Posts

How to Optimize Results While Machining with Miniature End Mills

 The machining industry generally considers miniature end mills to be any end mill with a diameter under 1/8 of an inch. This is also often the point where tolerances must be held to a tighter window. Because the diameter of a tool is directly related to the strength of a tool, miniature end mills are considerably weaker than their larger counterparts, and therefore, lack of strength must be accounted for when machining with them. If you are using these tools in a repetitive application, then optimization of this process is key.

Key Cutting Differences between Conventional and Miniature End Mills

Runout

Runout during an operation has a much greater effect on miniature tools, as even a very small amount can have a large impact on the tool engagement and cutting forces. Runout causes the cutting forces to increase due to the uneven engagement of the flutes, prompting some flutes to wear faster than others in conventional tools, and breakage in miniature tools. Tool vibration also impacts the tool life, as the intermittent impacts can cause the tool to chip or, in the case of miniature tools, break. It is extremely important to check the runout of a setup before starting an operation. The example below demonstrates how much of a difference .001” of runout is between a .500” diameter tool and a .031” diameter tool.

The runout of an operation should not exceed 2% of the tool diameter. Excess runout will lead to a poor surface finish.

Chip Thickness

The ratio between the chip thickness and the edge radius (the edge prep) is much smaller for miniature tools. This phenomena is sometimes called “the size effect” and often leads to an error in the prediction of cutting forces. When the chip thickness-to-edge radius ratio is smaller, the cutter will be more or less ploughing the material rather than shearing it. This ploughing effect is essentially due to the negative rake angle created by the edge radius when cutting a chip with a small thickness.

If this thickness is less than a certain value (this value depends of the tool being used), the material will squeeze underneath the tool. Once the tool passes and there is no chip formation, part of the plowed material recovers elastically. This elastic recovery causes there to be higher cutting forces and friction due to the increased contact area between the tool and the workpiece. These two factors ultimately lead to a greater amount of tool wear and surface roughness.

Figure 1: (A) Miniature tool operation where the edge radius is greater than the chip thickness (B) Conventional operation where the edge radius is small than the chip thickness

Tool Deflection

Tool deflection has a much greater impact on the formation of chips and accuracy of the operation in miniature operations, when compared to conventional operations. Cutting forces concentrated on the side of the tool cause it to bend in the direction opposite the feed. The magnitude of this deflection depends upon the rigidity of the tool and its distance extended from the spindle. Small diameter tools are inherently less stiff compared to larger diameter tools because they have much less material holding them in place during the operation. In theory, doubling the length sticking out of the holder will result in 8 times more deflection. Doubling the diameter of an end mill it will result in 16 times less deflection. If a miniature cutting tool breaks on the first pass, it is most likely due to the deflection force overcoming the strength of the carbide. Here are some ways you can minimize tool deflection.

Workpiece Homogeny

Workpiece homogeny becomes a questionable factor with decreasing tool diameter. This means that a material may not have uniform properties at an exceptionally small scale due to a number of factors, such as container surfaces, insoluble impurities, grain boundaries, and dislocations. This assumption is generally saved for tools that have a cutter diameter below .020”, as the cutting system needs to be extremely small in order for the homogeny of the microstructure of the material to be called into question.

Surface Finish

Micromachining may result in an increased amount of burrs and surface roughness when compared to conventional machining. In milling, burring increases as feed increases, and decreases as speed increases. During a machining operation, chips are created by the compression and shearing of the workpiece material along the primary shear zone. This shear zone can be seen in Figure 2 below. As stated before, the chip thickness-to-edge radius ratio is much higher in miniature applications. Therefore, plastic and elastic deformation zones are created during cutting and are located adjacent to the primary shear zone (Figure 2a). Consequently, when the cutting edge is close to the border of the workpiece, the elastic zone also reaches this border (Figure 2b). Plastic deformation spreads into this area as the cutting edge advances, and more plastic deformation forms at the border due to the connecting elastic deformation zones (Figure 2c). A permanent burr begins to form when the plastic deformation zones connect (Figure 2d) and are expanded once a chip cracks along the slip line (Figure 2e). When the chips finally break off from the edge of the workpiece, a burr is left behind (Figure 2f).

