[SCzEngrgGroup]

Chipload is one of the things I have had the hardest time with. I don't understand the concept well. Is there a site, or something, that has a good explanation for the beginner? I mean, do I actually pull chips out of my swarf and measure them to determine how I am doing?

It's very simple - just how thick a chip each tooth will peel off. If you're turning 1000 RPM with a 2-flute cutter, and want a 0.001" chipload, then feed at 1000 * 2 * 0.001 = 2 IPM. For 1/8" and up, chipload scales linearly with cutter diameter. A good number as a base is 0.002" chipload for a 1/2" tool. So, 0.001" for a 1/4" tool, and 0.0005" for a 1/8" tool. Below about 1/8" you generally have to back off further, to keep from over-stressing and breaking the tool. If chipload is too light, the tool will get hot, and you'll have problems with the chips welding to the tool. When chipload is right, most of the heat leaves with the chips, and the tool stays relatively cool. So, if your chips are not hot, you're feeding too slow. If your tool breaks, you're feeding too fast. Calculate chipload based on tool diameter, then calculate RPM based on SFPM, and take a shallow cut. If you get good surface finish, then go deeper. When surface finish deteriorates, or the spindle slows down, you've gone as far as you can. Where that happens, depends on the particular machine. The whole trick is getting the right combination of RPM, feedrate, and DOC. Having any one parameter off will screw up everything. Going too slow is just as bad, if not worse, than going too fast.

For aluminum, use only uncoated 2-flute tools. 4-flutes will clog, and carbide is a waste of money on a machine as lightweight as a Taig. You will find mist coolant highly beneficial. Flood is totally unnecessary, even on a much larger machine. I run a full-size CNC'd 9x49 knee mill with a 3HP spindle, and run 1/2" tools, 1/2" deep at 30+IPM using only mist coolant.

Regards,
Ray L.

[mike_mccue]

Thanks for the hi quality explanations.

Very Helpful!!!!

best regards,
mike

[Jeff-Birt]

Using carbide tools on such a small machine is a complete waste of money. There is absolutely no advantage.

Not exactly true. On larger tooling you may not be able to take advantage of the increased feeds/speeds that carbide tooling offers. But carbide will last longer and there may be a cost advantage in the long run, providing your not breaking tools left and right. With smaller tooling it is a completely different ballgame and a definite advantage. With 1/8" and smaller tools, when cutting aluminum, the biggest limitation is the 10K max spindle speed.

[SCzEngrgGroup]

Not exactly true. On larger tooling you may not be able to take advantage of the increased feeds/speeds that carbide tooling offers. But carbide will last longer and there may be a cost advantage in the long run, providing your not breaking tools left and right. With smaller tooling it is a completely different ballgame and a definite advantage. With 1/8" and smaller tools, when cutting aluminum, the biggest limitation is the 10K max spindle speed.

I'm not even sure I agree with that. I find I get almost infinite life out of my small HSS tools. The large ones tend to get dulled and/or broken, because I push them so much harder. I've been using the same 1/8" and 3/16" HSS endmills for almost a year now, and they've each done miles of cuts. It's the big ones I wear out. For those, carbide is helpful, for the added rigidity if nothing else. But that advantage isn't there on a machine the size of a Taig. No harm in using carbide if you get good pricing, but the economics don't work for me, and I find the extra sharpness of HSS helpful on the small tools.

Regards,
Ray L.

[Fixittt]

Carbide is not a good idea also due to the vibration within the machine as it cuts. These light weight do not absorb much vibration. We all know what happens if you drop a carbide endmill right? Now thing of that constant banging as its trying to cut.


Finding the correct chip load is often hard on small machines as it was mentioned....... A little thing I do is start off with fast RPM and slow feedrate. and adjust them untill I get the best looking chips. and remember, its always better to make dust then it is to snap an endmill. Sure you will rub it to death, but at least it had a life.... better then just snapping a new tool.......

[Jeff-Birt]

Carbide is not a good idea also due to the vibration within the machine as it cuts.

