Tag Archive for: RDOC

Successful Slotting With Miniature Cutting Tools

/2 Comments/in , , , , /by

Whether your tool is a 1” diameter powerhouse rougher or a .032” precision end mill, slotting is one of the hardest operations on the tool. During slotting operations, a lot of force and pressure is placed on the entire cutting edge of the tool. This results in slower speeds and feeds and increased tool wear, making it one of the nastier processes even for the best cutting tools.

With miniature tooling (for the purposes of this blog, under 1/8” diameter) the game changes. The way we approach miniature tooling is completely different as it relates to slotting. In these instances, it is vitally important to select the correct tool for these operations. A few of the suggestions may surprise you if you are used to working with larger tooling, but rest assured, these are tried and tested recommendations which will dramatically increase your success rate in miniature slotting applications.

Use as Many Flutes as Possible

When running traditional slotting toolpaths, the biggest concern with the cutting tool is getting the best chip evacuation by using the proper flute count. Traditionally speaking, you want to use the fewest amount of flutes possible. In Aluminum/Non-Ferrous jobs, this is typically no more than 2/3 flutes, and in Steel/Ferrous applications, 4 flutes is recommended. The lower flute count leaves room for the chips to evacuate so you are not re-cutting chips and clogging the flutes on your tool in deep slots.

Achieve Increased Efficiency With Miniature Tooling – Utilize Harvey Tool’s Speeds & Feeds Charts Today

When slotting with miniature tools, the biggest concerns are with tool rigidity, deflection, and core strength. With micro-slotting we are not “slotting”, but rather we are “making a slot”. In traditional slotting, we may drive a ½” tool down 2xD into the part to make a full slot, and the tool can handle it! But this technique simply isn’t possible with a smaller tool.

graphic showing difference between core sizes on 3 flute and 5 flute slotting tools

For example, let’s take a .015” end mill. If we are making a slot that is .015” deep with that tool, we are likely going to take a .001” to .002” axial depth per pass. In this case, chips are no longer your problem since it is not a traditional slotting toolpath. Rigidity and core strength are now key, which means we need to add as many flutes as possible! Even in materials like Aluminum, 4 or 5 flutes will be a much better option at smaller diameters than traditional 2/3 flute tools. By choosing a tool with a higher flute count, some end users have seen their tool life increase upwards of 50 to 100 times over tools with lower flute counts and less rigidity and strength.

Use the Strongest Corner Possible When Slotting

Outside of making sure you have a strong core on your miniature tools while making a slot, you also need to take a hard look at your corner strength. Putting a corner radius on your tooling is a great step and does improve the corner strength of the tool considerably over a square profile tool. However, if we want the strongest tip geometry, using a ball nose end mill should also be considered.

A ball nose end mill will give you the strongest possible tip of the three most common profiles. The end geometry on the ball nose can almost work as a high feed end mill, allowing for faster feed rates on the light axial passes that are required for micro-slotting. The lead angle on the ball nose also allows for axial chip thinning, which will give you better tool life and allow you to decrease your cycle times.

.078" harvey tool ball nose end mill for slotting
A .078″ ball nose end mill was used for this miniature slotting operation

Finding the Right Tool for Miniature Slotting Operations

Precision and accuracy are paramount when it comes to miniature tooling, regardless of whether you are slotting, roughing, or even simply looking to make a hole in a part. With the guidelines above, it is also important to have a variety of tooling options available to cater to your specific slotting needs. Harvey Tool offers 5 flute end mills down to .015” in diameter, which are a great option for a stronger tool with a high flute count for slotting operations.

miniature .010" harvey tool end mill
Harvey Tool offers many miniature end mill options, like the .010″ long reach end mill above.

If you are looking to upgrade your corner strength, Harvey Tool also offers a wide selection of miniature end mills in corner radius and ball nose profiles, with dozens of reach, length of cut, and flute count options. Speeds and feeds information for all of these tools is also available, making your programming of these difficult toolpaths just a little bit easier.

speeds and feeds chart ad

Achieving Slotting Success: Summary

To wrap things up, there are three major items to focus on when it comes to miniature slotting: flute count, corner strength, and the depth of your axial passes.

It is vital to ensure you are using a corner radius or ball nose tool and putting as many flutes as you can on your tool when possible. This keeps the tool rigid and avoids deflection while providing superior core strength.

For your axial passes, take light passes with multiple stepdowns. Working your tool almost as a high feed end mill will make for a successful slotting operation, even at the most minuscule diameters.

5 Things to Know About Helical’s High Feed End Mills

/3 Comments/in , , , , /by

Helical Solutions‘ High Feed End Mills provide many opportunities for machinists, and feature a special end profile to increase machining efficiencies. A High Feed End Mill is a High Efficiency Milling (HEM) style tool with specialized end geometry that utilizes chip thinning, allowing for drastically increased feed rates in certain applications. While standard end mills have square, corner radius, or ball profiles, this Helical tool has a specialized, very specific design that takes advantage of chip thinning, resulting in a tool that can be pushed harder than a traditional end mill.

