[pyropanda5]

I've recently been trying to get some steel machining under my belt with a PCNC1100 but I've run into nothing but chatter on my roughing operations. To give some background I'm using Fusion 360, a relatively new mill, two fogbusters with qualichem 251c and standard 4 flute AlTiN coated end mills from lakeshore carbide. The first project I tried to tackle was machining an exhaust flange for a Miata turbo which is essentially a 2-inch circle with 4 bolt holes made out of a piece of hot rolled A36. My order of operations was to deck it off with Tormach's 38mm face mill then a 2D adaptive toolpath with a 1/2" end mill finish it with a 2D contour, a boring operation on the .443" bolt holes with a 1/4" end mill, and a nice 0.01" chamfer on all machined pockets with a 1/4" chamfer mill. The facing pass turned out great and the helix at the start of the 2D Adaptive sounded fine. The trouble started when it went into its roughing passes; nothing but horrible chatter. I was running a 0.4" depth of cut, 0.15" optimal load (stepover for those unfamiliar with Autodesk HSM), 3500 rpm, and 25 ipm. After this, I tried just about everything I could, higher rpm, lower rpm, higher optimal load, lower optimal load, higher feed rate, lower feed rate, etc. I ended up just letting the program finish so I would at least have a part done. In addition to that, I tried switching to a 3/8" tool and went through the same proccess but to no avail. I've attached my fusion 360 file with the part and tool paths with the 1/2" tool. I would appreciate any assistance with this as i have no idea what I'm doing wrong.

[nutzilla]

Go with 250-350 Sfm, .0015 chipload, and .125 width of cut. Let me know how it works out. I'm a Cnc programmer btw.

[GLCarlson]

NYC CNC has a video -using LSC tooling, no less- that talks about how to optimize a cut, specifically in 4140.

The things I picked up specifically were that a small radius on the cutter (030) is a very good thing- the difference is amazing vs no radius. And while DOC can be pretty deep, width is a key variable to adjust (ie, chipload). I routinely use .07 for a stepover now, as a starting point, at 1800 rpm and 7 ipm with a 1/4" 0.625 coated carbide 4F cutter. That generally works, if not optimally.

[IMT]

... width is a key variable to adjust (ie, chipload)...

Please don't confuse the terminology. Chipload is the actual thickness of the chip being cut. Width of cut (WOC) is the step over from pass to pass.

The WOC you can take depends on several factors, some of which can be estimated by the various calculators available (tool rigidity, machinability of the material, WOC, DOC, chipload) while others (machine stiffness, workpiece and fixture rigidity etc...) are specific to your setup. I recommend starting with a low WOC <=.030 and work your way up. The LSC variable flute tool NYCNC demonstrated works great on mild steel, stainless, and alloy steel.

[GLCarlson]

[QUOTE=IMT;2032058]Please don't confuse the terminology. Chipload is the actual thickness of the chip being cut. Width of cut (WOC) is the step over from pass to pass.

/QUOTE]

Good point, thanks.

[Bryan Turner]

Here's a setup for your Tormach 1100 speeds and feeds in steel (with the SFM recommendations by nutzilla above):
Speeds and Feeds

RPM 2670, IPM 20, DOC 0.4, WOC 0.15 -> MRR 1.18, Chipload 0.0017, SFM 350

For HSM, you might try:
RPM 2940, IPM 80, DOC 0.4, WOC 0.046 -> MRR 1.4, Chipload 0.002, SFM 384

--Bryan

[Dallas J]

I just went through the same thing and have had very little luck roughing with normal endmills. And I was trying much-much less DOC and WOC. What has made me happy is just using a corncob rougher. 5000rpm, .25 DOC, .05 WOC, 30IPM with a 1/4" 4flute rougher. Removal rate is low still but I've at least been able to make my parts with confidence.

I bought some 3/8s 4flute bullnose endmills specifically for the part I have and cant get any reasonable removal rate without chatter.

