CNC Feed Rate, and CAM software

[eli2410]

Originally Posted by apples000

W're cutting 3/8" plate in three 1/8" passes with an HSS 3/16" 2 flute end mill using flood coolant. The CNC machine we're using isn't a super-heavy-duty one, but it isn't that wimpy either. We are considering going with a feedrate of 8 or so IPM, and a plunge rate of 5. The spindle rpm will be maxed at 5300 rpm, which I may decrease because I'm worried some aluminum will melt.

We're also curious as to how people make their toolpaths. We have MasterCAM, and a free solidworks plugin, and this is the first year we've used MasterCAM (we have just upgraded from x2 to X4). MasterCAM has many more features, but takes a little bit of getting used to. The software feels like with was written in the early 90's. The "undo" feature only works on certain things. You can't undo a change to a toolpath.

We plan on using climb milling, where outside cuts are clockwise, and inside cuts are counter clockwise (I think), but we'd like some input from other teams as to what works best.

So, last year we used MasterCAM to cut our aluminum, which I believe was 6061. Great product. We switched to EdgeCAM, which is not nearly as good.

Anyway, we use 1/8" and 1/4" inch end mill bit. The 1/8" is an Onsurd 62-606 (or 63-606 can't remember) and the 1/4" is an Onsurd 62-622 (or 63-622, can't remember, I'll check tomorrow and post it on here). We use a spindle speed of 14000 and a plunge of 6 for both tools (no ramping because it makes the part wrong. We plunge straight in). We use a feed rate of 42 IPM for the the 1/4" and 24 IPM for the 1/8". We do depth cuts of .15 for the 1/4" and .05 for the 1/8". We add .02" to the plate thickness to make sure it goes through the plate. We have a Techno 4896 with mist coolant, which we use on the aluminum. If you do use these feeds and speeds, make sure to use the coolant.

If you have any other questions, please post. I'm happy to help out. I'm curious, what machine do you have?

[scottandme]

Originally Posted by sanddrag

Don, where are you buying your Onsrud router bits. Link?

McMaster - "Router bits for Aluminum". 3317A25 is perfect. 18K RPM, ~50IPM on a full slot 1/8" DoC.

Originally Posted by sanddrag

For anyone, what feedrate should I be using when going on a helix plunge into the material with a 3 flute square corners endmill? My CAM package always puts the plunge rate at half the pocketing feed rate, but I worry and back it off a bunch, to like 20 IPM. I'm ramping down on a 3 degree helix.

Best bet is to look up the datasheet for your endmill/call the mfg. I've seen helical ramp angles around 10-20 degrees for some of the "high performance" aluminum endmills, with feed at ~100% of normal feed. Aluminum is pretty forgiving.

[Cory]

Originally Posted by sanddrag;1329576:

Don, where are you buying your Onsrud router bits. Link?

A single flute cutter is useless at 6000 RPM. the main reason routers use them is because at 24000 RPM if you run the recommended chip load for a 3 flute cutter you'd be at 216 IPM. a single flute gets you down to a more reasonable 72 IPM.

[sanddrag]

Originally Posted by Cory

A single flute cutter is useless at 6000 RPM. the main reason routers use them is because at 24000 RPM if you run the recommended chip load for a 3 flute cutter you'd be at 216 IPM. a single flute gets you down to a more reasonable 72 IPM.

Which is exactly what I need on my router that has a 20k RPM spindle.