Tool Path Best Practices for Miniature End Mills

Because of the fragility of miniature tools, the tool path must be programmed in such a way as to avoid a sudden amount of cutting force, as well as permit the distribution of cutting forces along multiple axes. For these reasons, the following practices should be considered when writing a program for a miniature tool path:

Ramping Into a Part

Circular ramping is the best practice for moving down axially into a part, as it evenly distributes cutting forces along the x, y, and z planes. If you have to move into a part radially at a certain depth of cut, consider an arching tool path as this gradually loads cutting forces onto the tool instead of all at once.

Machining in Circular Paths

You should not use the same speeds and feed for a circular path as you would for a linear path. This is because of an effect called compounded angular velocity. Each tooth on a cutting tool has its own angular velocity when it is active in the spindle. When a circular tool path is used, another angular velocity component is added to the system and, therefore, the teeth on the outer portion of tool path are traveling at a substantially different speed than expected. The feed of the tool must be adjusted depending on whether it is an internal or external circular operation. To find out how to adjust your feed, check out this article on running in circles.

Slotting with a Miniature Tool

Do not approach a miniature slot the same way as you would a larger slot. With a miniature slot, you want as many flutes on the tool as possible, as this increases the rigidity of the tool through a larger core. This decreases the possibility of the tool breaking due to deflection. Because there is less room for chips to evacuate with a higher number of flutes, the axial engagement must be decreased. With larger diameter tools you may be stepping down 50% – 100% of the tool diameter. But when using miniatures with a higher flute count, only step down between 5% – 15%, depending on the size of the diameter and risk of deflection. The feed rate should be increased to compensate for the decreased axial engagement. The feed can be increased even high when using a ball nose end mill as chip thinning occurs at these light depths of cut and begins to act like a high feed mill.

Slowing Down Your Feed Around Corners

Corners of a part create an additional amount of cutting forces as more of the tool becomes engaged with the part. For this reason it is beneficial to slow down your feed when machining around corners to gradually introduce the tool to these forces.

Climb Milling vs. Conventional Milling

This is somewhat of a tricky question to answer when it comes to micromachining. Climb milling should be utilized whenever a quality surface finish is called for on the part print. This type of tool path ultimately leads to more predictable/lower cutting forces and therefore higher quality surface finish. In climb milling, the cutter engages the maximum chip thickness at the beginning of the cut, giving it a tendency to push away from the workpiece. This can potentially cause chatter issues if the setup does not have enough rigidity.  In conventional milling, as the cutter rotates back into the cut it pulls itself into the material and increases cutting forces. Conventional milling should be utilized for parts with long thin walls as well as delicate operations.

Combined Roughing and Finishing Operations

These operations should be considered when micromachining tall thin walled parts as in some cases there is not sufficient support for the part for a finishing pass.

Helpful Tips for Achieving Successful Micromachining Operations

Try to minimize runout and deflection as much as possible.This can be achieved by using a shrink-fit or press-fit tool holder. Maximize the amount of shank contact with the collet while minimizing the amount of stick-out during an operation. Double check your print and make sure that you have the largest possible end mill because bigger tools mean less deflection.

  • Choose an appropriate depth of cut so that the chip thickness to edge radius ratio is not too small as this will cause a ploughing effect.
  • If possible, test the hardness of the workpiece before machining to confirm the mechanical properties of the material advertised by the vender. This gives the operator an idea of the quality of the material.
  • Use a coated tool if possible when working in ferrous materials due to the excess amount of heat that is generated when machining these types of metals. Tool coatings can increase tool life between 30%-200% and allows for higher speeds, which is key in micro-machining.
  • Consider using a support material to control the advent of burrs during a micro milling application. The support material is deposited on the workpiece surface to provide auxiliary support force as well as increase the stiffness of the original edge of the workpiece. During the operation, the support material burrs and is plastically deformed rather than the workpiece.
  • Use flood coolant to lower cutting forces and a greater surface finish.
  • Scrutinize the tool path that is to be applied as a few adjustments can go a long way in extending the life of a miniature tool.
  • Double-check tool geometry to make sure it is appropriate for the material you are machining. When available, use variable pitch and variable helix tools as this will reduce harmonics at the exceptionally high RPMs that miniature tools are typically run at.
Figure 3: Variable pitch tool (yellow) vs. a non-variable pitch tool (black)

