Originally Posted by
UWP_Wes
I do not agree about the chip load. As you approach the max SFM (around 3000 in aluminum), decreasing the feed rate can destroy an end mill in fractions of a second.
UWP_Wes, why does reducing the feed rate destroy the end mill in fractions of a second? Is no reduction at all possible, or is there something more at work here?
My answer is that there is a particular phenomenon the governs how far you can reduce the feedrate. It's pretty straightforward to understand, and very quantifiable. It behaves the same regardless of surface speed, however, the cutter will fail faster if you're already at the surface speed limit because it will overheat, soften, and dull the edge that much faster.
You only need to maximize chipload to maximize MRR's. The sweet spot for surface finish will involve somewhat less chipload. The lower limit of chipload is a function of the radius of the cutting edge. That's not the radius of the tool, but the radius of the edge itself if highly magnified.
Here are the two cases:
The top one has a chipload > edge radius. Lower one has chipload less. Top one shears through the cut by getting the edge radius under the chip, while the bottom one has to scrape the material. That's what's referred to when machinists talk about running too slow and "burnishing" or "rubbing".
And yes, it will dramatically increase BUE in aluminum if you get close to this chipload range. You can see pretty graphically why from the drawing. The lower image is practically inviting the aluminum to weld itself to the edge.
But there are chiploads that do not burnish that are much less than the recommended chiploads which are aimed at MRR. Given that all chips leave a scallop behind but smaller chips leave a smaller scallop, you want to run less chipload to get a better finish.
The biggest issue is most cutters don't have a documented edge radius to go by. You have to pick a guestimate. 20% of recommended chipload as the absolute lower limit is a pretty good guestimate in my experience, but if you want to be on the safer side use a higher percentage.
Cheers,
BW
Try G-Wizard Machinist's Calculator for free:
http://www.cnccookbook.com/CCGWizard.html