How to Maximize High Balance End Mills

/1 Comment/in , , , , , /by

High speed machining is becoming increasingly widespread in machine shops all over the world due to the proven benefits of greater efficiency and productivity through increased spindle speeds and metal removal rates.  However, at such high spindle speeds, otherwise negligible errors and imperfections can cause negative effects such as reduced tool life, poor surface finish, and wear on the machine itself. Many of these negative effects stem from an increase in total centrifugal forces leading to vibration, commonly referred to in the industry as chatter. A key contributor to vibrations and one of the more controllable factors, is tool unbalance.

Why Balance is Critical to Machining

Unbalance is the extent to which the tool’s center of mass diverges from its axis of rotation.  Small levels of unbalance may be indistinguishable at lower RPMs, but as centrifugal force increases, small variations in the tool’s center of mass can cause substantial detrimental effects on its performance. High Balance End Mills are often used to help solve the problem of vibrations at the increased spindle speeds. Balancing is used to make compensation for the intrinsic unsymmetrical distribution of mass, which is typically completed by removing mass of a calculated amount and orientation.

infographic showcasing all aspects axii for high balance machining

Image Source: Haimer; Fundamentals of Balancing

Helical Solutions offers High Balance End Mills in both 2 and 3 flute options (see Figure 2), square and corner radius, along with coolant-through on the 3 fluted tools. These end mills are balanced at the industry standard of G2.5 at 33,000 RPM: G stands for the potential damage due to unbalance, which can be expressed as “Balancing Quality Grade” or G and 2.5 is the vibration velocity in MM per second. These tools are designed specifically to increase performance in highly balanced machining centers that are capable of elevated RPMs and feed rates. With high balance tooling, improved surface finishes are also achieved due to reduced vibrations during the machining process. Additionally, these end mills have been designed around current high-end tool holding, and come in a variety of neck lengths at specific overall lengths. These dimensional combinations result in maximum rigidity and reduced excess stick out, allowing for optimal performance and the ability to push the tools to the limit.

cnc high balance end mills in both 2 and 3 flute designs

High Balanced Tooling Cost Benefits

Machinists who choose to use High Balance End Mills will see certain benefits at the spindle, but also in their wallets. Cost benefits of opting to run this type of tool include:

Utilizing Tap Testers

What Tap Testers Do

Vibrations are your applications worst enemy, especially at elevated RPMs and feed rates. Using resources such as a Tap Tester can help decrease vibrations and allow you to get the most out of your High Balance End Mills by generating cutting performance predictions and chatter limits.

How Tap Testing Works

how to properly tap test a cnc tool

Image Source: Manufacturing Automation Laboratories Inc.

Tap Testing generates cutting performance predictions and chatter limits. In a tap test, the machine-tool structure is “excited,” or tested, by being hit with an impulse hammer. In milling, the machine-tool structure is usually flexible in all three directions: X, Y, and Z, but in milling applications where High Balance Tooling is used, the flexibility is commonly only considered in two planes – the X and Y directions. By hitting the X and Y directions with the impulse hammer, the impact will excite the structure over a certain frequency range that is dependent on the hammer’s size, the type of tool being used, and the structure itself. The frequencies generated from the initial hit will produce enough information that both the impact force measurement and the displacement/accelerometer measurement are available. Combining these two measurements will result in the Frequency Response Function, which is a plot of the dynamic stiffness of the structure in frequencies.

After the information from the Tap Test is gathered, it will then process the information into useful cutting parameters for all spindles speeds such as cut depths, speed rates, and feed rates. In knowing the optimum running parameters, vibrations can be minimized and the tool can be utilized to its full potential.

High Balanced Tooling Summarized

Keeping vibrations at bay during the machining process is extremely important to machining success. Because one cause of vibration is tool unbalance, utilizing a balanced tool will result in a smoother job, a cleaner final product, and a longer life of both the tool and spindle. Machinists who choose to use High Balance Tooling can utilize a Tap Tester, or a method for generating the perfect running parameters for your tool and machine setup to ensure that machining vibration is as minimal as possible.

Shank Tolerances, Collet Fits, & h6 Benefits

/1 Comment/in , , , , /by

A cutting tool’s shank is one of the more vital parts of a tool, as it’s critical to the collet-tool connection. There are several types of shanks, each with their own tolerances and suitable tool holder methods. One of the most popular and effective tool holding styles is a shrink fit tool holder, which works with h6 shanks, but what does this mean and what are the benefits of it? How is this type of shank different from a shank with standard shank tolerances? To answer these questions, we must first explore the principals of tolerances.

The Principals of Tolerances

Defining Industry Standard Tolerances

There are two categories of shank tolerances that machinists and engineers operating a CNC machine should be familiar with: hole basis and shank (or shaft) basis. The hole basis system is where the minimum hole size is the starting point of the tolerance. If the hole tolerance starts with a capital “H,” then the hole has a positive tolerance with no negative tolerance. The shank basis system is where the maximum shank size is the starting point. This system is relatively the same idea as the hole basis system but instead, if the tolerance starts with a lowercase “h,” the shank has a negative tolerance and no positive tolerance.

Letter Designations

The limits of tolerance for a shank or hole are designated by the appropriate letter indicating the deviation. For instance, the letter “k” has the opposite minimum and maximum designations as “h”. Tolerances beginning with “k” are exclusively positive, while tolerances beginning with “h” are exclusively negative. The number following the given letter denotes the International Tolerance (IT) grade. For example, a tolerance with the number 6 will have a smaller tolerance range than the number 7, but larger than the number 5. This range is based on the size of the shank. A hole that has a 0.030” diameter will have an h6 tolerance of (+0.0000,-0.0002), while a 1.00” hole with have an h6 tolerance band of (+0.0000,-0.0005).

