The geometry for the 1/8 bits that come with the nomad are:
Flutes = 2
Tool Dia. = 0.125
Shank Dia. = 0.125
Overall Len. = 1.5
Flute Len. = 0.5
Stickout (assuming it’s fully seated in the collet) = 0.72
Taper Angle = 90
For the ball nose select Ballnose and for the flat end mill select Normal
Cut depths and widths are purely dependent on the type of cut you are doing. For example, if you are doing a plunge into a pocket, then slotting it, you have no choice but to set the cut width = diameter of the cutter.
If you are not limited by the type of cut, lets say you are using adaptive clearing, and you want to maintain an ideal cutter engagement, then you want to use the cut optimizers (these are the little things next to the depth and width boxes).
At the end of the day, what really matters is what the machine can handle, what the cutter can handle, and what kind of finish you want. Here’s a good approach at making that happen:
- set the HP Limit to ~0.03. Small machines like the nomad are limited by weight/rigidity and not by spindle horsepower.
- Make sure your cutter geometries are entered correctly, especially stickout, because this is how tool deflection is calculated.
- Decide if you are slotting, or using less of the cutter. Set your width based on high material removal rate (more of the cutter), or finishing (less of the cutter).
- Select your surface finish between 1%-100% Rough.
- Click Optimize near the cut dept. Select a deflection allowance based on what kind of cut you are making.
- Make sure the solution converges and gives a reasonable answer. It’s tricked me before!
7 Use those cut parameters.
You’ll instantly notice that the roughing cuts recommended by GWizard are wayyyy more aggressive than what Carbide3D recommends. If you did everything correctly, don’t worry, the machine will handle it (assuming you compensated the horsepower for machine rigidity). You don’t have to worry about breaking/clogging a cutter with these calcs. It’s the whole reason my approach is based around deflection.
- If the cutter stops mid cut: Turn down the horsepower limit. You’re reaching the rigidity limit of your machine.
- If a tool breaks: GWizard tricked you and the deflection calculation didn’t converge. You didn’t read carefully in the little box! Stop rushing!
- Surface finish is bad: Take a more conservative cut, 25% or less.
- Cutter stalled on plunge: Did you remember to enter the correct plunge numbers in the CAM software?
- Cutter stalled on ramp: Set your ramp feedrate closer to the plunge feedrate.
By the way, this was a quick type, so not everything is perfectly explained here. I also oversimplify some things. Best thing to do is read a machinists handbook from cover to cover if you really want to know how to choose your cut parameters.