I have a production application where I need to cut approx. 0.5" wide slots
about 0.040" deep accross 5/16 dia mild steel round stock. Volumes will be in the 500K per year range...

I have the option to lay the bars down horizontally and mill use the bottom
of an end mill or stand it up and mill useing the side of the end mill.

Speed and cost of cutter per part are critical.

My standard end-mill feed and speed calculator does not really differentiate between these two types of cuts and therefore says use the same speads and feeds.... But I don't think I know the whole picture.

Any thoughts on which method is more efficient/ longer cutter life?

Thanks!

Not exactly sure on what you are doing, but I think you would have better cutter life on the sides. More cutting surface. It may have more deflection though depending on the length and type of EM.

It takes a little time to ramp the EM into a part as well.

Thanks Lee

I am a bit puzzled because you describe it as a slot and then say you can mill it using either the end or side of the cutter.

The speed and feed would be the same cutting either way and I think cutter life would not be much different; cutting across with the end means the cutter is entering the curve surfaced gently so chipping the corner is less likely.

If you could de some experimenting you may find the side can be quicker, and cheaper, by using a smaller diameter(i.e. lower cost) cutter running faster; going across with the tip would require a 1/2 cutter and between 3/8 and 1/2 prices jump by quite a few dollars for most cutters.

But the fixturing method will also be important because you may be going at a crazy speed during the cutting, and then using a lot of time to reload the machine.

Are you going to be using air or hydraulic clamping or just vises. With custom jaws holding multiple parts in vises you will probably fit in more parts per load if they are vertical, but you are going to need so fancy jaws to clamp each part equally.

It is an interesting problem because even though the number is fairly high the price per part will have to be low so the total amount of money is not really large.

Sorry, I did not paint a clear picture of what it is, if you can picture the tube laying flat on a table and going accross it with about a 1/2 end mill, 0.04 deep, that is what I mean by a slot... to cut it with a side of an end mill the end mill would have to be relieved above the cut.

Thanks for your input....

..... the end mill would have to be relieved above the cut.

Thanks for your input....

Oh, a really narrow Tee Slot cutter.

If it was me I would be thinking of using an endmill with inserts,it would be faster to replace inserts and be running again instead of changing an endmill out becouse it went dull.If you were to lay the part horizontal you should be able to do quite a few parts on a corner,iscar makes some nice mills for this down to .375 I think,we have some for putting 1.1 deep slots in mild steel and the tools last a long time.If you have machine capeable of high rpm's you can blase through it, we take .060 doc at 75 ipm 6500 rpm.

When standing straight up you are only using the bottom .040 of the end mill.
When cutting with the side you are using .500 worth of cutting edge.

More cutting edge means longer life as any particular point on the cutting edge sees less material removal. I'd expect 4-6 times the tool life.

In side milling the chip is thinned due to the limited engagement. The chip on an endmill is thinner on the side that it is in the front. You increase the feed rate to make up for this. For example when side milling with a 1/2 endmill at .600 inch deep but only .030 engagement in 4140 I feed at 200-240 IPM. When slotting full width at only .100 deep I have to slow down to 40-60 IPM.

Side milling is one of those high speed machining "secrets". Sandvik's feed and speed calculator takes this into account if you let it work with "effective chip thickness". It's also documented in the technical section of their catalogs. In addition you get to run higher SFM because the teeth spend more time in the air (tool runs cooler).

I'm guessing the slots must be pretty close to the end of the shafts to allow you to do this op by side milling without having a tool length problem.
Bob

Yes the slots are close to the end, the furthest point I should have to reach
is about 1.5" down.

Thanks, for all the input, now I just need to figure out how to hold the darn
things.... :)

With the small depth high quantity have considered cold forging.
A hard tool. A nice Jig.
1 BANG and you are done !
Great possibility for automation.
Grain structure has more strength.

With side milling you will have rigidity issues, especially with 1.5 tool overhang. I would opt for end milling using tialn coated carbide. If it also suits use a corner rad cutter (.015) as it is the sharp tips that have the biggest issue with chipping/wear. You can use a stub length and will get amazing tool life.

Also like Neal said, for very little up front cost you could make/have made a swaging machine that pounds these through in full automation at 1 second a piece. Supposing the deformation of material displacement is not an issue. It will keep an operator (or 2) hopping to put parts in the feeder fast enough.

.....
Also like Neal said, for very little up front cost you could make/have made a swaging machine that pounds these through in full automation at 1 second a piece. Supposing the deformation of material displacement is not an issue. It will keep an operator (or 2) hopping to put parts in the feeder fast enough.

How little up front cost? I would have expected there should be an extra zero on the parts per year number. At 1 second each you will only keep your two operators busy for 139hrs per year, and that is a very short utilization time to amortize much expense on tooling that has a single function.

If side milling you could use a large cutter to eliminate any flexing.
Maybe even HSS for such a small cut.
I mount a 6 inch side milling cutter in my shell mill adapter. These cutters look like circular saw blades.

Load/unload ergonomics is going to be the key to making money here as the cutting time is only going to be at most a couple of seconds
Even how far you retract the tool is going to have a big influence on cycle time. (unless of course you've got one of those nifty 2000 IPM rapid machines) I'd look at putting a bunch of parts on the table as starting/stopping the spindle for each part is going to kill ya.

This job begs for automatic loading but I'm guessing it doesn't have a lot of money in it. We hit a wall at about 300 pcs per hour when manually loading as this is about the limit one person can handle,

Bob

Geof (and others)

Start with a used flywheel press (they are either really cheap or free for the taking) and 30-40k for the rest of the machine.
The operators can go and do other profitable jobs when the run is done.
Accounting work to be done by others - just a suggested solution.

I have also made machines for parts like this that were a little slower (2-3 seconds) that did the job by broaching. You could double the time and reduce the costs by having manual load/unload.