It is important to note that most sources list IT tolerances in millimeters, while the graph below has been translated to inches. Operations that require more precise manufacturing, such as reaming, will have lower IT grades. Operations that do not require manufacturing to be as precise will have higher IT grades.

graph showing shank tolerances vs diameter

Preferred Collet Fits

Different types of combinations of hole basis and shank basis tolerances lead to different types of collet fits. The following table offers insight into a few different types of preferred fits and the shank tolerances that are required for each.

infographic of collet fits and the associated clearance
Image: Machinery’s Handbook 29th Edition.

Shrink Fit Tool Holders

The shrink fit holder is one of the more popular styles of tool holders because of its ability to be more customizable, as evident in the chart above. In this method, a collet is heated to expand, then cooled to contract around the shank of a tool. At room temperature, a cutting tool should not be able to be inserted into a shrink fit holder – only when the holder has undergone thermal expansion due to the introduction of a significant amount of heat should the tool fit. As the holder cools, the tool is held tighter and tighter in place. Typically, a holder is heated through a ring of coils by an induction heater. It is important to heat the holder uniformly, paying mind to not overheat it. Doing so could cause the shank that is being held to expand within the holder and remain stuck.

shrink fit tool holder

Benefits of Shrink Fit Tool Holders

  1. Gripping power. The shank is held flush and uniform against the holder, resulting in a tighter connection.
  2. Low runout. A more secure connection will result in extended tool life, and a higher quality surface finish.
  3. Better balance for high RPM. With a tighter tool-to-holder connection, the opportunity exists for more aggressive running parameters.

Explore More About Tool Holders With Our Cutting Tools Explained Webinar

Shank Tolerances Summarized

Understanding shank tolerances is an intricate part of the machining process as it impacts which tool holder is appropriate for your job. A secure holder connection is vital to the performance of the tool in your application. With an h6 shrink fit holder, the result is a secure connection with stronger gripping power. However, only certain shanks are able to be used with this type of holder. From the letter designation assigned to a shank, to whether that letter is upper or lowercase, each detail is vital to ensuring a proper fit between your tools shank and its corresponding shrink fit holder.

Best Practices of Tolerance Stacking

/10 Comments/in , , , , /by

Tolerance stacking, also known as tolerance stack-up, refers to the combination of various part dimension tolerances. After a tolerance is identified on the dimension of a part, it is important to test whether that tolerance would work with the tool’s tolerances: either the upper end or lower end. A part or assembly can be subject to inaccuracies when its tolerances are stacked up incorrectly.

The Importance of Tolerances

Tolerances directly influence the cost and performance of a product. Tighter tolerances make a machined part more difficult to manufacture and therefore often more expensive. With this in mind, it is important to find a balance between manufacturability of the part, its functionality, and its cost.

Tips for Successful Tolerance Stacking

Avoid Using Tolerances That are Unnecessarily Small

As stated above, tighter tolerances lead to a higher manufacturing cost as the part is more difficult to make. This higher cost is often due to the increased amount of scrapped parts that can occur when dimensions are found to be out of tolerance. The cost of high quality tool holders and tooling with tighter tolerances can also be an added expense.

Additionally, unnecessarily small tolerances will lead to longer manufacturing times, as more work goes in to ensure that the part meets strict criteria during machining, and after machining in the inspection process.

Be Careful Not to Over Dimension a Part

When an upper and lower tolerance is labeled on every feature of a part, over-dimensioning can become a problem. For example, a corner radius end mill with a right and left corner radii might have a tolerance of +/- .001”, and the flat between them has a .002” tolerance. In this case, the tolerance window for the cutter diameter would be +/- .004”, but is oftentimes miscalculated during part dimensioning. Further, placing a tolerance on this callout would cause it to be over dimensioned, and thus the reference dimension “REF” must be left to take the tolerance’s place.

close up of a shaped of slot from a corner radius end mill and its tolerances
Figure 1: Shape of slot created by a corner radius end mill

Utilize Statistical Tolerance Analysis:

Statistical analysis looks at the likelihood that all three tolerances would be below or above the dimensioned slot width, based on a standard deviation. This probability is represented by a normal probability density function, which can be seen in figure 2 below. By combining all the probabilities of the different parts and dimensions in a design, we can determine the probability that a part will have a problem, or fail altogether, based on the dimensions and tolerance of the parts. Generally this method of analysis is only used for assemblies with four or more tolerances.

stacking tolerances
                                                               Figure 2: Tolerance Stacking: Normal distribution

Before starting a statistical tolerance analysis, you must calculate or choose a tolerance distribution factor. The standard distribution is 3 . This means that most of the data (or in this case tolerances) will be within 3 standard deviations of the mean. The standard deviations of all the tolerances must be divided by this tolerance distribution factor to normalize them from a distribution of 3  to a distribution of 1 . Once this has been done, the root sum squared can be taken to find the standard deviation of the assembly.

Think of it like a cup of coffee being made with 3 different sized beans. In order to make a delicious cup of joe, you must first grind down all of the beans to the same size so they can be added to the coffee filter. In this case, the beans are the standard deviations, the grinder is the tolerance distribution factor, and the coffee filter is the root sum squared equation. This is necessary because some tolerances may have different distribution factors based on the tightness of the tolerance range.

