1/16" bit feeds and speeds

[mmak2916]

Anyone here have experience with 1/16" bits? I'm doing some pocket cuts that are .0625" deep in solid wood (birch/walnut). I tried Freud 04-096 bit but even when it was out of the box, the edge cuts showed some fraying. Any suggestions on feeds and speeds for a small bit like this? It'll be used for production runs so I don't mind spending a little extra knowing that it'll do its job well. I would like to find a quality bit that cuts the top/bottom and sides clean.

Thanks!

[Brady Watson]

A 2-flute carbide end mill will work fine for this. All end mills 1/8" and smaller have an 1/8" shank. If you have a spindle get an 1/8" collet. If you have a router, see what Precise Bits has for your router. I would avoid router bits, especially ones that are necked down from a 1/4" shank. These are a waste of money.

Speeds depend on the design, but you should be able to get it in one pass depth. Start at MS,1.2,0.7 and 18,000 RPM. The smaller tools like higher RPM. Feather in more XY speed as needed. You'll probably be OK up to 2 IPS or so, but start slow and add speed a little at a time while observing what is going on. Listen to what the bit is telling you.

-B

[mmak2916]

Thank Brady! Can you recommend a specific brand/part# so I can check it out?

I did a quick search on Google and found this. Would something like this work?
http://www.ebay.com/itm/1-16-0625-2-FLUTE-CARBIDE-ENDMILLS-NEW-Kyocera-Tycom-/151248427803

Thanks!

[bill.young]

Amana makes a 1/16" bit with a 1/4" shank that I use and have good luck with, mostly for cutting engraving plastic but some plywood. If you want to give one a try, Amazon has them for around $20 with Prime shipping if you don't have a local Amana dealer.

http://www.amazon.com/Amana-Tool-45190-Straight-Diameter/dp/B000637TRS/

Bill

[scottp55]

M, Never used his 1/16", but here is his identical Kyocera in 1/8"D. Cut in Purpleheart a minute ago for you. 1.1,.5, 15K in one pass .0625" depth at 40% stepover, Climb cut using Offset toolpath.
Button was cut with their Kyocera .125"D 45degree engraving(same $4 price).
Very prompt service and delivery, use them quite a bit in last 6 months. TRY to make sure the bits are Kyocera though. Ordered one time without checking close enough, and it didn't cut as clean.
scott

[Brady Watson]

Thank Brady! Can you recommend a specific brand/part# so I can check it out?

I did a quick search on Google and found this. Would something like this work?
http://www.ebay.com/itm/1-16-0625-2-FLUTE-CARBIDE-ENDMILLS-NEW-Kyocera-Tycom-/151248427803


Technically yes...but I doubt it could be considered a quality tool. I recommend avoiding Ebay for tooling unless it is a premium brand.

I recommend Harvey Tool part number 72062. It's $11.90 ea via HarveyTool.com (http://www.harveytool.com/prod/Square-Miniature-End-Mills/Signature-Series--Miniature-End-Mills-/Browse-Our-Products_180/Miniature-End-Mills---Square_212.aspx_Q_keywords_E_72062) & cheaper via ObergBrothers.net (call them on the phone) - Mention me & you'll get a better price.

There are 3 criteria to keep in mind when selecting an end mill (and you should always use 2-flute for routing) - these are OAL (overall length), CEL (cutting edge length) and of course, diameter. Avoid HSS (high speed steel) - you should go for good micrograin carbide. It will outlast cheap tools and router bits.

Again, I'd avoid the 1/4" to 1/16" tools because they are 99% of the time ground from a lower quality carbide. Also, you are paying for a 1/4" blank, but 3/16" of it is being ground away to yield the 1/16" tip. Why pay for that? If you are a 'garage band' CNC guy you can get by with the cheap tools...but you mentioned production.



-B

[MogulTx]

Scott,

How do you do the celtic pattern in the button? Is that done with a Vee-bit? Those really look fantastic.

[scottp55]

Thanks,
VBit/VCarved
http://www.ebay.com/itm/10-60-degree-angle-carbide-bits-for-scoring-or-engraving-Kyocera-Tycom-/381160527372?pt=LH_DefaultDomain_0&hash=item58bef0160c
Too deep on that one(.12") looks almost as good at .06" depth, and that would only be one pass, and easier to clean for customers. We're using their 30,45,60,and 90"s in 1/8" and the Northern shop just finished 450 buttons last week of the fluted design using the 30's and 60's
I like the Celtic though:)
scott
Padauk was their 90 degree.

[mmak2916]

I'm constantly impressed by the knowledge and advice from this Shopbot forum! I'm so glad I bought a Shopbot...

@Scott - Thank you for your sample test images, looks great. I ordered two bits to test out since they were cheap enough.

@BillYoung - I have bought the Amana 45190 bit and it's on the way so I will test it against the 1/16" endmill.

@Brady - Thank you for bit suggestion! I will look into the Harvey Tool bit and perhaps order it as well!

I will report back soon on how these bits perform...stay tuned.

