Measuring Resharpened Tools
Tips and tricks for finding the true measurements of CNC cutter bits after sharpening. December 6, 2006
Question
We're getting into unfamiliar territory - compensation for re-sharpened bits. Does anyone have good methods for measuring the new tool diameters? A two flute tool is not too difficult to check, but we have several 1 flute and 3 flute tools to deal with. Will I need any special equipment beyond a standard set of (digital) calipers?
In the past, we have not bothered to do this, as the .00 whatever difference in cut sizes really doesn't have a measurable impact on our final products (all custom exhibits, all the time: no mass production). A change in company structure and the addition of several hundred re-sharpened CNC tools has me taking a second look at this process.
Forum Responses
(CNC Forum)
From contributor M:
A competent re-sharpening shop should measure the tools for you and indicate their respective diameters. Otherwise, first mic them and then cut and measure a test part, making any necessary adjustment to its diameter.
From contributor F:
When I send tools out to be resharped, I specify on the packing list to mark new diameters on end of the shank. My service does this for me. Takes the guess work or test cuts out of the equation.
From contributor B:
I also have the sharpening service write the new diameter on the tool shank. In addition to that, we purchased an anvil caliper on E-bay at a very reduced price from what a brand new unit costs. This provides a method of measuring three edge tooling. The other alternative has already been mentioned - run a test cut and measure the cut.
From the original questioner:
Unfortunately, I'm getting a big box of tools that have already been sharpened, and they were not marked. Measurement (one way or another) is the only option for now. Bits that we have sharpened in the future will be a different story.
The only thing I'm concerned about with test cuts is machine runout and inaccuracy contributing to incorrect measurements. I'll give that a try first and see where it leads us, but I'll continue looking for a bench measurement solution.
Is an "anvil caliper" a brand name or a special style of caliper? I tried a search on E-bay, but nothing really jumped out at me.
From contributor G:
Since 1989, we (Courmatt) have put the OD on the tooling. We also match the sets. Your service company should also put the OD. With a single, 2, 3, 4 flute tool, you require different measuring equipment.
From contributor T:
Yes, the OD should be documented for you by the person sharpening your tools, but obviously yours aren't. Sometimes I run into the same situation, so I simply load the cutter into the spindle and then cut a slot in a piece of laminate or solid surface and then measure the width of the slot. It's always gotten it close enough for me.
From contributor R:
In order to accurately measure odd flute bits, you would have to purchase what is known as flute micrometers (mics). They are modified micrometers that have a "V" on the fixed anvil, allowing you to place two flutes within the "V" and measure to the protruding flute. These can be purchased online though Enco, MSC, Travellers, etc.
From contributor O:
I prefer using an optical comparator, placing the tool in a v-block. Accurate and fast, especially if you have a bunch of tools to verify. It's worth the money if you are getting into precision products. It's great for checking groove widths, profiles, etc. Using "denture mold," you can check features hidden from the comparator's view.
From contributor B:
To answer your question, the proper name is a V-Anvil Micrometer. Starrett makes a couple of different models. A No. 485 series is what you might be looking for, when needing to measure three edge tools. I was lucky enough to find one in very good condition on E-bay for half the cost of a new one, and it works perfectly for applications such as this.
Someone else pointed out the concept of having tools sharpened in sets. This is something we do also. We send out several at a time to be sharpened to the same diameter. This helps to eliminate fat finger errors when inputting diameter offsets at the controller. Every step that can aid in preventing human related errors has the potential of saving you large sums of money from crashes that you may never encounter. Just remember - never rush or allow distractions when measuring, calculating and inputting tool diameter and height compensations.
From contributor C:
You can buy all the gizmos you want, but consider what we do. If you have a 3/8 bit, put it in the machine with the correct 'H' offset and run a quick test program. We use a 2" x 2" square about 1/8" deep in a scrap piece of MDF. After running it, measure the actual dimensions. If it is .016" under (say 1.840 x 1.840), then your compensation for 'D' would be .008". Even if you measure a tool diameter, it needs to be checked, so why not do this in the first place? We even do this on new tools and find them up to .002" off.
From contributor B:
Contributor C has brought up a portion of the topic that was missed. Generally, new tools will have an acceptable tolerance between the actual diameter of the tool versus the listed size for such tool. We mainly use Onsrud tooling, which has a manufacturer tolerance of + zero/ - .004. This means that it would be perfectly normal for a .5" diameter tool (that is brand new) to have a true diameter of .496".
As for the thought of running a test cut for all tools... I think this might be overkill, time consuming and risk for damage to tool or machine, if the tool height offsets are entered incorrectly. With the applicable measuring equipment and a knowledge of their proper use, you will have more accuracy than will be needed for producing parts on your CNC router. As stated before, take your time measuring and prevent distractions when calculating offsets and entering them in your controller.
From contributor I:
Contributor C, while your method has some validity to it, the tool parameters do not work the same on all machines. Many depend on inputting actual values and not just a corrector value.
Also, when you run your test program, can you tell me how much of your size variance is due to tool pressure? I'll bet if you run it once with a conventional cut and once with a climb cut, you will see two different dimensions.
Based on the "make a cut" method of measuring diameter... I think the best would be to cut into a sheet of something firm and non-porous like nylon or delrin. Make a dado and measure the width of the groove. This will be the most true method, as there will be no tool pressure to deal with and your caliper will not press into the wood that you would normally be cutting.
From contributor A:
We have a simple center line cut program and 1/2" solid surface at the CNC that we check our cut widths on re-sharpened tools. It's worked well for us.