The statistical analysis method is used if there is a requirement that the slot must be .500” wide with a +/- .003” tolerance, but there is no need for the radii (.125”) and the flat (.250”) to be exact as long as they fit within the slot. In this example, we have 3 bilateral tolerances with their standard deviations already available. Since they are bilateral, the standard deviation from the mean would simply be whatever the + or – tolerance value is. For the outside radii, this would be .001” and for the middle flat region this would be .002”.

For this example, let’s find the standard deviation (σ) of each section using equation 1. In this equation represents the standard deviation.

standard deviation

The standard assumption is that a part tolerance represents a +/- 3  normal distribution. Therefore, the distribution factor will be 3. Using equation 1 on the left section of figure 1, we find that its corrected standard deviation equates to:

tolerance stacking

This is then repeated for the middle and right sections:

standard deviation

After arriving at these standard deviations, we input the results into equation 2 to find the standard deviation of the tolerance zone. Equation 2 is known as the root sum squared equation.

root sum

At this point, it means that 68% of the slots will be within a +/- .0008” tolerance. Multiplying this tolerance by 2 will result in a 95% confidence window, where multiplying it by 3 will result in a 99% confidence window.

68% of the slots will be within +/- .0008”

95% of the slots will be within +/- .0016”

99% of the slots will be within +/- .0024”

These confidence windows are standard for a normal distributed set of data points. A standard normal distribution can be seen in Figure 2 above.

Statistical tolerance analysis should only be used for assemblies with greater than 4 toleranced parts. A lot of factors were unaccounted for in this simple analysis. This example was for 3 bilateral dimensions whose tolerances were representative of their standard deviations from their means. In standard statistical tolerance analysis, other variables come into play such as angles, runout, and parallelism, which require correction factors.

Did You Know that Harvey Performance Company Brands Partner With the Industry’s Premier Cam Software Providers to Deliver Tooling Libraries?

Click Here to Learn More

Use Worst Case Analysis:

Worst case analysis is the practice of adding up all the tolerances of a part to find the total part tolerance. When performing this type of analysis, each tolerance is set to its largest or smallest limit in its respective range. This total tolerance can then be compared to the performance limits of the part to make sure the assembly is designed properly. This is typically used for only 1 dimension (Only 1 plane, therefore no angles involved) and for assemblies with a small number of parts.

Worst case analysis can also be used when choosing the appropriate cutting tool for your job, as the tool’s tolerance can be added to the parts tolerance for a worst case scenario. Once this scenario is identified, the machinist or engineer can make the appropriate adjustments to keep the part within the dimensions specified on the print. It should be noted that the worst case scenario rarely ever occurs in actual production. While these analyses can be expensive for manufacturing, it provides peace of mind to machinists by guaranteeing that all assemblies will function properly. Often this method requires tight tolerances because the total stack up at maximum conditions is the primary feature used in design. Tighter tolerances intensify manufacturing costs due to the increased amount of scraping, production time for inspection, and cost of tooling used on these parts.

Example of worst case scenario in context to Figure 1:

Find the lower specification limit.

For the left corner radius

.125” – .001” = .124”

For the flat section

.250” – .002” = .248”

For the right corner radius

.125” – .001” = .124”

Add all of these together to the lower specification limit:

.124” + .248” + .124” = .496”

Find the upper specification limit:

For the left corner radius

.125” + .001” = .126”

For the flat section

.250” + .002” = .252”

For the right corner radius

.125” + .001” = .126”

Add all of these together to the lower specification limit:

.126” + .252” + .126” = .504”

Subtract the two and divide this answer by two to get the worst case tolerance:

(Upper Limit – Lower Limit)/2 = .004”

Therefore the worst case scenario of this slot is .500” +/- .004”.

Drill / End Mills: Drill Style vs. Mill Style

/0 Comments/in , , , , , , , /by

Drill / End Mills are one of the most versatile tools in a machinist’s arsenal. These tools can perform a number of different operations, freeing space on your carousel and improving cycle times by limiting the need for tool changes. These operations include:

  1. Drilling
  2. V-Grooving
  3. Milling
  4. Spot Drilling
  5. Chamfering

Shop Harvey Tool Dill/End Mills Today – Fully Stocked in Multiple Styles

The ability of the Drill / End Mill to cut along the angled tip as well as the outer diameter gives it the range of operations seen above and makes it an excellent multi-functional tool.

5 unique drill mill operations

Drill Style vs. Mill Style

The main difference between Drill / End Mill styles is the point geometry.  They are defined by how the flutes are designed on the end of the tool, using geometry typically seen on either an end mill or a drill.  While mill style tools follow the features of an end mill or chamfer mill, the drill style geometry uses an S-gash at the tip.  This lends strength to the tip of the tool, while giving it the ability to efficiently and accurately penetrate material axially.  While both styles are capable of OD milling, mill style tools will be better for chamfering operations, while drill style will excel in drilling.  The additional option of the Harvey Tool spiral tipped Drill / End Mill is an unprecedented design in the industry.  This tool combines end geometry taken from our helical flute chamfer cutters with a variable helix on the OD for enhanced performance. Versatility without sacrificing finish and optimal performance is the result.

graphic showcasing the tool face differences between and mill and drill mills
Left to Right: 2 Flute Drill Style End, 2 Flute Mill Style End, 4 Flute Mill Style End