High Efficiency Milling for Titanium Made Easy With Helical’s New HVTI Cutter

Titanium is a notoriously difficult material to machine, especially in aggressive toolpaths, such as those associated with High Efficiency Milling (HEM). Helical Solutions’ new line of tooling, the HVTI-6 series of end mills, is optimized specifically for this purpose, and proven to provide 20% more tool life than a competitor’s similar tool.

At face level, these new Helical end mills feature corner radius geometry, 6 flutes, and are Aplus coated for optimal tool life and increased cutting performance. But there is much more to these end mills than the typical geometry of standard 6 flute tools. The HVTI-6 was designed with a combination of a unique rake, core, and edge design that give it a leg up over standard 6 flute tools for Titanium while cutting HEM toolpaths. Click here to watch the HVTI-6 in action!

End Mills for Titanium

The design of the HVTI-6 was the result of significant testing by the Harvey Performance Company Innovation and New Product Development teams. These teams spent many months testing tools, doing in-depth analysis on materials and tool geometry, and pushing these tools through dozens of hours in the cut at testing sites across the country.

The new HVTI-6 cutter experienced higher metal removal rates (MRR) and 20% longer tool life while performing HEM in Titanium when compared to a standard 6 flute tool offered by a Helical Solutions competitor. This type of tool life improvement will produce huge cost savings on tooling, as well as shortened cycle times and lower cost per part.

Helical HVTI Titanium

The Harvey Performance Innovation team targeted Titanium grade Ti6Al4V for their testing, which accounts for the vast majority of the Titanium being machined in North America. The test part was designed and programmed to allow for a more defined agility test of the tool, taking the tool into key geometry cutting exercises like tight corners, long straight line cuts, and rapid movement.

Many hours were spent with Lyndex-Nikken, manufacturers of high-quality rotary tables, tool holders, and machining accessories, at their Chicago headquarters. By working with the team at Lyndex-Nikken, the Harvey Performance Company team was able to test under optimal conditions with top-of-the-line tool holders, work holding, and machining centers. Lyndex was also available to provide their expert support on tool holding techniques and were an integral part of the testing process for these tools. Video of the impressive test cuts taken at the Lyndex facility can be seen below.

WATCH THE HVTI IN ACTION

In these tests, the HVTI was able to run HEM toolpaths at 400 SFM and 120 IPM in Ti6Al4V, which served as the baseline for most of the testing.

While the standard 6 flute tools offered by Helical will still perform to high standards in Titanium and other hard materials (steels, exotic metals, cast iron), the HVTI-6 is a specialized, material-specific tool designed specifically for HEM toolpaths in Titanium. Advanced speeds and feeds for these new tools are already available in Machining Advisor Pro, and the complete offering is now available in the Helical CAM tool libraries for easy programming.

To learn more about the HVTI 6 Flute End Mills for Titanium, please visit the Helical Solutions website. To learn more about HEM techniques, download the HEM Guidebook for a complete guide on this advanced toolpath.

Axis CNC Inc. – Featured Customer

Axis CNC Inc was founded in 2012 in Ware, Massachusetts, when Dan and Glenn Larzus, a father and son duo, decided to venture into the manufacturing industry. Axis CNC Inc has provided customers with the highest quality manufacturing, machining, and programming services since they’ve opened. They specialize in manufacturing medical equipment and have a passion for making snowmobile parts.

We sat down with Axis CNC Inc to discuss how they got started and what they have learned over there years in the manufacturing world. Watch our video below to see our full interview.

