Neal Demazure serves in a sales capacity at DATRON Dynamics. His superior technical aptitude has been critical to his success in helping customers solve complex manufacturing challenges through the placement of custom, application-specific solutions. Neal has extensive knowledge in both industrial manufacturing and dental milling technology.
This Blog on Machining Strategy is based on the Single Flute End Mill Webinar that I did with my brother Dann Demazure who is an Applications Project Manager here at DATRON. The video of that webinar is below, as is the part milled with the strategies detailed herein. The point of both the webinar and this post is to prove that the single flute end mill is really a “utility” cutting tool that should be in every machinist’s toolbox regardless of whether they are running a conventional VMC like a Haas or a high-speed machining center like a DATRON. To that end, the live milling demonstration done as part of the webinar, was performed at 15,000 RPM to emulate the results you might get with a conventional VMC, and also at 35,000 RPM to show the results you can expect with a high-speed milling machine. The intention was NOT to compare conventional machining with high-speed machining, but instead to present the single flute as a viable and ideal tool for both types of milling machines.
At the end of the video above you can see the milling strategies detailed in this blog used in a live milling demonstration that produced this aluminum part.
Machining Strategy – Slotting:
Tool p/n: 0068806A
Tool Type: 6mm dia. single flute, 4-in-1
Width of Cut: 100% (6mm/0.236″)
Depth of Cut: 0.0787″ per pass
@ 15,000 RPM: 94.5 inch/min feed
@ 35,000 RPM: 220 inch/min feed
Machining Strategy – Entry Angle:
Tool p/n: 0068806A
Tool Type: 6mm dia. single flute, 4-in-1
Width of Cut: 100% (6mm/0.245″)
Total Depth: 0.118″
Entry angles: 5, 15, 25, 90
Chipload: 0.0007″ – 0.0027″
I get the question all the time when someone is trying to wrap their head around how milling works without flood coolant – what about that chips? It’s a fair question, and an important one given how much havoc chip accumulation can be in a milling process, as well as how much work it can take to clean chips up or out of a machine tool. In this blog post, we’ll spell out exactly what happens with the swarf that’s created in a milling process where the coolant is sprayed in a fine mist and evaporates just as the cut is completed.
Chip Accumulation & It’s Effect on the Milling Process
One of the main functions of flood coolant, aside from the obvious cooling and lubricating the cut itself, is to wash the resulting chips away from the cutting process – and thereby preventing them from being re-cut or clogging up the cutting tool. Knowing this, many traditional machinists are concerned that with an evaporative coolant applied as a fine mist they’ll encounter significant interference in the milling process with the chips they’ve just created. Fortunately, this is not at all the case in the vast majority of milling situations.
The evaporative coolant used in DATRON equipment is applied using an atomizing system called a MicroJet. This system feeds pressurized air together with the coolant to the MicroJet nozzle, which atomizes and sprays the evaporative coolant directly at the cut. Since the cooling fluid evaporates upon contact with the cutting process (and wicks the majority of the heat away in the process) the resulting chips are perfectly dry as they clear the endmill flutes and are ejected away from the cutting tool.
Since the chips are dry by the time they land, clearing them away requires much less effort than it does when the chips are soaked in flood coolant. The chips do not stick to the inside of the machine cabin, to the fixture, to each other, or to anything really. As a result, should the machine head come to an area where chips have accumulated, the same high-pressure air/coolant blast that cools the cut will also blow the chips away before the cutting tool even comes in contact with the workpiece. For this reason, in the majority of cases, the chips do not pose any sort of risk to the milling process.
Of course, there are exceptions to every rule. Even with evaporative coolant and a high-pressure air blast, it is possible for chips to have a hard time getting out of the way. In my experience this can happen when you have a very small diameter tool, that is milling at a depth that is several multiples of its diameter, in pocket that isn’t a whole lot bigger than the tool itself. Since you don’t have flood coolant to carry these chips out of the pocket, care must be taken to select a cutting tool with a properly designed chip channel to sufficiently eject the chip from such a pocket.
Chip Management & Disposal
Most machines with flood coolant either come standard with or have optional chip conveyors. Chip conveyors are systems that live at the bottom of a machine tool and actively move chips out of the machine cabin, either via an auger or a conveyor belt. From there they are brought up a few feet so that they can be dumped in a bin or barrel. For the machine operator used to this process, it can be a bit puzzling to look at a DATRON machine and see no chip conveyor of any sort.
