Max size of face mill

Hello guys,

I have vf6 wizh iso 40 taper and i am wondering what size face mill can i put on...now i have 50mm but that is way too small for bigger surfaces.
What size are you using that still works for roughing, becouse i think the spindle power is maybe not up to the diameter of a biiger face mill ?

thx

It really depends on your materials and what type of work your doing.
3 inch is pretty comfortable on a 40 taper Haas. For light DOC you could go bigger. I would not go much bigger than 4 inch and expect to take much of any depth of cut.

I agree 3" is a great size for cat 40. Anything bigger In a Haas will have to be flagged as "oversize" to prevent a tool change collision.
Carl

I have a pair of Carboloy Octomills that are 3.150" cut diameter in my VF-5 with a side mounted carousel and they work great.

But I do have them set as Large tools.

I wish I could assign pockets in this machine as the way the side magazine loads tools, I could very easily have long small tools in between the large tools.

The tools swivel out of the magazine rather than being pulled straight out as my other machines do.

If anybody knows a way to assign pockets in this machine, Please drop me a line.

I have bet the Haas repair guy that if he can find out for me I will pay him.

Have a great Day

Mohawk

Thank you for the tips I will buy a 3 inch then!

well , i boght i sumitomo wex 3 inch cutter with five round inserts...if i go 2mm deep, i have problems with the spindle being always over 100% 700 rpm/ 300 mm/min and inserts wear out quickly, material is 1.1730!

what depth of cut are you usually doing? how long does the inserts last I am milling dry becouse i still dont have air hose installed with coolant i think they weared out even quicker!

thank you

We use a 5" Iscar octomill on a CAT40 holder for facing aluminum. We often take near full width cuts at about .060 depth. This is on a TREE VMC with a 25HP spindle. We've never stalled the machine even when due to operator error we ended up cutting about 0.500 deep on a 4" wide aluminum bar... We considered that to be a good test for the machine. The finish has always been good and we never see very much step in the cuts. I'm not saying I recommend this but it's certainly possible. We do need to leave an empty pocket on each side of the tool in the ATC for clearance.

I would be tempted to run that 3" facemill more around the 1 000 rpm area, and 600mm per minute (0.12mm per tooth) - 800mm per minute (.16mm per tooth). See if that runs any better. DOC is good i'd say.. maybe try 1.5mm instead.

if your material is only 1.173 wide (i'm guessing that's what you meant?) i would grab the 2" cutter since it's more than wide enough.

The torque curve on the 40 taper 7500 max rpm vf's peaks at 1200 rpm then falls off fast at 2000 rpm. I try to look for face mills that run comfortably in that range (sometimes loosing dia.) since overloading the spindle tends to ruin the inserts since the chip load changes. I like to use the max tool load feature in the control just for saftey measures. All set aside, I'll use a 2" for hogging then 3" for lite finishing. it's easier on the machine too.

Thx for all the tips...I think u are right about using 2 inch for bigger cut...i will try that!

jbhill said:

We use a 5" Iscar octomill on a CAT40 holder for facing aluminum. We often take near full width cuts at about .060 depth. This is on a TREE VMC with a 25HP spindle. We've never stalled the machine even when due to operator error we ended up cutting about 0.500 deep on a 4" wide aluminum bar... We considered that to be a good test for the machine. The finish has always been good and we never see very much step in the cuts. I'm not saying I recommend this but it's certainly possible. We do need to leave an empty pocket on each side of the tool in the ATC for clearance.

Click to expand...

I will second this cutter. I started using in the VF-1 and it cuts like a dream, especailly in Alum with those razor sharp polished inserts. Heavy fast cuts...

1000 RPM cutting aluminum with a 3" facemill? This seems really slow to me.

With a carbide insert tool you should be exceeding 2000 sfm (we aren't in the dark ages, anymore - surface speeds of 15k are becoming common), which means you should be around 3000 RPM on the absolute low end. Let's assume a .008" chip load per tooth with a full 3" diameter cut at .08" deep - that equals 120 ipm.

According to the Haas Calculator on my machine you only need 10 horsepower to achieve this. I typically run much faster, and do it without any tool wear and horsepower issues. I do have the 12k 30 horse gearless spindle on my Haas, but I refer to the 10 hp requirement for these speeds and feeds. I have an older octamill 3" facemill that I run around 6k rpm and can push to 250 ipm for cuts around .08 deep. I know that a .100" deep full diameter cut with my 2" Shearhog is no problem at 250 ipm - 7-8k RPM.

Am I missing something here? I understand maximizing the machine torque RPM - it just seems that is normally super slow for today's cutters - my machine max's torque at 2100. Sim - what are your speeds and feeds (and/or surface speeds and chip loads) with that tool?

Acuvue - are you milling aluminum dry? I know that some new coatings allow it in some applications.

On our haas vf2ss with a 3 1/2'' sandvik balanced face mill we run 8k and .08 to .125 DOC and 150 to 200ipm feed on a well fixtured or clamped part
Either on aluminum or plastic. But can slow the rpm down to about 1200 on annealed steels with a DOC of about .020 to .040 depending on the hardness.
But on 1018 or 4140 annealed thats what i'll run. And dry at that, with air mist of course.