High speed machining

[RACINGCONVERTERS]

I am looking for some insight on maching 1018 crs in a high speed manor. I have heard that it can be done but I do not know anything about it.

Is anyone in here doing it?

How are you doning it?

 

I am just trying to find new approaches to some of the parts that we make and any information would greatly appreciated.

 

Thanks in advance.

[Cobra Driver]

Do you have a machine that will do HSM? Spindle, controller and rigid tooling are all key.

[Goldorak]

do you tried feed milling (small DOC, huge feed)

it usually faster than anything in soft material

[RACINGCONVERTERS]

Rigidity may be the issue. The machine is a Haas VF-2SS with TR160 table on it.

12000 Rpm

833 IPM feed

High speed look ahead

The tooling we have made shoud be able to handle anything the machine can throw at it.

[mold100]

Yes any machine can take lighter cuts faster, but accurately, rigidity, and correctly are majors factors. CAM (you have), a rigid machine with High RPM, a fast contoller (fanuc 16i,18i,21i, heid430,530tnc, seimens 840D are a few), good tooling are all factors, without any one of them it puts a stick in your spokes.

 

You beat with your last post, you can do it with an ss to some extent your not cutting anything heat treated, you wont be using a 2" toriod at 4800 rpms 120ipm at .125 doc.

[Rick Henrickson The Boeing Co.]

You can help your HAAS a bit with better tool holders.

Nikken has endmill chucks with split tapers that face contact your spindle and a better fit in your spindle, some tools require less pressure with the same feed. I wouldnt recomend getting to wild with your HAAS but you can do some things to help it.

[RACINGCONVERTERS]

The parts we cut require small diameter cutters. Ex. Most roughing done with 3/8" no rad, .5 loc, 1.3 stickout, 4fl custom steel grind carbide. Right now we are cutting at 2200Rpm about 220sfm and .0035 chip load which is about 2 hrs of roughing

[mold100]

When your roughing you may want to consider using a bull nose maybe with a .06 corner it will help tool life.

[mold100]

Wow, I would be running with a bull nose in crs in the 600sfm range the down side to your app is tool length, all though I would start using the longer reach with less flute, the cutters with stub flute way out perfom longer flutes because the tool core is sacrificed for flute length. Oh also are you roughing with that small of a chip load?

[mold100]

Here goes, 1018 crs with Jabro 950120-mega64

12 mil, ran at 4200 rpms 80ipm .1874 doc, just air no coolant. The cutter is about 160.00 though it lasts quite a while.

[Surface]

I've got a steel job here. I've been playing with some high-speed techniques in my VF2ss.

 

Profile cutting: 3/8 dia AlTiN 5-flute endmill. .77 z-depth (stock thickness), .062 stepover. Dry

7130rpm (700 sfm)

feedrate: 210ipm (.006 fpt)

 

I'm sure some air-blast would help my tool-life, but even without, same endmill moved around 75lbs of HRS.

[Redfire427]

With your machining parameters, there are really two ways to go. You could use a Hanita Vari-mill at full depth with 50% stepover or you could use one of the new feedmills from Jabro, Millstar, Pokolm-Voha, etc. I have run the 3/8 dia. at 8000 rpm, .013 doc and 250 ipm. Lasts forever in H13, I can only imagine you would get great results in 1018.

[Goldorak]

+1 for feed mill

 

iscar makes an interchangable tip (multimaster) and they are great

 

8000 rpm .015 DOC 400 ipm (max of my machine!)

 

even with extra lonf shank they wont vibrate but you will get lot of deviation due to shank rigidity and speed

 

with a 2in cutter i can easily reach 10in deep without problem !

[Cobra Driver]

It may not seem like much of a cut but that Iscar highfeed mill removes steel in a hurry. The only problem is there is LOTS of heat buildup. We had a 2 inch stainless mold plate warp .015 on us.

[cobra95kev]

To keep this good thread going...

 

I am going to be finishing some P&W engine mounts made out of 15-5 Stainless and was hoping to get some opinions on speeds and feeds. The stuff Rockwells at about 40HRC. I am going to be machining them on an OKUMA horizontal 50 taper.

The part is a pretty basic shape with mostly open pockets on it and I am going to try to use the High Speed Waterline and High Speed Horizontal finish paths for the first time.

The tool I am using will be 3/4" coated carbide with .25r. It will have to stick out of the holder about 2.75".

 

What kind of surface speed and FPT do you guys think I should be able to run? I am going to use .2" stepdowns on the waterline toolpath, .070" radial then .030" radial for the final finish pass.

 

Any comments would be really helpful.

 

Thanks

Kevin C.