Staying on the dreaded side lock endmill holder theme, there is a significant quality gap, though this was not a comprehensive test. We measured two 3/4" stub length toolholders from two suppliers with a 3-point bore gage. After calibrating off of a ring gage, the first bore measured 0.751" and the second 0.75005". We also measured ten random 3/4" carbide blanks (as we did in the earlier post with 1/2" blanks). We then loaded each of the ten blanks in each holder (tightening the screw on the round blanks, no flats) and measured the total indicator runout (TIR) in a high end tool presetter. Toolholder #1 ranged 0.0011" to 0.0012" in TIR and Toolholder #2 from .00020" to 0.00030". 

Side lock toolholders are still in use because, they still work in some applications. As we pointed out in an earlier post: https://goo.gl/gEaNuP
 by design endmills are trying to twist and pullout of toolholders. Many other toolholders are held by friction only. Think of it this way; if you wanted to drive a gear or a sprocket from a motor shaft, would you rely on a press fit? You would use a key and a screw (or a spline). Dynamically, side lock holders can be made very short (1.75" gage length minimum) with significant damping.

Draw your own conclusions.

​Before toolholder experts start throwing up their hands that I am discussing side lock endmill holders, the fact remains it is likely still the most popular toolholder is use today (rivaled by the ER collet chuck), therefore including them in our research is both relevant and responsible.

When measuring runout on a side lock holder once, we noticed extreme runout. We had measured both the bore of the holder and the shank of the endmill, but this runout was TWICE what it should have been based on those measurements. AND, it was perpendicular to the screw hole, not inline as we expected. What we found was the flat on the endmill was ground so the bevel of the screw made contact with the angles of the flat. We get what they were going for here, a more accurate taper to taper contact, but when we applied prussian blue and reassembled we found uneven contact points.

The tightening of the screw made contact on the center line as intended as shown by the lower arrow, but the twisting and downward force of the screw cause the tool to pivot in the bore. The end of the toolholder bore acted as a fulcrum.

Two of the four endmill brands tested had these narrower flats. Amazing what you find when you measure stuff.

​When looking at carbide endmills, you will see a specification for shank diameters called H6. This from the ISO-286-2 tolerances for shafts. For our 1/2" example, the standard says within the shaft diameter range of 10-18mm the tolerance is +0/-11 microns which converts to +0.0000/-0.000433". 

Most carbide endmill manufacturers purchase pre-ground carbide rod already cut to length with a chamfer on one end that will be the shank end. Below is a sampling of ten 1/2" rod blanks measured at three points. Blue is the chamfer/shank end, red is the middle and green is the cutter end. 

To meet the H6 tolerance, the rod cannot be under 0.499567". Blank #1 exceeds the tolerance only on the shank end and should be rejected. Blank #8 does not exceed the tolerance on the blank end, but is up against it on the cutter end and middle. 

Some manufacturers have tighter shank tolerances of H5 (+0/-0.000315) and H4 (+0/-0.000197). Again these were for a 1/2" shank.

Making it work I am going to punt on part of this to John Bradford of Makino below.
https://goo.gl/sTcwyg

​I would add to his great recommendations that you test the runout in the spindle at operating temp. Use a good 50 Millionths test indicator and a mag base or gage stand with fine adjust shafts. We will part from our normal advice and say that pre-balanced holders will work here (the endmill has so little mass) and that the holder’s projection or diameter will not make a difference one way or another. Runout and balance are key, but the tool is still very flexible and dynamics are in play. While we can't tap test miniature endmills there is some science that can be applied. The Harmonizer by MLI can record the sound of the cut and determine resonate speeds where the flexing is at its worst and need to be avoided. This will work with spindle speeders and air spindles if you can adjust the output speed. https://goo.gl/WLeUy4

On standard spindles and toolholders, RCSA can be used to model the miniature endmill and predict stable speeds. Once you get a process dialed in you will want repeatability of the tool stick-out. The rings used on PCB drills might be a good solution if the shanks are 1/8" or 3mm.

