I’m running a Nomad3, with Fusion360. When changing over from my prototype runs in plastic to make my part in 6062 aluminum, I need to change the feeds and speeds accordingly. My question…
In F360, the settings of spindle RPM, surface speed, cutting feedrate, feed per tooth, and feed per revolution are (obviously) all related. When I change one in Fusion, others compensate. But which should I be setting, and which should I allow F360 to derive from my inputs?
Furthermore - what suggestions do you have for a single flute O cutter, 1/8" diameter?
Give it a spindle RPM and feedrate(s), the rest will follow.
The magic value in aluminium is a chipload of 0.001", so assuming you want to max out RPM at 24000 on the Nomad3, the associated feedrate for this single flute endmill needs to be:
FR = 0.001 x 1 (flute) x 24000 = 24 ipm
With a possible complication that if you are going to use a small stepover (optimal load), you will need to compensate for chip thinning, which will call for a higher feedrate than this.
I can’t remember what recommended setting CC library has for a #274Z in aluminium, check that too to confirm that I’m not telling you silly things.
Depth per pass: depends on the type of toolpath you will create (adaptive or regular), the answer can be anywhere between 5% of the tool diameter and 100%.
Be sure to use ramping entry, too. Ideally helical ramping. And some air blast if you can (though single flute have great chip evac)
Yes.
Fusion360 also has entries for the lead-in/lead-out feedrates (which apply only during…lead-in/out), but to be honest I almost always paste the same value in all fields, I’m not a metalhead cutting anything so hard that it requires to have slower lead-ins.
Thanks - that’s hugely helpful. Running a job with these settings now, so we’ll see.
Fusion360 has tons of options, but I’m drinking from the firehose. It doesn’t tell you which are dependent or independent values in their software.
I’ll let it calculate lead in, lead out, ramp, and plunge, because those aren’t used much (by me) and they’re slower anyway. But I find “Cutting Feedrate” and “Surface Speed” to be tough to discern, when reading online. Same for “Feed per Tooth” and “Feed per Rev”.
I’ll just set RPM, Cutting Feedrate, and Feed per Tooth from here on out, and let it figure the rest.
You shouldn’t need feed per tooth (nor feed per rev) as this is derived entirely from RPM, feedrate, and number of flutes of the tools (that F360 knows)
Makes sense. But F360 will let you type those in, and then it screws up everything else to compensate. I wish they’d grey out those fields that are just informational, rather than tempt me to type there.
Really appreciate the help - the part just came out of a facing operation, and it’s butter smooth. I think I can speed up my stepover a little because it took forever to cover the surface in 0.3mm increments. I may go 1mm next time, but the 0.2mm step down seemed perfect.
Another quick Q - I have a small operation that requires some 2.8mm holes, which I’ll bore with a 1/16" 2-flute cutter. If I start with the tool settings that worked above, what should I tweak to migrate to 2 flutes (from 1) with a cutter that’s half the diameter?
Keep the spindle speed the same, and slow the Cutting Feedrate?
If you go for shallow cuts like you do, you should be able to go up go 50% stepover or more (this is what happens when slotting anyway…not desirable, but works fine at such limited depths)
I know there’s a lot of stuff in there and it’s initially confusing.
The useful thing about the Feed Per Tooth being editable is that you can set a spindle speed and then just type 0.03mm into the Feed Per Tooth and Fusion will calculate the Cutting Feedrate for you.
You’re right, initially just stick to the RPM and Cutting Feedrate (with width and depth of cut of course) and use the feed per tooth as a bug-check on what you’ve done, but later, it’s handy.