Drill Mills: Tool Offering

Harvey Tool currently offers Drill / End Mills in a variety of styles that can perform in different combinations of machining applications:

Mill Style – 2 Flute

This tool is designed for chamfering, milling, drilling non-ferrous materials, and light duty spotting. Drilling and spotting operations are recommended only for tools with an included angle greater than 60°. This is a general rule for all drill mills with a 60° point. Harvey Tool stocks five different angles of 2 flute mill-style Drill / End Mills, which include 60°, 82°, 90°, 100° and 120°. They are offered with an AlTiN coating on all sizes as well as a TiB2 coating for cutting aluminum with a 60° and 90° angle.

harvey tool 2 flute mill style drill end mill

Mill Style – 4 Flute

4 flute mill-style Drill / End Mills have two flutes that come to center and two flutes that are cut back. This Drill / End Mill is designed for the same operations as the 2 flute style, but has a larger core in addition the higher flute count. The larger core gives the tool more strength and allows it to machine a harder range of materials. The additional flutes create more points of contact when machining, leading to better surface finish. AlTiN coating is offered on all 5 available angles (60°, 82°, 90°, 100°, and 120°) of this tool for great performance in a wide array of ferrous materials.

harvey tool 4 flute mill style drill mill

Drill Style – 2 Flute

This tool is specifically designed for the combination of milling, drilling, spotting and light duty chamfering applications in ferrous and non-ferrous materials. This line is offered with a 90°, 120°, and 140° included angle as well as AlTiN coating.

2 flute drill mills drill style

Helical Tip – 4 Flute

The Helically Tipped Drill / End Mill offers superior performance in chamfering, milling and light duty spotting operations. The spiral tip design allows for exceptional chip evacuation and surface finish. This combined with an OD variable helix design to reduce chatter and harmonics makes this a valuable tool in any machine shop. It is offered in 60°, 90°, and 120° included angles and comes standard with the latest generation AlTiN Nano coating that offers superior hardness and heat resistance.

Slaying Stainless Steel: Machining Guide

/17 Comments/in , , , , /by

Stainless steel can be as common as Aluminum in many shops, especially when manufacturing parts for the aerospace and automotive industries. It is a fairly versatile material with many different alloys and grades which can accommodate a wide variety of applications. However, milling steel can also be immensely difficult. Stainless steels are notorious end mill assassins, so dialing in your speeds and feeds and selecting the proper tool is essential for machining success.

Material Properties

Stainless steels are high-alloy steels with superior corrosion resistance to carbon and low-alloy steels. This is largely due to their high chromium content, with most grades of stainless steel alloys containing at least 10% of the element.

Stainless steel can be broken out into one of five categories: Austenitic, Ferritic, Martensitic, Precipitation Hardened (PH), and Duplex. In each category, there is one basic, general purpose alloy. From there, small changes in composition are made to the base in order to create specific properties for various applications.

For reference, here are the properties of each of these groupings, as well as a few examples of the popular grades and their common uses.

CategoryPropertiesPopular GradesCommon Uses
AusteniticNon-magnetic, outstanding corrosion and heat resistance.304, 316Food processing equipment, gutters, bolts, nuts, and other fasteners.
FerriticMagnetic, lower corrosion and heat resistance than Austenitic.430, 446Automotive parts and kitchen appliances.
MartensiticMagnetic, moderate corrosion resistance – not for severe corrosion.416, 420, 440Knives, firearms, surgical instruments, and hand tools.
Precipitation Hardened (PH)Strongest grade, heat treatable, severe corrosion resistance.17-4 PH, 15-5 PHAerospace components.
DuplexStronger mixture of both Austenitic and Ferritic.244, 2304, 2507Water treatment plants, pressure vessels.

Tool Selection

Choosing the correct tooling for your application is crucial when machining stainless steel. Roughing, finishing, slotting, and high efficiency milling toolpaths can all be optimized for stainless steel by choosing the correct style of end mill.

Traditional Roughing

For traditional roughing, a 4 or 5 flute end mill is recommended. 5 flute end mills will allow for higher feed rates than their 4 flute counterparts, but either style would work well for roughing applications. Below is an excellent example of traditional roughing in 17-4 Stainless Steel.

Slotting

For slotting in stainless steel, chip evacuation is going to be key. For this reason, 4 flute tools are the best choice because the lower flute count allows for more efficient chip evacuation. Tools with chipbreaker geometry also make for effective slotting in stainless steel, as the smaller chips are easier to evacuate from the cut.

helical solutions ball end mill for stainless steels

Finishing

When finishing stainless steel parts, a high flute count and/or high helix is required for the best results. Finishing end mills for stainless steel will have a helix angle over 40 degrees, and a flute count of 5 or more. For more aggressive finishing toolpaths, flute count can range from 7 flutes to as high as 14. Below is a great example of a finishing run in 17-4 Stainless Steel.

High Efficiency Milling

High Efficiency Milling can be a very effective machining technique in stainless steels if the correct tools are selected. Chipbreaker roughers would make an excellent choice, in either 5 or 7 flute styles, while standard 5-7 flute, variable pitch end mills can also perform well in HEM toolpaths.

helical solutions chipbreaker end mill for hem in stainless steel

HEV-5

Helical Solutions offers the HEV-5 end mill, which is an extremely versatile tool for a variety of applications. The HEV-5 excels in finishing and HEM toolpaths, and also performs well above average in slotting and traditional roughing. Available in square, corner radius, and long reach styles, this well-rounded tool is an excellent choice to kickstart your tool crib and optimize it for stainless steel machining.