Below are 5 things that all machinists should know about this exciting Helical Solutions product offering.

1. They excel in applications with light axial depths of cut

A High Feed End Mill is designed to take a large radial depth of cut (65% to 100% of the cutter diameter) with a small axial depth of cut (2.5% to 5% diameter) depending on the application. This makes them perfect for face milling, roughing, slotting, deep pocketing, and 3D milling. Where HEM toolpaths involve light radial depths of cut and heavy axial depths of cut, these utilize high radial depths of cut and smaller axial depths of cut.

2. This tool reduces radial cutting forces

The end profile of this tool is designed to direct cutting forces upward along the axis of the tool and into the spindle. This reduces radial cutting forces which cause deflection, allowing for longer reach tools while reducing chatter and other issues that may otherwise lead to tool failure. The reduction of radial cutting forces makes this tool excellent for use in machines with lower horsepower, and in thin wall machining applications.

3. High Feed End Mills are rigid tools

The design and short length of cut of these end mills work in tandem with the end geometry to produce a tool with a strong core, further limiting deflection and allowing for tools with greater reach lengths.

Push Harder in HEM With Helical Solutions’ High Feed End Mills

4. They can reduce cycle times

In high RDOC, low ADOC applications, these tools can be pushed significantly faster than traditional end mills, saving time and money over the life of the tool.

5. High Feed End Mills are well suited for hard materials

The rigidity and strength of High Feed End Mills make them excellent in challenging to machine materials. Helical’s High Feed End Mills come coated with Tplus coating, which offers high hardness and extended tool life in high temp alloys and ferrous materials up to 45Rc.

In summary, these tools with specialized end geometry that utilizes chip thinning and light axial depths of cut to allow for significantly increased feed rates in face milling, slotting, roughing, deep pocket milling, and 3D milling applications. The end profile of a High Feed End Mill applies cutting forces back up into the spindle, reducing radial forces that lead to deflection in long reach applications. Combining this end geometry with a stubby length of cut results in a tool that is incredibly rigid and well suited for harder, difficult to machine materials.

Selecting the Right Chamfer Cutter Tip Geometry

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

A chamfer cutter, or a chamfer mill, can be found at any machine shop, assembly floor, or hobbyist’s garage. These cutters are simple tools that are used for chamfering or beveling any part in a wide variety of materials. There are many reasons to chamfer a part, ranging from fluid flow and safety, to part aesthetics.

Due to the diversity of needs, tooling manufacturers offer many different angles and sizes of chamfer cutters, and as well as different types of chamfer cutter tip geometries. Harvey Tool, for instance, offers 21 different angles per side, ranging from 15° to 80°, flute counts of 2 to 6, and shank diameters starting at 1/8” up to 1 inch.

After finding a tool with the exact angle they’re looking for, a customer may have to choose a certain chamfer cutter tip that would best suit their operation. Common types of chamfer cutter tips include pointed, flat end, and end cutting. The following three types of chamfer cutter tip styles, offered by Harvey Tool, each serve a unique purpose.

Harvey Tool Chamfer Cutters

Pointed and Flat End Chamfer Cutters

Three Types of Harvey Tool Chamfer Cutters

Type I: Pointed

This style of chamfer cutter is the only Harvey Tool option that comes to a sharp point. The pointed tip allows the cutter to perform in smaller grooves, slots, and holes, relative to the other two types. This style also allows for easier programming and touch-offs, since the point can be easily located. It’s due to its tip that this version of the cutter has the longest length of cut (with the tool coming to a finished point), compared to the flat end of the other types of chamfer cutters. With only a 2 flute option, this is the most straightforward version of a chamfer cutter offered by Harvey Tool.

Type I Chamfer Cutter overview

Type II: Flat End, Non-End Cutting

Type II chamfer cutters are very similar to the type I style, but feature an end that’s ground down to a flat, non-cutting tip. This flat “tip” removes the pointed part of the chamfer, which is the weakest part of the tool. Due to this change in tool geometry, this tool is given an additional measurement for how much longer the tool would be if it came to a point. This measurement is known as “distance to theoretical sharp corner,” which helps with the programming of the tool. The advantage of the flat end of the cutter now allows for multiple flutes to exist on the tapered profile of the chamfer cutter. With more flutes, this chamfer has improved tool life and finish. The flat, non-end cutting tip flat does limit its use in narrow slots, but another advantage is a lower profile angle with better angular velocity at the tip.

