18mm Baltic Birch furniture help

[rscherer]

I'm fairly new to using a cnc and recently purchased an axiom iconic 8 machine. I've been playing around with parametric furniture designs using 18mm baltic birch. The first few projects came out pretty good but required a lot of sanding on the machined (cut) edges. I'm using the 1/4 down-cut spiral plunge bit (2 flute) that came with my package. I'm wondering if there are any better bits (diamond/coated) or perhaps some guidance on best feed rate and spindle speed. I'm using Vcarve Pro and I think it auto selects the speeds when I choose the 1/4 plunge bit. Also, the squealing loud noise during the cutting process is beyond miserable. Thanks in advance!

[dadealeus]

Love the designs.

Running a pure down-cut into (effectively) a 3/4" channel is going to shove a lot of chips down into your work-piece. This does two things:

1) The debris being pushed downward into the cut will often "leak" under your workpiece (if it's not near a hold-down). This will cause the workpiece to lift off the table slightly, causing tearout on the backside of the plywood because it's not flush with the spoilboard - hence your increased need for sanding.

2) The chips, not being properly evacuated, will be re-cut into fine dust - generating excessive heat - dulling your tool and causing a lot of the whining you're hearing.

As a potential solution, I'd look into a nice compression bit as an alternative. It will leave you with much less tearout (since you're effectively getting a downcut on both sides at once), and should result in far less heat buildup if your feeds are fast enough. You can actually get away with a 1/8", 2-flute compression bit doing a single pass in 3/4" plywood (the video refers to a single-flute, but I have personally tested a 2-flute and it works well):

-but you're going to get a lot of tool deflection - so if you're using dogbones and such, you're going to need to run some tests to see if the deflection is within acceptable tolerances for your needs.

Personally, I'd opt for a 1/4" compression bit and give that a shot. You should be able to hit 3/4" birch plywood in a single pass (making the cut process quite quick), and have a lot less sanding due to reduced tearout.

Just my opinion, but I hope it helps.

[dadealeus]

On a side note, if you want to run that 1/4" downcut you have, try starting with these feeds and speeds and adjust from there for your plywood:

1/4" Downcut - 2 Flute
Depth of Cut: .25"
Max Width of Cut: .25"
RPM: 10,000
Feedrate: 120 IPM

Plunge Rate: 60 IPM

Shallow depth of cut (for downcut tools) allows the chips to be removed by vacuum or compressed air between stepdowns. If you go deeper in one pass, you're going to get too much debris crammed into your cut channel.

I'm not sure what the Iconic line is capable of, but if you can't hit that feedrate, then lower the RPM proportionally. For example, if you can hit 50% of that IPM (60 IPM), then lower the RPMs by 50% as well (5000 rpm).

In general, people new to CNC milling have a tendency to run their feeds too slowly (I did). -it seems counterintuitive, but if you're hearing whining like that and if you're seeing dust rather than actual cuts of small pieces of wood, then you're running too slowly through the material. You want to blade on the tool to cut small slices of the material off and toss them away from the cut area - not grind the cut like sandpaper (which makes that whining sound). So, if you are hearing the whining, you need to push the tool through the material faster, or slow down the RPMs on your spindle until you are seeing chips of material instead of dust.

If you start getting a lot of chatter (bouncing of the tool), then you need to back off on both feed and RPMs until your machine can handle it. You may also need to try a smaller tool (like a 1/8" bit). Just depends on your machine, your material, etc.

I use a program called GWizard to help determine rough feeds and speeds for all the materials I cut (HDU foam, aluminum, plywood, pine, walnut, maple, HDPE plastic, PPO plastic) and it's great at getting some good starting values that you can then fine-tune.