5 flute hem end mill for stainless steel

Running Parameters

While tool selection is a critical step to more effective machining, dialing in the proper running parameters is equally important. There are many factors that go into determining the running parameters for stainless steel machining, but there are some general guidelines to follow as a starting point.

Generally speaking, when machining stainless steels a SFM of between 100-350 is recommended, with a chip load ranging between .0005” for a 1/8” end mill up to .006” for a 1” end mill. A full breakdown of these general guidelines is available here.

Machining Advisor Pro

Machining Advisor Pro is a cutting edge resource designed to precisely calculate running parameters for high performance Helical Solutions end mills in materials like stainless steel, aluminum, and much more. Simply input your tool, your exact material grade, and machine setup and Machining Advisor Pro will generate fully customizable running parameters. This free resource allows you to push your tools harder, faster, and smarter to truly dominate the competition.

Dial In Your Stainless Steel Machining Application With Helical Solutions’ Machining Advisor Pro

In Conclusion

Stainless steel machining doesn’t have to be hard. By identifying the proper material grade for each part, selecting the perfect cutting tool, and optimizing running parameters, headaches from milling steel can become a thing of the past.

Harvey Tool: Behind the Scenes

/0 Comments/in , /by

Many of our end users have had great questions about our manufacturing process, how we keep all of our tools in stock, and more. Now for the first time, we decided to open our doors and show you how we manufacture and fulfill the Harvey Tool product. We partnered with John Saunders from NYC CNC to create a “Factory Tour” video, covering topics like our CNC grinding machines and setups, tool manufacturing, and our warehouse organization and fulfillment procedures.

In the video below, we first toured our Rowley, MA warehouse and fulfillment center with Fulfillment Manager Megan Townsley. After that, we head up to Maine to check out how the Harvey Tool product is manufactured and inspected with VP of Operations Brian McKahan.

7 Facts Revealed in Our Factory Tour (Plus 3 More That Didn’t Make the Cut)

We know you’re busy making amazing parts, and might not have time for the entire video. To save you time, here are some of the highlights and facts you should know about Harvey Tool.

When We Say Miniature, We Mean Miniature

Our miniature end mills are in stock in diameters down to .001″. In fact, our Stub and Standard end mills cover every diameter from .001″ to .120″, meaning we will always have you covered when it comes to micro-machining. Although it is hard to see with the naked eye, you can get an up-close look at the famed .001″ end mill by jumping to the 35 minute mark in the tour video.

Micro-Tools Require Precision Grinding

We utilize advanced CNC grinding technology to manufacture our miniature tools at our plant in Maine. Brian MacKahan, VP of Operations, does an excellent job of breaking down our manufacturing process beginning at the 21 minute mark of the tour video. If you just want to see some miniature CNC grinding in action, jump ahead to the 26 minute mark.

Our Inspection Process is Rigourous

All of our tools are sent through an extensive inspection process, both at our plant in Maine and at our headquarters in Massachusetts. To check out the Massachusetts inspection room, head to the 19 minute mark of the video. If you want to see some more in-depth inspection at our facility in Maine, you can jump to the 35 minute mark.

Yes, We Have It In Stock

If you need it, we have it. All 20,000+ tools from our catalog are kept stocked and ready to ship to you the same day. If you need more proof, jump to 15:30 in the tour video, where you will see John Saunders choose a randomly selected Undercutting End Mill from our catalog and find it in our warehouse, in stock and ready to head out to a shop.

We Maintain a 99.8% Order Accuracy Rate

Our fulfillment team handles all of your orders with precision and accuracy. We maintain a 99.8% order accuracy rate, with fulfillment team members checking every order multiple times to ensure you receive exactly what you need. You can learn more about our order fulfillment process and accuracy rates by moving to the 5 minute mark in the video.

We Sell More Than Miniature

Miniature end mills have always been our bread and butter, but did you know that we have many larger diameter tools in stock as well? At the 9 minute mark in the video, you can see John pull out a 3/4″ Long Reach Ball Nose End Mill from our shelves. If you are interested in larger diameter specialty tooling, jump to 12:15 in the video to check out one of our large diameter Corner Rounding End Mills.

When You Call, You’ll Always Talk to An Experienced Tech Expert

Though we didn’t catch it on tape, John Saunders was blown away by our tech team during his visit. He got a chance to pick their brains about a problem he was having and a few minutes later, he received a recommendation for the right compression cutter to tackle his unique operation. This tool was later showcased in one of his “Widget Wednesday” videos.

When you choose Harvey Tool, you will never get an automated system or countless steps before you are able to talk to a real person about your applications. Our industry-leading technical support team is available over the phones or via email every Monday-Friday from 8 AM EST to 7 PM EST. You can reach them by calling 800-645-5609, or by sending an email to [email protected].

We Value Our Distributor Network

We value our large distributor network, and we ask that all orders are placed with your local dealer. To find the closest distributor to you, use the “Find a Distributor” tool on our website.

We’re Hiring!

We are currently hiring for many different positions, including open CNC Machinists positions for all shifts at our manufacturing plant. If you want to be a part of the Harvey Performance Company team, check out our Opportunities page for more information.

Helical Solutions: Behind the Scenes

/0 Comments/in , , /by

We have shown our end users bits and pieces of our manufacturing process on our website and via social media, but for the first time we decided to open our own doors to the public and show you every step behind how we manufacture and fulfill the Helical Solutions product. We partnered with John Saunders from NYC CNC to create a “Factory Tour” video, covering topics like our CNC grinding machines and setups, tool manufacturing, and our warehouse organization and fulfillment procedures.