Type II Chamfer Cutter overview

Type III: Flat End, End Cutting

Type III chamfer cutters are an improved and more advanced version of the type II style. The type III boasts a flat end tip with 2 flutes meeting at the center, creating a center cutting-capable version of the type II cutter. The center cutting geometry of this cutter makes it possible to cut with its flat tip. This cutting allows the chamfer cutter to lightly cut into the top of a part to the bottom of it, rather than leave material behind when cutting a chamfer. There are many situations where blending of a tapered wall and floor is needed, and this is where these chamfer cutters shine. The tip diameter is also held to a tight tolerance, which significantly helps with programing it.

Type III Chamfer Cutter overview

In conclusion, there could be many suitable cutters for a single job, and there are many questions you must ask prior to picking your ideal tool. Choosing the right angle comes down to making sure that the angle on the chamfer cutter matches the angle on the part. One needs to be cautious of how the angles are called out, as well. Is the angle an “included angle” or “angle per side?” Is the angle called off of the vertical or horizontal? Next, the larger the shank diameter, the stronger the chamfer and the longer the length of cut, but now, interference with walls or fixtures need to be considered. Flute count comes down to material and finish. Softer materials tend to want less flutes for better chip evacuation, while more flutes will help with finish. After addressing each of these considerations, the correct style of chamfer for your job should be abundantly clear.

The Geometries and Purposes of a Slitting Saw

/7 Comments/in , , , , , /by

When a machinist needs to cut material significantly deeper than wide, a Slitting Saw is an ideal choice to get the job done. These are unique due to their composition and rigidity, which allows it to hold up in a variety of both straightforward and tricky to machine materials.

What is a Slitting Saw?

A Slitting Saw is a flat (with or without a dish), circular-shaped tool that has a hole in the middle and teeth on the outer diameter. Used in conjunction with an arbor, this tool is intended for machining purposes that require a large amount of material to be removed within a small diameter, such as slotting or cutoff applications.

Other names include (but are not limited to) Slitting Cutters, Slotting Cutters, Jewelers Saws, and Slitting Knives. Both Jewelers Saws and Slitting Knives are particular types of saws. Jewelers Saws have a high tooth count enabling them to cut tiny, precise features, and Slitting Knives have no teeth at all. On Jewelers Saws, the tooth counts are generally much higher than other types of saws in order to make the cuts as accurate as possible.

Key Terminology

slitting saw terminology chart

Why Use a Slitting Saw?

These saws are designed for cutting into both ferrous and non-ferrous materials, and by utilizing their unique shape and geometries, they can cut thin slot type features on parts more efficiently than any other machining tool. Non-Ferrous slitting saws have fewer teeth, allowing for aggressively deep depths of cut.

harvey tool slitting saw

Common Applications:

  1. Separating Two Pieces of Material
    1. If an application calls for cutting a piece of material, such as a rod, in half, then a slitting saw will work well to cut the pieces apart while increasing efficiency.
  2. Undercutting Applications
    1. Saws can perform undercutting applications if mounted correctly, which can eliminate the need to remount the workpiece completely.
  3. Slotting into Material
    1. Capable of creating thin slots with a significant depth of cut, Slitting Saws can be just the right tool for the job!

When Not to Use a Slitting Saw

While it may look similar to a stainless steel circular saw blade from a hardware store, this tool should never be used with construction tools such as a table or circular saw.  Brittle saw blades will shatter when used on manual machines, and can cause injury when not used on the proper set up.

In Conclusion

Slitting Saws can be beneficial to a wide variety of machining processes, and it is vital to understand their geometries and purpose before attempting to utilize them in the shop. They are a great tool to have in the shop and can assist with getting jobs done as quickly and efficiently as possible.

Get to Know Machining Advisor Pro

/2 Comments/in , , , , /by

Machining Advisor Pro (MAP) is a tool to quickly, seamlessly, and accurately deliver recommended running parameters to machinists using Helical Solutions end mills. This download-free and mobile-friendly application takes into account a user’s machine, tool path, set-up, and material to offer tailored, specific speeds and feed parameters to the tools they are using.

How to Begin With Machining Advisor Pro

This section will provide a detailed breakdown of Machining Advisor Pro, moving along step-by-step throughout the entire process of determining your tailored running parameters.

Register Quickly on Desktop or Mobile

To begin with Machining Advisor Pro, start by accessing its web page on the Harvey Performance Company website, or use the mobile version by downloading the application from the App Store or Google Play.

Whether you are using Machining Advisor Pro from the web or your mobile device, machinists must first create an account. The registration process will only need to be done once before you will be able to log into Machining Advisor Pro on both the mobile and web applications immediately.

machining advisor pro

Simply Activate Your Account

The final step in the registration process is to activate your account. To do this, simply click the activation link in the email that was sent to the email address used when registering. If you do not see the email in your inbox, we recommend checking your spam folders or company email filters. From here, you’re able to begin using MAP.

