CNC Programming Z Axis Angled Slot Cut

[Gene-Yo]

I need some help or guidance on how to program a slot which starts at -0.10" depth and over a 4" movement it ends at 0.00". So a gradual movement from -0.10 to 0.00" smoothly over 4".

Slot width would be 3/8" wide using a .1875" bit with cutting speed of 1.5" per minute.

I readily use some CNC engraving software with Mach3 but not sure how to create a program for this type of Z movement.

I am also open to paying a nominal fee for someone to create this program and can explain more in detail / email a drawing.

[fordav11]

what you want is not clear.
Mill or Lathe?
If lathe do you have Y axis?
If lathe is the slot on the face or diameter?
If mill what is the X,Y position of the slot.
etc etc

A drawing would be better.....

[sinha_nsit]

If it is a mill, what is so great about it (or I have not clearly understood what you want).
Just place the tool (bottom-cutting) at start xy, dig Z-.1, then G01 to end xy with Z0. Repeat the process for widening the slot.

[G0G90]

... wo,
if you want a slight radius on the bottom of the slot, just program the cutter path and add your Z to the line. HOWEVER, since the inclination is exclusive of the cutter, you'll need to add that to your path.
Easier method, - put the piece in your fixture with the 1.432 degrees and not worry about the Z move.

[G0G90]

... wo,
if you want a slight radius on the bottom of the slot, just program the cutter path and add your Z to the line. HOWEVER, since the inclination is exclusive of the cutter, you'll need to add that to your path.
Easier method, - put the piece in your fixture with the 1.432 degrees and not worry about the Z move.

I'll reiterate; using a cutting tool that spins on an axis, will cut a form that is proportional to the angle. Starting with a square form @ 90 degrees (perpendicular), to matching the diameter @ 0 or 180 (parallel).
Any inclination in between will result in a proportional radius or elliptical shape on the cutting face.

This is why you don't use a boring bar to hold roundness - it's too dependent of your machine's alignments and other influences.

[Gene-Yo]

I have attached a PDF which gives more information. It would be cut on a CNC Router or Mill (3 axis). The depth of the slot would angle up like a swimming pool where its deep then gets shallower and shallower at a gradual angle.

The slot cut would get shallower so there is no noticeable steps or rough spots.

[G0G90]

I'd still angle the work piece instead of the cutter.
Also, consider using a larger mill as well to reduce any potential overlap marks and keep the surface more flat. - 5/16" with three cuts.
It would really help if you showed a print with tolerances.

[Gene-Yo]

Feasibly I could use a 3/8" bit which is the same size as the hole being slotted and just run it slow like 0.75" per minute. That would also work.

I cannot angle the piece because there will be a more cutting that will happen to the face. Everything else I can program and cut myself but just don't have the software tools to program a slot which goes from .10" deep to 0.0" deep over a 4" travel, etc.

[G0G90]

and you can't make this into a seconday-operation?
Does the bottom of the slot not matter in this case? - and only the width?

Then, the trick is to extrapolate the Z value so that this incline is all inclusive of your 4" width.
Here; using your .10:4 ratio, figure your entire path length including ramp-on and ramp-off.
Using a .1875" dia. cutter and additional .05" for clearance on both ends, your length becomes X4.2875". L=4+(.1875/2)+(.05*2)
Substitute and solve for Z:
Z=.1/4*4.2875 = .1072"
Now, since you want to split the ramp-on, and ramp-off values, do the same to the Z:
Z start = (.1-.1072)/2+.1 = Z-.1036
and Z finish = .0036
OR;
G0G90X-.2375 Z-.1036
G1 X4.2375 Z.0036 F1.5

This will keep your ramp start and finish to the exact dimensions. (more or less since the bottom won't be flat)
(there are other ways using trig however, proportions will work in this case)

[Gene-Yo]

O.K. that's a huge help! Thanks for putting this on paper and I will try to cut shortly.

[texaspyro]

G0G90X-.2375 Z-.1036
G1 X4.2375 Z.0036 F1.5


I think you will want to cut the slot starting from the 0 inch depth end and cutting down to the -0.1" end. Otherwise doing that initial Z plunge at G00 rapid rate into the material could be entertaining.

[deneyeone]

Unless the part is tilted there will be a flat the same dimeter as the tooling at the depest point.