Adam Stein

Follow

--

If you just want a rundown of typical CAM settings, read on. If you need insight on how to adjust these settings, read the longer guide.

The word “typical” is doing a lot of work here. I’m assuming you’re doing 2D work in wood with a 1/4" or 1/8" flat end mill bit. These settings might work in other contexts as well, but the further you drift from this scenario, the more likely you are to need to make changes.

In the interest of keeping this document as short as possible, I skip mention of any settings where you should take the default.

Create a new set-up by choosing CAM > Setup > New Setup.

Work Coordinate System (WCS)

Orientation: Select X & Y axes Note: most of these options for this field are variations on a theme. Use whichever works, and adjust the other WCS parameters accordingly.

X Axis: Select an edge in your model that is aligned with the X axis.

Flip X Axis: (optional)The X (red) axis should be pointing in the direction of ascending X values. If not, check this box to flip its orientation.

Y axis: Select an edge in your model that is aligned with the Y axis.

Flip Y Axis: (optional)The Y (green) axis should be pointing in the direction of ascending Y values. If not, check this box to flip its orientation.

Origin: Stock box point

Stock point: Choose the lower-right point on the top edge of the stockAssume you are looking straight down at the stock from above, oriented as it will be in the bed of the ShopBot. Make sure to place the origin on the top of the stock, not the bottom.

Model

Model: Select the bodies that contain your cuts.

Stock

Stock Side Offset: 0.5 inchChoosing a value of at least bit diameter * 2 makes it easier to see your cuts during simulation. However, if your model matches your true stock size exactly, you may want to set all of these to zero.

Stock Top Offset: 0

DimensionsThese values are automatically calculated based on your prior selections. Review them to verify your selections. If the Z value is way too large, for example, you probably didn’t properly orient your axes (i.e., Fusion thinks your X or Y axis is the Z axis). If the Z value is close but not quite right, you might have forgotten to set the ply of your stock correctly. In short, make sure these values describe the dimensions of the physical thing you are making. If they don’t, figure out why before proceeding with any cuts.

Take the defaults on this tab. If you are feeling saucy, change the Program Name/Number to something more human-friendly.

Create a pocket cut by choosing CAM > 2D > 2D Adaptive Clearing.

Tool

Tool: select toolFor starter projects, there’s a decent chance you will be using either a 1/4" or 1/8" flat end mill, and you don’t need to be concerned with other tool parameters such as material.

Coolant: DisabledUnless you’re using a coolant, in which case, choose that.

Feed & Speed

Note: Feeds and speeds are a complicated area, and I considered leaving this bit blank to force you to deal with them yourself. But in the interest of creating a “just works” guide, I’m providing the following heavily caveated values: IF you are cutting wood, and IF you are using a 1/4" or 1/8" straight end mill, you are unlikely to kill yourself using the following values, although you may break a bit.

Nevertheless, I highly recommend that you talk to someone who is experienced on your particular machine to check your feeds and speed settings if you are not feeling confident.

Spindle Speed: 12,000 rpm

Surface Speed: Default (calculated for you)

Ramp Spindle Speed: Default (should match spindle speed)

Cutting Feed Rate: chip load * # of flutes * spindle speedFor wood and 1/4" bits: chip load = 0.01For wood and 1/8" bits: chip load = 0.005

So for a 2-flute 1/4" bit: 0.01 * 2 * 12,000 = 240 inches per minute

The thing is, you’re not going to actually achieve that speed for small cuts, which is why you should educate yourself about feeds and speeds…

Lead-in feed rate: Same as cutting feed rate

Lead-out feed rate: Same as cutting feed rate

Ramp feedrate: Same as cutting feed rate

Plunge feedrate: 50% of cutting feed rate

Pocket Selections: select the bottom of the pockets you want to clear

All of the defaults are fine.

Passes

Direction: ConventionalThis is another complicated topic…

Multiple depths

Multiple depths: check

Maximum Roughing Stepdown: 1/2 of bit width

Stock to leave: uncheckedI’m assuming that you don’t plan to do a finishing pass, so all material will be removed as part of the roughing operation. If this isn’t the case, you will need to check this box and set some further parameters.

Generally you can take all the defaults here. But if you are cutting pockets that are not much bigger than the width of the bit, you may need to adjust the ramp parameters.

Create a contour cut by choosing CAM > 2D > 2D Contour.

To do a through-cut, you need to cut all the way through the stock. Set the bottom of the cut to 50/1000" (1/20 of an inch) below stock (or below selected contour, assuming the contour is aligned with the bottom of the stock). Remember to make your tabs higher than you would otherwise, to compensate for the extra depth of the cut.

