Newbie Plunge Cutting Question

edojan

edojan

Registered
Registered
Joined
Jan 10, 2016
Messages
29
Hello folks, my name is Ed, I am a newbie and I live in Canada . I have just got my first milling machine (hi torque 3990 from LMS) and I look forward to learn machining. I have a question about plunge cutting and here is the context: I am installing the DRO and needed to reduce the height of one of the mounting brackets by about 1/2 of an inch (the bracket is made of 0.4 inches thick aluminum)
I used a 1/2 " 2-flute "premium" end mill which came with my machine (HSS / cobalt, made in Korea) and successfully shaved off the metal from one side of the bracket. It took a good 30 min to cut the metal from one side of the braket by shaving a few thousands at a time at about 1000 rpm. But then I grew inpatient and remembered that what I watched a video that clamed that so called plunge cutting was a much better way to remove larger amounts of materials especially when using a non-rigid setup or underpowered milling machines. So I gave it a try on the second side of the bracket. The first two "plunges" were great - the end mill plunged into the aluminium with some chatter but it wasn't excessive. Then on the third "hole" it started developing a very loud screeching sound. The forth plunge I did not complete because the sound is quite loud and there is also chatter. I don't think that this sound is normal and I have tried to change the RPM and lower the feed speed but this made no difference. I have also examined the end mill under the magnifying glass but I seems perfectly fine. Please comment what in your opinion is causing this and what is the best kind of end mills to use for plunge cutting - e.g. would so called roughing end mills be more suitable for the job or is this me who is doing something wrong?
 
It sounds like there are some places that you can improve your technique. I am sure others will chime in as well.
I do recommend roughing mills. Get yourself some solid carbide 1/2", 3/8", and 1/4" ones from Enco. They are fairly cheap and will make using your little mill much more enjoyable.

Shaving a few thou at a time is generally considered bad practice. A cut that shallow is a finishing cut and should be used for that purpose, not for roughing.
I have never used your machine, I looked it up and it is small and low on power. But it should be able to do what you are asking it to do, it will just take a bit longer. You will have to experiment to discover the limitations of the machine, but I would think it would be able to handle a 0.050" deep cut on 0.4" wide material. Cutters should be pushed, not babied. Getting all delicate with a cutter just reduces tool life, takes extra time, and takes the fun out of the hobby.

Consider, the only thing that is cooling the end mill is the metal itself. The cutter needs to be cutting into cool metal to so it has a nice cool chip that can draw the heat from the cutter itself. When you get done milling the work and the tool should be cool enough to touch (ideally), and the chips should be so hot they stick to your skin when you get hit by them. In practice, this is hard to achieve, but it is what you should aim for. This is the fundamental concept behind chip load, it is the ideal amount and size of chip for a given cutter and RPM. In theory, a correct chip load will give the chip just enough to dwell time in the cutter to draw the heat out, and eject before it starts transferring heat back into the cutter.

Plunge cutting is a more efficient way to remove large amounts of stock, it is easier on both the machine and the cutter. It also produces a chip that is easier to clean up, rather than those nasty ones you get from side milling. I usually plunge 1/4 to 1/3 of the tools diameter, and I use less than 120 degrees of the tool circumference. When you make plunge roughing cuts, you want to lower the head until it is just above the work and lock it. Lock the unused x or y axis as well. Then plunge with the quill. The idea is to take nibbles off the work, not full diameter cuts.
On your material, I would make a plunge 1/2 the width of the material, and advance the table about 0.150" per plunge. This way only about 90 degree of the tool is buried, and you are cutting about 1/3 the diameter of the mill.

The screaming sound you heard is chatter. The cause of the chatter could be a dull mill, loose gibs, improperly clamped work, too aggressive a cut, center plunging with a non-center cutting mill, or incorrect RPM.
Hopefully someone with experience with a machine like yours will chime in on the RPM.
 
For plunge cutting you need a center cutting end mill or a standard end mill with plunging only less than as wide as the cutting edges width from O.D toward the center. Really, center cutting end mills are not really great for center cutting the full face of the end mill either. The surface feet per minute speed at the center is zero so you are just extruding metal. I typically plunge cut in steps about 1/3 the diameter of the end mill across the work. That works fine, even using most standard non center cutting end mills.
Edit: Looks like Joshua beat me to it again (and put up a better post...) 8^)
 
You can also use a drill to rough a piece out then go back with the end mill to clean it up. I usually don't have large surfaces to cut long lengths so I use the end mill all the way but if I'm cutting a4" slot I'll go through with a drill & poke a bunch of holes usually overlapping 1/4-1/3 of the diameter back into the last. Then it is easy to go back & finish the slot & not ware out my more expensive mill.
 