Using Machining Advisor Pro

A user’s experience will be different depending on whether they’re using the web or mobile application. For instance, after logging in, users on the web application will view a single page that contains the Tool, Material, Operation, Machine, Parameter, and Recommendation sections.

machining advisor pro

On the mobile application, however, the “Input Specs” section is immediately visible. This is a summary of the Tool, Material, Operation, and Machine sections that allow a user to review and access any section. Return to this screen at any point by clicking on the gear icon in the bottom left of the screen.

machining advisor pro

Identify Your Helical Tool

To get started generating your running parameters, specify the Helical Solutions tool that you are using. This can be done by entering the tool number into the “Tool #” input field (highlighted in red below). As you type the tool number, MAP will filter through Helical’s 4,800-plus tools to begin identifying the specific tool you are looking for.

machining advisor pro

Once the tool is selected, the “Tool Details” section will populate the information that is specific to the chosen tool. This information will include the type of tool chosen, its unit of measure, profile, and other key dimensional attributes.

Select the Material You’re Working In

Once your tool information is imported, the material you’re working in will need to be specified. To access this screen on the mobile application, either swipe your screen to the left or click on the “Material” tab seen at the bottom of the screen. You will move from screen to screen across each step in the mobile application by using the same method.

In this section, there are more than 300 specific material grades and conditions available to users. The first dropdown menu will allow you to specify the material you are working in. Then, you can choose the subgroup of that material that is most applicable to your application. In some cases, you will also need to choose a material condition. For example, you can select from “T4” or “T6” condition for 6061 Aluminum.

Machining Advisor Pro provides optimized feeds and speeds that are specific to your application, so it is important that the condition of your material is selected.

Pick an Operation

The next section of MAP allows the user to define their specific operation. In this section, you will define the tool path strategy that will be used in this application. This can be done by either selecting the tool path from the dropdown menu or clicking on “Tool Path Info” for a visual breakdown and more information on each available toolpath.

Tailor Parameters to Your Machine’s Capabilities

The final section on mobile, and the fourth web section, is the machine section. This is where a user can define the attributes of the machine that you are using. This will include the Max RPM, Max IPM, Spindle, Holder, and work holding security. Running Parameters will adjust based on your responses.

Access Machining Advisor Pro Parameters

Once the Tool, Material, Operation, and Machine sections are populated there will be enough information to generate the initial parameters, speed, and feed. To access these on the mobile app, either swipe left when on the machine tab or tap on the “Output” tab on the bottom menu.

Please note that these are only initial values. Machining Advisor Pro gives you the ability to alter the stick out, axial depth of cut, and radial depth of cut to match the specific application. These changes can either be made by entering the exact numeric value, the % of cutter diameter, or by altering the slider bars. You are now able to lock RDOC or ADOC while adjusting the other depth of cut, allowing for more customization when developing parameters.

machining advisor pro

The parameters section also offers a visual representation of the portion of the tool that will be engaged with the materials as well as the Tool Engagement Angle.

MAP’s Recommendations

At this point, you can now review the recommended feeds and speeds that Machining Advisor Pro suggests based on the information you have input. These optimized running parameters can then be further refined by altering the speed and feed percentages.

machining advisor pro recommendation

Machining Advisor Pro recommendations can be saved by clicking on the PDF button that is found in the recommendation section on both the web and mobile platforms. This will automatically generate a PDF of the recommendations, allowing you to print, email, or share with others.

Machining Advisor Pro Summarized

The final section, exclusive to the mobile application, is the “Summary” section. To access this section, first tap on the checkmark icon in the bottom menu. This will open a section that is similar to the “Input Specs” section, which will give you a summary of the total parameter outputs. If anything needs to change, you can easily jump to each output item by tapping on the section you need to adjust.

machining advisor pro mobile

This is also where you would go to reset the application to clear all of the inputs and start a new setup. On the web version, this button is found in the upper right-hand corner and looks like a “refresh” icon on a web browser.

Contact Us

For the mobile application, we have implemented an in-app messaging service. This was done to give the user a tool to easily communicate any question they have about the application from within the app. It allows the user to not only send messages, but to also include screenshots of what they are seeing! This can be accessed by clicking on the “Contact Us” option in the same hamburger menu that the Logout and Help & Tips are found.

Click this link to sign up today!

Optimizing Material Removal Rates

/0 Comments/in , , , /by

 What is the Material Removal Rate?

Material Removal Rate (MRR), otherwise known as Metal Removal Rate, is the measurement for how much material is removed from a part in a given period of time. Every shop aims to create more parts in a shorter period of time, or to maximize money made while also minimizing money spent. One of the first places these machinists turn is to MRR, which encompasses Radial Depth of Cut (RDOC), Axial Depth of Cut (ADOC), and Inches Per Minute (IPM). If you’re aiming to boost your shop’s efficiency, increasing your MRR even minimally can result in big gains.