While it should be noted that the flagship M10 Pro does have an optional chip conveyor, it is true that the majority of DATRON machines in the field do not. The reason for this comes back to the fact that the chips are dry by the time they leave the endmill flute, and are therefore much easier to manage.
If you look carefully at any DATRON you’ll find that there is a significant amount of area below the machining table but above the bottom of the machine. This area serves as the chip-tray and is designed to be a large space that chips can accumulate in without interfering with the machine operation or milling process. This chip-tray is removable in every DATRON so that when it comes time to dispose of the chips they can be shoveled, dumped, or vacuumed out. This area is large enough to accommodate the result of several days of continuous milling, yet still be accessible enough to dispose of its contents without difficulty. Much care is taken to design the inside of the machine cabin with little to no accumulation points so that the chips fall naturally down to the chip tray. Machine operators who have managed both flood coolant and evaporative-mist coolant machines commonly comment that cleaning up dry chips is no more easy or difficult than cleaning up wet chips, it’s just different.
4 Ways to Ensure Consistent Depth of Cut (even on surfaces that are anything but flat): As far as your CNC is concerned, the world is all sunshine and roses: your cutting tool never deflects or wears, your fixture is rigid and free of vibration, and the surface of your workpiece is perfectly flat. However, those of us with gray matter here in the real world, know that the truth of the situation is anything but perfect – tools wear, fixtures flex, and that surface you’re about to cut is about as flat as the good Earth itself.
The video above explains it all! Video courtesy of #rapiddtm – visit them on Facebook!
Here at the DATRON blog, we’ve talked a bit about how to wrangle in tool deflection, and we’ve shared some tips about best practices for workholding. Today, we’re going to cover a few tricks you can use to maintain a consistent depth of cut when engraving, marking or milling surfaces that aren’t exactly the poster child of flatness.
Defining Flatness: Simply put, the term “flatness” is used to describe an area between two parallel lines within which a surface must lie. This specification will often work in conjunction with other dimensional call outs on the print to describe the range of possible locations of a given surface:
As you may or may not have realized by now, no surface is perfectly flat – indeed very few surfaces even come close to perfect flatness – and when it comes to manufactured parts, flatness costs money. So, if it doesn’t have to be flat, or if the print doesn’t define it as flat, you have to assume that it really isn’t flat. Depending on what you need to do to a particular surface, it’s flatness (or lack thereof) will need to play a key role in your milling strategy.
Consistent Depth of Cut Method 1: Qualify the Surface
If you are able to do so, qualifying the surface is far and away the easiest and most sure-fire way to make sure that the surface you’re about to work on is reasonably flat and true. Qualifying a surface is just fancy machinist talk for face milling the entire surface, taking off a few thousandths at a time until the whole surface is reasonably uniform in terms of flatness. A qualification pass is often the first step you will see when watching a milling process on a shop floor or online and this is for a number of reasons, not least of which is to ensure flatness of the surface in question.
When starting with a piece of billet or raw stock, qualifying a surface is almost always an option and in general is just good machinist practice. Sometimes, however, qualifying the surface simply is not an option – such as when working with die cast material, a forging, or with otherwise completed parts that simply need marking or serialization. In these cases, a different strategy will need to be employed in order to achieve a good result.
Consistent Depth of Cut Method 2: Use of a Spring-Loaded Engraving Tool
If all you need to do is a basic engraving or part marking process, and your surface is a little “all over the map” a spring-loaded engraving tool may be just what the doctor ordered. Spring-loaded tools come in a few different varieties, with the most popular versions being a spring-loaded version of a traditional split shank engraving tool and a spring loaded “drag engraving bit”, also known as a “scribe” tool.
Spring-loaded engraving tools incorporate a compressible mechanical system between the spindle interface and the cutting tool. These tool assemblies usually have anywhere from 0.20” to 0.40” of spring travel, so they can absorb a fairly dramatic change in Z height while still keeping a consistent downward pressure on the workpiece. Spring loaded engraving bits utilize a tipped split shank engraving tool and as such can produce a variety of engraving widths and depths. Drag engraving or scribe tools literally only are dragged across a surface and are not designed to incorporate a rotational element into the process. As a result, scribe tools a truly only a good fit for very shallow part marking.
