# Broken Bit. Need Help With Feeds and Speeds



## tomwaggoner (Feb 22, 2011)

I am using a 12000rpm bosch router. I am cutting through 1/2" baltic birch using a 1/8" dia compression spiral bit. I snapped a bit yesterday running it at .17" deep at 80IMP. The first part I cut out I ran it at 100IMP with the same depth/pass. It actually was doing fine until the final pass where it was cutting depth and also the 0.03" side tolerance. I'm trying to figure it all out. Is the 0.03" too much? Should I increase the number of passes? I really want to stay with the 1/8" for the level of detail. Also is there a spreadsheet or table I could use to determine appropriate depth/pass? I've heard the machinists handbook (I have the 29th edition) but I haven't been able to find a table in there. Excel would work too. Thanks for any help!

Tom

Amana Solid Carbide Mini 1/8 Compression Spiral Bit


----------



## Cherryville Chuck (Sep 28, 2010)

I don't have a CNC but if I were doing that handheld I would go as fast as the router would turn. The general rule is don't go deeper than the diameter of the bit. Feed speed I can't answer since I go by feel.

If no one comes along that can answer you I suggest you contact Onsrud. They cater heavily to the CNC market. I've recommended to several people to try them for advice on the questions you are asking and they posted after that they had never talked to more knowledgeable and helpful people. You can get a phone number off the net. You can also find them by searching ebay for Onsrudcutter2010. They have a few items for sale there and you can send them a message through ebay to find out how to contact them.


----------



## tomwaggoner (Feb 22, 2011)

I talked with Gary from Onsrud. Great guy. He said I should be in the 20-40ipm range and at about 1/8"/pass. I bought two more of the Amana bits to give them a shot,. if they dont work Gary gave me the number for an Onsrud one that should do the trick.


----------



## subtleaccents (Nov 5, 2011)

For 1/2" baltic Birch ply - MDF - pine ply I cut at full depth taking a .20 final pass using a 1/8" spiral up cut or the compression (depending on part shape) @ 75 to 85 IPM spinning at 18000 RPM. I don't drop spindle RPM down to 12000 until I am using a 3/8" or larger diameter bit.

I very seldom use any Amana products, never had much luck with their quality. For the CNC I use either Onsrud or Bosch solid carbide bits based on the material type and bit design.

I mentioned to another forum member, I cut 1/2" Corian at full depth with a 1/8" spiral up cut at 75 IPM and 18000 RPM without issue. There is a lot more resistance and heat build up on the bit with the Corian than wood.


----------



## mattt (Feb 3, 2014)

Check out htt p://www.cnccookbook.com/GWCalcFeedsSpeeds.htm

htt p://zero-divide.net/?page=fswizard for online feed & speed calculators


----------



## tomwaggoner (Feb 22, 2011)

Keep breaking them. The feeds and speeds calculator seems real theoretical,. especially for smaller stuff. So here is the officially where I am at.

Here is what I am using:
Velox 4x4 CNC
-max speed 100imp
-Bosch EVS 1617 router (2.25HP/ 12 Amp motor 8,000-25, 000 RPM)

I am trying to cut out a shape like this out of 1/2" baltic birch plywood.









The first time I cut it out I used an amana compression spiral 1/8" bit and it did ok at 100imp 0.125"/pass., the edges were a little rough,. but the next few times I went to cut out pieces I have snapped my bits at slower speeds. Once at 80imp,. another at 40imp,. I slowed it down to see if it would help the finish and under the advise of another cnc operator. 

I am just looking for and optimal feed and speed using that bit that I can run and not break bits. mini-compression-solid-carbide,. and maybe that isn't the bit I should be using. I dunno,. I am trying to figure this all out. 

I appreciate you taking the time to read this and would very much so appreciate any help you could lend.


----------



## Trimax (Apr 9, 2009)

as x machinist a rule of thumb is a depth of 1/2 of the bit diameter or half the feed double the speed
but thats cutting metal


----------



## Stick486 (Jan 4, 2013)

since it's CNC work I'd use two different bits 3/8 - 1/2" for roughing to very near desired cut out... a 1/4" bit may last the entire cut out...
and then the 1/8" bit for final where it is acting in cut mode as an absolute minimal material remover and mostly as a edge treatment cutter/cleaner...

the bits are breaking because of a combination of heat, dullness and lateral forces...
it wouldn't hurt to stop every so often and clean the residues and glue off of the bit...
doing this will let the bit cool some also...


----------



## Cherryville Chuck (Sep 28, 2010)

I agree with Stick. You only need the small radius in a few spots. Do the rest with a 1/2". Plywood is one of the hardest materials there is on bits.


----------



## Ladelmann (Aug 9, 2014)

These posts are so helpful! Thanks to all!


----------



## mattt (Feb 3, 2014)

If you are taking at least .003" per tooth then the chips will carry away the heat and the bit will stay cool to the touch- you can actually feel the heat in the chips and when you stop the router, the bit will be barely above room temperature. Check out one of the calculators I linked above to figure out what combination of rpm and feed speed you need to get the right chipload. Typically you want .003-.010" per tooth.

I smoked a few bits before I started keeping an eye on chip load.


----------



## tomwaggoner (Feb 22, 2011)

*I think I pinpointed the problem.*

So I kept breaking bits,. 5 total,. so I decided to go with Onsrud bits as the Amana brand kept letting me down,. I went with a 3/16" downcut.,. I'm still not paying ultra attention to chip load,. but I know when I did get down with this piece the bit was room temperature. I ran it at 70imp with an RPM of around 18K with a .125" per pass. Everything was going good till the final pass. I should be kicking myself,. so the plywood is 1/2",. but not really 0.50",. I was making it so the second to final put was 0.45" and the piece was pretty much cut free,. so the final cut I was going through to 0.52" and also taking out 0.005" side tolerance and all of a sudden the table started making tons of noise,. lull and behold one of the small fingers was grabbing the bit HARD. It made it around and kept going to finish,. but yeah I think that was my problem,. so I took some advice and placed makers on the pieces that get cut free and used my brad nailer to secure them down,. I was super excited to see the bit make it all the way through without breaking. Total learning experience on my part. Now I think I can refine it even more to be even more successful. Thank you for this forum and thank you for your help. I will be sure to post more as I grow in the industry 

-Tom


----------

