This topic is old, I know…but I’ve done the searches and still don’t know what to do…so I’m reaching out with SPECIFICS:
I cut wood 99% of the time…Walnut, Cherry, Maple, Oaks (White/Red), Mahogany are my staples.
I now own the 5.1 Pro with the 80mm Spindle
I picked up a few 1/2 Shank bits and would like to get some feeds and speed recommendations for getting some time reductions in my designs:
These all have 1/2 Shanks, are straight bits, made from solid carbide, are upcut, and have two flutes:
1/2"
3/8"
1/4"
Would someone mind some recommendations for the parameters for setting up the tools to get faster results — I don’t need to drive the machine to its limits, but having this spindle ought to drastically reduce cutting times…yes?
The general consensus seems to be that you can start w/ the feeds and speeds for the Shapeoko HDM, but decrease the Depth per Pass to about half as a starting point (for the 80mm VFD, maybe the 65mm would want a smaller dimension), then with test cuts, gradually increase the Depth per Pass until one begins to impact surface finish, then back off.
@fenrus I haven’t seen you around in a long time - but you’ve always been THE “go to” guy for feeds and speeds (among other things). Would you have an opinion on my 1/2 shanked bits?
Yes, and if we sold 1/2" shank tooling we would have official feeds and speeds — as it is, we’ve gotten up to 8mm:
which maybe would be a suitable starting point? Certainly the added diameter will increase rigidity and should improve the potential for surface finish.
For further feeds and speeds the community has worked up:
I have a license to G-Wizard and can put a few in to see what it says on diff between 1/4 and 1/2.
Apparently the guy that owned it died so you can’t get a new license but existing ones are supposed to work.
I have not used it in a while.
When I do I felt like it gave numbers that I was not comfortable with.
OneFinity forum seems to support:
General Recommendations (Wood/MDF/Hard Plastic)
Spindle Speed (RPM): 18,000–20,000 RPM.
Feed Rate: 70–120 Inches Per Minute (IPM).
Pass Depth: 0.25" to 0.5" (1/2 to 1x the bit diameter).
Plunge Rate: 20–40 IPM (roughly 1/2 of feed rate).
I also found: General Rule for Feed Rate Adjustment
If you are switching from a 1/4" shank to a 1/2" shank of the same cutting diameter:
Keep the RPM the same (since the cutting diameter hasn’t changed).
Increase the Feed Rate gradually. You can often push a 1/2" shank 20–50% faster than its 1/4" counterpart because it won’t deflect as easily.
Increase Depth of Cut: You can often double your pass depth, which effectively doubles your overall material removal rate even if the IPM (inches per minute) remains similar.
This is the type of stuff I was looking for…I think. Does anyone see issues with it?
Tool maker recommendations are pandora’s box because most assume a 3/8" and def 1/2" shank is going in 5KW and up industrial machine.
1F chart is about the range I’m in with 3/8" shank bits on the 5.0 with 65mm spindle and similar woods. Depends a lot on the size and shape of cut.
3/8" XLong Rougher
An 8" x 4" rectangular pocket:
18K
.313" pass depth (83% of tool diameter)
.188" stepover (50%)
F100 / Plunge 40 with ramps
On harder woods I do “ride the dial” (digitally) a little slower -10% on the initial raster inside out, +10% wider out
On a smaller pocket say 3" x 1.5" reduce to .250" pass depth and F80. Quicker direction changes and harder to clear chips in the tighter pocket.
3/8" compression bit - finishing cuts no more than 1/16" on above pockets
no problem with .75" cut depth the tool engagement is so low after roughing
F80 / Plunge 50 with lead ins
With all of these I’ve started slower and gradually increased until I stopped liking the sound I heard. Hope this helps.
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.
If I understand this correctly you are asking how much more you can push a 1/2" shank tool regardless of the diameter of the cutter. If that’s correct, then there’s functionally no difference at this level of machining. There’s some exceptions for when you get to things like metal. For the most part the rigidity isn’t significantly increased if the stickout and cutting length are reasonable though.
Here’s an example using Millalyzer:
Only thing I’m changing between these examples is the shank.
So again with the same stickout (1.2") and cutting length (1.0") you pickup 2.65lb more to deflect the tool 0.001". But that works out in this test cut (0.50" deep, slotting, 20KRPM, 160IPM/4064mm/m, in black walnut) to only being a cut difference of 0.00021"/0.0083mm more deflected. You are going to reach another limit before this minor shank difference matters.
Where you will see differences is that in general the rest of the tool will not be the same. The length of cut, overall length (and therefor stickout) and carbide grade used will typically all be different. Typically not in beneficial ways.