While these tools will not be of much assistance when it comes to milling or drilling applications, they perform very well for shallow to moderate depth part marking. However, there are some drawbacks to this type of tool: a common shank size for these tools is ¾”, which may be too large for some spindles. Also, since these tools are a mechanical assembly they are usually limited to 10,000 RPM max. This limitation may force you to slow your feed rate down, increasing your cycle time.
So, if you need to tool up to serialize a thousand cast aluminum parts, a spring-loaded tool will likely get the job done. However, if you are planning on completing a milling or drilling process, or if the job requires a deep, wide, or intricate/high-quality engraving, you may need to turn to other methods to get the job done.
Consistent Depth of Cut Method 3: Use of a Touch Probing System to Map an Irregular Surface
Depending on what type of milling machine you have at your disposal, use of a probing system to touch off on the workpiece a number of times to “map” the surface may be possible. Surface mapping by way of a touch probe can be one of the faster, more elegant solutions to this problem – as it uses the technology within the CNC machine to compensate for irregularities in the Z height of the workpiece. This means you can really limit the introduction of new variables in your process and just stick with your tried and true cutting tools, fixturing, and feeds/speeds.
Surface mapping via touch probing usually involves giving the machine several basic details about what you wish to probe: size of the probe area, pitch of the probing grid, and so on. From there the machine will touch off on the workpiece as many times as is necessary to probe the specified area to the desired grid pitch. Once the touch probing cycle is complete, the machine control will take the cut file that has been programmed to be cut on a flat 2D surface and modify it with the variation in Z of the workpiece that was found during the probing cycle. This way, when the cutter goes about the process of milling or engraving on the surface, it’s depth will vary automatically so you get a consistent depth of cut regardless of variation in the Z height of the surface.
Not all CNC machines offer touch probing, and surface mapping isn’t always an option when they do. But if your machine has probing and surface mapping it’s not a bad idea to get familiar with it – you never know when it might come in handy.
Consistent Depth of Cut Method 4: CMM Surface Mapping and Image Projection in CAM
When all else fails … when you can’t qualify the surface, when a spring-loaded tool won’t do what you need and your CNC machine doesn’t have touch probing, when you have a CMM laying around that’s available for use and you don’t mind doing a bunch of CAM work, there is an option of last resort.
Photo above courtesy of #rapiddtm – visit them on Facebook!
Using a CMM to map a surface in order to compensate for height irregularity is very similar to doing so on the CNC machine itself – however without the luxury of having the mapping, milling and NC integrated into one, the process becomes much more labor intensive.
This process is involved enough that an entire article could easily be written for this alone. In an effort to be concise I’ll reduce it down to a step-by-step summary:
1. Load the workpiece onto the CMM
2. Manually measure as many points as is necessary to realize the full surface variability within the working area
3. Export the resulting point cloud into your CAD software
4. Create splines linking the measured points to create a 3D surface map
5. Export 3D surface map to CAM software
6. Project artwork / milled features onto the 3D surface
7. Generate needed tool paths and post the cut file out to your CNC
8. Load workpiece onto CNC and run the part
To be clear: this process would need to be repeated 100% for each and every part run. As you can likely tell, having to use this method could easily take a job that would be done start-to-finish in about a day using touch probing in the machine, and stretch it out to take several days – simply due to the tedious nature of having to use a CMM to map the surface.
Nothing in this world is perfect – but the ability to manage imperfections to produce a good result no matter what is one of the things that separates good machinists from great ones. I hope the methods described in this post will give you an advantage next time you’re faced with a workpiece that looks more like a potato chip than a pancake.
In the world of computer-controlled milling equipment, there’s always been something of an understanding when it comes to work envelope and precision: as the ability of a machine to achieve ever smaller numbers when it comes to positional accuracy and repeatability goes up, the size of the work envelope (and therefore the largest part you can physically fit in the machine) must go down. Now, like any rule of thumb, there are exceptions to this out there – but these exceptions generally carry with them one significant caveat: they’re expensive as all get-out. Enter DATRON MLCube LS Large Format Milling Machine with linear scales.
