Not sure what I did wrong here, well I assume I went too fast / too hard but… I have an HDM, I used the carbide 1/4" #201 and tried to cut a 2.5mm deep pocket in Aluminum. It did it, a lot faster than I expected. Seems like it melted all of its chips into these lines, and perhaps jumped and skipped a section. I was able to pry the melted chip things with a pair of pliers in most places.
I have a nice vacuum with a sweepy as well as an air cooling nozzle on the bit. Oh and I accidentally tried this with a 1/8" cutter too and watched it explode
I’m using a pocket operation here in fusion360, multiple depths with maximum step down 1mm. These are my tool settings, way too aggressive?
A couple of thoughts:
Amazon 6061 may not be 6061-T6. If the temper is softer, it will be gummy and wrap up on the cutter without adequate coolant. It could also be a completely different alloy.
I will typically get mine from Midwest Steel in MN, but the shipping costs for small quantities are crazy. Another one to consider would be Speedy Metals.
Slotting is one of the hardest operations on an endmill. One has no choice but to take 100% width of cut (Ae).
I couldn’t tell which toolpath you were using. Also, your tool shows that the selected stepdown (Ap) is .125, ie 3.2 mm, and Ae is .1" or 2.5 mm. Did you override this in the tool path?
Fusion 2D pocket is a pretty dumb tool path. It pays to use helix ramp-in to get to depth, if you are going to cut a step down of .125" (which is 50% too diameter). It should certainly be do-able.
But you might want to start with width of cut (Ae) of 10%, or .025". Your feed rate is decent as long as you are using carbide.
It is potentially too aggressive, I would try similar settings, but take a shallower stepdown. 1/8" depth of cut and 0.1" s̶t̶e̶p̶d̶o̶w̶n̶ stepover is not impossible, but not something I would use as a starting point without more experience and a positive identification of the alloy and temper. Cut that depth of cut in half and see if the machine is any happier.
There’s one more setting that’s important to take a look at, which is the cut direction (climb vs conventional). On a benchtop machine, climb (sometimes also identified as “left”) usually gives better results.
Using an air blast setup would also help. Not only getting chips out of the way, but cooling the material. I’d bet that aluminum felt pretty warm after that ordeal.
What is the difference between depth of cut & stepdown?
For a 1/4" single flute, I use about 0.010" (0.25mm) DOC, and 0.125 stepover. Or vice versa if using adaptive. 12000 RPM & 60 IPM. I also use mist coolant on all aluminum.
Well new strategy worked a lot better. This is with the #278-Z and new feeds and speeds to match that bit. This took about an hour and a half but it came out clean, adaptive roughing pass, pocket clean (to get these slots to work in fusion), then bore and contour. Thanks for all the advice.
In your original cut, your surface speed was very high (1200, vs a recommended 400-1000) for this material. You need to drop the RPM or use a smaller diameter cutter.
With surface speed that high you’d need to clear big chips fast to lose the heat which is tricky to do when slotting.
Also, are you sure the cutter was in good condition? That looks like it could have been dull.
I’d guess it wasn’t dull to begin with but I’d bet the edge built up pretty darn quick.
Maybe it needs a nice long and relaxing bath in a lye solution. Come back good as new
That lines up with what worked the second time surface speed was a little under 400. The cutter was brand new, only used on wood once, the single flute cutter did a great job though.
Surface speed really depends on the material being cut and the material of the cutter.
A good rule of thumb for HSS cutters is 90 sfm for mild steel and 300 sfm for AL.
Good quality carbide should be 3-4x that: for AL, that could be 900 sfm to 1200.
Lower surface speed will not hurt anything, except for making the process that much longer. The key is to have the correct feed rate: you don’t want the tool rubbing on the material. Thankfully, Fusion will calculate that, as long as the tool data is entered fully.
You mentioned something really important in this post: endmill was used on wood. Wood is abrasive and can easily take the sharpness off the cutting edges. This is particularly important for gummy materials like 6061, while steel requires a tougher, more blunt edge.
Here are some settings I have used with the HDM for 6061 with consistent great results. Since I cut a lot of aluminum, I removed all the MDF waste board and sealed the gaps between the T slots with silicone so I could use a continuous blast of mist coolant with around 30 psi compressed air (cooling, lubrication, chip clearance, increased tool life). Coolant makes a huge difference for aluminum. I use carbide DLC end mills. I hope this helps. Merry Christmas!
Sorry forgot to mention that if you are using aggressive cuts or larger mills like 1/4" or 1/2", you need proper workholding. Plastic clamps will not hold (you may end up damaging your workpiece and breaking your mill). And use Carbide Create Pro with the ramping option on as Will said. This also make a huge difference (10 - 20 degrees).
