CAM Pocketing/Contouring Methods

We have a new to us CNC machine (Fryer MB-14 Bed Mill 5hp spindle 4200 RPM max). We are using HSMExpress CAM software in SolidWorks.

Hoping for a little help selecting the best technique(s) for pocketing and contouring. Consider a 1/4" AL gear plate that requires several pockets and the outside contour. We have 1/4", 1/2", and 3/4" carbide and HSS 2-flute end mills available.

For the pockets should we use:
a) the 2D Pocket operation which plunges/ramps to a depth, clears the entire pocket and then repeats at the next depth.
b) the 2D Adaptive Clearing operation which seems to spiral down through the entire depth and then works its way out until the pocket is cleared.
c) other?

For outside contour should we:
a) ramp/contour a groove down until the depth is reached?
b) work for the outside and come in similar to the adaptive clearing?
c) other?

On a mill, Option B. On a router, I’ll often use Option C for outside contouring.

Here’s a recent thread that gets into depth on what you’re asking: http://www.chiefdelphi.com/forums/showthread.php?t=124902

I saw that thread, lots of good information about plunging and ramping but I’m still wondering about using the side of the cutter to clear out a pocket/contour. The CAM program defaults to a huge side cut in the Adaptive Clearing mode and I was hesitant to load the cutter up too much for fear of breaking the bit. Haven’t seen any calculators for this.

My defaults for a 1/4" 3 flute tool in 1/4" aluminum are 40% radial cut width at full depth when pocketing. You should be able to do the same, albeit at a lower feed since you have a slow max spindle speed. The main limiting factor here is ability to clear chips so you are not recutting them.

If you’re using a half inch end mill, and you’re going slowly, you should have a problem going with a pretty big side cut if you do it in steps (try 0.1" each step). If you want to go faster, look into getting a three/four flute bit for roughing. To echo what Cory said, make sure you clear the chips away. We’ve hooked an air line onto the machine before to blow them away, but it makes a huge mess.

I’d also recommend doing a finish pass. I know in MasterCAM there’s an option to leave a small amount of material (I think we used 0.050) on your rough cut, the when you go for the finish pass you are removing only 0.05" so you’ll get a great surface finish.

Finally, if you’re looking for a calculator for these sorts of things, try g-wizard.

Perfect. Do you spiral through the material? If so, what ramp angle do you use?

I try to drill plunge points with a larger tool. That can be a pain on a machine without a tool changer.

If the pocket is big enough I will use the helical entry option, with the default parameters. If not I’ll just plunge slowly (10 IPM or so, with full flood coolant).

You can get a recommended ramp angle from your end mill manufacturer.

In my experience, helixing in at a 4 degree angle is quite decent (that’s on high-end VMC’s with aluminum optimized tooling, though. Your mileage may vary.) One good way to tell is how the chips accumulate. If they’re birdnesting around the top of your tool, ramp in slower, and get better coolant. Flood, if possible (although you don’t have an enclosure. Mist coolant and air jet, probably.) Ramp along pass isn’t quite as good, if you’ve got that option, but it can do a better job sometimes of keeping the entry contained within the machined area.

Cory’s suggestion of drilling the entry points is a good one, if possible. End mills hate, hate, hate, cutting down. Even ramping isn’t very good. Your mill has the option of having a toolchanger, it says (CAT40? Seems overkill for 5HP…) For cutting the outside, your tool shouldn’t have to plunge through the part, just profile from the outside in. Internal pockets, use whatever stepdown your cutter can take (may or may not require multiple passes.) If you leave maybe 2-3% of your cutter diameter for a finish pass, you can take all of that in one pass for finish and accuracy. Same rule for finishing outer walls.

Last note: I don’t know whether HSMExpress has any constant-engagement toolpaths (trochoidal?) If so, use them. They’ll limit the engagement in corners (where engagement angle normally spikes. For example, 50% cutter engagement turns into 75% when you hit an internal 90 degree corner), allowing you to turn the whole cut up, and keeping your tool safe.

EDIT: Sorry, that 50% cutter engagement spikes to 100%. My bad, long day.

A cutter programmed for a 40% step over will see nearly 100% engagement when it hits inside corners of the same radius size. An inside corner radius that is 3 times the cutter radius will see the engagement of 52%.