Why use 1/8" bits with 1/8" collet

[TDA (John Torrez)]

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).

@Mute10

For the compression bits, is that because the stepper motors don’t have the torque, or because their router doesn’t?

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.

@CNCInspiration

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

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

@wilmatos1989

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.

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.