In the video below, we first toured our Gorham, Maine manufacturing plan with Plant Manager Adam Martin. Then, we ran a few tests with the Helical tools on our Haas machine, before heading back to our warehouse in Massachusetts to talk about fulfillment and new products with Fulfillment Manager Megan Townsley.

7 Facts Revealed in Our Factory Tour (Plus 3 More That Didn’t Make the Cut)

We know you’re busy making amazing parts, and might not have time for the entire video. To save you time, here are some of the most important facts you should know about Helical.

We Take Quality Control Seriously

Our high performance end mills go through an extensive inspection and quality assurance process before they end up in your machine, with multiple inspection points along the manufacturing journey. At the 17 minute mark of the video, you can learn more about how we monitor the quality of the tools in batches as they are manufactured. If you skip ahead to the 29 minute mark, you can see some of our more advanced inspection machines in action.

We Stand Behind Our Tools with Our Renewal Services

Our Tool Renewal service is a great way to maximize your cost-savings and avoid having to re-purchase new tools without sacrificing any aspects of the original design. At Helical, we do not re-sharpen tools. Rather, we restore your tools to their original geometry. We will review the condition of your used tools and return the cutting edge to its original sharpness and strength, allowing the tool to retain its outstanding performance. The renewed tools go through the same rigorous inspection, edge prep, and coating process that we follow for all our of our new tools. To learn more about our Tool Renewal services, head to the 23:30 mark in the video.

Our Tool Coating Is Done In-House

We have multiple tool coating machines in-house which allow us to take the ground tools right off the line and transfer them to our coating room to have Aplus, Zplus, or Tplus coatings added. These machines also have the capability to create roughly 20 different coatings, which are reserved for specials and custom orders. If you want a close-up look at the coating room and learn how the PVD coating process actually works, head to the 35 minute mark.

Our Standard Catalog Items Are Stocked and Ready for Your Machine

We don’t make our standard catalog tools to order. All of our standard tools are stocked and ready to make some chips in your machine. We also introduce hundreds of new tools to our annual catalog to keep providing our customers with the latest in high performance tooling technology. You can check out our new tools for 2018, including our new High Balance Tools and Metric Tooling, by heading to 52:20, or take quick look at our rows of stocked tools in our warehouse by jumping to 56:55.

Diamond Wheels Grind Carbide Tools

Diamond grinding wheels are the essential tool (outside of the machine) when it comes to grinding carbide. We have a unique management system for our diamond wheels, and a redressing process which can see these wheels last up to a year or more before they need replacement. Adam goes through our “frozen wheel” room with John at the 32:45 mark in the video above.

We Track Every Batch of Tools With Laser Etching

Our tools are all laser etched on-site with our logo, phone number, and tool description, but also with a specific batch number. These batch numbers allow us full track-ability of every tool so we can quickly asses any questions or concerns a customer may have about a tool. With these numbers, we are able to track the tool’s journey all the way back to which machine it was made on, which grinding wheel was used, and who ran the program. We have a couple of these laser etching machines in Maine, which you can see in action at the 42 minute mark.

If You Can Dream It, We Have Probably Made It

We have had some crazy tool drawings come in to our custom tool program over the years, including oddly shaped form tools, tools with a crazy long length of cut, “paper cutters”, and more. You can see some cool examples of custom tools we have manufactured by jumping to the 20 minute mark. If you are more interested in how we actually make them, head to the 27 minute mark to see one of our large custom tools being ground on our Walter machines.

Our Technical Resources Are Second To None

We don’t leave you hanging after your purchase of Helical tools. We have a multitude of technical resources and How-Tos available here on our blog, and we also offer the HEM Guidebook, a complete guide to High Efficiency Milling techniques.

If you are looking for information on speeds and feeds, we suggest you try our Machining Advisor Pro application. This application is designed to increase metal removal rates and shop productivity by generating customizable running parameters optimized for your Helical Solutions end mills. You can click here to get started with Machining Advisor Pro today.

You Will Always Get a Real Person When You Call Helical

If you have technical questions about an upcoming job, a special application, or tooling selection, you can contact Helical by phone at 866-543-5422. Our technical experts are available over the phone Monday-Friday from 8 AM to 5 PM EST, and you will always get a real person to talk to with no automated systems to navigate through. You can also reach our team by email at [email protected].

Questions about where to buy Helical tools? You can give our team a call, or you can find your local distributor by using the “Find a Distributor” tool on our website. Simply choose your state to see a complete list of authorized distributors in your area.

We’re Hiring!

We have a current list of our open opportunities on our website! Open jobs include CNC Machinist, Quality Control Inspector, and Customer Service Representative.

Harvey Tool Fall 2018 Catalog Contest

/0 Comments/in /by

Show Us How You #MachineTheImpossible with Harvey Tools!

Has Harvey Tool helped you #MachineTheImpossible? If so, snap a picture of your finished part, the Harvey Tool used, and tell us your story for a chance to be featured on the cover of our Fall 2018 catalog!

Did Harvey Tool help you get through a tough application? Did a miniature end mill help you machine an intricate feature? Did you use a variety of tools to make one impressive part? Have you had to substitute a tool unexpectedly? We’d like to see! Show us how you #MachineTheImpossible.

