CNC Feed Rate, and CAM software

[Levansic]

The proposed plunge speed is what caught my eye. A good rule of thumb is 1/10th the fully engaged (100% cutter width cutting) feed, and avoid straight plunges like the plague.

If you plan to do NC cutting, as opposed to hand cranking, you really should step up to carbide cutters. They can cut 2-4 times faster and last 10 times longer in total cut. Additionally, you can get some great ZrN coated mills, with edge geometries suited to cutting aluminum (proper rake and adequate clearance), and cut up to 10 times faster, without suffering the dreaded aluminum buildup on the cut edge. Aluminum buildup leads to galling, essentially friction welding. This breaks endmills.

I will second the 3-flute cutter as a great go-to for aluminum. It is more rigid and allows 50% more feed than a 2-flute, and has better clearance than a 4-flute. Chip evacuation is critical for aluminum.

-- Len

[mplanchard]

Sounds like you're learning.
What ever you use, first make certain any long hair is tied back, no baggy clothing and safety glasses. Never machine alone.

Mastercam has been around since the early 1980s. Started in Conn. USA.

Having the SolidWorks - Mastercam experience is a good one.

Mastercam has a lot of teaching materials and a certification. I would check with them but a machining handbook is good for any team for mfg.

Before you machine, run your part through DFM Xpress inside of SolidWorks. You will get a series of messages if holes are too close to edges or too deep or tools just can't machine that square hole.

You can design features in SolidWorks that cannot be machined or too expensive or will add too much stress. DFM Xpress helps answer questions before manufacturing.

Try to review with a mentor if you can. Marie

[Jared]

I just got back from cutting 0.25" aluminum plate on a Tormach PCNC 1100. We used a 1/8" and 3/16" two flute endmill. Like Cory said, we started with 12.8 IPM from G Wizard, but we got a bad finish on some of the bearing holes, so we slowed down to about 8 IPM, and got a great finish. It's hard to tell in the picture, but we got a pretty rough finish on the part. You could probably use the 12.8 IPM for roughing, then take a final pass with a really small cut width as a finishing cut. When we slowed down, the little scrape marks from tool deflection went away. It's also really important that you get the coolant on the actual bit.

Also, you should definitely slow down the plunge rate. We had 6 to begin with, and broke a 3/16" end mill, and we were fine once we brought it down to 4.

I also agree with your opinion of MasterCAM, but once you get used to the silly setup, it's actually really powerful. It'll automatically do all sorts of cool stuff, like tabs, finish cuts, and depth cuts for you. I do agree that it's not perfect though, the command "regenerate all dirty operations" isn't exactly obvious.

[Mr. Mike]

Roy uploaded this to CD-Media back in June.

ME Consultant
By: roystur44
New: 06-21-2013 12:12 PM
Updated: 06-21-2013 12:12 PM
Total downloads: 62 times

Machining Calulator

ME Consultant is a powerful collection of machining calculators and data tables organized inside a graphical interface. It's intended primarily for CNC programmers, engineers, planners, machinists, and hobbyists involved with machining or machined products. ME Consultant is freeware and there are no restrictions on its use

[DonRotolo]

Cutting speed and spindle speed are both functions of the tool manufacturer's recommended chip load. Too little and too much chip load are both bad.

For example, I use an Onsrud single-flute cutter on a router. It needs to see 0.004-0.008 chip load. At 10,000 RPM, that means I need to move about 0.006 per revolution, which comes to cutting at 60 IPM. (With 3 flutes, you'd need to move 3x faster, or 0.018" per rev - so speed would be 3300 RPM for 60 IPM, assuming the same recommended chip load)

Now we consider cutting depth: My machine is definitely unable to cut at 1D (meaning 1/4" deep for a 1/4" cutter); instead I cut at 1/2D. If my machine was beefy enough, the tool can handle 2D.

That's for conventional milling around a perimeter. For slotting, I'd cut it down near the minimum 0.004" chipload.

Lastly, this includes either an air blast (wood, plastic) or air with mist coolant blast (for aluminum) to make sure all chips evacuate the cutitng path. Re-cutting chips is very bad. Also, there is a vacuum system (a 2.25" shop vac) that scavenges the chips and keeps the machine clean.

The bottom line: There is science behind selecting feeds and speeds, the tool manufacturer is your friend, so go and do the math.