[tikka308]

I am the proud new owner of a PCNC1100 (delivered last week). Unfortunately I am having troubles with my cuts. By way of background, I ran a TAIG cnc mill for the past three years, so while the Tormach is a serious upgrade, I am not new to the CNC or chip-making world.

The attached photographs demonstrate my problem. This is a piece of 6061 which I am milling with a 3/8" 2-flute HSS end mill, taking 0.0625" DOC, about 45% stepover, 4000 RPM and 30 IPM. I am calculating my S&F in G-Wizard (and this is a recipe I have used on other mills). I am using a Trico MD-1200 coolant system. It should be a conservative cut for the Tormach.

The bottom finish is excellent. But the side finish is a problem. It appears to be chipweld. I am surprised because I have used this same tooling and coolant system on my taig with no problems. I have tried different end mills, including high quality (putnam, OSG) with similar problems - both 1/4" and 3/8". The bottom finish is superb, but the side is a disaster.

Any suggestions about what could be causing the poor finish on the sides only?

[jeffrey001]

Where you climb milling, if not try it.

Jeff

[twocik]

Here's my thoughts....

I'd try 5134 at 20.5 IPM, then bump it up and see how things go. I'd also make sure you're in CW on the main panel and mach. Last I would check for backlash and fine tune the mill. The mills are usually tuned out of the box, but mine needed adjustment before I could get to work.

[Magnum164]

In pic two is that the chip size you are cutting that is hanging off the end? If that is supposed to be the finishing cut, looks kinda large to me.

But I am new to CNC and may not be pushing my tools hard enough My finishing cuts are just a few thou at most.

[jeffrey001]

Just look at your website, http://www.nyccnc.com

Nice stuff, very interesting.


Any update about the finish on your part.

Jeff

[tikka308]

@ Magnum164 - no, that's not the chip size, it's just a piece hanging around for some reason - although I will/should investigate why it is there. The chips were a nice (e.g. normal) size and the fact that the bottom surface is so clean tells me there cannot be THAT much chatter (if any) in the tool....

@twocik - Thx - I'll try that tonight.

[Scott_M]

As Jeffery already said it sure looks like you were using conventional milling.
You will get a much better finish ( especially in alum. ) with climb milling.

Scott

[Freddy Bastard]

Your problem is heat. Check the flutes of your tool for wear (or try another tool) and check if you can put more coolant. This is really not normal to get this finish. The best way to cut this is with a constant ramping.

[LENS_CAD]

You probably know most of this stuff from your Taig experience, but my rules for milling aluminum are:
-climb milling
-2 or 3 flute high helix cutters
-flood coolant (to keep the chips from sticking)
-leave room for chips to escape

Len <><

[BlueFin]

As everyone said, it "looks" like you were conventional milling, in 6061 I always run max RPM, for me it's 4500, climb cut, lots and lots of coolant, blast all the chips away because if they are re-cut they smear all over the place. 30 IPM is a bit much for a 3/8" end mill, maybe 20 IPM to start, I use 40% step over on 1/2" end mill, but maybe 25% step over on 3/8" because they seem to deflect really easy when pushed hard. Also program a finish pass, climb cut, where you are removing about .010" to .015" of material. I was using .005" for a finish pass and my friend said that mills need to "load up" to a sweet spot of torque and then will cut the best. If the finish pass is too light it will bounce around and vibrate more.

[tikka308]

@BlueFin - thanks - great advise. I'll try 5100 RPM at 20 IPM and use more coolant. And climb mill... Question: anybody know it it's OK to start the machine (cold...) and run at 5100 RPM (series II mill...) or do I need to let it warm up? I don't recall seeing anything about a warm up in the manual, but at 5100 RPM, it's really huffing (versus, say, at 2,000 RPM, it's very quiet.

