Mine survived for 25 hours of working. Stepover 40%, 2mm stepdown, 650mm/min, 12000RPM, hard wood (ash-tree). After 25 hours it started to work like you can see attached photo. Actually, I expected it to live 10X times longer and this frustrates me.
Lots to consider. If you only use the bottom 0.5mm it, coatings on wood are not needed, quality of the metal, and use. That said, I have had some last 2 hours and some 30+ for me in MDF, in regular not glued wood I would think they would last a crazy long time if you are not over heating and using a majority of the cutting edge.
MDF is full of glue, which kills endmills pretty quick. Same with plywood. Ignoring metals, plywood will kill your endmills the fastest. The stepdown is what Ryan is talking about. If all you ever cut is .5mm, then that’s really all that is being used on your endmill. It will dull and the rest of the cutting edge will still be sharp, but you won’t be able to use it.
I’m basically using the same endmills Ryan sells in the shop, which I think are Kyocera. 1/8", 1/16" Single flute and double flute. I also have a couple 1/4" double flute that I use on the lowrider, and a 1" surfacing bit I got from amana tools.
Agree on the glue in MDF. Additionally, the most common routers used for the mpcnc/lowrider spin too fast to make anything other than dust in mdf (since they can’t reach the appropriate feed rate), so you make a lot of dust instead of chips. That is in general for MDF though, Even the Shopbot Buddy we have just makes dust. Dust means heat, heat kills endmills.
I have just read same 30 seconds ago in another local forum From 2 separate sources I interpolate that with feed of 1 m/min I should reduce RPM to 4800-5000 (while so far I did 12000 and I witnessed dust).
However, which size of particle is dust and which one is chip?
While I can’t quantify what size makes a “chip”, maybe this graphic will help. The reason it’s more difficult to get chips when cutting MDF (for most hobby routers) is because it’s literally dust and glue.
I got dug into other forums and bits selling websites. They say how to calculate parameters.
Here is data for flat end spiral bits: say, 2 flute bit. 1 flute should cut a chip of 0.05-0.15mm thick. Therefore 1 turn of a bit should cut 0.1-0.3mm of material. Therefore if you spin 12000 RPM then your feed rate should be [0.1-0.3]*12000 => 1200 - 3600 mm/min. If you make your bit cut less per revolution - then it’s not cutting but tearing material, so heating and fast wear out.
Of course MPCNC cannot afford 3.6 m/min. But 1.2 m/min is affordable and also spindle can be slowed down a little.
Also should take this into account. When stepover less than 50% then a single cut that a flute makes is thinner than theoretical. So above stated formula should be adjusted correspondingly.
I was wrong. MPCNC can handle way more than 1.2m/min of feedrate. I tried 9KRMP with 2.16 m/min, 20% stepover and 3mm stepdown it worked just fine (oak). I assume it’s not the limit but I was close because that chinese spindle apparently can be only 10.5KRPM as per my laser tachometer.
Of course, central node should be stiff and without backlashes to afford minimal deviation of the bit.
Gonna push feedrate to the limit and see what happens.
and Fusion 360’s algorythm where it first cuts with 6mm depth and then refines by 2mm stepover where material is left in order to finalize roughing. Also 10500RPM - 30% stepover and 4.063m/min.
Thus I successfully achieved 0.3mm material removal per revolution of a 6mm flat end 2 flute bit, just as per recomendations.
I can say that MPCNC is capable of doing this intencity. Maybe it’s because I reinforced it. However, on 4m/min the moving trajectory under load is not always smooth and some inertion (asumingly) vibration is noticed on head node. Maybe better to slow down spindle and feed rate. Or maybe should use stronger and shorter pipes (this also will be tested in my second hybrid MPCNC).
I estimate that I increased bit’s life by at least 5 times by a factor of feedrate which is still not too long. I hope that it’s will also be increased by a factor of cutting instead of tearing material. A good hope is supported by comment of one of sellers that such bits life for very long time and are being broken more often (on strong machines) than become dull.
Yes. However, this only should be possible if you can handle such depth (1*D of bit for oak) with recommended combination of feedrate and spindle RPM. Luckily I proved that it’s possible. And, 2X longer life time because of depth factor, s0 at least 10X now, not bad.
They use 1D as a standard for easy reference, if you are using a single flute or other large fluted endmill and get good chip evacuation I can easily pocket wood and plastic at 4D, Slotting is 1-3*D for me.
The speeds we use might make a lot more sens if you use mm/s. You have 3m/min and 4.063m/min which does not sound all that different and even wondering why the .063 is in there until you realize, that is 50mm/s (much faster than I even rapid) and 67.72mm/s. Those speeds are pretty nuts for this machine and could be the cause of your movement issues, the junction deviation calcs do take time to process, and on small cuts the accels will not let you get anywhere near that so you could very well not actually be changing your speeds. I really suggest 8-15mm/s and deeper. If you think about it that way your 1D@50mm/s is the same as the recommended 4D@12.5mm/s with the exception of making your endmill last 4X as long and the machine moving smoother and the steppers having at least 2X the torque. If you do want to keep cutting fast I suggest larger pulleys to slow down the steppers.
Yes, here comes the problem. My dust removal system seems to be quite powerful. However, it can’t evacuate chips well even from 1*D slots. Or, if you meant bit’s structure designed to evacuate chips well, mine also don’t.
Yes but:
Spindle should do only 2400-4800 which is ok on a high margin. But will decrease sppindle’s power from 500W to 100-200W;
I am 3D milling, not cutting. So anything deeper than 1*D doesn’t make sence in my case.
But I will try to simulate in Fusion360, maybe it makes sence.
But what is the point to that considering that larger pulleys apply greater lever…?
Steppers have a rapid decrease in torque with RPM, a larger pulley will keep the RPM down. There is a balance point and at the speeds you are going I am sure a larger pulley would result in a net return on torque. I don’t have 12V specs for our steppers but you are running at 93rpms and the torque starts to fall of sooner than 50 @12V (They seem to be peak at 30 from the looks of a generic stepper plot).
It is not a big deal just a good exercise in double checking all my calcs from a few years ago.
From 2 separate sources I interpolate that with feed of 1 m/min I should reduce RPM to 4800-5000 (while so far I did 12000 and I witnessed dust).
