True Mill to the Rescue

[lkenney]

I have been learning to use Truemill and find that it has increased my production even with the haas VF-0 (1992). This weekend I was catching up on a bunch of prototype jobs. The main one was some protoype triggerguards for a new rifle being designed. As you well know most of the material from the raw stocke becomes swarf before you can call it a trigger guard. I think that I am taking about 92% by weight off the 1018 steel stock.

Anyway I have been running the VF-0 at about 3500 rpm at 20 IPM with a TiAIN 1/2" 4 flute generic end mill about .400" deep and thought that was pretty good for such an old machine.

I have a spreadsheet from someone at Surfcam that showed heavier machines running a 1/2" end mill at speeds from 5600 to 12,000 rpm in 1018 steel. frustrated with the time it was taking to chew through this job.

I reprogrammed all TrueMill cuts for the 1/2" end mill to 6000 RPM and 60IPM still at the 0.400" depth. I shut both doors and stepped back, punched green and let her rip. The little Hass just hunkered down and went at it. We never went of 40% on the load meter and the chips just flew. The first piece was a little rougher than i wanted so I turned on the TrueMill finish cut at 6000 RPM and 35 IPM Job done lookiing sweet. 34 minute job down to 7 1/2 minutes.

Had time to sit down later and get mad about politics.

Have a great day

Eagle

[tnik]

if your only running at 40% load, why not try to push it more?

[Eagle View]

This old Haas is not built that heavy, I am getting far more than I ever thought I could so why risk damaging an old machine.

Eagle

[tnik]

true.. I missed where you said how old it was..

[Maguillacutty]

I machine most of my parts using TrueMill. Taking cuts at full depths saves a **** load of time on my end. vs standard traditional toolpaths where I have to use a few steps in (z) to accomplish my depth. The more you futz around with its features the better you get. Still not very aggressive but on the VF-3 we got only 7500rpm spindle max. But when contouring(Aluminum), I run a 1/2 3 flt endmill .5 deep @7500rpm 114ipm. 78deg engagement angle. I play around alot.

[tnik]

yea, usually with aluminum, if I have pocketing to do, or alot of roughing to do, I'll use truemill. It's when I get into the stainless or carbon steel when I tend to break endmills or stall out the machine.. VF-4 and VF-2 , 7500rpm max on both.. I like playing around, but most of the operators that we have here don't like playing.. They will just run at the programmed speeds and feeds.. If I want something done, gotta do it myself :/

[malonet]

Hello Everyone,

We are using Surfcam Velocity 3 (waiting on 4), but I have not used the Velocity cutting much. We cut a lot of stainless steel, ie. 304,304L, 316 etc. Any one out there used the Velocity on stainless? These parts will be run on machines such as Mori-Seiki, Mazak and OKK 20 x 20 and 40 x 20 size vertical machines. Speed/feed/radial and axial depth of cuts? I have several jobs coming up that I will have to remove quite a bit of metal. Thanks in advance for your replies.

[tnik]

Originally Posted by malonet Speed/feed/radial and axial depth of cuts?

http://www.camcadtech.com/truemill_speeds_and_feeds.htm

Just google for "surfcam truemill speeds and feeds"

[Jason S]

I just ran some 3/8" thick 304SS plates, had to cut 6 windows 4" x 5" 6 plcs. I used a 2" 4 flute mits feedmill, ran it 1200 sfm,.05 ipt,.05 d.o.c,120^ t.e.a. and airblast, it ran 7 min. I like to program the conventional way first then I do it in Truemill to see what the difference is in time. Amazing stuff.

[Maguillacutty]

Your lucky to have your machine equipped with an air blast. I really wish I had one. Then I could really crank it up. I hear a mill chuck is recommended as well for maximum performance?

[Maguillacutty]

I just ran some 304SST 2"X3"X2" tube/rectangular bar stock. On a Haas VF6
I was running a .500 2flt end mill (2.5 flt lenth) at 1800RPM with a feed of 9.0 IPM .290 depth of cuts, 65 deg tool engagement.

[tnik]

now running that slow in a truemill path, are you saving time vs. using a different cutter and regular paths?