I have been struggling to figure out the proper speeds and feeds lately. I have gone through the math but I just can't seem to make it apply to the X2. I machine mostly 6061 aluminum with end mills between 1/4 and 1/2. I thought I had things working just 'OK' with the 1/4 but started using a 3/8 to save on some machining time but it didn't work out very well. Plunging was a nightmare. It would shake the entire machine.

I have a belt conversion and for the 1/4 end mill, I was running on the slower pulley at maximum (around 1700 RPM) with a Z-feedrate of about 1ipm, an xy feedrate of around 5.5, and a depth of cut of .1. I was using new endmills and noticed the finish on the Z was not too great. I tried these same rates with the 3/8 and it was even worse. I monkied around with it for a while last night and noticed that with the 1/4 end mill (two flute btw) if I put the belt on the other pulley and run it at max (around 4K RPM), .5ipm in the Z, around 5.5 in the xy and with a depth of cut of about .05 that it seems OK but I'm afraid I may be dulling the end mill.

Realistically, what should I expect to be able to do in 6061 with a 1/4 or 3/8 end mill on an X2? I have done the speed/feed formulas and the RPMs come out to something like 6K plus but I have read others state that it should be 1500.

thanks,
Kevin

What are you using for a cutting lubricant/coolant?

I am using a Noga minicool mister with kool-mist coolant - I have used WD40 in the past. It seems better but I don't really want to stand there spraying the cutter the whole time.

The X2 is not good at plunge milling. This is because there is too much flex in the machine. I have seen the whole head wobble when plunging into metal, and thats when I decided to lap the ways, and have a look at the Z axis. I measued deflection at the head to more then 0.3mm when I put about 40kg pressure on it. Now I have it down to 0.1, and it's all in the connection between the collumn and the base now.

If you have enough room for it, try not to plunge directly into the material, but make a linear movement on 2 axis (Z and X or Y) or a ciruclar interpolation with Z feed.

My software offers that. I will give it a shot. What about xy feedrates? do you thin .1 DOC and 5.5IPM @ 4K RPM is reasonable?

Check that your endmills are center cutting, some are not and even some cheap ones that should be are not sharpened correctly.

With High Speed tooling you can run at 800 surface feet per minute on aluminum so with a 3/8" cutter run at your maximum.

Your suggested DOC and feedrate are conservative but you may be limited in power; feedrate can often be 0.001" per tooth which gives 8.0ipm and DOC can be 1/2" cutter diameter. However, these may be simply impossible on a lightweight machine.

They are center cutting for sure - Brubaker tool is the specific brand. I will try it tonight and just crank the RPMs up and see what happens.

thanks

I cut 6061 with a 4 flute 1/4 HSS endmill @ 4500 rpm .075 DOC @ 10 IPM.
It's a nice middle ground, cuts away the material fast enough but still leaves a good finish.
1700 rpm is way too slow for that small of an endmill.
If you use 300 SFM in this calculator (http://www.americanmachinist.com/Calculators/SpeedsFeeds.aspx)for aluminum you can see the RPM recommendations.
I've seen SFM recs. for aluminum up to 1200 but that's for the big boys.
Our hobby machines do well at the lower end of the recs.