I'm machining an iron casting, class 30, in my VMC, 3/4" dia mill 4" loc, yes it's long and I can't go bigger in dia as I need a 3/8 radius in the corners.

Niagara end mill HSS TiN, 4.48 fpm, 360 rpm flood coolant. Tech guy at niagara said go higher in rpm so I tried 636 and the mill sings. Problem is I get a wave in the finish, like it's cutting with a end mill that varies in diameter, About 2" down from the top I get a bluge and at 3" down I get a bulge instead of a flat surface.

hold it ...much worse, I went out to measure the bulges and I also have a .050 taper in the last 1/2" at the bottom, how does just the bottom of the mill spring away?

I did several of these by hand on my index mill, now I have 8 pcs so I'm trying to do it CNC.

Carbide end mill? I was using a plain HSS mill before but it has chips in some edges and leaves lines.

Thank You, Randy

Remove 333 from email address to reply.

Reply to
Loading thread data ...


We need some more info before trying to give you the reasoning of your problem. Are you climb milling or conventional milling like in the manual mill ? (I'm guessing here) What type of spindle is in this machine ? What type of Toolholder are you using (Solid endmill holder or collet)? If collet, what style ER TG etc.) How many flutes does this endmill have? What is the helix angle of the flutes on the endmill? What width of cut (Radial Depth of Cut) is the endmill taking ? I don't know about the higher RPM but if you increase your chipload per tooth it takes care of most chatter due to the tool rubbing instead of cutting. But in the corners you need to slow it down as the corners load the tools with more pressure.

You have to mean IPM Inches per Minute instead of FPM Feet per minute, right ?

Your scenario of 360RPM and 4.48 IPM calculates out to 70SFM and chipload would be around .004 with a 3 flute endmill, .003 with a 4 flute endmill. Cast Iron can be cut with carbide at a higher SFM, like above 500SFM and more depending on material specs and process.

I suspect the cutter is rubbing itself to death. Especially if you are not climb milling. It will rub and rub until the cutter loads enough pressure against the part to begin cutting. This action also work-hardens the material slightly which makes the next flute work even harder. This can progress thru the process multiplying the effect. The rest of the equation can most likely be answered when you give the answers to the questions above.

But if you are using a solid endmill holder, that's not the best situation for keeping the tool from deflecting.

If the spindle is anything less than a CAT50 you asking for trouble as the endmill is sticking out like a lever and then add to that the length of the holder and width of cut and that basically equates into the side load / deflection of the tool which typically results in the appearance you are noticing.

I hope we can help you out.


Reply to

What JR said, and... have you thought of using a bullnose endmill? Say 1

1/4 or 1 1/2 dia.
Reply to

JRWheels wrote:

Cast Iron: is is grey iron?

On any cast iron if you want *economy* roughing, collect the shops old chipped worn carbide 2 flute 3/4" end mills, go to a grinder and break the blade corners about 1/16th" [they may already be slightly chipped] try to get the flat edges as equal as you can eyeball it. This will emulate a bull nose and still cut extremely well. Push them hard for roughing passes. Abuse them, they are not used up yet just because they are no longer perfect for finish work. Candidates for these end mills may be the ones that leave those ugly little streaks when side cutting, streaks mean nothing in roughing. Use good tools for work that need to be "pretty" but make your company some money and get in there and hog off that excess. I prefer using older shop worn tools like this over high dollar insert cutters for roughing. Drown the tool in coolant but push them hard in CI! If nobody is complaining about the noise you may be running too slow. The feed rate should be fast, if you get chatter, you are either taking a too light cut or feeding too slow. You would be surprised at how much CI a 2 flute carbide will remove successfully when the rpm's and feedrates are matched well. Again, the CI's Brinnell can keep the whole show from running at peak material removal rates, also the cleaning of the parts when they reach the finishing room is also important. Extra sand and "burn in" on finished castings as well as chilled edges and interrupted cuts on CI can be tool killers as well. Chill, too much sand and burn in will kill a huge insert cutter and get real expensive fast. It is easy to blow the whole end off a big insert mill in crappy CI castings. But if you have nice clean parts, push it, flood it, they will run!

Reply to

Try ZCarb or VariMill type carbide endmills. Very little chatter and in most instances they can rough and finish. We use them all the time for cast iron.

-- Bill

Reply to


With only eight pieces to run I doubt you want to experiment too much with expensive tooling.

Forget the gadfly and go with the recommendations from the other guys that have done it rather than the one who only dreams about it. Pay special attention to Michael for he is an expert, came from a foundry background and knows what he is talking about for he has many years of hands on experience.

Go with the experts and forget the eggspurt, Tom

Michael wrote: snip

Reply to



std helix

.05 on ruff passes with a roughing end mill, .01 left for finish

Seems to be the case. at .003 fpt I get no chatter, When I followed the tech guys advice and upped the speed without changing FPM I got chatter.

