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)

Titan Ring Design – Featured Customer

Officially started in 2015, Titan Ring Design is a high quality machine shop that designs rings, as well as mechanical tie clips, art based designs, and freelance custom designs. While working at a machine shop that produced top notch parts for just about every type of field you can imagine, now owner of Titan Ring Design, Trevor Hirschi, noticed that the machining industry is mostly about cranking out a mass quantity of the highest quality parts as quickly as possible. This often resulted in compromised tolerances and part finishes, something Trevor aimed to change. Quality always comes first in his projects.

Whether you are looking for a band for an upcoming wedding, looking to replace or upgrade your current wedding ring, or just want something unique and beautiful, Trevor’s designs are different than anything else. Trevor was able to take the time and answer some questions for us about his business, machining techniques, tooling, and a lot more.

How was Titan Ring Design started?

Titan Ring Designs is a part time, passion/hobby business of mine that I sort of started at the time I was ring shopping for a wedding ring back in 2013. I didn’t like what was available on the market and was inspired by a former Oakley designer to machine my own. I had been introduced to machining in High School at a technical college and had been working as a machinist since graduating in 2007, so I decided to make my own wedding ring. It sort of snowballed into my business in 2015, after finally deciding to make it official with a business license and some sales. Some further work experience in California for McWhinney Designs brought me greater motivation and encouragement to keep going and helped me get to where I am today. I now offer several different CNC Milled [wedding] rings, as well as a mechanical tie clip, some occasional art based designs, and freelance custom design and mill work. I also teach machining full time  at the same tech college I graduated from in my own education and enjoy sharing my knowledge and love for machining with those interested in the career.

What capabilities does your shop have?

Custom Design in CAD/CAM, 3axis CNC Mill work, Small Scale Lathe Work, Tumbling, Finishing, Assembling, 3D Printing/Rapid Prototyping. I cut 6-4 Titanium primarily, but also work with Stainless Steel for fasteners, Aluminum and some Steel for fixtures, and Polycarbonate for prototyping ideas. I teach machining technology full time, so I have access to SolidWorks, MasterCam, Fusion360, and NC Simul. We currently have a Haas OfficeMill 3axis, Levin High Precision Instrument Maker’s Lathe, Prusa i3 MK2S 3D Printer in the shop.

What sets Titan Ring Design apart from the competition?

There are lots of people making interesting rings today, but most are done on lathes. Anyone can make a round part on a lathe. Very few of them make rings on a mill, and I feel that gives the opportunity to be creative and allows you to think outside the box more. I try to stand out in that field by offering something that makes you think about the value of the design process more by interrupting and challenging the norm. I also like to take on work that is outside of jewelry, but still highly design related. Most other ring makers stick with just rings.

What is your favorite part of the job and what other passions do you have?

Making cool stuff! Most machinists only end up making whatever comes through the shop, which can be cool, but most of the time you have no idea what you’re making, just some part for Customer X, Y, or Z. Being a small, design centered business, I get to come up with ideas for what to make next, and most of the time I start out making something that wasn’t ever intended to be marketed, it was simply something I wanted for myself that I found others were interested in too. I discovered machining in high school and fell in love with it when I started making parts for my dirt bikes and truck. I’ve been hooked ever since but I do have other passions. I’ve always had a big interest in LED lighting and flashlights. I’m perpetually working on different ideas for making one of my own, which will happen eventually. I’m also a bit of a health-nut and enjoy being outdoors and spending time with my family.

Who is the most famous contact that you have worked on a project with?

I made a ring for an NFL player once, but I don’t follow football and his name didn’t stick out to me so I’ve forgotten who he was. I also had the privilege of working for McWhinney Designs and made some truly remarkable products in the openable wedding ring niche market. I gained more skill in design, machining, craftsmanship, and engineering while working for Jeff McWhinney. We’re good friends and often work together to help each other when one of us gets stumped on something.

What is the most difficult project you have worked on?

I was commissioned to design from the ground up and machine was a custom set of all-titanium cabinet door handle pulls for a very high end wine cabinet. Each handle was an assembly of 32 pieces, all machined from billet 6-4 Titanium. They required over 400 individual CAM toolpath operations, 35 unique machine setups, and well over 300 hours to complete, including finishing and assembly. More than anything, it was extremely time intensive in programming, set up, and machine time. The design was a fair bit challenging in my mind and initial modeling, but didn’t compete with what it took to actually produce them. I grossly underestimated and underbid the job. But in the end, I really enjoyed making a truly one of a kind, Tour-De-Force product, even if it was completely overkill for its purpose. I enjoy making that kind of stuff, and the lessons you learn from it.