Huh? I can make my Bridgeport Series II vibrate as well, but only if I'm doing something stupid. If you have a lot of vibration then you have a problem that you need to fix. Could be machhine is not trammed properly, dull tooling, improper feeds/speeds, etc.

[Riceburner98]

I've used nothing but carbide on my Taig since the day I bought it. (cheap on eBay) The only time I break a tool is when I'm the idiot (or the Z hangs up) and forget to raise the Z before doing a rapid.. Also at 10k RPM for extended periods of time, you'll (well, I do..) fry the stock Taig spindle bearings pretty quick. I gave up on the Taig's slow feeds and replaced the X and Y axis with linear slides / ballscrews. The Z is still stock Taig as well as the spindle. I just couldn't take 40ipm rapids any more. The best upgrade I did while the Taig was "stock" was to swap the "PacSci" motors that came with it for the Xylotex 269 (??) oz motors, and swap the Xylotex board with "real" stepper drivers and a 48v power supply. (IM483 drivers on eBay for $30 each. But the Gecko 4-channel would work just as well) I think I saw a max of 60ipm on the stock Taig leadscrews with that setup. Too much backlash and not enough speed led to the linear slides which gets me 400ipm +. I'll cut with a 1/8" endmill at 10k rpm and 120ipm, small depth of cut, then a cleanup pass afterwards a bit slower and full depth. The Taig is a great "starter" mill for small fun stuff like this. But now it's just too small and it's time to build a new one. It's an addiction!

Now, use a "real" mill like a Bridgeport (or the Grizzly we have at work) and take that full .5" depth of cut like butter and you'll really hate the Taig. LOL Wish I could CNC the Grizzly...

[vonnieda]

It's very simple - just how thick a chip each tooth will peel off. If you're turning 1000 RPM with a 2-flute cutter, and want a 0.001" chipload, then feed at 1000 * 2 * 0.001 = 2 IPM. For 1/8" and up, chipload scales linearly with cutter diameter. A good number as a base is 0.002" chipload for a 1/2" tool. So, 0.001" for a 1/4" tool, and 0.0005" for a 1/8" tool.

Thanks! That's the clearest explanation I've seen of it, and now I get it.

Jason

[tikka308]

Just throwing in my $0.02 -

1) I cut 6061 Aluminum at 0.05 DOC, 6,000 RPM with a 2-flute, 0.25" HSS end mill (chipload of 1thou) quite frequently with no problem.

2) I use carbide exclusively when cutting steel on my TAIG. I cut 1018 and, sometimes, 4140 and as I understand it, HSS would simply dull after a few minutes of cutting. I've been using Altrax 4-flute 0.25" carbide endmills from enco (about $7 a piece) and they work well.

FYI - I'm using a Trico MD-1200 misting-type coolant for both aluminum and steel.

[vonnieda]

Just throwing in my $0.02 -

1) I cut 6061 Aluminum at 0.05 DOC, 6,000 RPM with a 2-flute, 0.25" HSS end mill (chipload of 1thou) quite frequently with no problem.

Thanks. This kind of information is just what I was hoping for. Some basic numbers that I can try out and see what's going on.

Thanks,
Jason von Nieda

[Riceburner98]

Just throwing in my $0.02 -

1) I cut 6061 Aluminum at 0.05 DOC, 6,000 RPM with a 2-flute, 0.25" HSS end mill (chipload of 1thou) quite frequently with no problem.

2) I use carbide exclusively when cutting steel on my TAIG. I cut 1018 and, sometimes, 4140 and as I understand it, HSS would simply dull after a few minutes of cutting. I've been using Altrax 4-flute 0.25" carbide endmills from enco (about $7 a piece) and they work well.

FYI - I'm using a Trico MD-1200 misting-type coolant for both aluminum and steel.

If you don't mind my asking, what kind of speeds / feeds to you use on the steel? I haven't had very good results on the few steel parts I've tried.. Ended up taking .005" passes I think.