First detail cutting

[Steven O Smith]

I normally use a 1/4" bit, 1/4" deep at 200ipm with good results. I'm working on a project that will need something smaller to make a small corner radius, cutting wood, likely maple or cherry for interlace/knots. I think a 1/16" diameter end mill is as small as I want to go. I use a Bosch 1617evs with the standard 1/4, 3/8, 1/2" collets that came with it.

Do I need a precision collet?
A downcut will leave a lot less fuzz, but does it add too much to the risk of breaking the tiny bit? Straight cut?
Advice on feeds and speeds will be appreciated.

Thanks,
Steve

[Jerome Stanek]

I had to do a job that had hundreds of small shapes and needed small radius corners. I did a rough cut with a 1/4 inch bit then a finish cut wit a 1/8 bit this was in 3/4 MDF. It took a long time like 3 hours each for a full 4x8 sheet.

[Steven O Smith]

Fortunately this is a small piece, molding for the door of the medicine cabinet I'm making.

[Grant Wilkinson]

You may want to consider a tapered ball nose for the fine work. I have a 1/4" shaft one that has a 1/16" diameter tip. It is a lot more break-resistant than a straight 1/16" end mill. It somewhat depends on how deep you want it to go and if the taper will work on your project.

[Derek Kessler]

I've had success using a 1/16" end mill, and while precision collets add that extra stability, I found them more crucial when working with even smaller bits. For your setup, it might not be an absolute necessity but could still offer advantages.

[Jerome Stanek]

I got some 1/16 bits from carvewright that work really good. They are 1/4 shank

[Jim Becker]

Relative to your question about a precision collet, with CNC work, collet accuracy is always going to be a plus. While this is a normal thing for folks with a spindle, if you can get that setup for your particular router, I think it can be worth the investment, especially if your projects will use smaller tooling more and more. You get a good grip and should have less run-out, too. Watch your speed control, too...chipload matters because that's what takes the heat away from the tooling. Heat is your enemy as it both dulls the tooling and can make it more susceptible to breaking. For the really small stuff, I buy the multiple packs...it helps influence Murphy's Law to not let something break because you have a replacement or three already sitting there. Tools that you don't have another like to break more.

[Michael Burnside]

I'm with Jim and I've had to pay the price for the lesson. Last year I had to do some delicate carving on some drawer faces and I wanted to use a 1/4" shank, 1/16" bit with 1/2" LOC. I had 4 of them since this was a big project and I wasn't sure I'd get it right the first time. Speeds and feed, I know now, were dead on, sitting at around the -20% nominal value. Each time into the carve the bit would randomly break. I'd never broken a bit before that wasn't me being stupid or making a mistake in toolpath setup. I couldn't understand what was going on even after messing with feeds/speeds.

After destroying the 3rd bit, I measured the runout of what I thought was a "good collet". The runout was 0.002-0.003", barely visible to my eye. The thing is, runout that high may not be noticeable to a larger bit, but it really changes the effective chipload and performance of smaller bits. I went to MSI, ordered a set of RegoFix precision collets 1/8" 1/4" 3/8" 1/2" (~55 bucks each) and I was stunned at the difference, not only in quality, but "sound" of my spindle and sub 0.001" runout (essentially zero). I changed nothing and that little 1/16" bit cut all 6 drawer fronts without issue. I've since donated or thrown away all other collets and I only use RegoFix.

[Jim Becker]

And if you ever drop a collet...get a new one. They are disposables in the CNC world in that respect. IE don't drop them!!

[Terence McGee]

Going down to a 1/16" bit allows for tighter curves and finer features that really make projects pop.


Just make sure to take it slow and easy since those tiny tools are fragile. I'd skip the downcut and stick to a 2-flute straight end mill because they have a lesser chance of breaking. Run the RPMs faster, like 30k and take passes under 0.5mm. And definitely invest in an ER collet for maximum stability.


Other than that, it just takes some test pieces to get used to the performance at smaller sizes. You'll get the hang of speeds and feeds though 🙂

[Steven O Smith]

I use a Bosch 1617evs router in my machine. I carefully cleaned mating parts and found that my 1/4" collet has 3 mils runout. I took the collet off and measured the inside taper of the router chuck. Amazingly, it was around 0.1 mil over several repeat measurements (my indicator has 0.1 mil divisions). I think it will be smart to buy a precision collet for tiny bits.

[John TenEyck]

Precision collets will help, but IMO are not necessary to get good results if you just slow down. The chipload will stay below the max from that simple change. If you wear out the bit because the chipload is too low, so be it, they are cheap. I have used a lot of 1.5 mm (1/6") endmills and the only time they've broken is when I went too fast or the DOC was too high. Same thing with 1.0 mm bits. The comment someone made about using a tapered ballnose EM is spot on as to being able to push them a lot harder, as long as a tapered sidewall is OK.

If at all possible, run a clearance pass with a 1/8" bit first, and then just clean up the remaining areas with the 1/16" bit. By doing that I can run a 1.5 mm bit at 50 ipm and 1.5 mm doc in hardwood, which is twice the chipload with a higher doc than that recommended by my software for that bit. If you can't run a clearance pass first, just slow down. 25 ipm at 0.050" doc should be fine in hardwood.

All of these are with an upcut endmill. I don't get much edge fuzz with these little bits. You'll have to slow down even more with a downcut endmill unless you can run a clearance pass first.

Use the shortest bit and smallest shank you can. There's no advantage of using a 1/4" shank for a 1/16" bit if you don't need a lot of reach, nor one with a 3/4" cut length if you only need 1/2". I know I'm in the minority, but I see no advantage for hobby work by spending a lot of money on bits. I use low/mid range price bits like SpeTools and they give me very good results with more than acceptable life.

John

[al ladd]

These guys make a 1/8" collet for your Bosch for under $25. The money saved by getting 1/8" shank bits on Ebay by the ten pack will pay for that pretty quickly. And there other 1/8" shank bits that are cool too.
https://elairecorp.com/boschcollets/

[John TenEyck]

These guys make a 1/8" collet for your Bosch for under $25. The money saved by getting 1/8" shank bits on Ebay by the ten pack will pay for that pretty quickly. And there other 1/8" shank bits that are cool too.
https://elairecorp.com/boschcollets/

I use collets from Elaire in the Makita router on my CNC. The are very well made. I can't say the runout is any less, however; it never seemed to be an issue with the stock Makita router 1/4" collet, but when I needed an 1/8" one I bought both the 1/8 and 1/4" collets just to have an extra 1/4".

FYIW, 1/8" bits are my go-to bits with my Makita router on the OneFinity. I use 1/4" bits when they make sense, but for most things I do 1/8" bits are the better option. They require less power and put less stress on the machine and workpiece. Cut quality seems just as good if you use appropriate feeds and speeds. There is a time penalty, but I'm a hobbyist so it's pretty much irrelevant.

John

[Steven O Smith]

I bought a 1/4" collet and nut from Precise Bits. I went for the middle accuracy (0.2 mil runout). I just measured the runout with a 1/4" Whiteside engraving bit; the needle on the indicator didn't twitch up next to the collet or at 1" away (so ~0.1 mil). I'm very happy with the results. I also decided to use tapered bits instead of straight end mills, as suggested here.