You can see more of a technical breakdown I went through with this on the 8mm vs 1/4" here:
Main points being that things like the rest of the tool geometry are more important in rigidity even when shrinking both the shank and tool diameter.
Hope that’s useful. Let me know if there’s something I can help with.
I purchased a beefier spindle with 1/2" shank capability - expecting that this meant I could lower the time for my jobs. If that’s not the case, what’s the point of the extra money?
Having worked with Routers for some 30 years, I have seen the differences between cutting with a 1/2" shank and a 1/4" shank - without being scientific, with a 1/2" shank, you can push a lot more before your fillings start to fall out.
So an 80mm spindle SHOULD let me go faster…and a 1/2 bit SHOULD let me tolerate more push without as much rattle —
More or less it depends on the other factors. As an example let’s say that we have the same tool above in a 1/4" and 1/2" shank. But even though there’s only 1" worth of cutting length we are leaving 2" of the tool sticking out of the router/spindle. In this example the 1/2" shank would be of benefit.
It’s vastly more resistant than the 1/2" tool even at the 1.2" of stickout.
Vastly more matters here than the shank size.
Typically the reason for larger spindles is if you are either power limited or to use larger cutting diameter tooling. There’s ways you can reduce time by using it that way. But a 1/4" diameter cutter on either shank is going to be limited more by other factors first barring if you have a required stickout that’s fairly long.
I’m with you on this. Don’t know how to answer in a way that doesn’t sound like bashing C3D - but same is true for competitors in this price range. I had the same expectation. I bought cutters rated at 400in/min. The SO5 rapids are 200-250in/min max. Motors, lead screws, gantry must all have been engineered for a certain max speed.
Any time I see discussion of feeds and speeds it never mention spindle power. Coming from handheld or invert router, we know 1-3/4 HP might struggle where 2-1/4 doesn’t, all else equal. I had read a recommendation of Avid. It was out of my price range but I bookmarked. The base spindles start at 3kw and go up to 8kw. The C3D 80mm is 2.2kw. If run too fast the motor and leads will bind or lose steps and lurch forward ripping not cutting (or so Ive heard…) Not bashing just mean there’s a limit in a certain price range / class.
In any system, something has to be a limiting factor — for an SO5 Pro or HDM, installing a 2.2KM 80mm VFD w/ ER-20 collet removes the spindle as the limiting factor — moreover, it opens up the possibility of:
larger/longer tooling
using 1/2" metrology gear
and it has the added benefit of water cooling, so less concern about overheating.
Lastly, the added rigidity should make for nicer surface finishes achieved more easily.
Given that before it was available the SO5 Pro was described as being limited by the spindle, there should be a range of material removal rates greater than that which the 1.5KW spindle is capable of, but less than that which overtaxes the machine — implementing this is left as an exercise for the reader.
Yeah…that’s the remarkably frustrating part. I want to get information that’s usable as quickly as possible, so I can use this tool effectively. I get no pleasure in “exercises” - time is money.
I get that Carbide is a “kit-company” and you will spend time making and setting up your machine. You are rewarded by lower costs while still getting high quality. However, in this case, we have an upgrade to a machine that appears to be not quantified - even informally. It must have a reason that it’s offered…Surely, someone thought through why it pays to upgrade…and that data ought to be readily available for those who do. That’s my opinion. YMMV.
I had a water cooled 65mm and decided to upgrade to a water cooled 80mm with 220 when I ordered my 5.1 pro.
I am using a 3rd party spindle and they also have a 1.5kw 80mm water cooled model. I asked about that in this forum and was told that the 220 would be able to be pushed harder.
Interesting, that vendor sends out an email periodically with thoughts on spindles and this was in one last week: Why 220V behaves better than 110V
At the same power level, 220V draws roughly half the current of 110V.
That matters because:
• Lower current means less voltage drop under load • Wiring losses are reduced • Power is more stable during acceleration and cutting • VFDs and power supplies run cooler and happier
I am no electrician so can’t evaluate that statement.
But maybe having a larger selection of bits and the ability to have longer stickout alone is worth the cost of entry.
You seem focused on the shank size for some reason. When it comes down to it. With straight or reduced diameter tooling. The diameter of the cutter is what’s going to be your weak point.
Traditionally reduced diameter tooling like you describe is actually more prone to breakage than straight shank tooling. They like to break at the reduction transition.
I would recommend using straight shank feeds and speeds.
I’ve been running most of my 1/4” and larger tooling in dense plywood at 250-275ipm ( yes I’ve adjusted the max feed rates to meet max firmware rates to allow this) at 2xD depth for a couple years now with an 80 mm spindle.
