Cutting steel with 1100 PCNC and tool pull out?

Hello Forum,

I have a 4 year old 1100 PCNC that I use for work and love very much except for when I try and machine steel. Today I had a job where I needed to machine some 1144 in a simple, circular pattern (Fusion 360) using a brand new Guhring .50" mill for steel (RF100). I used conservative DOC WOC and used G-wizard's SFM/RPM and the tool still pulled out of the TTS holder! On my first attempt I was using an ER collet holder and the tool pulled out of the collect. On my second attempt with reduced DOC/WOC and a .50 allen screw holder the TTS pulled out of the R8 collect in the Spindle. Fortunately nothing was damaged but I find it very frustrating.

I called Tormach and they called me back later the same day. I had already ordered an New R8 collet today because when I removed my original R8 collet, it had some surface rust on two side, 180 degrees opposite one, another. I have a pneumatic draw bar and I had tightened the draw bar after the first pull out today. There was no rust on the inside of the spindle.

Has anyone else had issues with this? Cutting steel with a Tormach 1100 PCNC? Did you find a solution? Tormach suggested using a narrower mill (.375" or .250") but I would hope you could use a .500" mill, and I need to remove material up to a depth of 1.00" from the stock. I feel a .25 or even .375 mill will not be as rigid?

Any positive, constructive suggestions will be appreciated. Thanks, Cismontguy

Attachment 442450

A full length .5 endmill is difficult for me to use as well in aluminum, it will chatter and where there is chatter there is pullout regardless of the cutter size, its just worse with the larger ones.
I usually stick with a .25 as I have much better luck with those regarding chatter.
R8 collets and TTS are an easy to use setup but definitely not ideal when it comes to chatter/pullout!
I havent tried a name brand collet, I often wonder if that would help as mine only grips on the bottom 1/8" of the collet.

If you use a 1/2" mill, and want to go 1" deep, you have to make it up in shallower radial depth of cut. Consider going as low as .020".

I've done steel (mainly 1018 and 303), titanium (6-4 and grade 2), and aluminum (mainly 60610. I use a 3/8" end mill in aluminum, a 1/4" end mill in steel, and 3/16" end mill in titanium as the biggest, and I haven't had pull-out. I used to use 1/2" in aluminum and I would get pull-out, somewhat depending on how hard I cranked the drawbar, and how hard I pushed the cutter/spindle.

(I also used the superfly on titanium. That lit the chips on fire. Literally!)

So, you can get reasonable surface finish at depth with a 1/2" end mill, without pull-out, if you baby the radial depth of cut. If you don't like the finish of stepping down (and who does?) you may get better MRR by hogging with a 3/8" or 1/4" with longer stick-out, and then use the stiff 1/2" as a finish pass along the walls.

to push an endmill hard, even on a Bridgeport I forget the collets and use an r8 end mill holder with set screw.

Tormach had a white paper on tool pull out a few years ago, but I couldn't find it to link it.

Dave

I've given up on using any endmill over 10mm or 3/8th apart from one insert cutter I use for the extended length - like you, I used to get pull out and chatter all the time with 1/2" endmills.
And to be honest, if you use a rougher (corn-cob) you can get amazing removal rates with a 1" depth of cut, then use a finishing endmill for a light peripheral clean up. The roughers massively reduce the load on the spindle and don't seem affected by pull-out like a full flute endmill does.

Hello Forum,

I wanted to get back with my results and what I found regarding machining steel on the PCNC 1100 Series 3. First, I did order and receive a new R8 collet from Tormach for my machine. It is a different brand than came with my machine. Lyndex-Nikken part # 50568. I installed it according to the manual and used some anti seize on the outside of the collet taper. Second, I re-viewed John Saunder's WW144 on YouTube, where he did a test on speeds and feeds for cutting steel with the Tormach (770 in this case). I used his initial speeds and feeds which were very different than my original speeds when I experienced the tool pull out. His optimum was 3400 RPM, 25.5 IPM .375 DOC, .050" WOC 225 SFM. I ended up using a 5 flute ATS brand .375 diam, 1.00" LOC Carbide end mill with 0.030 radius. My DOC was .375", WOC .050" 2215 RPM 6.6 IPM and it worked perfectly. I had some chatter on the first pass at the 12 and 6 o'clock positions of my round stock. I used Pathpilot's sliders to change the RPM and Rate of feed until this went away. The numbers came out to what you see above. Slower IPM, but its a different end mill than John S. was using.

Picture shows the results. Will flip it over and machine the other side, now. Cismont guy
Attachment 442902