LinkBack URL
About LinkBacks
What is the flute length on the endmill, and what was your feedrate?
| | |
Please be gentle. I cut aluminum for the first time on my X3 CNC conversion and the contour finish isn't "smooth". Attached is the pic of the slanted pattern I get on my cut.
Background:
- X3 Mill
- 3/8" diameter 4 flute steel cutter, 2.5" long
- 2000 rpm
- climb cut
- half inch aluminum stock material
At first I didn't use coolant, just a wet vac to manually suck up chips. Switched to using WD-40 half way through. Periodically brushed the chips away.
Noticed that the part got hot. When I squirted WD-40 at the cutter it would steam up. Yeah, I probably should have stopped but I'm experimenting and I want the part cut.
What mistakes am I making?
Thanks
What is the flute length on the endmill, and what was your feedrate?
Oops:Originally Posted by HimyKabibble
- 16 ipm
Too dumb to know the flute length. Bought the endmill when I had a Sherline CNC 10 years ago. Just know it is 4 flute, 2.5" inches long, 3/8" diameter, and steel.
thanks
I just ran a job today. 0.090" carbide 3 flt extra length necked down 0.157 flt length 0.850" stick out axle DOC 0.032 radial DOC 0.090 (full diameter) 7500 RPM 7 IPM flood coolant. Had to compensate for about 0.0025" tool push off on the finish pass. Never skipped a beat.
http://www.kirkcon.com/
OK, so let's do some math:
SFPM = PI * ToolDiameter * RPM / 12 = PI * 0.375 * 2000 / 12 = 196 FPM
That's kinda slow - For aluminum, you really want to be 1.5-2X that. But maybe you're limited by your spindle?
For a 3/8" endmill, you want to be around 0.004" chipload for roughing, which would mean:
Feedrate = Chipload * # Flutes * RPM = 0.004" * 4 * 2000 = 32 IPM
You're running about half that feed. You need to reduce depth of cut enough to allow you to run something close to that feedrate. On an X3, I would think you should be able to do perhaps 0.050-0.100" depth when doing full-width slotting, more with a lower radial engagement.
You also indicated the tool and/or work were getting hot. That's a clear indication of too low feedrate - slow feedrates lead to the tool and work getting hot. A higher feedrate will put the heat into the chips, and the tool will stay cool. When you've got it right, the chips should be coming off very hot, and the tool should stay cool. Since you are limited in rigidity, you have to start shallow, then go progressively deeper, and see how deep you can go before the surface finish goes to he11. But you MUST maintain a good chipload! On that machine, you really should not need coolant at all, if you're using the right cutting parameters.
Next problem is using a four-flute endmill - not well suited to aluminum, as it will tend to clog up under heavy cuts. It would be OK for finishing, and light peripheral cuts. A two-flute would be much better for heavy cutting. I find I get as good, if not better, finish with a two-flute. Three flutes are better still, but I don't know any sources for HSS three-flutes, and carbide is really of little or no value on these small machines, so no point spending the extra money. Though, cnctoybox.com has some nice, very inexpensive carbides.
As for surface finish, what you're seeing is chatter and/or flexing due to the limited rigidity of your machine. A heavier cut may, or may not, help chatter, but will aggravate rigidity problems. Unless your machine has truly zero backlash climb cuts may also be problematic.
Are you doing a roughing cut then a finishing cut? You generally want to do a roughing cut, about 0.010" over-size, then take off that last 0.010" with a finishing cut. The light load will make rigidity less of an issue.
Regards,
Ray L.
Ray,
Thanks for the info. I will digest this and do some more experimentation. The X3 spindle will only do 2000 RPM. I also think my bit was dull.
I didn't get an email saying there were any responses from CNCZone so I thought my question went ignored and was kinda bumbed out.
By the way, here is a video of what the plate was for. Another power drawbar with a floating head. I only had to machine the base plate and a spacer.
http://www.youtube.com/watch?v=tbUNKx5wrmw&list=UUPw_8uMdPFrSkW8e4MuBlZQ&index=1&feature=plcp]Movie_0004.wmv - YouTube
Now I just need to learn how to machine with this thing!
Chatter is a sympathetic vibration, the diagonal lines reflecting the helix angle of the tool.
Sometimes you can get rid of it with a simple rpm change on the finishing pass, but once the pattern has set in it tends to echo through to subsequent cuts.
Experiment with speeds, feeds and lubes and see what your machine favours for each tool. If it doesn't favour anything you might try a tool with more than one helix angle, that makes it much harder for it to find a sympathetic vibration.
I did notice that the diagonal line did match the helix angle of the endmill. Also noticed that my endmill was kind of dull compared to the new endmills I just bought.
As Ray pointed out, I found that doing a couple of rough cuts and then a few finish cuts while working towards the final surface on the contour toolpath made a difference.
Looking at getting a fog buster to see if that helps since WD-40 is just not pratical.
thanks for the help
Posting Permissions
| | |
