# Estimating and Measuring Tool Deflection

Troubleshooting slop in the cut, a CNC owner wonders: How much do toolbits actually bend? Hey. You do the math. February 19, 2013

Question
I cut 3/4 MDF with a two flute 3/8 compression bit at 18,000 rpm 700 ipm. I use a tool with 1 1/8 cutting surface and it sticks out of the collet about a total of 1 3/4 inches. What would you think would be the most tool deflection I should expect to see? I realize this is not an exact science but are we talking about .001", .004", etc.?

Forum Responses
(CNC Forum)
From contributor R:
I know what I am about to say won't fully answer your question but here goes anyway. I would say that the tool deflection should not be perceivable to the eye or touch if the following things are true:

1. The spindle speed and feed rate are correct regarding chipload for the material being cut and tool used (which in your case the math is correct, so this is not your issue, assuming your machine is able to cut at those speeds).

2. The machine table is flat and level.

3. The gantry is parallel to the table across the X and Y axis.

4. The machine is heavy enough to not move while cutting at the speed it is being run at.

5. The machine is able to accelerate rapidly enough to actually achieve the cut speed before it exits the cut or makes a corner.

6. There is no damage to the router spindle motor, collet, or tool holder.

7. The motor spindle is plumb on the Z axis.

8. The tool being used to cut is secure in the collet (I have had this happen).

9. The tool is not being run too dull.

I have seen that open gantry machines tend to have a little more flex at the extreme edge of a table vs. a closed gantry design. This is a possible culprit depending you your machine.

The ability of the machine to reach full cutting speed is a critical point but also not answerable without knowing what tool you are running. If it can't reach speed quickly enough it can cause too much force to be on the tool and therefore the tool has no choice but to deflect.

If the machine is a lighter machine then you might want to slow down both the spindle and feed speeds (maybe 14,000rpm and 560ipm). See what that produces. Lastly, use 1/2 tooling. It is much more stout and in my opinion worth the cost difference. I have applications for both 3/8 and 1/2 tools and the 1/2 tools seem to wear better.

From contributor O:
Well you should be able to cut some trial pieces to determine the accuracy/potential deflection. Do you hear any chirping sounds (high frequency oscillation) from the bit particularly at sudden changes in direction? With smaller diameter bits I like to keep them short and close into the collet to avoid this problem, some bits I order cut down short from new.

From contributor C:
I know you said the collet is in good condition but when was it last changed and how much has it been used? A collet is a wear item made mostly out of spring steel. You could be seeing the first signs of collet wear without the collet marks.

From contributor D:
I've said this on here before, and I get some pretty hot replies. My opinion only is that tools do not bend. Tool deflection is a broad encompassment of slop in your machine at numerous points, starting with the collet. Point in case being I can use the same carbide router bit with the same feeds and rpm on the same piece of wood and get more deflection with our lighter built machine than with the heavier duty one. A dull, tiny 3/16" bit run on the lighter machine climb cutting will deflect more - but is it the bit, or the additional pressure needed to make the cut and the slop manifesting itself? If I take that same dull bit and chuck it in the bigger machine and drive it down the same path at the same speed and rpm, guess what – snap, every time.

Try to bend a piece of carbide. Examine it closely as you do so, and you'll notice something- you can’t. It is brittle - it will shatter into two or more shards. I've accidentally dropped a carbide insert before. It fell three feet onto a concrete floor and shattered. To believe that a solid carbide bit is bending around the z axis, constantly, at several thousand rpm to me is not possible.

From contributor K:
To the original questioner: Why are you asking the question? Are you having trouble shooting a tool or a machine?

From the original questioner:
This is exactly the information I needed. Without going into unnecessary detail the issue I've had is poor cut quality. Every tool guy will say it's a machine problem and machine guys will say its bit deflection. At this point, since with your help, we've quantified tool deflection to be .001 or less. This will help a lot in terms of now I only have about five other possible problems to look at instead of six. I'll keep crossing them out one by one.

From contributor L:
We've had problems with re-sharpened bits giving a ripply cut. You can actually hear the difference. Some do, some don't. The problem is corrected by changing bits. Change out to a new high quality bit and see if the condition remains. If it is a machine problem start at the collet, try a new one. Try a new tool holder and nut as well. The spindle would be next, but it’s difficult to diagnose. How long they can run before having issues is a function of what sort of crashes they've had.

From contributor M:
I think a lot of the "area of grey" comes from the terminology. Tool deflection doesn't intuitively mean direct deflection of the tool itself, but more total deflection in the cutting system. Everywhere there is a union on your machine, there is slop, and it may be measured in millionths, ten thousandths or thousandths of an inch, but it's there.

Most router's will have some form of the following:

1. Tool to collet union.

2. Nut to collet union.

3. Nut to holder union.

4. Collet to holder union.

5. Holder to retention knob union (non-hsk).

6. Holder to spindle union.

7. Retention knob to spindle union (non-hsk).

8. Spindle components to spindle components union (several depending on mfg).

9. Spindle to spindle housing union.

10. Spindle housing union to plate/bearings/ways/ball screws (multiple).

So, there is a lot going on and I only typed a quick synopsis. Backlash in the CNC industry historically has dealt more with the wear/looseness within the ballscrew/nut union - specifically when reversing direction. All else falls in the play or "slop" category.

Machinists who machine more rigid materials to more exacting tolerances have worked around this for years. Often deploying roughing, semi finishing, and finishing passes to account for all of the above variables, and more, before making the "money" cut. This is more evident in CNC lathes than routers or mills, you can take a brand new CNC lathe, make a cut to a specific dimension under specific cutting conditions and measure that dimension with a micrometer and be within a few ten thousandth’s of your target dimension. You can then re-run your tool over the same material, same program, and remove material. This is because the forces during the first cut exposed all of the stacked "slop" that was induced in the entire system to more of a degree than the next cut (there was no added deflection due to load, so the cutting edge was on a mechanically different path).

Add to this that making carbide is an industry, and everyone out there trying to sell you cutters will assure you their cutters are the best. This just further dilutes the debate. There is also harmonics which is very specific to individual cutting systems that have a definite effect on the cut quality.

The reason I bring this up is most of this never comes into play machine wood, plastics, or even aluminum. Most machinists work off the principle “carbide will break before bending” (generally three times stiffer than steel) and they are dealing with much tighter tolerances and more difficult to machine materials. The amount of bend you could ever possibly attribute directly to the tool is minute compared the known slop that is everywhere else.

From contributor S:
Don't rule out part deflection either. Bottom line is after making sure you have a tight part, and your tool/ collet/spindle setup is the shortest and tightest you can make it, try different combinations of speeds, feeds, and spindle direction with each type tool available (2 flute, 4 flute, high helix, etc.). The best combination will yield the least amount of deflection. There is no shortcut, just get busy "tweaking". You might even find things that don't make sense.