I'm machining a six-throw crankshaft from a 2-1/2" rod (4140 or 1144). My plan is to first turn the mains, and then mill away excess material from the throws before turning the rod journals (I may even rough mill the rod journals on a rotary table) Milling steel has always been a slow process for me, and I would rather not spend hours (or days) doing this. It would either be done on a Bridgeport Series I CNC or a Cinncinatti manual mill. I'm thinking about buying an indexable mill, possibly a 1-1/4", and I'm wondering if this is the right way to go. What's the best tool for fast stock removal? What if I qualify that by limiting the tool cost to around $100?

An 1.25" insert endmill is a large tool. You need quite a bit of power to run it, and quite good clamping on the part to resist the forces.

How long is this crank? Somehow I'm having trouble imagining something with journals over 1.25" wide and a throw of only what.....3/4"?

If you can post a picture of the model, it might give us a better idea of where the tool has to fit, and so on.

Do you have a 4th axis to hold the part? I would find it a daunting task to do much milling of the throws with a manually operated dividing head. I mean you could but it would be about as much fun as milling a circle face up on the table, while cranking X and Y by hand :D

Hu: Thanks for the reply. You wrote:

An 1.25" insert endmill is a large tool. You need quite a bit of
power to run it, and quite good clamping on the part to resist the
forces.

How much horsepower would be enough to cut steel with a 1.25" insert mill? Both of my mills are 2hp. Does that suggest an optimum mill size (or type)? I'm not absolutely hung up on using a 1.25" mill, that just happens to suit one particular part of this job. As to clamping, I have a 6" Kurt vise, among other things. Don't worry about that part of it.

How long is this crank? Somehow I'm having trouble imagining
something with journals over 1.25" wide and a throw of only
what.....3/4"?

The journals are 1.08" across - that's why the 1.25" mill - to plane down the 1.08" disks resulting from turning down the mains first. Good guess on the throw.

If you can post a picture of the model, it might give us a better
idea of where the tool has to fit, and so on.

Picture a 2.5" diameter rod 10" long with 7 grooves .45" wide on 1.53" centers, cut down to the main journal diameter of .875". Next thing is to mill down the disks (almost to the main diameter, to rough form the rod crank webs) as rapidly as possible.

Do you have a 4th axis to hold the part? I would find it a daunting
task to do much milling of the throws with a manually operated
dividing head. I mean you could but it would be about as much fun as
milling a circle face up on the table, while cranking X and Y by hand

Unfortunately, I don't have a 4-axis CNC machine big enough to handle this. That would be nice. I don't like the idea of sitting there cranking a rotary table, but for a one-off thing it's ok. The Series I is a Boss 5, so adding a CNC rotary table would be an interesting challenge. As to milling a circle by cranking X and Y by hand, I did something like that once (more of an ellipse, actually), before I got the CNC mill.

Forget about this particular configuration for a minute. Let's say I had a block of steel, and I wanted to mill it down as quickly as possible with my 2hp mill. What would be the optimum type of mill for this? Just for comparison, what if I had, say, a 5hp mill?

Thanks - Richard

For a 2hp mill even a 3/4" diameter 3 insert tool is pushing it. Depending on what kind of spindle and toolholders you have, you do not want to aggravate chatter issues by using a huge overhanging holder large enough to swallow a 1.25" shank tool, so you would want a reduced shank endmill of some sort.

However, a 3/4" endmill is probably a good size tool to have, as it will fit in tighter situations than just the present job, and that includes situations such as the tool not leaving large corner radii, and not having all that extra travel distance to enter and leave the cut (due to larger tool radius). Probably you can also run a smaller tool at a higher rpm, and still use the same chipload per tooth, and thus use a higher feedrate (if the two tools in comparison have the same number of inserts).

I assume you would want to use an endmill narrow enough to machine the excess away between the flanges for each rod journal.

It might be worth considering building an indexing fixture (for lathe) to hold the work in the various phase angles needed to machine the throws on the lathe. This would involve eccentric turning which is not all that productive, but it does get you a round journal at the end of the procedure.

My guess here would be a 3/4 or 1" mill using APKT style inserts. Positive cutting action and you can get 4 teeth in this small dia. Inserts are kind of expensive though when you consider they only have 2 usable corners and I doubt you can get one for $100 ( usually sell for about $160 -$200).

I Like the Valenite V590 insert endmills. I have used a 1" 3 flute at 3055rpm and 27 IPM on a Haas TM-1 with a 0.100" DOC. and no problems in 1018 steel.
They do make smaller cutters in this series. I know of a 0.750" but I think that they go to 0.625". I Had 1 job that required that I remove 18 pounds of steel in the roughing opp and these cutters made short work of that.

Hu: Thanks again for the reply. My Cincinnati mill is pretty solid, but the largest collet is 1", so no 1.25" shanks, I agree. I've heard that insert mills can be run at high speed, but I assume that will require coolant, right?

Use coolant on the advice of the tool manufacturer. I tend to favour dry roughing with carbide because of thermal shock and early degradation of the cutting edge due to that. It can be very difficult to get coolant flow right into the cutting zone, plus the tool goes into the shadow of the cutter body once per rev, so this is why I cut steels dry with carbide on the mill. On a shielded machine, an air blast is beneficial to keep the chips from accumulating near the cut zone.

I use airblast on steels and coolant on aluminum. The type of material is the limiting factor for RPM or I should say SFM. Aluminum seems to have no limit on RPM as does cutting air.

A band saw is a pretty effective way of removing metal. It comes off in big hunks.

You might consider using a roughing end mill. We always called them corn cob end mills. You can run a 5/8 cutter 1 1/2 deep in steel on a bridgeport no problem. Try that with a regular cobalt end mill.

FWIW - I have a Tormach (1-1/2 HP) - and just got a 2-1/2" Sandvik facemill from EBay. It's overkill for my machine, but I did get it to work pretty well, makes a mess of my shop tho :) - throws chips (hot ones) everywhere.

I mill a 2" hunk of steel, .03 DOC at 20 to 25 IPM. I went up to .04 one time and it shut down my spindle, not enough HP. The other thing is the finish is like a cloudy mirror so it's nice.