John Force Racing – Featured Customer

John Force Racing has been dominating the motorsports world for over 30 years, winning 20 championships and hundreds of races in the National Hot Rod Association (NHRA) drag racing series. John Force Racing features both Funny Car and Top Fuel teams, and just recently in 2017 they won both the Funny Car and Top Fuel championships in the same season.

John Force Racing invested in Force American Made to develop and create parts and components that would help drive all the teams to success and safety. The 84,000 square foot shop is located in Brownsburg, Indiana (just outside of Indianapolis) and is the heartbeat of John Force Racing. Thousands of parts are forged by Force American Made and its team of employees every season giving the team a competitive edge that has led to the team’s on-track success.

The Force American Made team has relied on Helical Solutions tooling to get the best performance and quality out of their CNC mills for years. The Harvey Performance Company team was invited out to Indiana to take a tour of Force American Made and spend some time with Tom Warga, Lead Machinist, to talk with him about his experiences with Helical Solutions tooling, his first time trying Machining Advisor Pro, the success they have had using the new Helical tool libraries for Mastercam, and the value their distributor, Dolen Tool, brings to the shop. Check out the video interview below to see the inner-workings of Force American Made and how Helical Solutions tooling has contributed to the success of this motorsports dynasty.

Chipbreakers vs. Knuckle Rougher End Mills

Knuckle Roughers and Chipbreakers are common profiles found on roughing end mills that, while fairly similar in appearance, actually serve different functions. Chipbreakers refer to the notches along the cutting edge of a tool that work to break up chips to prevent common evacuation mishaps. Knuckle Roughers refer to the serrated cutting edge of a tool, which works to enhance cutting action for an overall smoother operation.

Determining the appropriate style of tool is a very important first step to a successful roughing application.

Understanding the Two Styles

Chipbreaker End Mills

To aid chip evacuation, Chipbreaker End Mills feature a notched profile along the cutting edge that break down long chips into smaller, more manageable pieces. These tools are often utilized in aluminum jobs, as long, stringy chips are common with that material.

Each notch is offset flute-to-flute to enhance the surface finish on the part. This works by ensuring that as each flute rotates and impacts a part, following flutes work to clean up any marks or extra material that was left behind by the first pass. This leaves a semi-finished surface on your part.

In addition to improving chip control and reducing cutting resistance, these tools also help in decreasing heat load within the chips. This delays tool wear along the cutting edge and improves cutting performance. Not only are these tools great for hogging out a great deal of material, but they can be utilized in a wide array of jobs – from aluminum to steels. Further, a machinist can take full advantage of the unique benefits this tool possesses by utilizing High Efficiency Milling toolpaths, meant to promote efficiency and boost tool life.

Knuckle Roughers

Knuckle Rougher End Mills have a serrated cutting edge that generates significantly smaller chips than a standard end mill cutting edge. This allows for smoother machining and a more efficient metal removal process, similar to Chipbreaker End Mills. However, the serrations chop the chips down to much finer sizes, which allows more chips into the flutes during the evacuation process without any packing occurring.

Designed for steels, Knuckle Rougher End Mills are built to withstand harder materials and feature a large core. Because of this, these tools are great for roughing out a lot of material. However, due to the profile on the cutting edge, tracks along the wall can sometimes be left on a part. If finish is a concern, be sure to come in with a finishing tool after the roughing operation. Knuckle Roughers have proven the ability to run at higher chip loads, compared to similar end mills, which makes this a highly desired style for roughing. Further, this style of rougher causes a lot of heat and friction within the chips, so it’s important to run flood coolant when running this tool.

Key Differences Between Knuckle Roughers & Chipbreakers

While the two geometries offer similar benefits, it’s important to understand the distinct differences between them. Chipbreakers feature offset notches, which help to leave an acceptable finish on the walls of a part. Simply, the material left on an initial flute pass is removed by subsequent passes. A Knuckle Rougher does not feature this offset geometry, which can leave track marks on your part. Where part finish is of upmost importance, utilize a Knuckle Rougher to first hog out a great deal of steel, and work a final pass with a Finishing End Mill.

