I am looking into compression bits to possibly do full depth cuts of 3/4” Baltic birch. Every post I’ve seen says the S3 or S4 were not rigid enough to do it, but I’ve seen that the S5 is supposed to be much more rigid than the predecessors. So…has anyone done full DOC in ply (any kind) in the S5, and if so what speeds and feeds did you use?
I snapped a 1/4” whiteside (RD2100) down cut bit at .25” DOC, 90 IMP, 18000 rpm. So I’d weary to do a full DOC.
Note, I own the S5 and will be doing more production runs in the near future so I’m trying to figure out what the upper limit of the machine is!
I will be running some plywood over the next couple days, I’ll try and report back my results with the F&S. I have mostly used downcut endmills for wood previously, but I just got a couple of 1/4" compression endmills to test.
Are you looking for any particular type of toolpath? Contour/Adaptive/Pocket?
I don’t have a S5 so I can’t comment on its limit, but I’ll say this:
machine rigidity is one thing, but at such high DOC targets (3/4"), proper chip evacuation might be a bigger problem, and especially with a downcut endmill which does a very good job of packing chips at the bottom of the cutting slot. An upcut would minimise that issue.
while I understand how it’s tempting to use a compression bit to do full depth cuts in one pass with both top and bottom edges coming out clean, the next best thing is to use a regular upcut endmill to do the contour cut with a bit of radial stock to leave, and then run a finishing contour pass at full depth with the compression bit: the effort (on the compression bit and the machine) is minimal then, and you still get the clean top and bottom edges. It does require an extra tool change though.
I do cut outs of various parts. So contours and pockets are my most used tool paths. Looking into ramping but the basic CC version doesn’t support it. I know Fusion360 had it but haven’t had time to play around with it.
Brian, take a look at this machine that can take a DOC of 3/4" in anything. C3D has made a very capable machine in the S5, but there’s really no comparison to industrial grade machines that can cut this way all day long. We small time operators can’t afford/justify a machine that can do that.
That doesn’t mean the Shapeoko machines can’t do those kind of jobs, though. It just takes longer.
I’m currently using an upcut and my problems arise when I cut perpendicular to the grain. It tears veneers apart and even on Baltic birch I get 1/4” - 1/2” slivers torn out, which is longer than the offset I’d use to account for the tear out if I did a touching pass first. So downcut is my only option.
Trying to also understand the right F&S for down cuts for proper heat management. I know I may not be able to do full cuts, but want to make sure I optimize my current set up
It depends on the material and endmill. With a 1/4" compression endmill in baltic birch, I generally start at 0.375" DOC, 50 IPM, and 20k RPM.
As long as you get below the up-cut portion of the compression endmill, you’re using it correctly. So you don’t HAVE to go full depth of cut in one shot. If your goal is speed, there are many instances, even on industrial machines, where multiple depths of cut is faster. And if your goal is speed… you’re going to have to pony-up for a more advanced program than basic CC. Either with money (CC Pro, Vectric VCarve) or with time (F360). You will need ramping toolpaths, and preferably with a lead-in/lead-out. Them’s the breaks of your goal is speed.
If your goal is to cut a shape with a compression endmill in an S5 Pro, this would be my strategy:
-A compression endmill with a short upcut section.
-Multiple depths of cut at a faster feedrate than you would if attempting it in one pass.
-First cut is deeper than needed to get into the downcut section of the endmill.
-Do a finishing pass at the final depth.
Depending on the type of toolpath greatly varys how much the SO5 can handle, or maybe its just down to the 1/4 tooling isn’t stiff enough. I’ll try and inculde all the relevant info for the speeds and feeds I ended up using the last couple days, but if I forgot anything important just let me know.
Adaptive (Roughing) - 22k RPM, 96 IPM, .75" DOC, .1" optimal load, 7 deg ramp angle, .02 stock to leave. To me this sounded and looked great, you could probably run even faster or higher optimal no problem.
Contour(Slotting) - 22k RPM, 54 IPM, .375 DOC, .02 stock to leave. This wasn’t perfect, sometimes it would sound chattery, others not. But in the end it cut just fine.
Contour Finishing pass - 22k RPM, 120 IPM .75 DOC. I thought this was a good balance of speed and finish quality.
This was my first time using a compression endmill and it didn’t blow me away in terms of performance, a regular downcut produced a much better top edge finish, but obviously the bottom edge suffers then. Using a downcut and the changing out to a compression/upcut may be how I handle it going forward.
Woops I guess I typed this all up days ago and then forgot to actually hit send…
I’ve got some 5/16 that I’ll be using and testing out on aluminum, although the little bit of aluminum I have already cut leaves a great finish compared to what my old SO3 ever did.
What router do you have? I literally just burnt mine up trying .375" DOC, 54IPM after about an hour running a job. It was probably going to die soon anyway, but I don’t think I could do much more than that. I’d think a much higher HP motor would be need to run at those speeds, not a compact router.
I’ll say though, that a cheap compression bit gave me wonderful cut profiles at that speed and depth. 2 passes, no finishing pass.
It would be easy to determine how hard the spindle is being pushed if you had access to the VFD parameters and were able to have the VFD (or Carbide Motion) display the spindle current/torque. Also remember that increasing the spindle speeds proportionally decreases tool torques and forces for the same material removal rates and minimizing tool stick-out from the collet minimizes the likelihood of tool breakage.
Have you had any vibration issues or excessive noise when moving your gantries at the same time?
There is another thread on here where a guy did and I am wondering if you shared any of his concerns. Is yours the 2x4 or the 4x4 model? If you are having rigidity issues they may be related problems
While my machine is loud when moving I mostly put that down to the table acting as a drum essentially. I have not run that square/diamond circle pattern yet, but I will try and do that today and report back with the results.
That would be awesome, Thanks. I have an RMA and can send my machine back. But now trying to make sure I want to. I don’t see any other machines for the same money I would want.
Also remember that increasing the spindle speeds proportionally decreases tool torques and forces for the same material removal rates and minimizing tool stick-out from the collet minimizes the likelihood of tool breakage.