[joeyjrc]

I'm cutting some deep pockets in aluminum with my 770. 3/8 end mill, I have a 2 flute HSS or a carbide 3 flute.
1.250 deep, .750 wide by around 3.0 long pocket, also has some bump outs and various depths. I have around 15 or so parts to do
I finished one but it was rough, took for ever, chips packing up, end mill crying for help, bad vibrations. I tried different speeds and feeds
But nothing really worked well, I'm taking around .125 deep cuts at full diameter, maybe it's too much, flood coolant on, chip brush in hand
Fighting chips.
Any suggestions on speeds and feeds. My end mills are both brand new, I haven't tried the carbide yet, it's a nice 3 flute high helix designated for aluminum, looks pretty bad ass. My HSS end mill is also for aluminum.
Thanks
Joe

[mike sr1]

I would try reducing the depth of cut, keep your feeds and speeds up and enough coolant to keep the pocket cleaned out.

[RussMachine]

Blast the pocket with coolant. Use enough to flush the chips out.
I would ramp down, and only step over 50%.
Try reducing your depth of cut to .050 .
I have a job that requires a 5.5" diameter circle, 1/2" wide groove to be milled 1.25" deep.
I use a 1/2" extra-long, 2-flute HSS, Aluminum cutting endmill.
I run it at 6000 RPM, .004 feed, and ramp down .035 per pass.
I feed it pretty slow, since the endmill is extra-long and likes to chatter, but it works.
The secret is blasting the chips out with coolant.

[LRF]

You need to provide more info:
1. material grade
2. RPM
3. Feed IPM
4. Step over
5. Are you ramping your down feed and what are the parameters
6. If using a CAM program to write code, what are you using?
7. Cutter stick out distance

[mike sr1]

I would use a half inch endmill for a pocket that deep, and as short as possible, long length small diameter equals chatter, thats a fact.

Carbide cutters are stiffer than HSS ones, that may help also.

I only use long length cutters for wood or plastic mainly, and always try to use the largest diameter and the shortest cutter possible for a given job in aluminum or steel, as chatter ruins the finish. Also take a light finish cut when done.

When I make a part I dont want to hear any chatter, if I do I adjust the settings or adjust cutter length to where it goes away. I sharpen most of my own cutters and that will give you first hand knowledge as to how shorter longer cutters react to chatter.

Also going too slow on the feedrate will cause the cutter to rub and thats not good either.

It all amounts to getting a "feel" for machining, what works and what doesnt etc.

I also dont like to push machining limits, but then I dont do it for production either.

I hope you get it figured out, good luck on your project.

[joeyjrc]

I can't use a half inch because the corners call for a .188 radius. I had my HSS end mill running 1500rpm and 3 ipm. I drilled a 3/8 hole in one of the corners to full depth and used that as my plunge spot. I don't have cam software, I write all my code by hand. I'm an experienced machinist and I know how to cut metal I'm just not too experienced with my tormach and what it can do in aluminum.

[mike sr1]

In aluminum I would run the rpm 5140, full flood coolant.A 3/8 endmill may chatter some in the corners as the radius is the same size as the cutter.

As Russ suggested lighten up on the doc .125 is too much for that size long length cutter.

Another option is to hog it out with a .5 cutter then finish with the .375

The Tormach will pull that cutter just fine.

[joeyjrc]

Thanks, I'll give that speed and feed a try with less depth of cut. I would like to keep it to 1 tool so I can just use an r8 collet instead of the tormach holders, I like the holders but the end mill will be hanging out even more with one. The r8 direct in spindle is more rigid.
Thanks again,
Joe

[LeeWay]

I found that 6063 aluminum machines terribly where 6061 machines very well. Aluminum type may be part of the issue you are having. 6063 turns out rough even with new end mills. It is quite a bit more gummy than 6061.

[sansbury]

Try this for feeds and speeds calculations.

FSWizard - Free Advanced CNC Speed and Feed Calculator

Personally I would want a 1/2" endmill for roughing that out. I hear what you're saying about not wanting to change tools, but IMHO using a machine like this without fixed-height tooling is like buying a V8 car and disconnecting half the spark plugs.

[joeyjrc]

I have know idea what grade aluminum it is, my customer is not a machinist and hasn't a clue how to answer that question.
The one I finished actually turned out looking nice when done , it just sounded real bad and I thought my machine was going to vibrate apart.

[LEARN]

like stated above either blast the pocket with coolant or a mist will do. Your step down is a bit aggressive a well. I would cut it down to .35mm step down and for step over no more than 80% of the cutter .

[chevalier]

What about "plunge roughing / finishing"? What I mean is using the Z axis instead of the usual XY toolpath.
Sandvik has some useful Youtube videos.

this is just one video
Tips film: Plunge Milling - YouTube

Chevalier

[Hirudin]

Good idea!

[KrausMotor]

Good idea, but what operation would you use in Sprutcam for plunge milling?

[mountaindew]

I have spent many hours reading sandvik coromant web site!
Found their examples on tool use and setup some of the best anywhere.
Also they have extensive equations for everything
As for sprut you can define a path with 2d contour and make it mill any place or shape you want.
Takes a bit of messing around if you don't plan first, but I know it can be done.
Just wanted to comment on sandvik web site. "all tool suppliers should provide information like they do"
md

[Jabs1542]

The sandvik stuff does look promising. I'm interested in the CoroCut QD but I can't find a price or US supplier - Mountaindew, do you know where to get this stuff?

[mountaindew]

The sandvik stuff does look promising. I'm interested in the CoroCut QD but I can't find a price or US supplier - Mountaindew, do you know where to get this stuff?

Not off hand . Check amazon with a quick search for the name sandvik coromant ! bet that will give you some vendors then filter and contact direct based on your needs to find exactly what you want.
ps I would SET down first! Any company with that quality of a web site and tools to match will be very proud of them and charge accordingly "industrial stuff"
md

[MichaelHenry]

The sandvik stuff does look promising. I'm interested in the CoroCut QD but I can't find a price or US supplier - Mountaindew, do you know where to get this stuff?

Try here:

Find us

and click on the Find Distributor link or call the 800 number on the same page. I'm told that local distributors often sell items from companies like Sandvik Coromant at a discount, compared to the normal big tool distributors like MSC, I keep meaning to check on that claim one day.

Mike

[chevalier]

I was not suggesting Sandvik is the only tool to use in this situation. My post was to suggest a possible alternative method to rough out deep pockets. This principle of Z axis roughing could be done using slot drills. Its the concept of having the machining forces taken predominately in the Z axis to reduce the forces in XY plane, thus helping "less ridged" machines when producing these type of parts.

chevalier