[wildwhl]

Haven't watched it yet - but guessing some decent information will be found here: https://www.youtube.com/watch?v=SzBFJ7oRo8c

WW

[nutzilla]

I just went through the same thing and have had very little luck roughing with normal endmills. And I was trying much-much less DOC and WOC. What has made me happy is just using a corncob rougher. 5000rpm, .25 DOC, .05 WOC, 30IPM with a 1/4" 4flute rougher. Removal rate is low still but I've at least been able to make my parts with confidence.

I bought some 3/8s 4flute bullnose endmills specifically for the part I have and cant get any reasonable removal rate without chatter.

Did you switch to lower gear? I have to do that to my pcnc 440.

[nutzilla]

I just went through the same thing and have had very little luck roughing with normal endmills. And I was trying much-much less DOC and WOC. What has made me happy is just using a corncob rougher. 5000rpm, .25 DOC, .05 WOC, 30IPM with a 1/4" 4flute rougher. Removal rate is low still but I've at least been able to make my parts with confidence.

I bought some 3/8s 4flute bullnose endmills specifically for the part I have and cant get any reasonable removal rate without chatter.

Chatter is usually cause my too low of a chip load.

[Dallas J]

I hear ya, but going faster with less RPM wasn't fixing it. Which is what I assume the OP is facing. Will try same thing but with reduced DOC since I think I was shooting for 0.375 DOC with a .375 EM. See if I can find a happy zone like John S. was showing.

[bobeson]

I have encountered a lot of grief when working with steel on my pcnc1100, and found a few key factors besides feeds and speeds that affected the amount of chatter I was experiencing.
Most of the considerations relate to machine rigidity.

The machine needs to be in a top-notch state of tune, particularly including properly adjusted: gibs, ball screw bearings, motor couplings, way lube, and column tram.
Minimize tool runout to equalize chip loads per tooth.
The spring-loaded power draw bar introduces lots of flexibility, and swapping the draw bar belleville springs out for an equivalent-length solid bushing improves performance substantially.

I find high-speed steel tools more effective for steel on the pcnc - they cut more easily at low speeds. I stick with 3/8" max end mills, with 5/16" and 1/4" doing a lot of the heavy lifting. Yes, this slows things down quite a bit.

How deep of a skin cut are you taking off this hot-rolled stock? A lot of folks recommend 0.060-0.100" removal to get out of problems from the skin. I try to use 1018 for most of my steel work. A36 is tricky stuff.

[popspipes]

I have encountered a lot of grief when working with steel on my pcnc1100, and found a few key factors besides feeds and speeds that affected the amount of chatter I was experiencing.
Most of the considerations relate to machine rigidity.

The machine needs to be in a top-notch state of tune, particularly including properly adjusted: gibs, ball screw bearings, motor couplings, way lube, and column tram.
Minimize tool runout to equalize chip loads per tooth.
The spring-loaded power draw bar introduces lots of flexibility, and swapping the draw bar belleville springs out for an equivalent-length solid bushing improves performance substantially.

I find high-speed steel tools more effective for steel on the pcnc - they cut more easily at low speeds. I stick with 3/8" max end mills, with 5/16" and 1/4" doing a lot of the heavy lifting. Yes, this slows things down quite a bit.

How deep of a skin cut are you taking off this hot-rolled stock? A lot of folks recommend 0.060-0.100" removal to get out of problems from the skin. I try to use 1018 for most of my steel work. A36 is tricky stuff.

I agree with everything you have said, but I hadnt thought of replacing the Bellevilles with a solid spacer- makes sense though, springs can equate to vibration.

I consider my Tormach to be a good aluminum machine with cutters under 1/2", its a bit too lightweight for a steel cutting machine, even the Bridgy has its limitations and it weighed 1000 pounds more, just my opinion though.

I really like the slider knob box sold by adapted cnc, makes the speeds and feeds adjustable during the cut, setting up a new program I find it really handy. I always did it this way on the Bridgeport.

Most of my machining was 304 stainless though, very unforgiving stuff at times ha!