How to Participate

Using #MachineTheImpossible and @harveytool, tag your photo of the finished part and the Harvey Tool end mill(s) used to machine it. Remember, don’t share anything that could get you in trouble! Proprietary parts and trade secrets should not be on display.

Official Contest Rules

Contest Dates:

  • The contest will run between June 1, 2018 and June 15, 2018. Submit as many entries as you’d like! Entries that are submitted before or after the contest period will not be considered for a feature on the catalog cover. (But we’d still like to see them!)

The Important Stuff:

  1. Take a photo of your finished part and the Harvey Tool end mill(s) used to machine it.
  2. Share your photo on social media using #MachineTheImpossible and tagging @HarveyTool.
  3. Detail the story behind the project (tool number (s), operation, running parameters, etc.)

Catalog Cover Feature

All submissions will be considered for a featured spot on our Fall 2018 catalog cover. Of these entries, the most impressive will be put up to popular vote.

We’ll pick our favorites, but the final say is up to you. Stay tuned for details on when official voting will open to the public!

Need More Incentive?

The Top 10 selected winners will also receive a Harvey Tool Prize Pack and be entered into consideration to appear as a “Featured Customer” on our blog!

The Fine Print:

  • Please ensure that you have permission from both your employer and customer to post a finished part.
  • All entries must be the original work of the person identified in the entry.
  • No purchase necessary to enter or win. A purchase will not increase your chances of winning.
  • On June 25, 2018 the top 10 winners will be announced to the public. The Top 10 selected winners will receive a prize. The odds of being selected depend on the number of entries received. If a potential winner cannot be contacted within five (5) days after the date of first attempt, an alternative winner may be selected.
  • The potential winners will be notified via social media. Each potential winner must complete a release form granting Harvey Tool full permission to publish the winner’s submitted photo. If a potential winner cannot be contacted, or fails to submit the release form, the potential winner forfeits prize. Potential winners must continue to comply with all terms and conditions of these official contest rules, and winning is contingent upon fulfilling all requirements.
  • Participation in the contest constitutes entrant’s full and unconditional agreement to and acceptance of these official rules and decisions. Winning a prize is contingent upon being compliant with these official rules and fulfilling all other requirements.
  • No purchase necessary to enter or win. A purchase will not increase your chances of winning.
  • The Harvey Tool Catalog Contest is open to residents in US and Canada who are at least 18 years old at the time of entry.

Ideal Tooling for Machining Composites

/0 Comments/in , , , /by

Composite Materials

A material is classified as a composite if it is made up of at least two unique constituents that when combined yield beneficial physical and mechanical properties for a number of different applications. A binding agent that is the matrix material is filled with either particles or fibers of a second material that act as reinforcements. The combination of strength, weight, and rigidity make composites extremely useful for the automotive, aerospace, and power generation industry. Often the matrix material of particulate-reinforced composites is some form of plastic, and the reinforcement material is either glass or carbon particles. These are sometimes called “filled plastics,” and are typically very abrasive materials. Many composites are layered with varying fiber orientations, which increase the strength of the material and are called fiber-reinforced composites.

Common Problems When Machining Composites

  1. Delamination of composite layers
  2. Uncut Fibers
  3. Fiber tear-out
  4. Uneven tool wear
  5. Poor surface finish due to “competing” materials

These problems are all caused by unique conditions created by composite materials, and can be very tricky to correct.  The simple fact of cutting a combination of multiple materials at the same time introduces many factors that make it difficult to strike the right balance of the proper tool for the job and appropriate running parameters.  The following tool styles provide solutions for a wide array of composite concerns.  Composite Drilling Applications can face the same issues, and proper drill choice can help as well.

Straight Flute End Mill

Straight Flute Composite Cutters are designed to prevent delamination of layered materials by applying all cutting forces radially, eliminating axial forces from a typical helical cutting edge. Cutting action is improved with a high positive rake angle for shearing fibers and eccentric relief for improved edge life. Shallow ramping operations can be performed with this tool, but the largest benefits are seen in peripheral milling applications.

straight flute end mill

Compression Cutters

The Compression Cutter consists of an up cut and down cut helix. The top portion of the length of cut has right-hand cutting teeth with a left-hand spiral. The lower portion of the length of cut has right-hand cutting teeth with a right-hand spiral. This creates opposing cutting forces to stabilize the material removal process when cutting layered composites to prevent delamination, fiber pullout, and burs along the surface. Compression of the top and bottom of the workpiece keeps the layered bonded together.

compression cutter end mill

Chipbreaker Cutter

The Chipbreaker Cutter is ideally suited for roughing and profiling composites with a high percentage of fiber fill. The notch-like chipbreakers shear fibers and shorten chips for improved material evacuation. This specialized geometry is great for keeping chips small and avoiding “nesting” of stringy fibrous chips around the cutter.

chipbreaker for composite materials

Diamond Cut End Mill

Diamond Cut Composite Cutters come in two different geometries: End Mill Style and Drill Mill Style. Although the end mill style tool is center cutting, the drill mill style has a 140° point angle, making it more suitable for plunge cutting. This is great for clearing out pockets in the middle of composite sheets.

diamond cut end mill for composites

End Mills for Composites – Diamond Cut – End Mill Style

diamond cut drill mill for composites

End Mills for Composites – Diamond Cut – Drill Mill Style

Both the end mill and drill mill style share the same downcut geometry on the outside diameter. This diamond cut tool receives its name from the combination of left-hand and right-hand teeth. The tool is predominantly a downcut style – a geometry that allows for these tools to effectively rough and profile high fiber reinforced or filled composites, breaking up chips and shearing through fibers.

