Hey eric from our discussion the other day in milling 1.5" solid oak at full depth
here are the specs
Feedrate: 200ipm
non-contact feedrate: 200ipm
RPM: 14285
Optimal Load: .0625
DOC: 1.5"
conventional
Tool:
Onsrud
High Speed Steel
2 Flute Downcut
.5" cutting edge diameter
IM.PRESS.IVE!!!
I can barely get the bit and collet on my machine in less time… 
Super cool…
WOW!!! Very impressive, it wasn’t struggling at all.
lol oh yes sir
Tricodial milling is great for hogging out massive amounts of material you can do the same with a 1/4" tool on the dewalt maybe not quite as fast but is you set it up right the x-carve would have no problem doing that
but you need a cam package like Fusion 360 in order to do it
but all in all I think it did great and I love the fact that I was able to maintain the tool manufactures recommended chip load of .007" I imagine that I could push it faster maybe 400 or 500 ipm but what really gets me with the spindle is that I am only turning the tool 14000 rpm (below the lowest setting on the dewalt)
in fusion I also have the ability to speed up the non-contact feedrate which would speed things along maybe a cutting feed of 400ipm and a non-contact feed of 700ipm
I guess Items like this is really why I have moved away from Easel and actually I did rather quickly after I first started
nothing against Inventables or easel cause dont get me wrong easel is great for many many things and I think all users should start on a program like that
but milling like in the video above is where you will start to make profit with your goods applying that type of milling you will max out the speed of the x-carve long before you max out the router as that strategy puts very low load on the tool compared to the amount of material being removed
oh no lol that was done on my big machine
but can easily be done on the x-carve applying the same methods and will be easier on the machine than conventional machining
What kind of depth per pass could you get using Trochoidal milling on your X-Carve?
I would have no problem going 1" or more its all about the optimal load setting you set
aka: cutter engagement
to be completely honest I am not sure what that setting should be and how to calculate it properly if anyone knows please let me know how to do that
on the X-carve I have done .75" depth at an optimal load of .040" in softwood like pine
have not done any tests in any other material
Fusion has that capability called Adaptive clearing. There are downsides to it:
I personally switched back to pocket clearing because it tends to be 10-20% faster cutting than adaptive clearing for typical models I’ve been working on.
To be clear I’m not an expert on it, and it definitely is awesome in some cases, but for a lot of models I’ve been doing it hasn’t been worth it for the above reason.s
Also the deeper you cut, the smaller “step over” it does to maintain chip load. So you end up just spending more time moving the deeper you cut.
oh yeah for sure that is what I did to make that I designed it in Fusion 360 and used there adaptive clearing toolpaths
idk I see what your saying about having to run a finish pass after its done but really imp that should always be done right just to protect the final dimension from any tool deflection or tear out in the wood
you are right lol on the computation for generating the tool path do you have any suggestions on how to speed that process up on large models?
do you know how to calculate the optimal load?
Chip load is generally defined by the manufacturer as I understand it, and will vary significantly from bit to bit. However, rigidity of the machine will usually determine your max chip load for our hobbyist machines. The cool thing is that rigidity just determines how much you can cut per revolution of the spindle (DOC + stepover + bit diameter == surface area removed per rotation generally), but with faster spindle speeds you can move faster (and generally need to to reduce rubbing heat generation). So for a machine like the X-Carve you will want to go faster but while removing less surface area per rotation of the spindle ie lower DOC+stepover. I’m not sure how this general concept translates for different materials.
I generally cut wood (Red oak + Poplar + Pine) at 100IPM with 1/2 bit diameter DOC and 1/2 bit diameter stepover. Biggest bit I’ve used with these settings si 1/4 Ballnose. Haven’t tried to find the limit yet, just hate 2+ hour cuts so been turning up the speed a lot
I’m still learning though, so I’m not a guru or anything.
yeah but I am meaning optimal load setting not chip load
the chip load is easy to figure out
but I guess I am not understand how to figure out the optimal load when tricodial milling
Found this post about the topic, seems spot on from my experience/understanding.
Optimal load is the depth of pass the software should shoot for on each “scoop” into the material. It should be no more than 40% of the diameter of the cutter, and frequently should be less when in harder materials as you don’t want to overload the spindle or the axis motors and stall or skip steps.
so if I am reading that right optimal load should equally stepover amount used in conventional milling seems to me that doing that takes the advantage away from tricodial milling right??
I mean the whole pourpose of tricodial milling is to remove more material at full depth and being easier on the tool
seems to me if you are conventional milling using a pocket toolpath strategy and only doing 1x tool diameter depth of cut and 40% tool diamter stepover that is easy on the tool compared to
tricodial milling at 3x tool diameter and 40% tool diameter stepover you would be putting more of a load on the tool because you have the entire flute length engaged each time vs. 1x tool diameter in the pocket strategy
see what I am saying? just calculating out optimal load as you would a stepover makes no sense to me
Yes, but the rigidity of the machine is going to prevent you from doing a full DOC + 40% diameter step over in a lot of cases, depending on material of course. The extra movement from adaptive clearing seems to kill the added benefits in a lot of cases because of machine rigidity. But then again, I haven’t experimented with it quite enough to to know for sure.
Definitely worth continuing to experiment with, I’m interested in hearing your results on the X-carve. Seeing it’s capabilities on much more rigid machines doesn’t really translate as much IMO.
I mainly gave up on it because of toolpath calculation time, I’ll give it a few more goes this week as I’ve moved on to experiments where it’d be more applicable I think.
Estlcam is available in English - you can select the language after installation.