I fixed this problem from the last time by running a boring bar in an ER32 collet down the corners to releive them first.

4.48 IPM

You lost me, grind the whole lenght of flute so it has zero rake angle? or just chamfer the corner? I do have the depth programmed at 4.020" so the corner is not being used. A bull nose just has the ends radiused.

Problem is I have no carbide end mills that long, just the old HSS one I used on the manula mill and the new TiN coated one. I can't even find a 3/4 x 4 carbide mill in MSC or J&L supply. Niagara does say they make one, they have a distributor in Philly that I would need to call and order it.

Thanks for all replies. Randy Thank You, Randy

Remove 333 from email address to reply.

Reply to

You could try depth cuts. Try a rough and finish cut 1/2 in. or so deep. Play with the feed and speed at that depth until you get it good. Then repeat the 1/2 in. depth cuts until you get to the bottom. 4 flutes bend less then 2.

Reply to

Just a small hint from the "old farts like simple answers" department. If you did these successfully on your manual mill, with the same cutters and the same basic process, then maybe there's nothing wrong with the cutters or the process. Maybe you've got a machine problem, rather than a machining problem. That could include the VMC itself, or anything else that goes along with it. Workholding methods? Toolholding methods? Speeds and feeds that are significantly different from the manual operation, just because you thought the CNC could do more or better?

Did you suck the cutter up nice and tight in an R8 collet on the Index mill, and then hang it out a foot and a half with a 40 taper holder and a set-screw, when you switched to the CNC? Did you just accept slow cutting on the manual mill, and then try to go faster on the CNC? Have you tried duplicating the manual process with the same cutter, workholding, and the (approximate) speeds and feeds, that the CNC is now set up for?

If the effects are different from what they were before, then you can bet your left ear that the causes are different, too. Look at the causes that have changed - either intentionally or incidentally - and you'll no doubt find the source of your problems.

Machining isn't rocket science. It's the careful, sequential, methodical application of some very simple and basic principles.

Come to think of it, maybe rocket science should be more like machining, instead of the other way around.


Reply to
Kirk Gordon

instead of the other way around.

Still sitting in my .sig collection...

"Hell, rocket science isn't even rocket science. A NASA Rocket Scientist; Undernet; circa 1996"


Reply to
Black Dragon

application of some

An additional thought -- in the production environment we sometimes get so focused on maximizing production we forget that the objective is to maximize profit.

Given the small number of pieces you have to machine, it may well be that you are better off reducing the feeds/speeds, etc. and accepting a slightly longer floor to floor piece part time.

Other expedients could be using a honking big roughing cutter with large nose radius to remove the bulk of the material and a pristine 3/8 em with sharp corners [your customer wants/needs stress risers in his product?] for the finish cut.

While cast iron is generally machined "dry" you may need coolant to flush the chips out of / away from the cut. Be advised/reminded that cast iron "fines" [dust & chips] are flammable, and are used in sparklers.

Unka George (George McDuffee)

There is something to be said for government by a great aristocracy which has furnished leaders to the nation in peace and war for generations; even a democrat like myself must admit this. But there is absolutely nothing to be said for government by a plutocracy, for government by men very powerful in certain lines and gifted with the "money touch," but with ideals which in their essence are merely those of so many glorified pawnbrokers.

Theodore Roosevelt (1858-1919), U.S. Republican (later Progressive) politician, president. Letter, 15 Nov. 1913.

Reply to
F. George McDuffee

seems to be in the casting, the previous casting were really nice, this lot has a lot of porosity. I ran a 1" 4fl at 320 rpm and 4.48 ipm across the bottom and it came out real nice, flat and square. next I might try the 1/2" depth cuts. Or i will do the inside with the 1" mill then finish out the corners with the 3/4" just to nip off the little bit left.

Now it's off to manual turning on the lathe. Reprogram tonight and try again Sat or Mon.

you did these

process, then maybe

machine problem, rather

that goes along with

significantly different

mill, and then hang it

to the CNC? Did you

CNC? Have you tried

(approximate) speeds and

your left ear that the

intentionally or

application of some

instead of the other

Thank You, Randy

Remove 333 from email address to reply.

Reply to

J&L has two listed that I see:

formatting link
or if that link goes dead:
formatting link
They're a little pricey! ~$300 ea.


Reply to

All I see there is 2-1/4" loc If you go to the catalog page they do have 1 with a 3" loc. But no 4" 'ers

I deal with a local co. here by the name of Alfred Maser Co. they are checking on the Niagra end mill for me.

Thank You, Randy

Remove 333 from email address to reply.

Reply to

My bad. I overlooked the loc requirement completely. Guess I was running on empty when I fired this one off...


Reply to

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.