Diamond Cut vs. Chipbreaker Style

The diamond cut tools have a higher flute count, which some may intuitively think would lead to a better finish, but this is not the case as this line of tools contains right-hand and left-hand teeth. There is a trade-off between an increased ability to shear fibers and leaving a poorer finish. The chipbreaker style tool, although not as effective as shearing fibers, is ultimately designed for the same purpose but leaves a better finish as all of the flutes are facing the same direction.

Composite Finisher

The Composite Finisher has optimized geometry for finishing in composite. A slow helix and high flute count for more contact points ultimately renders a smooth finish by minimizing fraying of fiber-reinforced and layered materials.

finishing end mill for composites

Coating or No Coating?

Composite materials, especially those with glass or carbon fiber, can be particularly abrasive and have a tendency to wear down the cutting edge of carbide tools. If one is looking to achieve the best tool life and maintain a sharp cutting edge, then choosing an Amorphous Diamond coated tool is the best option. This thin coating improves lubricity and wear resistance over its uncoated counterpart. Using a tool with CVD diamond coating can be very beneficial in extreme cases, when fiber fill percentage is very large. This is a true diamond coating, and offers the best abrasion resistance, but a slightly less sharp cutting edge as it is a thicker coating. PCD diamond tooling offers the best tool life. If it a solid diamond wafer brazed to a carbide shank, and can maintain the sharpest edge of any diamond tooling. However, PCD is limited to straight flutes, and can come at a higher price.

Composite materials are being increasingly utilized in today’s manufacturing world for their impressive strength to weight ratio. This growth has stimulated innovative techniques of cutting composites seen in the tool choices above. Harvey Tool’s variety of geometries helps any machine shop tackle composite cutting applications and will continue to offer groundbreaking solutions to these types of manufacturing problems.

Tips for Machining Gummy Materials

/11 Comments/in , , /by

Machinists face many problems and challenges when manufacturing gummy materials. These types of materials include low carbon steels, stainless steels, nickel alloys, titanium, copper, and metals with high chromium content. Gummy materials have a tendency to produce long, stringy chips, and are prone to creating built-up edge. These common problems can impact surface finish, tool life, and part tolerances.

bag of copper chips from cnc machining

Continuous Chip With a Built-Up Edge

Continuous chips are long, ribbon-like chips that are formed when the tool cuts through a material, separating chips along the shear plane created by the tool’s cutting edge. These chips slide up the tool face at a constant flow to create a long and stringy chip. The high temperatures, pressures, and friction produced when cutting are all factors that lead to the sticky chips that adhere to the cutting edge. When this built up edge becomes large enough, it can break off leaving behind some excess material on the workpiece, or gouge the workpiece leaving a poor surface finish.

Coolant

Using large amounts of coolant can help with temperature control and chip evacuation while machining gummy materials. Temperature is a big driving force behind built-up edge. The higher the temperature gets, the easier and faster a built-up edge can form. Coolant will keep local temperatures lower and can prevent the material from work hardening and galling. Long, stringy chips have the potential to “nest” around the tool and cause tool failure. Coolant will help break these chips into smaller pieces and move them away from the cutting action by flash cooling them, resulting in fracturing of the chip into smaller pieces. Coolant should be applied directly to the contact area of the tool and workpiece to have the maximum effect.

Tool Engagement

Running Parameters

The tool should be constantly fed into the workpiece. Allowing the tool to dwell can cause work hardening and increase the chance of galling and built up edge. A combination of higher feed rates and lower speeds should also be used to keep material removal rates at a reasonable level. An increase in feed rates will raise the temperature less than an increase in speed. This relates to chip thinning and the ability of a tool to cut the material rather than rub against it.

Climb Milling

Climb milling is the preferred method as it directs more heat into the chip than the tool. Using climb milling, the largest chip cross section is created first, allowing the tool to cut through the material much easier. The heat generated from friction when the tool penetrates the workpiece is transferred to the chip rather than the tool because the thickest part of the chip is able to hold more heat than the thinnest.

infographic showcasing the rotation and movement of a cutting tool in climb milling

Initial Workpiece Engagement

Sudden, large changes in force, like when a tool initially engages a workpiece, have a negative impact on tool life. Using an arc-in tool path to initially engage the material allows for increased stability with a gradual increase in cutting forces and heat. A gradual tool entry such as this is always the preferred method over an abrupt straight entry.

Tool Selection

A tool with a sharp and robust cutting edge should be selected to machine gummy materials. Helical has tooling specifically designed for Titanium and Stainless Steel to make your tool selection process easy.

Additionally, choosing a tool with the correct coating for the material you are machining will help to protect the cutting edge and result in a far lower chance of built up edge or galling than an uncoated tool. A tool with a higher flute count can spread tool wear out over multiple cutting edges, extending tool life. Tool wear is not always linear in gummy materials; as soon as a little bit of wear appears, tool failure will happen relatively quickly. Changing the tool at the first sign of wear may be necessary to ensure that parts are not scrapped.

7 flute end mill for gummy materials

Gummy Materials Summarized

Every material machines somewhat differently, but understanding what is happening when the tool cuts the workpiece and how this affects tool life and finish will go a long way to successfully completing any job.  Built-up edge and excess heat can be minimized by selecting the correct tool and coating for the material, and following the tips and techniques mentioned above. Finally, be sure to check your machine’s runout and ensure maximum rigidity prior to beginning your machining operation.