| | |
I have a small CNC mill—Roland MDX-540. According to the specs, the spindle is 400W and operates on 120V. The spindle speed can go up to 12,000 RPM. When doing my rough cutting on 6061, does anyone have any recommendations on speeds? I usually rough cut with a 1/4" flat end mill. I am get inconsistent results so I am trying to figure out if it's my settings or something mechanical. I already have a new belt that goes from the spindle to the motor on its way as the one I have looks really worn and may be slipping. The problem that I am having is that once in a while the spindle will get stuck in the block I'm cutting. Yesterday I had no problems and it ran like a champ at 10,000 RPM cutting about 35 inches/minute. Today to help with the problems I am cutting at 8,000RPM and 9 inches/minute but it still gets stuck sometimes. Sometimes it will just be cutting a straight path and the bit will slow down and sometimes speed back up and sometimes get stuck. My software has a meter that shows load on the spindle motor and it never really goes above 30% today—yesterday I was running it just under 50%. Does it mean my end mill is worn out? Any insight would be great!
Are you using a two flute mill or a four flute mill?
Are you using coolant/lubricant or cutting dry?
Generally with 6061 a two flute cutter with a high helix is best because there is more room for the chips and the helix helps evacuate them from the cut.
Also 6160 needs some coolant/lubricant. You do not have to flood it on when using small cutters on small machines but at least spray a bit on every few seconds.
An open mind is a virtue...so long as all the common sense has not leaked out.
Use a 2 flute uncoated carbide or HSS end mill
Use max spindle RPM
Hit it with a little squirt of WD-40 every inch of cutting or so. When it starts looking dry, give it a little more. There will be smoke if you are cutting aggressively. Probably better not to breath that.
Matt
Thanks for the input. So what's the rule for aluminum as far as a spindle speed? Max it out as Matt says—that's the best? If i have any cutting troubles does reducing the spindle speed help? Or just reduce the feed speed?
Surface speed for carbide in Aluminum is 600-1200 surface feet/minute. with a 1/4" endmill, that is a range of 9,000-18,000 RPM. Very few folks have a spindle capable of those speeds so "max it out" is the closest you will get. Keep the spindle speed and feedrate and just reduce the depth or width of the cut if you are having problems. If you get chatter playing with the speed and feed a little may help, but for poor finish or vibration or stalling, you just need to take a smaller bite.
Also consider that your "load meter" might not mean jack and you could well be overloading your spindle motor. From your description it sounds like lack of lubrication was your biggest problem but you didn't answer any of the questions posed so its hard to guess.
Matt
http://www.endmill.com/pages/trainin...d%20Drills.pdf
Last edited by keebler303; 03-16-2012 at 04:20 PM. Reason: Meant to put in a link
Max RPM, and your feedrate seems quite slow at that RPM. Probably building up lots of heat. Use lubricant as suggested. Watch for high helix end mills pulling out, not sure of the clamping system on that.
Sorry, didn't answer all the questions especially when I am here looking for a diagnosis!
Anyway, no cutting fluid. But I ran all day yesterday with no cutting fluid and no problems. Also, mill is not hot at all—just checked it.
Using a 2 flute mill with a high helix. I think it's carbide.
Based on that chart it think the problem is the default on my software is having me take too big of bites. I'm assuming Chip Load Per Tooth means how far down the Z axis goes each time it starts a new layer of removing material. The chart says .0020" per tooth which would mean .0040" for me since I have the 2 flute mill—right? I just checked the machine and it is doing .0083" for each layer of material removal. That must be why I had the troubles earlier although I have not had any problems for the past couple hours.
The 600 to 1200 (7200" to 14400") Surface Feet per Minute blows my mind. Currently I am running 15" per minute. So if I turn my spindle speed up to max (12,000) and lessen the bite its taking out of each layer to .0040", theoretically I can set my feed to 7200" per minute with a 1/4" mill? Am I interpreting everything correctly?
No you are not interpreting things quite correctly.
Surface speed, or surface feet per minute (SFM) is the peripheral speed of the cutter. Circumference in feet multiplied by rpm.
The rate at which the cutter is moved through the material is the feed which is mesured in inches per minute (IPM). This is feed per tooth multiplied by number of teeth multiplied by rpm.
An open mind is a virtue...so long as all the common sense has not leaked out.
So then I can't run at 12,000 RPM, right? On a .25" mill, each tooth is traveling .785" x 2 teeth x 12,000 RPM = 18,840 (1,570 SFM) which does not fall in the range of 600-1200. That means the max RPM I can run is 9171. Does that compute right?Originally Posted by Geof
Not the mill heating up! It's the cutter heating up in the material.
Here is one of many on line calculators
Surface Feet Per Minute
No you are still not getting it quite correct.
Take away the 2 from your calculation, the tooth count is irrelevant for the peripheral speed calculation.
The tooth count is only used for calculating the feed rate.
Incidentally don't worry too much about sticking within the 600 to 1200 range, it is possible to go much faster than 1200 FPM with carbide tools in 6061. We run 1/2" and 5/8" cutters at speeds up to 11,000 rpm which is well above 1200FPM.
But do use coolant.
An open mind is a virtue...so long as all the common sense has not leaked out.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