A unique benefit of Knuckle Roughers is the grind they possess – a cylindrical grind, compared to a relieved grind of a Chipbreaker End Mill. Because of this, Knuckle Roughers are easier to resharpen. Therefore, instead of buying a new tool, resharpening this profile is often a cheaper alternative.

Using Tool Libraries in Autodesk HSM & Fusion 360

The days of modeling your tools in CAM are coming to an end. Harvey Performance Company has partnered with Autodesk to provide comprehensive Harvey Tool and Helical Solutions tool libraries to Fusion 360 and Autodesk HSM users. Now, users can access 3D models of every Harvey and Helical tool with a quick download and a few simple clicks. Keep reading to learn how to download these libraries, find the tool you are looking for, how to think about speeds and feeds for these libraries, and more.

Downloading Tool Libraries

On the Autodesk HSM Tools page, you will find Harvey Tool and Helical Solutions tool libraries. Clicking either of the previous links will bring you to that brand’s tool libraries. Right now, all of the two brands more than 27,000 tools are supported in the tool libraries.

Once on the page, there will be a download option for both Fusion and HSM. Select which software you are currently using to be prompted with a download for the correct file format.

From there, you will need to import the tool libraries from your Downloads folder into Fusion 360 or HSM. These tool libraries can be imported into your “Local” or “Cloud” libraries in Fusion 360, depending on where you would like them to appear. For HSM, simply import the HSMLIB file you have downloaded as you would any other tool library.

Curt Chan, Autodesk MFG Marketing Manager, takes a deeper dive into the process behind downloading, importing, and using CAM tool libraries to Fusion in the instructional video below.

For HSM users, jump to the 2:45 mark in this video from Autodesk’s Lars Christensen, who explains how to download and import these libraries into Autodesk HSM.


Selecting a Tool

Once you have downloaded and imported your tool libraries, selecting a specific tool or group of tools can be done in several ways.

Searching by Tool Number

To search by tool number, simply enter the tool number into the search bar at the top of your tool library window. For example, if you are looking for Helical Tool EDP 00015, enter “00015” into the search bar and the results will narrow to show only that tool.

Fusion 360 Tool Libraries

In the default display settings for Fusion 360, the tool number is not displayed in the table of results, where you will find the tool name, flute count, cutter diameter, and other important information. If you would like to add the tool number to this list of available data, you can right click on the top menu bar where it says “Name” and select “Product ID” from the drop down menu. This will add the tool number (ex. 00015) to the list of information readily available to you in the table.

Harvey Tool Tool Libraries

Searching by Keyword

To search by a keyword, simply input the keyword into the search bar at the top of the tool library window. For example, if you are looking for metric tooling, you can search “metric” to filter by tools matching that keyword. This is helpful when searching for Specialty Profile tools which are not supported by the current profile filters, like the Harvey Tool Double Angle Shank Cutters seen in the example below.

Fusion 360 Tool Libraries

Searching by Tool Type

To search by tool type, click the “Type” button in the top menu of your tool library window. From there, you will be able to segment the tools by their profile. For example, if you only wanted to see Harvey Tool ball nose end mills, choose “Ball” and your tool results will filter accordingly.

Tool Libraries

As more specialty profiles are added, these filters will allow you to filter by profiles such as chamfer, dovetail, drill, threadmill, and more. However, some specialty profile tools do not currently have a supported tool type. These tools show as “form tools” and are easier to find by searching by tool number or name. For example, there is not currently a profile filter for “Double Angle Shank Cutters” so you will not be able to sort by that profile. Instead, type “Double Angle Shank Cutter” into the search bar (see “Searching by Keyword”) to filter by that tool type.

Searching by Tool Dimensions

To search by tool dimensions, click the “Dimensions” button in the top menu of your tool library window. From there, you will be able to filter tools by your desired dimensions, including cutter diameter, flute count, overall length, radius, and flute length (also known as length of cut). For example, if you wanted to see Helical 3 flute end mills in a 0.5 inch diameter, you would check off the boxes next to “Diameter” and “Flute Count” and enter the values you are looking for. From there, the tool results will filter based on the selections you have made.