There are many legitimate reasons that this convention has become the norm. In ball-screw-driven machine tools, using a ball screw with a very tight pitch to achieve stellar accuracy and repeatability usually results in a decrease in the maximum rapid rate – which is a real bummer if you need the machine to move large distances. Technologies such as linear motors are capable of moving very fast over long distances, but sacrifices often need to be made when it comes to resolution and accuracy of the encoders that feedback the motors motion to the machine’s control system. Even linear scale technologies, while being readily able to increase a numerically controlled machining system’s ability when it comes to accuracy and repeatability, must by default be an additional piece of hardware which accompanies the linear motor or ball screw/linear guide system. Any additional hardware, as any engineer will tell you, is subject to damage, misalignment, or in the case of milling equipment -contamination from the chips, dust and coolant that are part of the milling process. It would seem that the combination of large, capable, precise, and economical has been an elusive one in machine tool industry.
Fortunately, this very problem that the DATRON MLCube LS has been created to solve.
Linear Scales for Precision in Large Format Milling
The ML Cube LS represents the latest in a long lineage of ever improving portal/gantry designed CNC milling equipment from DATRON. Building on the success of the DATRON MLCube, which provides 3 m/s2 acceleration, advanced dynamics and jerk control, 0.1 micron resolution, and the ability to exercise up to 60,000 RPM across its 60“ by 40” work envelope, the MLCube LS makes the significant addition of an integrated linear scale system on X and Y axes.
To avoid the hurdles common to achieving tight accuracy across a large area, DATRON engineers have employed a unique combination of technologies that together present a robust and highly precise positioning system: the integrated measurement system. This integrated system marries the accuracy and repeatability advantages of the external linear scale, with the well-established and optimized mechanics of the ball screw-driven / linear guide axis. In the same way that unifying a servo motor with the associated ball screw by eliminating the drive belt, the ball screw/linear guide/linear scale system benefits in its operation and longevity overall by combining components and optimizing the system.
Benefits of Large Format Milling Machine MLCube:
Benefits if this unification are numerous, but in the case of the MLCube LS the most significant benefits show themselves where they matter most:
System is free of wear or maintenance
Highly resistant to contamination
Exact positional measurement is achievable even under dynamic load changes
Effects of thermal expansion are essentially eliminated
Scale system is completely free of external influence by magnetic fields or electromagnetic vibration
Positional accuracy is improved by 50% compared to the same machine without linear scales
But at the end of the day, the real question is: Why should I care about this machine? Well, fortunately, that’s the simple part:
With a starting price of just under $250,000 including typical options and a positional accuracy of ±25µ across nearly 17 square feet of workspace, the MLCube LS arguably offers the most capability, across the largest work envelope, with the highest degree of positional accuracy, for the least amount of money.
So whether you need to produce a few very large and precise parts, or you need to batch machine hundreds of small precise parts in one long unattended machining session – the MLCube LS offers advantages that are not easily matched.
Download DATRON MLCube LS Large Format Milling Machine Brochure
When it comes to CNC milling strategies for bulk material removal you may be asking the wrong question.
As the account manager for industrial CNC sales in the Northeast USA, I routinely get asked, “What is the biggest tool you can put in a DATRON machine?” And while I always take time to answer this question, it gives me a bit of a chuckle because DATRON high speed CNC milling machines are all about efficiency with small tools! Now, of course I understand that in spite of the fact that this equipment has huge headroom in the RPM department, it must at the same time be capable and efficient when it comes to milling out larger features and bigger parts – most of our equipment does after all have a work envelope of 30” by 40” – but in the world of high RPM and high speed cutting strategies large features or bulk material removal does not necessarily warrant a large diameter tool.
An easy example is the simple process of pocketing: taking a workpiece and milling out an area to create an open space. In this example we’ll assume the pocket is to be 0.75” deep by 2.75” wide by 7” long. Traditional machining methods would involve the use of something on the order of a 1” diameter end mill making a traverse path along the length of this part with standard step down and step over values at typical RPMs of less than 15,000.
In the world of high speed cutting and new school cnc milling strategies, a more efficient toolpath can be realized by use of a comparatively small tool, such as a 6mm end mill, and beginning with a helical toolpath that circles all the way down to the final depth. From there, a large percentage of the cutting flute can remain engaged in the material as the tool circles around removing material continuously as it widens it’s circular X/Y path until the full pocket has been created. This type of strategy, when combined with the right RPM and cutting tool geometry, can outperform a physically larger tool that is using lower RPM and traditional strategies.
To summarize, in the world of high speed machining it’s all about making a lot of small chips very quickly. The necessity of a dimensionally large tool to create a dimensionally large feature have been eclipsed by the advent and proliferation of high speed milling machines with the CAM strategies and cutting tool geometry to go along with them.