​"You can't get there from here"

Let's take a 1/4" endmill in a 10,000 RPM machining center. The endmill's recommended surface speed is 2000 SFM. To reach that you would have to run the tool at 30,558 RPM (SFM x (12/π)/Diameter = RPM). Because the largest and deepest stability lobes are at the fastest speeds, with only 10K RPM you are not going to get there. Endmills smaller than 1/4" and the lack of speed capacity gets magnified. At lower speeds, the cutting action of the endmill is compromised. A spindle speeder like the Colibri Spindles or an air spindle are a solution. It also makes me wonder if going back in time and using small cobalt endmills might be a forgiving alternative.

Another limiting issue is cost. Small carbide endmills are inexpensive. For example a ¼” endmill from one manufacturer sells online for $22.50, their ½” is $60.73 and their ¾” is $218.84. It it tough justify a lot of effort that yields little cost avoidance. Break and replace becomes a strategy.

Small endmills are VERY flexible (until they break) so very susceptible to forced (runout, unbalance) and self-excited vibration (dynamics). 

In the next post, we will (finally) offer some suggestions to improve small endmill performance.

​YEAH, BUT WHAT ABOUT SMALL ENDMILLS?

No matter what I present, I always get a "yeah, but..." from someone in the audience. Sometimes it's "...what about drills?" (We research milling. Do you go to KFC and ask "what about hamburgers?"). Sometimes, it is ".... what about small or miniature endmills?". 

So, I will address this is the next couple of posts (but, not drills).

Tap testing is applicable to endmills 3/8" (9mm) and larger. With a miniature hammer, you can go down to about 1/4" (6mm) as the video shows. After all, we are hitting it (lightly) with a hammer so there are limits. But, there are other reasons as well.

Carbide is brittle. Small diameter carbide is really brittle. Small endmills break for a lot reasons other than dynamics. They break in shipping. They break from handling. They break by setting them down on a table the wrong way. The effects of runout or unbalance are magnified as the cutter diameter gets smaller. If you can't get the chips out of they way they break. If the coolant gets diverted or block for a moment they break. 

To be continued....

These test results are sure to cause some controversy. Just six tools, so not an absolute conclusion.

The same 3/4" endmill, sticking out the same amount from six different toolholders (names are covered), machining slots in aluminum at the same feed rate (0.008 IPT or 10% of the worst measured runout) in the same CNC machining center. We measured the runout with a test indicator. Each tool assembly was tap-tested and then run at the maximum stable depth of cut and speed determined by each's unique stability lobe diagram. This was deemed a roughing cut, so the slot width accuracy and surface finish were not considered.

The productivity, as measured in metal remove rate (cubic inches per minute), did not correlate to the tool's concentricity or lack thereof. This reinforces the fact that the tool deflects at the first tooth impact with the workpiece and seems to imply that its dynamic characteristics (its vibration frequency + tooth impact frequency) may dominate its static ones. 

​This was my favorite line from the move The Social Network. I like to paraphrase it by saying:

"If you had the solution for chatter, you would have solved chatter"

...and that company/product would have 100% marketshare, but sorry  it doesn't work like that (and no one has 100%). You can't eliminate chatter, no product or process can. You can only avoid it. To avoid it you have to know where it is. By measuring the system's  (tool, toolholder, spindle) dynamics with a tap-test or RCSA you can determine the speeds and cutting depths that will avoid chatter and those that won't.

With HSM tool paths you hear a a lot about radial chip thinning. When milling with light radial engagement (AKA width of cut or step-over), anything under 50%, you are not cutting a full thickness chip and the tool manufacturer's feed rate limits are based on that full thickness chip load. Applying chip thinning formulas you can increase the feed rate to catch up to what would be the average chip thickness. In essence, you are cutting a longer thinner chip that has the same mass as the shorter thicker chip while staying under the chip load limit of the tool.

The same applies for axial depth of cut, instead of at the 50% engagement, full chip thickness is at the radius of the corner, be it a bull nose or ball nose endmill or a toroid (round) insert face mill. If you cut an axial depth of cut less than the full radius, you need to increase the feed rate to compensate for the thinning of the chip. In the illustration above, you can see the lower depth changes the lead angle and the chip thickness (the blue area to the right of the red line). 