[scottp55]

M,
Yep, Wouldn't be anywhere close to where we're at without the Forum on the learning curve:)
Currently only use 1/16'th on .07-.08" buttonholes using "profile/inside/spiral ramp option(Quick)" but have done almost 1,000 holes on the same bit, and only have 1 spare. So I'll be looking at the the Harvey,Amana, and Kyocera as well. Thanks Brady and Bill!
I do have one design for a Business Card holder that uses a 1/16" card display slot (Thanks for design suggestion Eugene), but when cutting "with the grain" the Hard Maple fibers love to wrap around the 1/16" bit(MillMonster 2F EM) and have to use compressed air to often....so hoping a different bit might solve that.
So post pics, and mention whether or not you run across that problem M?
scott

[shoeshine]

I'll just throw out, that I have had very good luck with the kyoceras. And at their prices I use em until i get a hint of tear out then toss.

they also make downspirals, they say for plastic, but I use em in wood just fine.

http://www.ebay.com/itm/1-16-0625-CARBIDE-2-FLUTE-ENDMILLS-DOWNCUT-FOR-SOFT-PLASTIC-/380715942183?pt=LH_DefaultDomain_0&hash=item58a4704127

[mmak2916]

Thought I'd share some of my findings of the two bits that I purchased. Using 1.1/0.5 @ 15,000RPM.

And the winner is...the Kyocera bit! It just needed light sanding for the edges to clean up. The largest pockets are around 0.5" x 0.4" and the smaller pockets are 0.25" x 0.15". The Amana bit tore up the edges significantly more. I could keep on testing with feeds/speeds to see if it'll be any better but I'm pretty happy with the results from the Kyocera bit.

Scott, with both bits I didn't experience the issue of the fibers wrapping around the bit, but I'm using birch and not maple...

24299

[knight_toolworks]

I'll just throw out, that I have had very good luck with the kyoceras. And at their prices I use em until i get a hint of tear out then toss.

they also make downspirals, they say for plastic, but I use em in wood just fine.

http://www.ebay.com/itm/1-16-0625-CARBIDE-2-FLUTE-ENDMILLS-DOWNCUT-FOR-SOFT-PLASTIC-/380715942183?pt=LH_DefaultDomain_0&hash=item58a4704127
those look about the same as I get off of ebay. I get 15 or more hours cutting out of a bit cutting bb plywood 1/8" 12k 1ips single pass.

[scottp55]

Congrats M.
Experiment with swapping the direction of your cut as well(swap from conventional to climb or versa visa) on the Amana(also looks like something funky going on --Identical toolpath?)
Also look at "Shoeshines" downcut. Pocket finish may be different, BUT should leave almost zero tearout.
Thanks on "No Fibers", My problem only showed up when "Profile-On Line" cutting with the grain of the wood.
Glad you made the cut....and felt like an idiot yesterday when I found two of Drillman1's 1/16" hiding in the back of my drawer:(
scott

[carolinasmith]

M, Never used his 1/16", but here is his identical Kyocera in 1/8"D. Cut in Purpleheart a minute ago for you. 1.1,.5, 15K in one pass .0625" depth at 40% stepover, Climb cut using Offset toolpath.
Button was cut with their Kyocera .125"D 45degree engraving(same $4 price).
Very prompt service and delivery, use them quite a bit in last 6 months. TRY to make sure the bits are Kyocera though. Ordered one time without checking close enough, and it didn't cut as clean.
scott

Hi, what is the convention for " 1.1,.5, 15K " ?? I recognize the 15K as the spindle speed but not the 1st or 2nd columns (? IPS).
I just ordered some 1/8 inch shank , 1/16 inch diameter with 0.375 cutting length bits from Drillman to experiment making larger size piece (think wooden jigsaw puzzle pieces for toddler hands) wooden jigsaw puzzles. I'm thinking less than 20 pieces filling a 12 in x 12 in board. I want to see if the puzzle pieces will fit well enough cutting on the puzzle pattern directly, without having to resort to cutting individual pieces and fiddling with allowances.

I plan to mill 1/4 inch maple and use food safe coloring (Arti Toymaker dye) and finish with cutting board (non-toxic) finish.

Was also thinking to cut two sets with the grain of one board perpendicular to the other and glue cutout pieces together (like plywood) to make thicker pieces that resist warping.

How many passes would likely be safe for a 1/16" bit in 1/4 inch maple? Thanks for any comments / tips.

Carolina

[scottp55]

Carolina...1.1(is IPS X,Y Move speed), .5(is IPS Z(plunge) Move speed), 15K is RPM:)
I'm VERY conservative, and usually stick with the 1/2 Diameter= Pass Depth with dense hardwoods....Never broken a bit though so probably slow, but not as much deflection on tiny bits either, and I get the edge quality I want.
If it's a Profile cutout toolpath, then maybe try a Spiral Ramp like I do to keep a constant force on the bit...slight spiral also fools the eye a little bit on the minute mill marks.
For Sugar Maple I'm set at 1, .5, 17K for both Drillman's .0625" Up and Downs....for Denser woods like Bloodwood etc. I'm down around .7-.8, .4,17K...bit stays room temp and finish is excellent......For Production, you may want to gradually increase feed/speed/pass depth until cut quality suffers/or bit breaks...then back off about 10%.
Machine is cutting Claro Celtic Dragon now with a Chinese .25mm TBN I've barely used...time to go babysit for another 4 hours:)
scott

[carolinasmith]

Thanks Scott, very helpful...