I have been having fantastic results / performance upgrading from the Shapeoko 3 XXL to the 5 Pro 4x4 with aluminum.
Generally I am using the recipes from Kevin’s recent video for aluminum on the 5 Pro, (adaptive, 2200mm/min, 6mm doc, 1.25 load) and using a quarter inch Zrn coated single flute endmill.
Watching some of NYCCNC videos, he generally opts for a 3 flute endmill.
What is the benefit, or is there a benefit on a machine like the 5 Pro?
I should add I do have a dual Fogbusters setup for airblast and coolant (water + alcohol).
My head says, it would let me lower my spindle speed but I am not sure if it would allow me to “push” the machine any faster / harder. Are there tool life benefits? Can I go a bit faster? Should I just be content and stop putzing?!
I’m not going to comment on the Shapeoko 5 speeds and feeds as I don’t own one.
I will suggest that it may be helpful to read the Shapeoko CNC A-Z online book’s section on feeds and speeds and chiploads:
A lot goes into figuring out what you want to change in a cutting recipe. For example, changing the RPMs changes that Surface Feet / Minute that you are running the cutter whereas changing the number of flutes changes the chipload that you’re running at.
My manufacturer has this table for SFM and chiploads by material and cutter diameter as a reference point:
I love that guide, kudos to whoever put that together.
Ultimately I am after something more practical, or I can just try it and maybe break a bit
Given “the math”, it would seem like if I was at 2200mm/min and 6mm DOC, if I added a flute I could go 4400mm/min all else being equal. Or, maybe a deeper DOC. Just looking for thoughts on the matter.
Right now I am running 2-3 hour aluminum jobs that would be awesome if I could speed up and not wear out the cutter, or break something. Most of the time spent is in multiple adaptive passes (As the material is 1" thick).
I am feeling like the main variable here is actually machine rigidity. I had a slight boo boo on a finishing pass in a tight inside corner where the .3mm leftover stock ended up being about 2.5mm. At a depth of 9mm, it caused the 5 Pro to miss a couple steps, which of course basically messed up the part/cut. In this case, 9mm was too much, but it was not adaptive either.
As a side question, is that the intention as to how stepper motors work? In that they have a certain amount of force or torque and then they frankly let go?
That’s exactly how steppers work, they have a series of steps which work like gear teeth, but formed in a magnetic field, when the shaft torque exceeds the available torque from the magnets and coils they slip, and they slip to some other tooth. An open loop stepper such as those on the Shapeoko machines does not know it’s position and the controller cannot easily know that it’s lost steps.
As for the cutters, before adding more flutes I might look into lubrication and chip evacuation as getting chips jammed into the flutes generally messes up the job quite a bit. The main advantage of single flute cutters is really effective chip evacuation. In other parameters they can be quite a bit worse than multi-flute cutters, vibration through variance in cutting load as an example.
I do have a dual fogbuster setup with both air and a mix of water, alcohol, and kool mist. I think my evacuation is on point. I am just practically trying to understand what going multi flute gets me.
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
The main benefit to increasing flute count is the ability to increase the feed while maintaining the chipload. This typically comes at the cost of flute volume and also changes the flute engagement(s) which can go either way. Usually though you are also going to be changing other factors in a switch from single to 3 flute which will also change the cut in other areas.
Not really. The things that will let/make you slow your RPM are related to surface speed and while this will change some based on different geometry the flute count wouldn’t be it. Things like rake, flute relief, cutter diameter, etc. could change this and they are most likely different in the tools you are looking at. Like for like though the flute count won’t effect it.
You would be able to feed faster but you aren’t really pushing it harder. Assuming like for like a single flute tool going 1000mm/m would have the same forces as going 3000mm/m with a 3 flute. However, it would be almost impossible to keep like for like on the rest of the tool.
Some example of the above. A typical 3 flute cutter is going to have a higher helix (flute twist). This is going to change the force direction and flute engagements which will change the cut. You will also typically have less flute volume meaning, as already mentioned, you need to be more carful about chip clearing. One of the other big things going from a single to multi-flute tool is that runout can have more effect on the cut. This can potentially change the per flute chipload up and down depending on the amount and location of the runout.
Most gantry machines will be deflection limited in metal. A higher flute count could help with this by letting you feed faster without increasing the cutting force. That still has to be balanced against the cons like chip clearing and runout though.
This though is not deflection. Deflection is basically the tool or machine bending into the cut due to cutting forces. Missed steps are from exceeding the motor power/configuration.
Hope that’s useful. Let me know if there’s something I can help with.