Thanks gents for your responses - this is really helpful. It appears that I was overloading the machine because all my "plunges" were at 100% of the tool diameter. I should try your suggestions. In the meantime could you please provide your input as to the following:
1. If I were to select a smaller / bigger size end mills for this job - what would be the advantages / disadvantages?
2. All other things being equal - two flutes vs four flutes for plunge cutting - what would you recommend and why?
3. Re: roughing end mills: there is a shop nearby that sells cobalt roughing end mills - there is a fine tooth and the regular tooth options: which one is better for aluminum? Or should I consider the carbide ones instead? Here are the links:
https://www.accusizetools.com/standard-tooth-tialn-coated-m42-8-cobalt-roughing-end-mills/
https://www.accusizetools.com/fine-tooth-tialn-coated-m42-8-cobalt-roughing-end-mills/

Now the same place sells carbide end mills for alluminum which one is better for the plunge cutting?
https://www.accusizetools.com/2-flute-carbide-tipped-end-mills-for-aluminum-centercutting/
4. What is the advantage of a roughing end-mill over a regular drill bit (again, all things being equal)?

Thanks again
Ed
 
It all depends on what your doing. Likely a 2 flute uncoated HSS end mill for you.
 
Roughing mills are intended more for full depth, full width cutting and not typically for aluminum. The cut that you are trying to do is a very small cut but the mill is small also. I would recommend going with smaller cutters (maybe 1/4" - 3/8") and stay with 2 flute cutters. I don't know what the maximum speed is for your mill but look up the tables for it and crank it as fast as you are able to. Aluminum cuts incredibly easily but it will also stick to the cutter easily. I have found that good ole WD40 works well as a cutting fluid.

On that mill, you should be able to do a full diameter plunge with it. Just keep the chips cleared. It would be nice to see a photo of what you are trying to do. If you go full depth (0.40"), try about a half diameter or slightly more conventional mill (not climbing). The chips will come off nicely to the side. You might break the occasional cutter but that's how you learn too.
 
In general if you are cutting aluminum you want to stick with endmills designed for aluminum. This normally means a 2 flute, high helix angle with additional clearance. Unless you have a high speed, high HP machine, carbide cannot be used to it's advantage. Having said that, carbide endend mills have a much longer life than HSS, and I use them almost exclusively in sizes less than 1/2 inch, above that, they start getting really expensive. Carbide router bits work great in aluminum (and as I proved the other day, in stainless steel too :)) , and you can get them at the local hardware store on a Saturday afternoon when you break one right in the middle of the job. I use both solid carbide and carbide tipped router bits, 1/2 inch shank where possible. Normally an end mill is perfectly happy taking a depth of cut (DOC) of at least 1/2 the diameter, many times you can take more. When surfacing a large area a 40% of diameter width of cut (stepover) will be the most efficient.

Unless I'm cutting deep pockets or something like that, I normally try to avoid plunge cutting, and never more than about 40% of the endmill diameter. Endmills do not like to plunge, even center cutting ones. If I do have to plunge, I will drill a starter hole at the first plunge point. I had a job the other day where I had to machine 5 deep flutes around the perimeter of a cylinder about 3.5 inches deep. I made 5 plunges per flute with a 4 inch DOC end mill at 30% diameter, then did a profile cut after removing the bulk of the material by plunging.

Course roughers have a higher material removal rate than fine or finishing roughers (how's that for an oxymoron ;)) Spindle speed normally remains the same, with a reduced feed, and an increase in DOC For your machine the main limiting factor is the machine stability. Normally a rougher will be happy cutting 2-3 x the diameter deep in any material it's designed for. Aluminum roughers generally are 3 flute for additional clearance and have a higher helix angle than those designed for steel.

As stated above WD-40 is about the best off the shelf cutting fluid available for aluminum. Keep the tool wet to prevent aluminum welding to the endmill.
 
Last edited:
You must log in or register to reply here.
Back
Top