We have a free embeddable calculators for both axial and radial chip thinning:
https://lnkd.in/eiaH9in

I have been giving small bites of the science of Machining Dynamics. Here is an 11-1/2 minute seminar on the subject from Dr. Tony Schmitz at the University of North Carolina at Charlotte that could be considered more of a masters class. ​

Think about where we are going with this.

SCENARIO ONE: You are bidding on a job. You can build a milling tool assembly online and open its Dashboard. You will know precisely how fast that tool will run and use that to program the part for your bid. If you are not sure that the performance is good enough, you can select another tool and its Dashboard to see if it will run better. You win more work because your bids are more competitive and you will make the parts in the time you estimated. No more surprises (or nightmares) during setup. You only buy the tools you know in advance will work. 

SCENARIO TWO: You need to move a job to another machining center in your shop. You can open the job’s tool Dashboards, switch to the new machine, and adjust the speeds (because they will be different) in the part program. You are back making parts, not stuck in setup chasing chatter.​

CNC Machining Centers:
We need access to each popular model of machine and spindle option to do a tap-test of an artifact (a tool blank of our design). Takes a couple of minutes for each test. We also need basic data about each model, nothing proprietary. It is all in your brochure, plus a torque/power curve if it is not.

Next, we need to accumulate solid models of the tooling. The typical 2D and 3D CAD files supplied by manufacturers are not sufficient for this application. We must build the models using specialized simulation software. 

Toolholders:
If you make toolholders for milling we need to build models with their internal and external dimensions.  We may also need to do a one-time test of the tool to toolholder connection stiffness.  

Milling Tools:
For carbide endmills, the models are relatively easy, but those for indexable milling cutters with inserts are more complex.  

If you are interested in participating in RCSA and the Machine Tool Genome Project, go to our website and send us a message.
https://lnkd.in/eYHeVeb

​RCSA, PART ONE

Here’s how RCSA works. A measurement of a machine tool’s spindle is made with a tap-test of an artifact. That has to be done only once. We then couple that measurement with solid models of the tooling to predict the tool point frequency to generate a Stability Lobe Diagram-powered Dashboard. This opens up the possibility that a Dashboard Database could be developed without the need of tap-testing EVERY tool in EVERY machine.

The challenge has been the sheer massive amount of data required. If you add up the number of models of machining centers, toolholders and cutting tools for milling available on the market plus the number of different workpiece materials, the total number of combinations (and therefore Dashboards) would be 4.8 quadrillion. 4.8 million billion. 4,800,000,000,000,000.

However, if we dig deeper into the numbers, an RCSA Dashboard database becomes feasible. Research reveals that the top 100 models of machining centers represent 71% of the total market sold. Tooling manufacturers have dozens of overlapping products. If we focus on the manufacturers' first choice tooling appropriate to each specific model and application, the numbers go down significantly.

Next, we will tell you what we will need to get this done.

​It is our objective to make the Stability Lobe Diagram-powered Dashboard accessible to everyone that does milling. There are three ways that Dashboards can be delivered. 

1. Direct tap-testing of a tool in a machine. This will be done by the end user themselves or could be offered by their vendor of milling machines, tooling or software. It will require tap-testing hardware and software that generates the Dashboard. 

2. A machine or tooling vendor will supply pre-tested Dashboards with their products. The first one to do this is Bad Axe Tooling Solutions:
http://www.badaxetool.com/

3. Receptance Coupling Substructure Analysis (RCSA) was invented by Dr. Tony Schmitz of the University of North Carolina at Charlotte. RCSA uses a one-time artifact measurement of a machine's spindle and couples it with a solid model of a toolholder and cutter. This presents  the potential for a pre-process database of Dashboards. We will discuss RCSA in more detail in the next post. 