What is your favorite project you have worked on?

It’s really simple and was initially designed just because I wanted it for myself, but I have a mechanical titanium tie clip that I really enjoy making. It’s quite unique in that, as far as I know, to this day, it is the only CNC machined mechanical titanium tie clip you’ll find anywhere in the world. It puts a little bling in your formal attire, for those times you have to go full suit and tie.

Why is high quality tool performance important to you?

Because I cut mostly titanium, tools wear out quickly if you don’t have a rigid set up, the right coolant, proper feeds & speeds, and of course, high quality tooling. Harvey Tool makes such a wide variety of micro tooling that works so well in the industry of making small titanium parts, where I like to fit into. I’ve used a fair spread across Harvey’s offering and have always been impressed with performance and the feeds and speeds guides are top notch too. I had an application that required a .0035” internal corner radius which landed me with a .007” end mill. It’s still hard to comprehend tooling in this league. My machine actually recommends only tooling under 1/4” shank size, so I don’t get into Helical’s range too often. But I’ve used Helical 1/2” end mills extensively at other job shops and they are definitely made for eating metal. I was using another tool brand’s key cutters for some undercut hinges and would wear through them much more often than I thought was reasonable. When I finally decided to try Harvey’s key cutters, I was blown away with how much longer they have lasted me. Truly a game changer!

If you could give one piece of advice to a new machinist ready to take the #PlungeIntoMachining, what would it be?

Be creative. Machining is such a rewarding career that has limitless possibilities of what you can achieve. Follow your passion and have fun with it! If you end up in a dead end shop doing something you don’t like, go somewhere else. There are so many shops that need help right now and chances are good that you can find a better shop that suits your style.

Is there anything else you would like to share with the In The Loupe community?

To those machine shops out in industry, do whatever you can to be supportive of your local trade schools that are teaching the upcoming machinist workforce. They really need your support and in turn will bring you the employees you depend on.

Please take the time to check out Titan Ring Designs website or follow them on Instagram @titanringdesigns

New Dublin Ship Fittings – Featured Customer

New Dublin Ship Fittings was established in 2017 by Lucas Gilbert, and is located on the scenic south shore of Nova Scotia, Canada.  Lucas began his career with a formal education in machining and mechanical engineering. In the early 2000’s, Lucas got into the traditional shipbuilding industry made famous in the region he grew up in, Lunenburg County, Nova Scotia. It is then when Lucas identified the need for quality marine hardware and began making fittings in his free time. After some time, Lucas was able to start New Dublin Ship Fittings and pursue his lifelong dream of opening a machine shop and producing custom yacht hardware.

Lucas was our grand prize winner in the #MadeWithMicro100 Video Contest! He received the $1,000 Amazon gift card, a Micro-Quik™ Quick Change System with some tooling, and a chance to be In the Loupe’s Featured Customer for February. Lucas was able to take some time out of his busy schedule to discuss his shop, how he got started in machining, and the unique products he manufactures.

How did you start New Dublin Ship Fittings?

I went to school for machine shop and then mechanical engineering, only to end up working as a boat builder for 15 years. It was during my time as a boat builder that I started making hardware in my free time for projects we were working on. Eventually, that grew into full-time work. Right now, we manufacture custom silicon bronze and stainless fittings only. Eventually, we will move into a bronze hardware product line.

Where did your passion for marine hardware come from?

I’ve always loved metalworking. I grew up playing in my father’s knife shop, so when I got into wooden boats, it was only a matter of time before I started making small bits of hardware. Before hardware, I would play around making woodworking tools such as chisels, hand planes, spokeshaves, etc.

What can be found in your shop?

The shop has a 13”x 30” and 16”x 60” manual lathe, a Bridgeport Milling Machine, Burgmaster Turret Drill Press, Gang Drill, Bandsaw, 30-ton hydraulic press, #2 Hossfeld Bender, GTAW, and GMAW Welding Machines, as well as a full foundry set up with 90 pounds of bronze pour capacity. We generally only work in 655 silicon bronze and 316 stainless steel.

What projects have you worked on that stand out to you?

I’ve been lucky to work on several amazing projects over the years. Two that stand out are a 48’ Motorsailer Ketch built by Tern Boatworks, as well as the 63’ Fusion Schooner Farfarer, built by Covey Island Boatworks. Both boats we built most of the bronze deck hardware for.

I’ve made many interesting fittings over the years. I prefer to work with bronze, so I generally have the most fun working on those. I’m generally the most interested when the part is very
challenging to make and custom work parts are often very challenging. I’m asked to build or machine a component that was originally built in a factory and is difficult to reproduce with limited machinery and tooling, but I enjoy figuring out how to make it work.

Why is high-quality tooling important to you?

When I first started I would buy cheaper tooling to “get by” but the longer I did it, the more I realized that cheaper tooling doesn’t pay off. If you want to do quality work in a timely fashion, you need to invest in good tooling.

What Micro 100 Tools are you currently using?

Currently, we just have the Micro 100 brazed on tooling but we have been trying to move more into inserts so we are going to try out Micro’s indexable tooling line. After receiving the Micro-Quik™ Quick Change System, we are looking forward to trying out more of what (Micro 100) has to offer. This new system should help us reduce tool change time, saving us some money in the long run.

What makes New Dublin Ship Fittings stand out from the competition?

I think the real value I can offer boat builders and owners over a standard job shop is my experience with building boats. I understand how the fitting will be used and can offer suggestions as to how to improve the design.

If you could give one piece of advice to a new machinist what would it be?

The advice I would give to new machinists is to start slow and learn the machines and techniques before you try to make parts quickly. There is a lot of pressure in shops to make parts as fast as possible, but you’ll never be as fast as you can be if you don’t learn the processes properly first. Also, learn to sharpen drill bits well!

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

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 High Feed End Mills 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, High Feed End Mills utilize high radial depths of cut and smaller axial depths of cut.

2. This tool reduces radial cutting forces

The end profile of a High Feed End Mill 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 High Feed 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.

4. They can reduce cycle times

In high RDOC, low ADOC applications, High Feed End Mills 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, High Feed End Mill 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.

Benefits & Drawbacks of High and Low Helix Angles

While many factors impact the outcome of a machining operation, one often overlooked factor is the cutting tool’s helix angle. The Helix angle of a tool is measured by the angle formed between the centerline of the tool and a straight line tangent along the cutting edge.

A higher helix angle, usually 40° or more, will wrap around the tool “faster,” while a “slower” helix angle is usually less than 40°.

When choosing a tool for a machining operation, machinists often consider the material, the tooling dimensions and the flute count. The helix angle must also be considered to contribute to efficient chip evacuation, better part finish, prolonged tool life, and reduced cycle times.

Helix Angles Rule of Thumb

One general rule of thumb is that as the helix angle increases, the length of engagement along the cutting edge will decrease. That said,
there are many benefits and drawbacks to slow and high helix angles that can impact any machining operation.

Slow Helix Tool <40°

Benefits

  • Enhanced Strength – A larger core creates a strong tool that can resist deflection, or the force that will bend a tool under pressure.
  • Reduced Lifting – A slow helix will decrease a part from lifting off of the worktable in settings that are less secure.
  • Larger Chip Evacuation – The slow helix allows the tool to create a large chip, great for hogging out material.

Drawbacks

  • Rough Finish – A slow helix end mill takes a large chip, but can sometimes struggle to evacuate the chip. This inefficiency can result in a sub-par part finish.
  • Slower Feed Rate – The increased radial force of a slow helix end mill requires running the end mill at a slower feed rate.

High Helix Tool >40°

Benefits

  • Lower Radial Force – The tool will run quieter and smoother due to better shearing action, and allow for less deflection and more stability in thin wall applications.
  • Efficient Chip Evacuation – As the helix angle increases, the length of cutting edge engagement will decrease, and the axial force will increase. This lifts chips out and away, resulting in efficient chip evacuation.
  • Improved Part Finish – With lower radial forces, high helix tools are able to cut through material much more easily with a better shearing action, leaving an improved surface finish.

Drawbacks

  • Weaker Cutting Teeth – With a higher helix, the teeth of a tool will be thinner, and therefore thinner.
  • Deflection Risk – The smaller teeth of the high helix tool will increase the risk of deflection, or the force that will bend a tool under pressure. This limits how fast you can push high helix tools.
  • Increased Risk of Tool Failure – If deflection isn’t properly managed, this can result in a poor finish quality and tool failure.

Helix Angle: An Important Decision

In summary, a machinist must consider many factors when choosing tools for each application. Among the material, the finish requirements, and acceptable run times, a machinist must also consider the helix angle of each tool being used. A slow helix end mill will allow for larger chip formation, increased tool strength and reduce lifting forces. However, it may not leave an excellent finish. A high helix end mill will allow for efficient chip evacuation and excellent part finish, but may be subject to increased deflection, which can lead to tool breakage if not properly managed.

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.

Show Us What You #MadeWithMicro100

Are you proud of the parts you #MadeWithMicro100? Show us with a video of the parts you are making, the Micro 100 Tool used, and the story behind how that part came to be, for a chance to win a $1,000 Amazon gift card grand prize!

With the recent addition of the Micro 100 brand to the Harvey Performance Company family, we want to know how you have been utilizing its expansive tooling offering. Has Micro 100’s Micro-Quik™ system helped you save time and money? Do you have a favorite tool that gets the job done for you every time? Has Micro 100 tooling saved you from a jam? We want to know! Send us a video on Instagram and show us what you #MadeWithMicro100!

How to Participate

Using #MadeWithMicro100 and @micro_100, tag your video of the Micro 100 tools machining your parts on Instagram or Facebook. Remember, don’t share anything that could get you in trouble! Proprietary parts and trade secrets should not be on display.

Official Contest Rules

Contest Dates:

  • The contest will run between December 5, 2019 to January 17, 2020. Submit as many entries as you’d like! Entries that are submitted before or after the contest period will not be considered for the top prizes (But we’d still like to see them!)

The Important Stuff:

  1. Take a video of your Micro 100 tool in action, clear and visible.
  2. Share your video on social media using #MadeWithMicro100 and tagging @Micro_100.
  3. Detail the story behind the project (tool number(s), operation, running parameters, etc.)

Prizes

All submissions will be considered for the $1,000 Amazon gift card grand prize. Of these entries, the most impressive (10) will be put up to popular vote. All entries put up to vote will be featured on our new customer testimonial page on our website with their name, social media account, and video displayed for everybody to see.

We’ll pick our favorites, but the final say is up to you. Public voting will begin on January 21, 2020, and a winner will be announced on January 28, 2020.

The top five entries will be sent Micro 100’s Micro-Quik™ tool change system with a few of our quick change tools. The top three entries will be offered a spot as a “Featured Customer” on our “In The Loupe” blog!

The Fine Print:

  • Please ensure that you have permission from both your employer and customer to post a video.
  • All entries must be the original work of the person identified in the entry.
  • No purchase necessary to enter or win. A purchase will not increase your chances of winning.
  • On January 28, 2020, the top 5 winners will be announced to the public. The Top 5 selected winners will receive a prize. The odds of being selected depend on the number of entries received. If a potential winner cannot be contacted within five (5) days after the date of first attempt, an alternative winner may be selected.
  • The potential winners will be notified via social media. Each potential winner must complete a release form granting Micro 100 full permission to publish the winner’s submitted video. If a potential winner cannot be contacted, or fails to submit the release form, the potential winner forfeits prize. Potential winners must continue to comply with all terms and conditions of these official contest rules, and winning is contingent upon fulfilling all requirements.
  • Participation in the contest constitutes entrants’ full and unconditional agreement to and acceptance of these official rules and decisions. Winning a prize is contingent upon being compliant with these official rules and fulfilling all other requirements.
  • The Micro 100 Video Contest is open to residents in US and Canada who are at least 18 years old at the time of entry.

Selecting the Right Chamfer Cutter Tip Geometry

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.

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 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 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.

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.

How Boring Bar Geometries Impact Cutting Operations

Boring is a turning operation that allows a machinist to make a pre-existing hole bigger through multiple iterations of internal boring. It has a number of advantages over traditional drilling methods:

  • The ability to cost-effectively produce a hole outside standard drill sizes
  • The creation of more precise holes, and therefore tighter tolerances
  • A greater finish quality
  • The opportunity to create multiple dimensions within the bore itself

 

Solid carbide boring bars, such as those offered by Micro 100,  have a few standard dimensions that give the tool basic functionality in removing material from an internal bore. These include:

Minimum Bore Diameter (D1): The minimum diameter of a hole for the cutting end of the tool to completely fit inside without making contact at opposing sides

Maximum Bore Depth (L2): Maximum depth that the tool can reach inside a hole without contact from the shank portion

Shank Diameter (D2): Diameter of the portion of the tool in contact with the tool holder

Overall Length (L1): Total length of the tool

Centerline Offset (F): The distance between a tool’s tip and the shank’s centerline axis

Tool Selection

In order to minimize tool deflection and therefore risk of tool failure, it is important to choose a tool with a max bore depth that is only slightly larger than the length it is intended to cut. It is also beneficial to maximize the boring bar and shank diameter as this will increase the rigidity of the tool. This must be balanced with leaving enough room for chips to evacuate. This balance ultimately comes down to the material being bored. A harder material with a lower feed rate and depths of cut may not need as much space for chips to evacuate, but may require a larger and more rigid tool. Conversely, a softer material with more aggressive running parameters will need more room for chip evacuation, but may not require as rigid of a tool.

Geometries

In addition, they have a number of different geometric features in order to adequately handle the three types of forces acting upon the tool during this machining process. During a standard boring operation, the greatest of these forces is tangential, followed by feed (sometimes called axial), and finally radial. Tangential force acts perpendicular to the rake surface and pushes the tool away from the centerline. Feed force does not cause deflection, but pushes back on the tool and acts parallel to the centerline. Radial force pushes the tool towards the center of the bore.

 

Defining the Geometric Features of Boring Bars:

Nose Radius: the roundness of a tool’s cutting point

Side Clearance (Radial Clearance): The angle measuring the tilt of the nose relative to the axis parallel to the centerline of the tool

End Clearance (Axial Clearance): The angle measuring the tilt of the end face relative to the axis running perpendicular to the centerline of the tool

Side Rake Angle: The angle measuring the sideways tilt of the side face of the tool

Back Rake Angle: The angle measuring the degree to which the back face is tilted in relation to the centerline of the workpiece

Side Relief Angle: The angle measuring how far the bottom face is tilted away from the workpiece

End Relief Angle: The angle measuring the tilt of the end face relative to the line running perpendicular to the center axis of the tool

Effects of Geometric Features on Cutting Operations:

Nose Radius: A large nose radius makes more contact with the workpiece, extending the life of the tool and the cutting edge as well as leaving a better finish. However, too large of a radius will lead to chatter as the tool is more exposed to tangential and radial cutting forces.

Another way this feature affects the cutting action is in determining how much of the cutting edge is struck by tangential force. The magnitude of this effect is largely dependent on the feed and depth of cut. Different combinations of depth of cuts and nose angles will result in either shorter or longer lengths of the cutting edge being exposed to the tangential force. The overall effect being the degree of edge wear. If only a small portion of the cutting edge is exposed to a large force it would be worn down faster than if a longer portion of the edge is succumb to the same force. This phenomenon also occurs with the increase and decrease of the end cutting edge angle.

End Cutting Edge Angle: The main purpose of the end cutting angle is for clearance when cutting in the positive Z direction (moving into the hole). This clearance allows the nose radius to be the main point of contact between the tool and the workpiece. Increasing the end cutting edge angle in the positive direction decreases the strength of the tip, but also decreases feed force. This is another situation where balance of tip strength and cutting force reduction must be found. It is also important to note that the angle may need to be changed depending on the type of boring one is performing.

Side Rake Angle: The nose angle is one geometric dimension that determines how much of the cutting edge is hit by tangential force but the side rake angle determines how much that force is redistributed into radial force. A positive rake angle means a lower tangential cutting force as allows for a greater amount of shearing action. However, this angle cannot be too great as it compromises cutting edge integrity by leaving less material for the nose angle and side relief angle.

Back Rake Angle: Sometimes called the top rake angle, the back rake angle for solid carbide boring bars is ground to help control the flow of chips cut on the end portion of the tool. This feature cannot have too sharp of a positive angle as it decreases the tools strength.

Side and End Relief Angles: Like the end cutting edge angle, the main purpose of the side and end relief angles are to provide clearance so that the tools non-cutting portion doesn’t rub against the workpiece. If the angles are too small then there is a risk of abrasion between the tool and the workpiece. This friction leads to increased tool wear, vibration and poor surface finish. The angle measurements will generally be between 0° and 20°.

Boring Bar Geometries Summarized

Boring bars have a few overall dimensions that allow for the boring of a hole without running the tool holder into the workpiece, or breaking the tool instantly upon contact. Solid carbide boring bars have a variety of angles that are combined differently to distribute the 3 types of cutting forces in order to take full advantage of the tool. Maximizing tool performance requires the combination of choosing the right tool along with the appropriate feed rate, depth of cut and RPM. These factors are dependent on the size of the hole, amount of material that needs to be removed, and mechanical properties of the workpiece.