For more information on the CNC Milling Strategy used on the aluminum housing shown above:
Download CNC Milling Strategy Application Notes with Bulk Material Removal (Aluminum Housing):
Technology that allows small to moderate sized labs to mill their own PFMs understructures, custom abutments and implant bars has matured significantly in the past few years. Not long ago, an average lab had to choose to either paying top dollar to have a large company mill these types of units, or go through the labor intensive process of casting. Today, a wide variety of milling equipment has become available which has unlocked the ability for CAD/CAM savvy labs to be more self-sufficient and profitable; however, there is still some uncertainty when it comes to when this is an appropriate and prudent step to take. In this post, we’ll focus on three key-indicators that your lab is ready to take its milling game to the next level.
1. You’re Already Scanning, Designing and Milling Soft Materials
If your lab already has built up the workflow and knowledge base to successfully operate CAD/CAM equipment for the purposes of milling zirconia, wax or PMMA – then you’re already half way there! In general, I advise against going right from having zero milling in your lab to bringing in metal milling – it’s a little akin to biting off more than you can chew. However, the process and workflow of a successful zirconia milling laboratory is very similar to that of a titanium or chrome-cobalt milling laboratory.
It is important to note that you might not necessarily be integrating metal milling equipment with your existing CAD/CAM infrastructure. Depending on the focus of your lab and your client base, new or upgraded scanning systems and/or CAM software may be necessary to achieve desired results (for example: implant bar manufacture places different demands on the CAD/CAM system compared to crown and bridge work). The thing to keep in mind is that if your team already has a good foundation of knowledge in CAD/CAM, the learning curve for new technology will be much more manageable.
2. Your Clients are Asking for Added Value from your Lab
Ever turn work away? Or worse yet, take a case on just to realize that it’s costing you money because you have to depend heavily on outsourced work to complete it? If your clients have been asking your lab to provide additional services and they’ve been doing it for a while – you have a market in your area that is hungry for a more capable and comprehensive laboratory to meet their needs. There are many ways to quantify this potential, which is a very necessary step on the path to making a business decision. Many labs will survey their client base, either via email, snail mail survey, or with a phone outreach program. If your clients aren’t getting their milled PFM crowns and bridges or titanium bars and abutments from your lab – where are they getting them? And most importantly, would they consider using your lab for a source of these units if you were to offer this service? This approach gives you a good idea of what the initial revenue impact will be if and when you begin to market additional capabilities.
3. Your Monthly Cost for Outsourced Milled Units is Regularly Greater Than $6,000
A few chrome-cobalt copings here, couple of abutments there, that bar case last week, plus the full arch that you weren’t quite sure your light duty table top mill could do a good job with…. It adds up quickly doesn’t it? Sure does. If you already have CAD/CAM technology in your lab and you’re confident that your client base would send more business your way if you had the capability in house, then it’s time to brush the dust off the last 18 months of your lab’s financial records. Why? Because the first two criteria alone are not sufficient to justify an equipment purchase. In order to move forward in full confidence that you’re making the right decision for your business you need to analyze your lab’s outsourced consumption for at least the past year and a half, preferably longer. This will give you both reliable information on both how much your lab outsources in an average month, but also data on growth trends which will allow you to forecast your labs needs in the future. The more data you have, the more clarity and confidence you will have in your decision.
Why are we looking at outsourced cost per month? Viewing the situation in this manner allows us to break the big question; “Will this equipment investment yield a good return?” into an easier question to answer; “Will this equipment make my business money on a monthly basis and if so, how much?”.
With the significant investment that is required to bring qualified metal milling equipment into your lab (generally from $100,000 to $300,000 or more) it is quite common for business (dental labs or otherwise) to lease the equipment instead of going with an outright purchase. In addition to making a “monthly ROI” easy to calculate, many financial advisors will tell you that leasing is the preferred method for purchasing capital equipment as it allows your business to maintain financial liquidity. Typical lease packages for manufacturing equipment will have a $1 buyout at the end of the lease period – so your manufacturing can continue uninterrupted at the end of the lease. At common rates, the monthly payment for a five year lease on a quality piece of milling equipment that is robust enough to handle regular milling in titanium or chrome-cobalt will range anywhere from $2,000 to $4,000 per month. With this in mind, a lab that consistently outsources $6,000 per month will see a return on investment in just over 2 years.
