get myself a good general purpose cutter (knife tool or roughing tool?) for steel and perhaps another one for alu/plastic and brass. It was a bad idea to buy that set of triangle insert cheapies. I'll probably end up getting a CCMT tool for steel and grind some HSS tools for alu/plastic and brass. Comments welcome... what has proved to be your best cutters for small lathes?

Harsh? You ain't seen nothing yet.:)

For small lathes really the best approach initially is to use HSS tools. For machining mild steel, brass, aluminum and plastics you do not have to use carbide and on a small machine you often do not have the power and rigidity to take full advantage of carbide.

Also using HSS forces you to learn how to grin a tool and which gives a good appreciation of how tools work.

When you do move on to carbide get the brazed carbide bits which are available in various shapes.

For small lathes really the best approach initially is to use HSS tools. For machining mild steel, brass, aluminum and plastics you do not have to use carbide and on a small machine you often do not have the power and rigidity to take full advantage of carbide.

I won't argue that it is a good idea to know how to grind and use HSS tooling. But as for small lathes not having the power or rigidity for carbide--all small lathes are not created equal and that wive's tale has gone on for far too long.

Lathes smaller than the 9x20's, it wouldn't surprise me to learn can't hack carbide. The ubiquitous 9x20 itself is also well known for a severe lack of rigidity. But there are a lot of other smaller lathes that work great with carbide.

With the right inserts, my Lathemaster 9x30 has always done extremely well with carbide. The newer heftier machines like the Grizzly G0602 like Hoss has, likewise.

There is quite a lot of data about using carbide with small lathes on my web page here, including what inserts to use:

http://www.cnccookbook.com/CCLatheSurfaceFinish.html

There are quite a few things I like to use HSS for, but they are mostly things I can't do with carbide anyway, like custom form tools.

The thing to keep in mind is that carbide is not just a function of your machine, it is a set of skills just like HSS. If you have the wrong inserts, or you baby things too much on feeds and speeds, your results will be poor. Like anything, it takes some experience to make it work well for you.

Cheers,

BW

You are correct Bob; you didn't read the 'often' and I did say 'full' advantage because I doubt many small hobby machines have the ability to do that. I also prefer to encourage novices to go with HSS because: 1, It imposes the discipline of learning to grind tools and what the different clearance and rake angle mean, and, 2, it reduces the frustration factor because when you feed a HSS tool jerkily or accidently plunge in too deep the tool will probably survive whereas carbide is almost certain to chip.

It was a bad idea to buy that set of triangle insert cheapies. I'll probably end up getting a CCMT tool for steel and grind some HSS tools for alu/plastic and brass. Comments welcome... what has proved to be your best cutters for small lathes?

Not all bad you get the right inserts and you will have better luck with them.
Here is what you want for aluminum/brass etc. uncoated, polished, and very sharp. It is what is in the turning tool in my pic above. Likely find them all over ebay.
http://www.usshoptools.com/current_year/all_products/2007_08_pdf/PGS_373.pdf

And you can get indexable HSS inserts.
https://www.travers.com/htdocs/pdf/0444cat.pdf

But I agree with Geof in that it is a good idea to learn how to grind a basic tool.

First cutting tool I made was a boring bar, I was about 13 and dad just picked up a 9" SB lathe cheap at an auction, it came with very few cutting tools and I needed to bore a hole out. Hacksawed the head off a railroad spike, welded a chuck of HSS to the end and ground on it until it looked somthing like the picture in the manual. It cut ok and got the job done.

I believe Geof's signature says it a lot when it comes to machining.:)

"An open mind is a virtue...so long as all the common sense has not leaked out. "

Thanks for all the advice on lathe tools - I'm going to have a play with grinding some HSS tools - it'll be a good learning exercise. :)

BTW - took some measurements and it looks like my cheap cutters use TCMT21.52 inserts.

Just thought I'd add this video to the thread since it's related to face milling and seems educational:

YouTube - Cutting Tool Design

Per the video, unless you have a really stout mill or lathe, always go with positive rake tooling. The lower cutting forces will be easier for your machine to deal with. The only advantage to negative rake is longer insert life.

Good video, not too complicated but explains things well.

Bod is correct about negative rake on smaller machines it may not be suitable. On big machines with plenty of rigidity and power it is fantastic for taking fast heavy cuts on ferrous alloy but not really applicable to aluminum alloys.