My team got a CNC router at the start of this season and we have been working out how to use it effectively through trial and error but one thing we haven’t fully figured out yet is what end mills to buy. We have been primarily using 1/8 or 1/4 flat endmills but we were wondering if any other teams had recommendations for endmills. Since we are still learning we are looking for fairly affordable end mills but we also want something capable of cutting aluminum reliably. Any help or suggestions would be greatly appreciated.
Seconded. We’ve recently begun using the WCP 4mm Endmill for both aluminum and polycarbonate and are very happy with the results.
I’m not sure what brand we use right now but based on the great feedback regarding huhao and HQMaster endmills i will be transitioning the team over once our current ones wear down.
These have worked well for us. They are only $5 each (less in qty of 10) and last a long time. We use them for aluminum and polycarbonate.
Shipping takes forever so plan ahead.
+1 to these, and also to Ozzyboards if you want more performance per tool.
Start feeds at 60IPM, 24K RPM, and adjust depth and width of cut to suit your machine’s rigidity.
Also if you don’t need the sharp corner, I’d recommend bull nose over flat endmills. They’ll wear slower.
Since we are currently clamping most of our flat material directly to our salvage boards, would we be able to run bull nose bits without having to substantially cut into the salvage boards to cut through the material?
You’ll have to cut at least as deep into the spoil board as the radius on the corner. For a 1/8” rounded or bull nose end mill, the corner radius is typically only 0.010”-0.020”.
For a CNC router cutting aluminum use any single flute carbide upcutting endmill. I high recommend the 4MM and 6MM endmills listed above. Keep the spindle RPMs in the upper usable range of your spindle.
If you need help with speed rate just ask.
Spoil boards are spoil boards, consider them consumable material.
Ok, thanks for the confirmation. I figured it would be something similar to that but wasn’t sure.
Some help with speeds and feeds would be greatly appreciated. We have been experimenting with some different speeds and depths but looking at some videos from another post and some earlier comments on this post we are clearly no where near the limits of the bits we are using which has so far been our concern.
I would buy a larger diameter surfacing bit 1-1.5” in diameter and surface the spoilboard periodically or as needed.
For tempered aluminum like 6061-T6, which is very common in FRC, a reasonable range for surface feet per minute (SFM) with an uncoated carbide end mill is 800-1200. For a typical quality end mill, chip load of 0.002-0.003" is reasonable for a 4 mm or 3/16" bit and 0.003-0.004 for a 6 mm or 0.25" bit.
In a CNC router with a high-rpm spindle, you definitely want to be using single-flute end mills to keep the chip load in a reasonable range for a reasonable bit travel speed.
To calculate speed and feed from SFM, chip load, and flute count:
speed (rpm) = 3.82 * SFM / bit diameter (in)
feed rate (ipm) = chip load (in) * speed (rpm) * flutes
For a 4 mm single flute end mill like those from WCP or OzzyBoards, conservative settings would be:
rpm = 3.82 * 800 / 0.157 = 19465
feed ipm = 0.002 * 19465 * 1 = 38.9
Getting more aggressive:
rpm = 3.82 * 1200 / 0.157 = 29197
Many CNC spindles max out around 24000 rpm, so let’s say that is a limitation here.
rpm = 24000
feed ipm = 0.003 * 24000 * 1 = 72
Capability for depth of cut is affected strongly by machine rigidity and spindle horsepower as well as the type of cut you are trying to make. Slotting, where the bit is cutting at it’s full diameter, presents the most challenge and limits the depth of cut.
For 4 mm bits or larger, depth of cut could reasonably be equal to the bit diameter for slotting in aluminum. However, for typical FRC machines, this may be too aggressive. Start with a light cut and work your way up. For my setup, slotting 1/8" aluminum in two passes (DOC = 0.07") with a 4 mm bit is essentially 100% reliable with no bit breakage, excellent tolerances, and nice surface finish but YMMV. For pocket milling with stepover <= 40% of the bit diameter, depth of cut can reasonably be up to 1.5 the bit diameter and experimentation will determine what your setup can handle.
+1 to all of this. The only thing I might argue is bumping up the chipload a little on a 6mm bit, but generally you can max out your machine with those numbers already.
If you don’t have GWizard by CNC Cookbook, get it. You will save the program cost many times over in saved tools and improved productivity.
We run ramp profiles with a max DOC about the tool diameter. For big clearing/bores we run full material depth and dial back the stepover to where its happy in power and deflection. This spreads tool wear out across more if the cutting edge and prolongs tool life. GWizard is critical for getting the stepover/feed/speed right for these ops. But when you do, and you master radial chip thinning, you’ll be able to remove material more that twice as fast as conventional speeds and feeds would suggest.
I agree with most of this post, but not gwizard. I have found it to be all but useless for CNC routers. Dialing back the “conservative” slider should not just decrease federate, for example. Once I started calculating the feeds myself I was actually able to start cutting to the limits of my tools. Maybe 95 could make a post showing how they use it, or their feeds and speeds?
Did you use the G-Wizard “Rigidity Compensation” tool? For my router it de-rated spindle power from 0.5hp to about 0.12hp (my machine isn’t very rigid) and when I keep spindle power under 0.12 things run nicely. Going much over that and things get bad, fast.
Here is an article on the ‘Gas Pedal’ you mentioned and Rigidity Compensation.
Here is a video on how to set it up.
This type of advanced setup computation is why G Wizard is worth every penny. The (spindle power) curve compensation is especially useful for CNC routers where the spindle’s power curve might vary quite a bit.