Click Here to Download the High Efficiency Milling (HEM) Guidebook

Calculating MRR

The calculation for Material Removal Rate is RDOC x ADOC x Feed Rate. As an example, if your RDOC is .500″, your ADOC is .100″ and your Feed Rate is 41.5 inches per minute, you’d calculate MRR the following way:

MRR = .500″ x .100″ x 41.5 in/min = 2.08 cubic inches per minute.

Optimizing Efficiency

A machinists’ depth of cut strategy is directly related to the Material Removal Rate. Using the proper RDOC and ADOC combination can boost MRR rates, shaving minutes off of cycle times and opening the door for greater production. Utilizing the right approach for your tool can also result in prolonged tool life, minimizing the rate of normal tool wear. Combining the ideal feed rate with your ADOC and RDOC to run at your tool’s “sweet spot” can pay immediate and long term dividends for machine shops.

The following chart illustrates how a 1/2″, 5-flute tool will perform in Steel when varying ADOC and RDOC parameters are used. You can see that by varying the ADOC and RDOC, a higher feed rate is achievable, and thus, a higher MRR. In this case, pairing a high ADOC, low RDOC approach with an increased feed rate was most beneficial. This method has become known as High Efficiency Milling.

Axial Depth of CutRadial Depth of CutFeed RateMaterial Removal Rate
 .125″ .200″19.5 IPM .488 in.³/min.
.250″.150″26.2 IPM.983 in.³/min.
.500″.100″41.5 IPM2.08 in.³/min.
.750″.050″89.2 IPM3.35 in.³/min.
1.00″.025″193 IPM4.83 in.³/min.

High Efficiency Milling

High Efficiency Milling (HEM) is a milling technique for roughing that utilizes a lower RDOC and a higher ADOC strategy. This spreads wear evenly across the cutting edge, dissipates heat, and reduces the chance of tool failure. This results in a greater ability to increase your MRR, while maintaining and even prolonging tool life versus traditional machining methods.

High Efficiency Milling Material Removal Rate

Obviously, with higher MRR’s, chip evacuation becomes vitally important as more chips are evacuated in a shorter period of time. Utilizing a tool best suited for the operation – in terms of quality and flute count – will help to alleviate the additional workload. Additionally, a tool coating optimized for your workpiece material can significantly help with chip packing. Further, compressed air or coolant can help to properly remove chips from the tool and workpiece.

In conclusion, optimizing workplace efficiency is vital to sustained success and continued growth in every business. This is especially true in machine shops, as even a very minor adjustment in operating processes can result in a massive boost in company revenue. Proper machining methods will boost MRR, minimize cycle times, prolong tool life, and maximize shop output.

4 Important Keyseat Cutter Considerations

/2 Comments/in , , , /by

Keyseat cutters, also called woodruff cutters, keyway cutters, and T-slot cutters, are a type of cutting tool used frequently by many machinists – some operations are impractical or even impossible without one. If you need one of these tools for your job, it pays to know when and how to pick the right one and how to use it correctly.

Keyseat Cutter Geometry

Selecting and utilizing the right tool is often more complicated than identifying the right diameter and dialing in the speeds and feeds. A keyseat’s strength should be considered carefully, especially in tricky applications and difficult materials.

As with any tool, a longer reach will make this tool more prone to deflection and breakage. A tool with the shortest allowable reach should be used to ensure the strongest tool possible.

A keyseat cutter’s neck diameter greatly affects its performance. A thinner neck allows for a comparatively larger radial depth of cut (RDOC) and more clearance, but makes for a weaker tool. A thicker neck reduces the cutter’s RDOC, but greatly strengthens the tool overall. When clearances allow, a keyseat cutter with a thicker neck and larger cutter diameter should be chosen over one with a thinner neck and smaller cutter diameter (Figure 1).

keyseat cutter geometry

Cutter width has an effect on tool strength as well. The greater a keyseat cutter’s cutter width, the more prone to deflection and breakage it is. This is due to the increased forces on the tool – a greater cutter width equates to an increased length of engagement. You should be particularly careful to use the strongest tool possible and a light RDOC when machining with a keyseat cutter with a thick cutter width.

Harvey Tool Keyseats

Harvey Tool Keyseat Geometries

Radial Depth of Cut

Understanding a keyseat cutter’s radial depth of cut is critical to choosing the correct tool, but understanding how it affects your tool path is necessary for optimal results. While it may be tempting to make a cut using a keyseat cutter’s maximum RDOC, this will result in increased stress on the tool, a worse finish, and potential catastrophic tool failure. It is almost always better to use a lighter depth of cut and make multiple passes (Figure 2).

keyseat cutter RDOC
When in doubt about what RDOC is correct for your tool and application, consider consulting the tool manufacturer’s speeds and feeds. Harvey Tool’s keyseat cutter speeds and feeds take into account your tool dimensions, workpiece material, operation, and more.

