I’ve had this question for awhile, and now since im out to replace my first set of bits I was wonder why should I use different size collets when I could mostly keep in my 1/4" collet and just buy 1/8" bits or smaller with a 1/4" shank. I know the 1/8" shanks are a little cheaper but is that it, is there anyother pros and cons?
I prefer my 1/8 bits with the 1/4 shank. It makes my life a little easier.
The drawback for me, at least, is that I keep dropping them, and they break. UGG. The 1/8 bit shears right off the 1/4 shank. So far, I have lost 2 bits to my clumsiness.
2 Likes
I agree with @SDGuy. I hate changing collets even though it is quite easy. If replacing your bits just get 1/8" bit with a 1/4" shank. I bought a 1/8" down cut bit from Grizzly that I use a lot.
I also have a groovee jenny 60 degree down cut bit but they make other bits that are equally as good.
Carbide3d bit are good and competitive but there are a lot of other bits out there to explore. What I do not recommend for a Shapeoko are the compression bits. For a compression bit to work properly you must make a full depth cut for it to work properly. Most Shapeoko machines do not have the power to take full depth cuts. People here on the forum have tried them but have been disappointed with them.
Depending on the age of your collet C3D sells Makita/C3d precision collets and you should have a spare on hand. I like the elairecorp collets.
They make both SAE and metric collets so you can extend your bit usage if you want to use metric bits.
1 Like
There are compression bits that can work with Shapeoko-class machines, they have a very short upcut region so that a ‘normal’ DOC still cuts as compression. Even though a thicker cut requires multiple passes, you still get the benefits of a compression bit - clean surfaces both top and bottom.
The ‘Jenny’ bit is such a bit, I have had good success with it in both hardwoods and softwoods. A DOC of 0.110 (or more) will cut as a compression.
2 Likes
For the compression bits, is that because the stepper motors don’t have the torque, or because their router doesn’t? Im working with a 2.2kw 80mm spindle from Pwncnc on a S5. I am still new where i don’t fully understand feeds and speeds enough to make deep cuts. But i can tell my spindle never has any issue, so i feel i could push it harder but im still afraid of breaking something so im sure my cut times are longer than they should be
One thing to consider is that if you have a 1/8" shank bit, you can go deeper then the usual 1/2" cut height if needed. Usually not able to do this with a 1/4" shank bit
3 Likes
You should buy some cheap bits and test what speeds you can achieve. I’m on the 1.2kw spindle and cut 200 IPM and 100% diameter DOC with a 1/8th. A little slower with a 1/4 bit.
1 Like
Wow im going extremely slow, i dont think I’ve gone above 60. But thats because im usually cutting smaller things and im worried about my motors constantly slamming to a sudden stop to move in a different direction. Is that something to worry about our does the machine now its limits and will slow down before the motors reverse.
I’m pretty sure it’s programed into GRBL. So the stops do decelerate before coming to a stop. Movements are not instant they speed up and slow down based on the acceleration profile.
I changed my acceleration parameters by half. I found it helped a little to get better surface finishes.
I am sure running 200IPM is harder on the machine than 60, but I’m not sure how much harder. I suspect the machine can handle the speeds well.
If you do run into issues when testing you speed numbers, make sure to tighten the couplers. That was the first issue I had when testing speeds. The machine came with screws that were not tight at all.
There’s not a single mention in this whole thread about what “machine” any of you are using. Feeds and speeds are “machine” dependent especially when one is looking for maximums.
I stated this in my above post when i said what spindle im using. I said I use the spindle on a S5 (Shapeoko 5 pro)
I break bits all the time due to ADHD moments. I have found that 1/8" shank bits are cheaper than 1/4" bits. I can get a pack of 5 down cut endmills for $25:
The 1/4in shank versions are more than twice that.
2 Likes
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.
To all the comments about not changing a collet. You really should at the very least remove and blow out the collets and bore at a tool change. You will build up swarf and resin inside the collet and bore as you cut. This will cause accelerated wear and potentially runout that will reduce the life of the collets, router/spindle, and bits if they aren’t clean.