Tool Libraries

Using Specialty Profile Tools

Due to the differences in naming conventions between manufacturers, some Harvey Tool/Helical specialty profile tools will not appear exactly as you think in Fusion 360/HSM. However, each tool does contain a description with the exact name of the tool. For example, Harvey Tool Drill/End Mills display in Fusion 360 as Spot Drills, but the description field will call them out as Drill/End Mill tools, as you can see below.

Below is a chart that will help you match up Harvey Tool/Helical tool names with the current Fusion 360 tool names.

Tool Name Fusion 360 Name
Back Chamfer Cutter Dovetail Mill
Chamfer Cutters Chamfer Mill
Corner Rounding End Mill – Unflared Radius Mill
Dovetail Cutter Dovetail Mill
Drill/End Mill Spot Drill
Engraving Cutter/Marking Cutter – Tip Radius Tapered Mill
Engraving Cutter – Tipped Off & Pointed Chamfer Mill
Keyseat Cutter Slot Mill
Runner Cutter Tapered Mill
Undercutting End Mill Lollipop Mill
All Other Specialty Profiles Form Mill

Speeds and Feeds

To ensure the best possible machining results, we have decided not to pre-populate speeds and feeds information into our tool libraries. Instead, we encourage machinists to access the speeds and feeds resources that we offer to dial accurate running parameters based on their material, application, and machine capabilities.

Harvey Tool Speeds & Feeds

To access speeds and feeds information for your Harvey Tool product, head to http://www.harveytool.com/cms/SpeedsFeeds_228.aspx to find speeds and feeds libraries for every tool.

If you are looking for tool specific speeds and feeds information, you will need to access the tool’s “Tech Info” page. You can reach these pages by clicking any of the hyperlinked tool numbers across all of our product tables. From there, simply click “Speeds & Feeds” to access the speeds and feeds PDF for that specific tool.

If you have further questions about speeds and feeds, please reach out to our Technical Support team. They can be reached Monday-Friday from 8 AM to 7 PM EST at 800-645-5609, or by email at [email protected].

Helical Solutions Speeds & Feeds

To access speeds and feeds information for your Helical Solutions end mills, we recommend using our Machining Advisor Pro application. Machining Advisor Pro (MAP) generates specialized machining parameters by pairing the unique geometries of your Helical Solutions end mill with your exact tool path, material, and machine setup. MAP is available free of charge as a web-based desktop app, or as a downloadable application on the App Store for iOS and Google Play.

machining advisor pro

To learn more about Machining Advisor Pro and get started today, visit www.machiningadvisorpro.com. If you have any questions about MAP, please reach out to us at [email protected].

If you have further questions about speeds and feeds, please reach out to our Technical Support team. They can be reached Monday-Friday from 8 AM to 7 PM EST at 866-543-5422, or by email at [email protected].


For additional questions or help using tool libraries, please send an email to [email protected]. If you would like to request a Harvey Performance Company tool library be added to your CAM package, please fill out the form here and let us know! We will be sure to notify you when your CAM package has available tool libraries.

Slaying Stainless Steel: Machining Guide

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, it is also one of the most difficult to machine. 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.

Category Properties Popular Grades Common Uses
Austenitic Non-magnetic, outstanding corrosion and heat resistance. 304, 316 Food processing equipment, gutters, bolts, nuts, and other fasteners.
Ferritic Magnetic, lower corrosion and heat resistance than Austenitic. 430, 446 Automotive parts and kitchen appliances.
Martensitic Magnetic, moderate corrosion resistance – not for severe corrosion. 416, 420, 440 Knives, firearms, surgical instruments, and hand tools.
Precipitation Hardened (PH) Strongest grade, heat treatable, severe corrosion resistance. 17-4 PH, 15-5 PH Aerospace components.
Duplex Stronger mixture of both Austenitic and Ferritic. 244, 2304, 2507 Water 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.

stainless steel machining

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.

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.

stainless steel machining

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.