Desired Slot Size

Some machinists use keyseat cutters to machine slots greater than their cutter width. This is done with multiple operations so that, for example, a keyseat cutter with a 1/4” cutter width can create a slot that is 3/8” wide. While this is possible and may save on up-front tooling costs, the results are not optimal. Ideally, a keyseat cutter should be used to machine a slot equal to its cutter width as it will result in a faster operation, fewer witness marks, and a better finish (Figure 3).

desired slot size

Staggered Tooth Geometry of a Keyseat Cutter

When more versatility is required from a keyseat cutter, staggered tooth versions should be considered. The front and back reliefs allow the tools to cut not only on the OD, but also on the front and back of the head. When circumstances do not allow for the use of a cutter width equal to the final slot dimensions as stated above, a staggered tooth tool can move axially in the slot to expand its width.

staggered toot
Machining difficult or gummy materials can be tricky, and using a staggered tooth keyseat cutter can help greatly with tool performance. The shear flutes reduce the force needed to cut, as well as leave a superior surface finish by reducing harmonics and chatter.

Having trouble finding the perfect keyseat for your job? Harvey Tool offers over 2,100 keyseat cutter options, with cutter diameters from 1/16” to 1-1/2” and cutter widths from .010” to ½”.

Optimize Roughing With Chipbreaker Tooling

/8 Comments/in , , , , /by

Chipbreaker End Mills feature unique notch profiles, creating a serrated cutting edge. These dividers break otherwise long, stringy chips into small, easily-managed swarf that can be cleanly evacuated from the part. But why is a chipbreaker necessary for some jobs, and not others? How does the geometry of this unique tool impact its proper running parameters? In this post, we’ll answer these questions and others to discover the very real benefits of this unique cutting geometry.

How Chipbreaker Tooling Works

As a tool rotates and its cutting edge impacts a workpiece, material is sheared off from a part, creating chips. When that cutting process is interrupted, as is the case with breaks in the cutting portion of the tool, chips become smaller in length and are thus easier to evacuate. Because the chipbreakers are offset flute-to-flute, a proper, flat surface finish is achieved as each flute cleans up any excess material left behind from previously passed flutes.

Benefits of Chipbreaker Tooling

Machining Efficiency

When chips are removed from the part, they begin to pile in the machine. For extensive operations, where a great deal of material is hogged out, chip accumulation can very rapidly get in the way of the spindle or part. With larger chips, accumulation occurs much faster, leaving machinists to stop their machine regularly to remove the waste. As any machinist knows, a stopped machine equates to lost money.

metal chips in cnc mill form chipbreaking

Prolonged Tool Life

Inefficient chip evacuation can lead to chip recutting, or when the the tool impacts and cuts chips left behind during the machining process. This adds stresses on the tool and accelerates rate of wear on the cutting edge. Chipbreaker tooling creates small chips that are easily evacuated from a part, thus minimizing the risk of recutting.

Accelerated Running Parameters

A Harvey Performance Company Application Engineer recently observed the power of a chipbreaker tool firsthand while visiting a customer’s shop in Minnesota. The customer was roughing a great amount of 4340 Steel. Running at the parameters below, the tool was able to run uninterrupted for two hours!

Helical Part No.33737
Material4340 Steel
ADOC2.545″
RDOC.125″
Speed2,800 RPM
Feed78 IPM
Material Removal Rate24.8 Cubic In/Min

 

Chipbreaker Product Offering

Chipbreaker geometry is well suited for materials that leave a long chip. Materials that produce a powdery chip, such as graphite, should not be machined with a chipbreaker tool, as chip evacuation would not be a concern. Helical Solutions’ line of chipbreaker tooling includes a 3-flute option for aluminum and non-ferrous materials, and its reduced neck counterpart. Additionally, Helical offers a 4-flute rougher with chipbreaker geometry for high-temp alloys and titanium. Harvey Tool’s expansive product offering includes a composite cutting end mill with chipbreaker geometry.

Helical Solutions 7 Flute Chipbreaker

In Summary

Chipbreaker geometry, or grooves within the cutting face of the tool, break down chips into small, manageable pieces during the machining process. This geometry can boost shop efficiency by minimizing machine downtime to clear large chips from the machining center, improve tool life by minimizing cutting forces exerted on the tool during machining, and allow for more accelerated running parameters.

Speeds and Feeds 101

/12 Comments/in , , , , /by

Understanding Speeds and Feed Rates

NOTE: This article covers speeds and feed rates for milling tools, as opposed to turning tools.

