I’m back at trying to figuring out cutting speeds. My primary goal is to cut MDF and plywood panels for different projects. I am using a Rigid R2400 router which has a 1/4" shank on it. So my preferred bit to cut 1/2" to 3/4" material is a 1/4" double flute cutting small amounts at high speed to keep the bit cool and get good chips off of it.
Based on the settings recommended by the bit manufacturer, these are the speeds they recommend for this bit:
(federate (IPM) = RPM x Flutes x chip size)
(mm/s = IPM x.423333)
(mm/min = mm/s x 60)
for .005 = 20,000 x 2 flutes x .005 = 200 IPM * .423333 = 84.6666 mm/s * 60 = 5079.996 mm/s
for .006 = 20,000 x 2 flutes x .006 = 240 IPM * .423333 = 101.59992 mm/s * 60 = 6095.9952 mm/s
for .007 = 20,000 x 2 flutes x .007 = 280 IPM * .423333 = 118.53324 mm/s * 60 = 7111.9944 mm/s
Now the MPCNC cannot push these rates in a single cut, but I used a 1mm cutting depth and that seems fine for the machine.
Sort of… read on… here are some issues I’ve come across…
Super slow router movements (I mean you can count the stepper steps it's sooo slow) initially when using Fusion 360 CAM and Repetier:
This I found was due to a mismatch in the units being used in Fusion 360 CAM workspace (inches) and what Repetier was using (mm). To fix this, look for the units entry in the tree when you are in Fusion 360 CAM workspace. I changed it to mm. This does not affect the units you use in the Design workspace btw.
Loose Belts (cutting chatter):
I noticed is that my belts were no where near tight enough. To fix this, I used new zip ties and really made sure there was no slack in the belts when done. When the machine moves, the belts are stationary (they don't sag or otherwise move at all).
Height of MPCNC frame above cutting surface:
My frame is designed around a cutting surface of 25"x49"x6" so it's big but I am using stainless 1" tube. I found that at this height, the router mounting on the Toolmount was so far from the cross bars that it caused a fair bit of movement at the bit. So I shortened the corner tubes by cutting them to 4" in length (I may even go further since I only cut sheets of material). This accomplished 2 things. The frame is more sturdy since it is not perched as high, and the distance between the bit and the cross bars is much closer so the Z assembly is far stiffer. This change alone meant a major change in stiffness, and as a result, much cleaner and faster cut (you can hear how much happier the bit is).
Cut depth of 1/4" 2-flute Up-cut:
At these speeds, which makes the bit happy, you have an issue with it wandering (chatter or worse) based on 2 things. First
, any flex in the machine will allow the bit to wander. This can cause a change in the line the bit takes through the material. You especially notice it when the load on the bit changes, for instance when it goes from complete load in full material to as it exits the material at an edge. The bit will release it's lateral tension and leave an angle on the piece at that point. Secondly
, the steppers can only take so much. So if there is too much pressure trying to push the bit through the material, it causes the steppers to miss steps. Nastiness ensues when that happens. So I used a 1mm cutting depth to get through 3/4" of material. Faster thinner cuts produces good chip out keeping the bit sharp and cool. Slower thicker cuts heat the bit up, smells like burning wood, and in the end is slower. I've tried the really slow speeds like 12-20 mm/s. On a 1/4" bit, this does not produce a clean cut at all and only causes the bit to heat up, burn material, get glued up and dull, making it worse as it continues to cut.
So my strategy for cutting sheet material is as follows:
- (1) Make the machine as stiff as possible (tight belts, minimize the Z height),
- (2) Cut the material at the speeds the bit wants (or pretty close),
- (3) Set the cut depth that allows for the proper speeds for the material you are cutting.
Hope this helps,