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, stainless steel machining headaches can be a thing of the past.

8 Ways You’re Killing Your End Mill

1. Running It Too Fast or Too Slow

Determining the right speeds and feeds for your tool and operation can be a complicated process, but understanding the ideal speed (RPM) is necessary before you start running your machine. Running a tool too fast can cause suboptimal chip size or even catastrophic tool failure. Conversely, a low RPM can result in deflection, bad finish, or simply decreased metal removal rates. If you are unsure what the ideal RPM for your job is, contact the tool manufacturer.

2. Feeding It Too Little or Too Much

Another critical aspect of speeds and feeds, the best feed rate for a job varies considerably by tool type and workpiece material. If you run your tool with too slow of a feed rate, you run the risk of recutting chips and accelerating tool wear. If you run your tool with too fast of a feed rate, you can cause tool fracture. This is especially true with miniature tooling.

3. Using Traditional Roughing

high efficiency milling

While traditional roughing is occasionally necessary or optimal, it is generally inferior to High Efficiency Milling (HEM). HEM is a roughing technique that uses a lower Radial Depth of Cut (RDOC) and a higher Axial Depth of Cut (ADOC). This spreads wear evenly across the cutting edge, dissipates heat, and reduces the chance of tool failure. Besides dramatically increasing tool life, HEM can also produce a better finish and higher metal removal rate, making it an all-around efficiency boost for your shop.

4. Using Improper Tool Holding

tool holding

Proper running parameters have less of an impact in suboptimal tool holding situations. A poor machine-to-tool connection can cause tool runout, pullout, and scrapped parts. Generally speaking, the more points of contact a tool holder has with the tool’s shank, the more secure the connection. Hydraulic and shrink fit tool holders offer increased performance over mechanical tightening methods, as do certain shank modifications, like Helical’s ToughGRIP shanks and the Haimer Safe-Lock™.

5. Not Using Variable Helix/Pitch Geometry

variable helix

A feature on a variety of high performance end mills, variable helix, or variable pitch, geometry is a subtle alteration to standard end mill geometry. This geometrical feature ensures that the time intervals between cutting edge contact with the workpiece are varied, rather than simultaneous with each tool rotation. This variation minimizes chatter by reducing harmonics, which increases tool life and produces superior results.

6. Choosing the Wrong Coating

end mill coatings

Despite being marginally more expensive, a tool with a coating optimized for your workpiece material can make all the difference. Many coatings increase lubricity, slowing natural tool wear, while others increase hardness and abrasion resistance. However, not all coatings are suitable to all materials, and the difference is most apparent in ferrous and non-ferrous materials. For example, an Aluminum Titanium Nitride (AlTiN) coating increases hardness and temperature resistance in ferrous materials, but has a high affinity to aluminum, causing workpiece adhesion to the cutting tool. A Titanium Diboride (TiB2) coating, on the other hand, has an extremely low affinity to aluminum, and prevents cutting edge build-up and chip packing, and extends tool life.

7. Using a Long Length of Cut

optimal length of cut

While a long length of cut (LOC) is absolutely necessary for some jobs, especially in finishing operations, it reduces the rigidity and strength of the cutting tool. As a general rule, a tool’s LOC should be only as long as needed to ensure that the tool retains as much of its original substrate as possible. The longer a tool’s LOC the more susceptible to deflection it becomes, in turn decreasing its effective tool life and increasing the chance of fracture.

8. Choosing the Wrong Flute Count

flute count

As simple as it seems, a tool’s flute count has a direct and notable impact on its performance and running parameters. A tool with a low flute count (2 to 3) has larger flute valleys and a smaller core. As with LOC, the less substrate remaining on a cutting tool, the weaker and less rigid it is. A tool with a high flute count (5 or higher) naturally has a larger core. However, high flute counts are not always better. Lower flute counts are typically used in aluminum and non-ferrous materials, partly because the softness of these materials allows more flexibility for increased metal removal rates, but also because of the properties of their chips. Non-ferrous materials usually produce longer, stringier chips and a lower flute count helps reduce chip recutting. Higher flute count tools are usually necessary for harder ferrous materials, both for their increased strength and because chip recutting is less of a concern since these materials often produce much smaller chips.