In general to reason why depends on the sources you are using. The carbide and diamond wheel cost go up much faster for higher grades of carbide and better finishing/performance diamond wheels. So higher end tool costs can climb a lot more for the same tool on a 1/4" vs 1/8" shank. Also watch out for the tool length. You want as little tool sticking out of the collet as possible without bottoming out the tool in the router/spindle. The longer that gets the more the tool will flex (like for like).
It can be this and/or machine rigidity. Taking a full depth cut adds more cutting forces and can cause the machine to deflect resulting in chatter. If it will or not depends on the depth, stepover, chipload (feed), and material.
Be careful doing this. It’s impossible to make the cutting edge of the tool the same diameter as the shank it’s ground on (barring tools with “land”). This means that you are going to be spinning a slightly larger cylinder than you cuts size inside the cut when over-plunging. This can result in a lot of issues but can be done in a pinch with a lot of hand holding. If you want to know more on this I posted about the reasons more here: Actual size of the #102 endmill - #7 by TDA
Both are hard in different ways. We actually have to have customers lower their acceleration on insane machines when using micro/nano tooling in some cases as that alone can snap them. More generally the higher the acceleration and junction deviation the more violent the motion gets in direction changes and can effect the cut.
The feed is more about the force generation for the chip. So any increase in chipload(feed), stepover, or pass depth will put more force into the machine and tool. This will cause more deflection but might not even be enough to notice or care about. It’s also a lot less violent of a change than anything with acceleration.
Hope that’s useful. let me know if there’s something I can help with.
7 Likes
That has been my understanding of compression bits.
Only plunge past the up cut zone & do multiple passes to final DOC.
I also stopped doing single bit path cuts on all my machines and only cut slots on profile cut outs to reduce compacting swaf into the tool path.
(1) Next Wave SD-100, (2) S3XXL, (1) DWC 2440, and by next weekend a DWC 4848. Edges have been fantastically clean a practically zero cleanup sanding. More runtime for a lot last sanding time for the win.
1 Like
I’ve been prototyping with our SP5 for the past 4 (?) months. Seems like a century 
We’re into architectural reproductions like gingerbread, trim, etc. So a lot of what we are doing is very intricate. You’re probably going to laugh, but by default, (a ton of people are probably going to give a ton of reasons why this is a bad idea… but…) we crank our RPMs up to 24k on a VFD spindle and usually max the feedrate. Now, we aren’t doing full bit plunges either. We’re semi conservative re: depth of cut. And a lot of what we do is relief carving vs. “into the wood”.
That being said, the profile of the bit has a ton of influence on the finish of your product. For example if you need to carve an intricate detail that’s close to another, then you want a bit that can reach your surface without foobaring your actual design/decoration. If you are using a tapered bit and that decoration is 1/4" above the surface, it’s getting shaved at whatever the degree the bit is in that 1/4" area. If you use a 1/8" shanked bit, then you can wiggle down to the surface without affecting that element of your design. We use endmills 102, 112, and 122 for exactly that reason.
We carve a wide variety of wood → Red Oak, Heart of Pine, Purpleheart, Canary Wood, Black Walnut, Hickory as well as furniture grade plywood, ponderossa pine (closets), etc. Nomad is my go to for standard bits for this machine. We use Amana for specialty bits like round overs and trim related things. We’ve tried the less expensive stuff and honestly, they just aren’t the same. We push the dog snot out of this machine and we’ve only broken one bit (251) and it wasn’t the machine or the bit’s fault either Some double sided tape got applied sloppy. Excess wasn’t trimmed. It wrapped around the bit and broke before the stop button could be hit. Stuff happens fast at 24k
1 Like
60 ipm is really slow for what the 5P/spindle can do. You’re starting point should be the bit’s mfg recommended chip load for the material you’re using.
1 Like
This topic was automatically closed after 30 days. New replies are no longer allowed.