Before using a cutting tool, it is necessary to understand tool cutting speeds and feed rates, more often referred to as “speeds and feeds.” Speeds and feeds are the cutting variables used in every milling operation and vary for each tool based on cutter diameter, operation, material, etc. Understanding the right speeds and feeds for your tool and operation before you start machining is critical.

It is first necessary to define each of these factors. Cutting speed, also referred to as surface speed, is the difference in speed between the tool and the workpiece, expressed in units of distance over time known as SFM (surface feet per minute). SFM is based on the various properties of the given material. Speed, referred to as Rotations Per Minute (RPM) is based off of the SFM and the cutting tool’s diameter.

HEM Guidebook Ad

While speeds and feeds are common terms used in the programming of the cutter, the ideal running parameters are also influenced by other variables. The speed of the cutter is used in the calculation of the cutter’s feed rate, measured in Inches Per Minute (IPM). The other part of the equation is the chip load. It is important to note that chip load per tooth and chip load per tool are different:

speeds and feeds formula
  • Chip load per tooth is the appropriate amount of material that one cutting edge of the tool should remove in a single revolution. This is measured in Inches Per Tooth (IPT).
  • Chip load per tool is the appropriate amount of material removed by all cutting edges on a tool in a single revolution. This is measured in Inches Per Revolution (IPR).

A chip load that is too large can pack up chips in the cutter, causing poor chip evacuation and eventual breakage. A chip load that is too small can cause rubbing, chatter, deflection, and a poor overall cutting action.

speeds and feeds formula

Material Removal Rate

Material Removal Rate (MRR), while not part of the cutting tool’s program, is a helpful way to calculate a tool’s efficiency. MRR takes into account two very important running parameters: Axial Depth of Cut (ADOC), or the distance a tool engages a workpiece along its centerline, and Radial Depth of Cut (RDOC), or the distance a tool is stepping over into a workpiece.

The tool’s depth of cuts and the rate at which it is cutting can be used to calculate how many cubic inches per minute (in3/min) are being removed from a workpiece. This equation is extremely useful for comparing cutting tools and examining how cycle times can be improved.

speeds and feeds

Speeds and Feeds In Practice

While many of the cutting parameters are set by the tool and workpiece material, the depths of cut taken also affect the feed rate of the tool. The depths of cuts are dictated by the operation being performed – this is often broken down into slotting, roughing, and finishing, though there are many other more specific types of operations.

Many tooling manufacturers provide useful speeds and feeds charts calculated specifically for their products. For example, Harvey Tool provides the following chart for a 1/8” diameter end mill, tool #50308. A customer can find the SFM for the material on the left, in this case 304 stainless steel. The chip load (per tooth) can be found by intersecting the tool diameter on the top with the material and operations (based on axial and radial depth of cut), highlighted in the image below.

hardness chart

The following table calculates the speeds and feeds for this tool and material for each operation, based on the chart above:

speeds and feeds

Other Important Considerations

Each operation recommends a unique chip load per the depths of cut. This results in various feed rates depending on the operation. Since the SFM is based on the material, it remains constant for each operation.

Earn an Immediate Boost to Shop Efficiency: Download the HEM Guidebook Today

Spindle Speed Cap

As shown above, the cutter speed (RPM) is defined by the SFM (based on material) and the cutter diameter. With miniature tooling and/or certain materials the speed calculation sometimes yields an unrealistic spindle speed. For example, a .047” cutter in 6061 aluminum (SFM 1,000) would return a speed of ~81,000 RPM. Since this speed is only attainable with high speed air spindles, the full SFM of 1,000 may not be achievable. In a case like this, it is recommended that the tool is run at the machine’s max speed (that the machinist is comfortable with) and that the appropriate chip load for the diameter is maintained. This produces optimal parameters based on the machine’s top speed.

Effective Cutter Diameter

On angled tools the cutter diameter changes along the LOC. For example, Helical tool #07001, a flat-ended chamfer cutter with helical flutes, has a tip diameter of .060” and a major/shank diameter of .250”. In a scenario where it was being used to create a 60° edge break, the actual cutting action would happen somewhere between the tip and major/shank diameters. To compensate, the equation below can be used to find the average diameter along the chamfer.

cutter diameter calculation

Using this calculation, the effective cutter diameter is .155”, which would be used for all Speeds and Feeds calculations.