The Machine Tool Genome Project website:
https://lnkd.in/eYHeVeb

t wouldn't seem to be hard. You fine balance a shell mill arbor first and keep it in the balancer. Then load the face mill and run the balance test again and determine where to remove material and how much, preferably by milling than drilling, but both would work. Add that dimension to the program to machine future face mills. You may have to make an orientation witness mark of there are uneven drive slots on the holder.

There will will be some variance, error stacking and the shell mill arbor connection is not the most repeatable, but it would be an improvement. Especially those for high speed milling of aluminum. You would also need to provide a source for pre-balanced shell mill arbors. I don't know if any one yet does, but they could.

We did an experiment years ago with modular tooling. We balanced the base holder (the one that goes in the spindle). Then we used it to balance a number of different modular components, extensions and cutters. One at a time using balancing rings. Then every combination we assembled measured well balanced, not perfect but far better than they did when the rings were removed. 

​If you sell TOOLHOLDER SYSTEMS for Milling you can tap test the customer's existing cutter in your toolholder and generate a Dashboard in less than one minute. You can repeat this with additional toolholders minimizing the customer's spindle downtime for trial and error testing. Dashboards will show you the maximum available speed and cutting depths their cutter will run in your toolholder.

You no longer have to absorb returns of used trial toolholders. You will know the answer before a cut is made. You will never again lose an order because the cutter could have run at FASTER speed in your toolholder, but you didn't know where.

At the bottom of our free calculator page we have created a custom Excel template that you can use to compare up to 20 of your toolholders with the customers's existing holders, calculate the customer's annualized savings and the return on investment (ROI) including any additional equipment required.

https://lnkd.in/euvsupn

This technology has never been more economical to implement and easier to use.

​If you sell CUTTING TOOLS for MILLING, being able to tap-test a tool and generate a Dashboard (in less than one minute) will create an immediate competitive advantage.

It will provide you maximum available stable speeds and cutting depths. You can optimize feed rates and thermal limits for high speed machining and make all of the calculations your customer needs for programming. You will save hours of trial and error tool testing (with no guarantee of success). You will know the answer from the start. GTO's become guaranteed ORDERS without the "trial".

The toolholder chosen can impact the performance of your cutting tool. You can ensure that you have the best possible combination and win more orders at the spindle. Make sure nothing holds back your cutting tool's performance. You can also use it for R&D to calculate the cutting force coefficients and process damping wavelength for specific geometries.

At the bottom of our free calculator page (that you can embed into your website), we have created some Excel spreadsheets that you can use for tool comparisons, calculating true costs and justifying your customer's investment.
https://lnkd.in/euvsupn

This technology has never been more economical to implement and easier to use.

​If you sell CNC MACHINING CENTERS, having the capability to tap-test milling tools and instantly generate Dashboards in less than a minute each can have a massive positive impact.

TURNKEYS – Select the absolute best tool and toolholder combination specifically for your machine. Test multiple tool configurations and find the winner. Return the rest, unused. Meet cycle time targets by unlocking hidden time from stable tools to compensate for the tough ones. Know definitively if a problem is with the tool or the workholding.

TIME STUDIES – Combine with your CAM and simulation programs to quickly deliver fast and accurate part processes specific to your machines without taking a cut.

RUNOFFS – Fully utilize your machines’ capabilities with the right tool selection with highest productivity, surface finish and accuracy. Don’t let the wrong tooling hold your machine back.

TOOLING – Provide customers with Dashboards with their initial tooling package on a new machine. They will be running optimally from day one.

SERVICE – Fix customers’ chatter problems on the spot. Benchmark new spindles.

USED MACHINES - Prove a used machine's current capabilities.

​The typical reason for grinding chip breakers into a carbide endmill are, as their name suggests, to break up long chips. However there is also an impact on the system's dynamics or it's tool point behavior.

If a dynamic measurement (tap-test) reveals a maximum stable depth of cut of 1" and the chip breakers remove 30% of the surface area of the cutting edges, then the cutting forces are reduced by 30%, deflection is reduced and the tool will be able to cut deeper than as measured (probably faster too, but you would have to measure its frequency to know by how much). 

If you are having stability issues when using a long axial depth of cut with trochoidal style tool paths, consider adding chip breakers.