[BlueFin]

Question: anybody know it it's OK to start the machine (cold...) and run at 5100 RPM (series II mill...) or do I need to let it warm up? I don't recall seeing anything about a warm up in the manual, but at 5100 RPM, it's really huffing (versus, say, at 2,000 RPM, it's very quiet.

I don't know about warm up as it relates to bearing life, but, I learned the long hard way that my Tormach will grow from a Z0 to a Z -.001" ~ .0015" from cold to warm/hot. Your very first part will be correct Z height, but then the next parts will be short because the spindle nose stretched out. I now run the spindle at 4500 RPM for 10 minutes before milling anything important.

[neilw20]

My SX3 needs 30 minutes at 3500 RPM so that Z is almost constant.
About 0.035mm, or about 0.0014"
It still changes slightly for 3 or 4 minutes when cutter is first under load, and if you stop cutting it shrinks a bit (5 microns) within 2 minutes.
Yes, I can measure it with my 1 micron resolution DTI.

[David Bord]

I get that kind of problem when not running enough coolant or using dull tools. The scallop looks much larger than what I normally see when cutting. Id up the RPM and slow it down a bit.

David

[tikka308]

Update: I re-did this cut last night with three changes:
1) Climb (versus convention) milling
2) Better coolant flow/pressure to get the chips out
3) Higher RPM, lower feed of 5100 RPM @ 20.5 IPM. (Compared to 4000 RPM @ 30 IPM when I had the bad results).

This remedied the issue - the part looks great now.

My only question is that 5100 RPM @ 20.5 IPM with a 2-flute end mill is only a 2thou chipload per tooth. G-wizard is telling me I can take almost twice that - 0.0036 CLPT. So I am going to experiment with higher IPM feed rates to see at what point the chipload starts causing finish problems... I have to think the Tormach is capable of more than 2thou per tooth...

[BlueFin]

I have fiddled with the settings on a production part that I make and finally ended up happy with; 1/2" Three Flute HSS Niagara 37 Degree Helix polished bright finish end mill, 4500 RPM, 45% step over, 25 inches per minute, and a fire hose of flood coolant. This comes out to be .0018" chip load per tooth. With a little bit of RPM bog down at it's heaviest cut I might be hitting .002" ~ + chip load.

After 1 hour of cutting like this, 10 gallons of flood coolant will be warm to the touch, and there is a pile of swarf that will almost fill a 5 gallon bucket. If I tried those same settings on a 3/8" two flute end mill I think it would deflect the end mill all over the place or maybe break off. I also have a 30 degree Niagra 1/2" three flute (identical to the one above, but just 30 degree instead) and at the same feed rates it screeches and squeals like a 1970's Burt Reynolds movie. The surface finish is not near as good either.

[tikka308]

BlueFin - Thanks! Everybody loves hearing about specific, proven recipes. I'll have to pick up one of these end mills. Just curious - where do you buy your end mills?

[BlueFin]

If ordering online I get the high end stuff from MSC and the cheap stuff from Enco, there is a AirGas just down the road from my house and if I need just one thing, and can wait a week for it I will order from them because there is no shipping (truck comes from Seattle once a week to each AirGas store).

MSC and Enco send out a sales flyer all the time and they often have the usual needed things on sale (taps, end mills, etc.)

I have been very happy with the larger diameter high helix Niagara three flutes in aluminum, for really small end mills the Atrax carbides are good, my Tormach has been running an Atrax 1/8" and then a 1/16" 4 flute for the last 3 hours on a steel job. The spindle is good and warm now.

Someday I will start using OSG, but I am still afraid of breaking those things. But I am told that they are cnc ground along the Helix, where other end mills are usually ground around the perimeter in a circular fashion.

[twocik]

Another great aluminum cutter that was recommended to me was a fast spiral 60° helix from McMaster-Carr. I mainly use this for finish passes, but works great either way.

Part Number: 29335A55

[CROSSHATCH]

Tikka! You upgraded, I hope to soon. I need to.