Tool

Tool: Choose your bitProbably you are using 1/4" or 1/8" flat end mill. Material doesn’t really matter.

Coolant: Disabled

Feed & Speed

See prior note about feeds and speeds. In a nutshell, these settings should work for wood, but if you are in any doubt, talk to someone who is experienced on your particular machine

Spindle speed: 12,000

Cutting feed rate: chip load * # of flutes * spindle speedFor wood and 1/4" bits: chip load = 0.01For wood and 1/8" bits: chip load = 0.005

So for a 2-flute 1/4" bit: 0.01 * 2 * 12,000 = 240 inches per minute

The thing is, you’re not going to actually achieve that speed for small cuts, which is why you should educate yourself about feeds and speeds…

Lead-in feed rate: Same as cutting feed rate

Lead-out feed rate: Same as cutting feed rate

Ramp feedrate: Same as cutting feed rate

Plunge feedrate: 50% of cutting feed rate

Geometry

Contour Selections: select the contours to cut outChoose the bottom contours of your cut.

Tabs

Tabs: checkedYou only need tabs if you are doing a through cut (all the way through the material), which is usually the case for contour cuts.

Tab Height: 0.1125"For through cuts, set the bottom of the cut to be -0.05" (1/20 of an inch below the bottom of the stock). Because tabs are measured from the bottom of the cut, you need to add the 0.05" offset back into the tab height:

0.05"+ 0.0625" = 0.1125

Tab positioning: up to youIf you choose “By distance,” Fusion will place the tabs for you, at specified intervals. Or choose “At points” to place them by hand. If you let Fusion place them for you, visually inspect them to make sure you like their placement.

Tab Distance: up to youThis parameter is only available if selected “By distance” for tab positioning. The stakes here are pretty low; for bigger pieces, you will generally want to bump this number up, so that you don’t have hundreds of tabs to sand off.

Tab Positions: click on your contours where you want tabs to appearThis parameter is only available if you selected “At points” for tab positioning.

Bottom Height

From: Selected contour(s)Or “Stock bottom,” because generally these are the same thing.

Offset: -0.05 inFor through cuts, to ensure that the bit goes all the way through the material, set the bottom of the cut 0.05" below the contours you have selected.

From: Selected contour(s) (default)

Offset: -0.05"

Passes

Sideways Compensation: Right (conventional milling)Complex topic, yada yada…

Multiple depths

Multiple depths: checked

Maximum Roughing Stepdown: 1/2 of bit widthThe default value here is insane, and will result in crazily long cutting operations. If you find the ShopBot only cutting minuscule amount of material with every cut, this setting is likely the problem.

Rough Final: unchecked

Take the defaults.

Create new drilling cuts by choosing CAM > Drilling.

Tool

Tool: choose your bitYou can drill with a flat end mill, as long as the cutting surface extends all the way across the bottom of the bit. Upcut bits will do a better job than flat or downcut bits at clearing wood chips, but you can get away with using any style of bit by using pecking to clear chips.

Feed & Speed

Spindle Speed: 12,000

Plunge Feedrate: 0.5 * chip load * # of flutes * spindle speedFor wood and 1/4" bits: chip load = 0.01For wood and 1/8" bits: chip load = 0.005

So for a 2-flute 1/4" bit: 0.5 * 0.01 * 2 * 12,000 = 120 inches per minute

Geometry

Hole mode: Selected faces

Hole face: choose one or more holes to drillClick on the actual inside face of the hole, not the contours that defines its top and bottom edges.

Select same diameter: optional, but probably checkedChecking this option tells Fusion to automatically drill all holes that are the same diameter as the one you selected for the “hole face” parameter. If you have a lot of holes in your model, this a lot faster than selecting each individually. The only reason not to check this box is if you need more control over the order of drilling operations.

You can mostly take all the defaults on this tab, although if you are drilling a large piece that isn’t entirely uniform in thickness, you can add some offset to both the retract height and top height to allow for some slop in the material.

Bottom Height

Drill tip through bottom: check this if you’re drilling all the way throughBreak-Through Depth: 0.05" Again, only if you are drilling through the material.

Cycle

Cycle Type: Deep drilling — full retract This causes the drill to peck (drill a partial hole, retract, drill a bit more, retract, etc.). Pecking is especially useful if you are using a straight or downcut bit, because otherwise material won’t clear very well. If you are using an upcut bit or drilling in very thin material, you may not need to peck.

Pecking Depth: bit widthI’m actually not sure how conservative you need to be here. The smaller the depth, the longer your drill operations will take, which may only be a consideration if you are drilling a lot of holes.