3 Steps to Shutting Up Tool Chatter

Cutting tools undergo a great deal of force during the machining process, which cause vibrations – also known as chatter or harmonics. Avoiding these vibrations entirely is not possible, though minimizing them is pivotal for machining success. Vibrations become damaging when proper machining steps are not followed. This leads to strong, part-ruining chatter. In these situations, parts have what is known as “chatter marks,” or clear vibration marks along the surface of a part. Tools can experience an increased rate of wear due to excess vibration.

Tool Chatter can be kept at bay by following three simple, yet often overlooked steps:

1. Select the Right Tool for Your Job

It seems elementary, but selecting the best tool for your application can be confusing. With so many different geometric styles for tooling – overall length, length of cut, reach, number of flutes – it can sometimes be difficult to narrow down one specific tool for your job. Oftentimes, machinists opt for general purpose tooling that can perform a variety of operations, overlooking the option that’s optimized for one material and job.

Opting for Material Specific Tooling is helpful, as each material has different needs. For example, steels are machined differently than aluminum materials. Everything from the chip size, to chip evacuation, is different. Variable Helix or Variable Pitch designs help to minimize chatter by reducing harmonics, which are caused by the cutting edge having repeated contact with the workpiece. In order to reduce harmonics, the time intervals between flute contact with the workpiece are varied.

Overall length is another important factor to consider when deciding on a tool for your job. The more overhang, or length the tool hangs from the spindle, the less secure the spindle-to-tool connection is, and the more vibration. Ensuring that your tool is only as long as needed for your operation is important to minimizing chatter and harmonics. If machining deep within a part, opt for reached tooling or an extended reach tool holder to help solidify the connection.

2. Ensure a Secure Connection

When it comes to secure tool holding approaches, both the tool shank and the collet are important. A loose tool, unsurprisingly, has more ability to move, or vibrate, during machining. With this in mind, Helical offers Shank Configurations to help the connection including the ToughGRIP Shank, which replaces a smooth, mirror-like surface with a rougher, coarser one for increased friction. Helical is also a licensee of the HAIMER Safe-Lock™, added grooves on the shank of a tool that work opposite of the spindle rotation, securely fastening the tool in place.

Machinists must also know the different types of collets available to them to identify if a better solution might be necessary. For example, Hydraulic Tool Holders or Shrink Fit Tool Holders promote a stronger connection than a Mechanical Spindle Tightening method.

For more information, see Key Tool Holding Considerations

3. Choose a Chatter Minimizing Strategy

How a tool is run can mean the difference between stellar job results and a ruined part. This includes both the parameters a tool is run at, as well as the direction by which it rotates – either a Conventional Milling or a Climb Milling technique.

Conventional Milling

In this method, the chip width starts from zero and increases gradually, causing more heat to diffuse into the workpiece. This can lead to work hardening, creating more headaches for a machinist.

tool chatter

Climb Milling

Most modern machine shops will use a climb milling technique, or when the chip width starts at its maximum and decreases during the cut. Climb Milling will offer a more consistent cut than traditional methods, and puts less stress on the tool. Think of it like weight lifting – doing the heavy lifting will be easiest at the beginning of your workout. Similarly, a cut in which the thickest chip is removed first helps the tool maintain its strength. Because the chip cutting process is more swift, vibrations are minimized.

decrease tool chatter

For more information, see Climb Milling Vs. Conventional Milling

In Conclusion

Vibrations are unavoidable during the machining process, but minimizing them can mean the difference between successful machining and scrapped parts. Following three simple rules can help to keep your chatter and harmonics under control, including: Selecting the right tool, ensuring a secure machine-tool connection, and using it in a climb milling strategy. Both Harvey Tool and Helical Solutions have tools that can help, including shank modifications and Variable Helix or Variable Pitch end mills.

Speeds and Feeds 101

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.

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.

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.

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.

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.

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.