Profile cuts in copper

The following was just a little experiment in doing profile cuts in copper with a 2-flute 1/8" square endmill (#102Z from Carbide3D store), to figure out which feeds and speeds would work. I used a 100mmx100mm (~4"x4") piece of 0.9mm (0.035") thick copper, used tape and glue to hold it onto the wasteboard, and cut simple profiles at increasing chiploads, to find the sweet spot.

The toolpath is a single contour/profile cut, which is not the best thing to do if you need a perfect finish (you should rather do a roughing cut followed by a light finishing cut to have perfect edges), but for the purpose of this test, it represented a worst case scenario i.e. slotting throughout the cut.

• the first step was to determine an adequate target chipload for a 1/8" endmill in copper. The guideline in the Feeds & speeds section for aluminium is from 0.0005" / 0.0127mm to 0.001" / 0.0254mm. Aluminium and copper are different, and their hardness varies with the specific type/temper used, but overall they both are in the 75-150BHN hardness range, so I assumed I could use the same target chipload (since my copper sheet was of unknown origin, I could not make any better informed decision anyway).

• stepover did not apply this since was a slotting cut. Therefore chip thinning did not apply either.

• I chose 12.000 RPM, to keep things quiet and since cutting force was not going to be a problem for such a shallow cut.

• to achieve the 0.0005" chipload at 12.000RPM with this 2-flute endmill, the feedrate needed to be 0.0005 x 2 x 12000 = 12ipm = 300mm/min

• plungerate should be low since this is metal AND I would not be using any ramping into the material, I picked 4ipm (100mm/min)

• for depth of cut the guideline is 5 to 10% of endmill diameter for large WOC in metals, 5% of 1/8" is 0.00625" and 10% is 0.0125", I selected a middle value of 0.008" / 0.2mm

• deflection would not likely to be a problem for this shallow cut, the calculator told me the deflection for those settings was actually 0.002mm (0.00008") for a 20mm (0.8") stickout.

I actually tested 9 feedrates, starting from below the recommended min chipload, to above the max recommended chipload: 200, 300, 400, 500, 600, 700, 800, 900, and 1000 mm/min, which correspond to chipload values from 0.008mm (0.0003") to 0.042mm (0.0016")

All the cuts completed without issue, but:

• the 200, 300, and 400mm/min cuts were a bit noisy with hints of chatter during some passes

• it got better at 500mm/min

• 600mm/min was the best cut (clean noise and clean cut)

• 700 to 1000mm/min cut got increasingly noisy and rough.

For this specific test, 600mm/min i.e. a chipload of 0.001" / 0.0254mm seemed to be the sweet spot, but it also showed that there is a good range of usable feedrates around this optimal value.

Profile cut in aluminium

• same 2-flute ZrN-coated 1/8" square endmill, #102Z

• material for this test was 2017 T6 aluminium (a remote European sibling of 6061)

• again target chipload for an 1/8" endmill in aluminium is 0.0005" / 0.0127mm minimum, I started from that.

• same 12.000 RPM speed

• to achieve the 0.0005" chipload at 12.000RPM with this 2-flute endmill, the feedrate needs to be 0.0005" x 2 flutes x 12000 RPM = 12ipm = 300mm/min

• plungerate of 100mm/min (4ipm) again.

• for depth of cut I tried the high end of the recommended range for metals, i.e. 10% of the endmill diameter, so 0.012" / 0.3mm

• predicted deflection is still negligeable at 0.001mm (0.00004") for a 20mm (0.8") stickout

• still using a simple slotting toolpath, but this time I used linear ramping and lead-in/lead-out options in VCarve.

Once the cut started, I could feel that the 300mm/min feedrate was a bit too low, so I gradually increased using feedrate override it until it sounded right, and ended up at +50%, i.e. 450mm/min (18ipm), i.e. a chipload of 0.00075", which happens to be right in the middle of the recommended range for this endmill size.

Adaptive clearing in aluminium

I needed to cut the following piece from 2017 T6 aluminium:

It is relatively small (about 0.8"x1.5"x0.4"), and holes are about 0.15", so I went for using a 1/8" endmill (same as before: 2-flute ZrN-coated 1/8" square endmill, Carbide3D's #102Z)

The majority of the cut was done with one 3D adaptive clearing toolpath for roughing:

• 10.000 RPM

• target chipload of 0.001"

• stepover ("optimal load" in Fusion360) of 0.012" (~10% of endmill diameter)

• target chipload adjusted for chip thinning for this stepover is 0.0017"

• feedrate was therefore 34ipm (= 0.0017" x 2 flutes x 10.000RPM)

• I used 13ipm plunge rate since helical ramping (shown in red below) allows it.

• I kept 0.02" axial stock to leave, and 0.02" radial stock to leave.

• 0.16" DOC (~130% of endmill diameter), which resulted in two passes (in blue):

I used a regular pocketing toolpath to cut the four holes, using the same feeds and speeds:

I added a horizontal finishing pass to shave off the 0.02" (axial and radial) excess material left during the adaptive clearing, and get to the final piece dimensions:

Finally, I used an adaptive toolpath to cutout the piece. I could have used a regular profile cut (slotting), but considering the small endmill (1/8") and relatively thick stock (0.4"), this seemed less risky albeit longer to execute:

I used an air jet throughout the cut to help chip evacuation, no coolant. This got me nice long chips, and a decent finish quality:

Retrospectively, I should have used much higher RPMs (while maintaining the same chiploads) to optimize this cut.