Non-linear Path

Feed rates assume a linear motion. However, there are cases in which the path takes an arc, such as in a pocket corner or a circular interpolation. Just as increasing the DOC increases the angle of engagement on a tool, so does taking a nonlinear path. For an internal corner, more of the tool is engaged and, for an external corner, less is engaged. The feed rate must be appropriately compensated for the added or lessened engagement on the tool.

non-linear path

This adjustment is even more important for circular interpolation. Take, for example, a threading application involving a cutter making a circular motion about a pre-drilled hole or boss. For internal adjustment, the feed rate must be lowered to account for the additional engagement. For external adjustment, the feed rate must be increased due to less tool engagement.

adjusted internal feed

Take this example, in which a Harvey Tool threadmill #70094, with a .370” cutter diameter, is machining a 9/16-18 internal thread in 17-4 stainless steel. The calculated speed is 2,064 RPM and the linear feed is 8.3 IPM. The thread diameter of a 9/16 thread is .562”, which is used for the inner and outer diameter in both adjustments. After plugging these values into the equations below, the adjusted internal feed becomes 2.8 IMP, while the external feed becomes 13.8 IPM.

adjusted external feed

Click here for the full example.

Conclusion

These calculations are useful guidelines for running a cutting tool optimally in various applications and materials. However, the tool manufacturer’s recommended parameters are the best place to start for initial numbers. After that, it is up to the machinist’s eyes, ears, and experience to help determine the best running parameters, which will vary by set-up, tool, machine, and material.

Click the following links for more information about running parameters for Harvey Tool and Helical products.

Why Flute Count Matters

/17 Comments/in , , , , , /by

One of the most important considerations when choosing an end mill is determining which flute count is best for the job at hand. Both material and application play an important role in this critical part of the tool selection process. Understanding the effects of flute count on other tool properties, and how a tool will behave in different situations is an essential consideration in the tool selection process.

Machining Advisor Pro (MAP) Takes Flute Count Into Consideration When Helping You Dial In Running Parameters.

Click Here to Get Started.

Tool Geometry Basics

Generally, tools with more flutes have a larger core and smaller flute valleys than tools with fewer flutes.  More flutes with a larger core can provide both benefits and restrictions depending on the application.  Simply put, a larger core is directly proportional to tool strength; the larger the core, the stronger a tool will be.  In turn, a larger core also reduces the flute depth of a tool, restricting the amount of space for chips to exist.  This can cause issues with chip packing in applications requiring heavy material removal.  However, these considerations only lead us part way when making a decision on which tool to use, and when.

flute count core

Material Considerations

Traditionally, end mills came in either a 2 flute or 4 flute option.  The widely accepted rule of thumb was to use 2 flutes for machining aluminum and non-ferrous materials, and 4 flutes for machining steel and harder alloys.  As aluminum and non-ferrous alloys are typically much softer than steels, a tool’s strength is less of a concern, a tool can be fed faster, and larger material removal rates (MRR) is facilitated by the large flute valleys of 2 flute tools.  Ferrous materials are typically much harder, and require the strength of a larger core.  Feed rates are slower, resulting in smaller chips, and allowing for the smaller flute valleys of a larger core tool.  This also allows for more flutes to fit on the tool, which in turn increases productivity.

end mill flute count

Recently, with more advanced machines and toolpaths, higher flute count tools have become the norm in manufacturing.  Non-ferrous tooling has become largely centered on 3 flute tools, allowing greater productivity while still allowing proper chip evacuation.  Ferrous tooling has taken a step further and progressed not only to 5 and 6 flutes, but up to 7 flutes and more in some cases.  With a wider range of hardness, sometimes at the very top of the Rockwell hardness scale, many more flutes have allowed longer tool life, less tool wear, stronger tools, and less deflection.  All of this results in more specialized tools for more specific materials.  The end result is higher MRR and increased productivity.

Running Parameters

Just as material considerations will have an impact on the tool you choose, operation type and depth of cut requirements may also have a big impact on the ideal number of flutes for your application.  In roughing applications, lower flute counts may be desirable to evacuate large amounts of chips faster with larger flute valleys.  That said, there is a balance to find, as modern toolpaths such as High Efficiency Milling (HEM) can achieve extreme MRR with a very small step over, and a higher number of flutes.  In a more traditional sense, higher flute counts are great for finishing operations where very small amounts of material are being removed, and greater finish can be achieved with more flutes, not worrying as much about chip evacuation.

flute count

Flute count plays a big role in speeds and feeds calculation as well.  One common rule of thumb is “more flutes, more feed,” but this can be a very detrimental misconception.  Although true in some cases, this is not an infinitely scalable principle.  As stated previously, increasing the number of flutes on a tool limits the size that the flute valleys can be.  While adding a 5th flute to a 4 flute tool theoretically gives you 25% more material removal per revolution with an appropriately increased feed rate, feeding the tool that much faster may overload the tool.  The 25% increase in material removal is more likely closer to 10-15%, given the tool is exactly the same in all other specifications.  Higher flute count tools may require speeds and feeds to be backed off so much in some cases, that a lower flute count may be even more efficient.  Finding the right balance is key in modern milling practices.