Many labs put off the decision on whether or not to adopt titanium or chrome-cobalt milling capabilities out of a fear that it’s too complicated or too costly, and for some labs it is. But when emotions are removed from the equation and the situation is reviewed logically, lab owners are often surprised at how easy and beneficial of a decision it can be.
Download Brochure detailing a Business-in-a-Box solution that delivers an all-inclusive CAD/CAM production center for screw-retained & fixed restorations.
The term “High Speed Cutting” (also known as high-speed machining) is one that has grown in the manufacturing industry significantly in the past 5 to 10 years. In spite of its newfound ‘buzzword’ status, the definition of this process remains somewhat elusive, or at best is defined loosely as simply milling at a sufficiently high RPM. The reality of high speed cutting is a bit more nuanced, but nonetheless demands attention due to the significant efficiencies it affords. In this post we will take a look into the inception and development of the high-speed cutting as a process. Research and development of high speed cutting methodology was advanced most significantly in the late 70’s and early 80’s by way of the Advanced Manufacturing Research Program, funded by DARPA. The goal of this program was to identify a means of faster material removal by use of significantly higher RPM and feed rates than were traditionally employed. This program tested cutting speeds (Vc) that ranged from as little as 0.05 in/min to as high as 960,000 in/min and beyond. Similar research was being done in Europe during the mid 1980’s at the Technical University of Darmstadt. The results of these research efforts was the realization that the ‘sweet spot’ of a high speed cutting process varies depending on that material being milled as well as geometry of the cutting tool. In general, these sweet spots are defined as follows:
Once the threshold into the HSM range has been reached, the benefits of this cutting method start to show themselves. The advantages of high speed cutting are realized in four major areas:
1.) Increased machining accuracy
As the cutting speed increases, the cutting force decreases due to a phenomenon called thixotropy – or the property of a material to be “work softened” due to the shear strain imparted on it by the tool’s cutting edge, and then to revert back to the original hardness properties once the cutting process is complete. This property is particularly true for aluminum alloys, which makes aluminum an ideal candidate for high speed cutting processes.
2.) Improvements in surface finish
General machining knowledge tells us that friction heat in a milling processes is generated equally on each side of the tools cutting edge (accounting for nearly 80% of all induced friction heat) with another 20% being generated by the deformation or bending of the resulting chip. In a high speed cutting process the chipload is evacuated at such a high rate that the majority (approximately 60%) this friction based heat does not have sufficient time to conduct into the surrounding workpiece or to the tool itself. As a result the machined surface finish exhibits superior quality with an appreciable reduction in temperature induced workpiece degradation.
3.) Reduced bur formation
Based on studies focused on high speed machining best practices, a notable decrease in bur formation is observed once a sufficiently high cutting speed has been achieved. This reduction in bur formation is a function of both the cutting speed itself but also proper geometric design of the cutting edge. In short, a cutting tool that has been properly design to suit the work material which is rotated at sufficient speed affects a cut that is rapid enough to shear the material completely and cleanly – thereby reducing or eliminating the formation of a bur.
4.) Improved Chip Evacuation
Similar to the reduction in bur formation, the improvement in chip evacuation enjoyed by those employing high speed cutting practices is primarily a result of the cutting tool geometry combined with the high energy state produced by the RPM being applied. With a cutting speed in excess of 500 m/min, and a cutting tool optimized to evacuate a large volume of chips in a short period of time, the resulting chipload can be ejected from the processing area with a high velocity, greatly reducing the possibility of re-machining of chips or damage to the work piece due to an abundance of residual chips. With spindle speeds in the range of 8,000 to 12,000 RPM becoming very common in the machine tool market, the ability to leverage the advantages of high speed cutting in steel, cast iron and nickel-based alloys is already available to manufacturers who are willing to adapt their strategies to those that fit with HSC best practices. High speed cutting of non-ferrous materials such as brass, aluminum and engineered plastics demands a significantly higher RPM capability, and as such those wishing to take advantage of the benefits of high speed cutting for these materials must focus on milling equipment capable of operating at high speed spindle speeds of 25,000 to 50,000 RPM or more. With the need for machined parts which display ever increasing levels of precision and quality, high speed cutting offers a means of working “smarter, not harder” – by taking advantage of a CNC milling system where a synergy between material, cutting tool and cutting speed allows performance levels unseen in traditional machining practices.
Learn More: Download the High Speed Cutting White Paper: