Bit Deflection with 3/8-Inch Bits
From the previous posts it sounds as if this actually is tool deflection. My machine is a Cosmec nr32 (sold by Holzher). I use Meizenheimer 3/8 compression bits (3" tool length 1 1/8 cutting area) for cutting through 3/4 melamine and 1/4 dss bits (2 1/2 length w/ 7/8 cutting) for making 1/4 deep dados for backpanels, etc.. The deflections I get are about .5mm - just enough to be clearly noticeable with a naked eye. What are your thoughts - tool deflection or not?
From contributor O:
Tool deflection is frequently audible; it takes a fair bit of force to deflect a 3/8" cutter. I agree that some backlash/slop in the machine is the more likely culprit, or slight part movement.
From contributor H:
I think it's tool deflection if it doesn't occur with the 1/2" bit. It happens during entry/exit when one side of the tool loads/unloads. I've had the same experience - 3/8" tool path has nibs, 1/2" doesn't. I suppose it's possible that the 3/8" tool being smaller exerts more force on the spindle than does a 1/2" tool, possibly causing it to move because of slop but I doubt it.
From the original questioner:
All the testing I've done does seem to point to tool deflection (deflects w/ 1/4 and 3/8 in either xy axis but not with 1/2). Iím just confused by being told by my tool supplier and a CNC tech it can't be tool deflection. I can't feel any movement in the spindle and know the parts aren't moving. I do lead in/out with about a three degree angle and then overlap the cut by an inch or so.
From contributor H:
"Iím just confused by being told by my tool supplier and a CNC tech". Don't be confused by what they tell you. They don't know everything. Some are very good at what they do, others are not so good. Another thing to try is to replace the collet with a new one. Also, just for grins change the direction of cut and see how that affects the nibs.
"Clamp that tool in a vise and see how far it bends with a pipe over it." What you are proposing is an inaccurate, static test. If the tool is in fact deflecting, then it happens under very different, dynamic conditions. Your theory "that the smaller gullet in a 3/8 is galling" has some merit. But, if the tool is being operated at with the proper chipload, then that shouldn't be an issue.
From the original questioner:
Maybe I should have directed the question as such - is anyone out there able to:
1. Use a 3/8 compression bit to cut out 3/4 melamine (over MDF) parts and achieve a perfect cut at the tool entry/exit point?
2. Use a 1/4 dss bit to cut a 1/4 deep dado for a back panel (slightly larger opening than 1/4 to allow for a 1/4 back) and achieve a perfectly oval routed out path? I use "pocketing" on Alphacam which doesn't allow for sloping/angled entry.
Since I was told this wasn't tool deflection I've always assumed this is some form of machine/collet "slop". But since some people seem to think this is tool deflection it's opened the issue up to me again. So, I'm thinking if anyone can achieve the above cuts it's probably not tool deflection but something I need to further investigate. If no one can achieve the above it's probably tool deflection. Thanks for all of your help on this.
From contributor M:
Myself and many others cut 3/4 melamine all day long in a nested based environment with perfect results. I can achieve 1100 IPM with a 3/8 3 flute compression bit and make 1/4 by 1/4 dados with a 1/4" 2flute bit at 600 IPM no problem - Onsrud or Vortex tooling.
From contributor G:
Yes there is tool deflection even a 3/4 tool can do this. Deflection can be caused by wrong chipload. If you are making dust, the chips (dust) are still in the gullets and the dust is making contact with your material prior to the cutting edge. Increase feed speeds or decrease RPM's. Too long of a cutting edge will also deflect or what we see is vibration.
From contributor D:
I'm curious if you get the nibs with a new sharp bit and collet. In the past while running a lighter, older Masterwood with iso tool holders and a newer SCM with HSK, I once ran out of new 3/16 bits and chucked a retired bit that cut somewhat ok on the old machine into the newer, heavier machine. As soon as the bit hit the stock it snapped. This leads me to believe the stiffer machine wouldn't allow the dull bit to climb over the wood like the lighter weight machine did, forcing it down a path the bit couldn't maintain. Same feeds and speeds. I could accept some bending of bits, but they sure don't seem to do it when they're sharp.
From contributor T:
One question - what is your lead in/lead out strategy at the entry/exit point? Linear, 3d, Angular, Radial,etc? How do you program the machine? More importantly, are you able to verify that the code is correct at the entry/exit points depending on your strategy? I have seen this be an issue on machines when people were using CAM programs to program their control but not sure if the code generated was exactly what it should be, and it wasn't.
Also, how do you load (position) your tool in the collett toolholder? My recommendation is always to never insert the grind of the tool gullet into the collet, but get the end of the grind for the gullet as close as possible to the face of the collet for rigidity. Collet condition, tool holder condition, spindle condition, bit shank condition - everyone of these (and many more) figure into the cutting solution when cutting at 16,000rpm plus so any rigidity precautions you can take at the onset reap returns in the end.
From contributor M:
I had a serious skepticism about tool deflection at first sight. It makes perfect sense to me that it is kind of hard for an analytical mind to imagine a 3/8 inch piece of carbide bending any realistic amount, right? One thing to keep in mind is that yes, carbide is very hard and brittle, but it will bend a finite amount with enough pressure before breaking. Reality is though it will not bend a whole lot and usually there are other contributing factors in addition to just the bit bending to consider, especially collet flex, which I conceptually lump in with tool deflection when parsing out the difference between tool and machine deflection. A collet is after all in a real way a very stiff spring.
Important things to remember:
1. As mentioned, chuck the bit properly, that is, all of the collet hits un-machined shank on the tool. No part of the machined edge should touch the collet.
2. No more tool should project from the collet than necessary. This is a big deal as it makes for more flex and vibration.
3. Collet should be proper for the shank of the tool, the tool should fully engage the interior of the collet surface all the way up if possible.
4. Pressures inside the gullet of the tool can get pretty high. I am sure Greg can speak to this. These pressures can be different on the cutting side and the offcut side, biasing the situation for deflection.
5. Dull tools not only generate heat, softening (albeit to a very small amount) both the collet and the tool. More importantly the pressures, especially in climb cutting from a dull tool are also very high. When combined with an overloaded gullet it is really significant. The slight flexing due to a dull tool also creates more heat and the whole thing gives out catastrophically soon after.
From contributor W:
Your tooling guy is right in one respect. The bit will not deflect without breaking, however, I think these last couple of responses are close to the answer. You have the problem in 3/8" bits and not 1/2" bits. What's the difference - the collet. Contributor T touched on one important point, and I agree with him to a point, you should try not to put the fluted part of the tool into the collet, but more importantly, you should try to fill the length of the collet as much as possible. This is where using 3/8" bits tends to be a problem.
Tooling manufacturers tend to make the unfluted shank portion too short. On my desk right now, I have a 3/8" up spiral that only has just over 1 3/16" of unfluted shank. That's not enough, especially on the longer ER40 and RDO 35 collets. The collet is a steel spring. That's where your deflection is likely coming from. If you don't fill the collet with the tool, the spring will deflect. That is compounded by the fact that there is more steel and less carbide in the router bit/collet combination for a 3/8" bit than there is for the 1/2' bit, thus, more possible deflection (steel bends, carbide doesn't).
From contributor L:
How often do you clean your collets? Any pitch or dust caked in there will cause slippage and flex. Being a smaller diameter bit the collets have much less surface area to grip and hold the tool properly. Combine that with a dulling tool and improper chip load from wrong feed rates and rpm attained for optimal cutting and youíre going to get a lot more unwanted movement. I have yet to ever see a bent solid carbide bit come through my shop.
From contributor P:
Make sure your bit is in the collet correctly. I also had some cutters (1/2") that had that scary chattering sound when they cut and when I inspected the collet the cutter didn't reach to the top of the collet with the flutes 1/8" away from the bottom of the collet. These cutters have to be tossed because they will always deflect due to insecure mounting. The cutter sounded fine cutting melamine. Hardwood was where the problem was amplified.
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
Comment from contributor A:
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?