Posts

The Advances of Multiaxis Machining

CNC Machine Growth

As the manufacturing industry has developed, so too have the capabilities of machining centers. CNC Machines are constantly being improved and optimized to better handle the requirements of new applications. Perhaps the most important way these machines have improved over time is in the multiple axes of direction they can move, as well as orientation. For instance, a traditional 3-axis machine allows for movement and cutting in three directions, while a 2.5-axis machine can move in three directions but only cut in two. The possible number of axes for a multiaxis machine varies from 4 to 9, depending on the situation. This is assuming that no additional sub-systems are installed to the setup that would provide additional movement. The configuration of a multiaxis machine is dependent on the customer’s operation and the machine manufacturer.

Multiaxis Machining

With this continuous innovation has come the popularity of multiaxis machines – or CNC machines that can perform more than three axes of movement (greater than just the three linear axes X, Y, and Z). Additional axes usually include three rotary axes, as well as movement abilities of the table holding the part or spindle in place. Machines today can move up to 9 axes of direction.

Multiaxis machines provide several major improvements over CNC machines that only support 3 axes of movement. These benefits include:

  • Increasing part accuracy/consistency by decreasing the number of manual adjustments that need to be made.
  • Reducing the amount of human labor needed as there are fewer manual operations to perform.
  • Improving surface finish as the tool can be moved tangentially across the part surface.
  • Allowing for highly complex parts to be made in a single setup, saving time and cost.

9-Axis Machine Centers

The basic 9-axis naming convention consists of three sets of three axes.

Set One

The first set is the X, Y, and Z linear axes, where the Z axis is in line with the machine’s spindle, and the X and Y axes are parallel to the surface of the table. This is based on a vertical machining center. For a horizontal machining center, the Z axis would be aligned with the spindle.

Set Two

The second set of axes is the A, B, and C rotary axes, which rotate around the X, Y, and Z axes, respectively. These axes allow for the spindle to be oriented at different angles and in different positions, which enables tools to create more features, thereby decreasing the number of tool changes and maximizing efficiency.

Set Three

The third set of axes is the U, V, and W axes, which are secondary linear axes that are parallel to the X, Y, and Z axes, respectively. While these axes are parallel to the X, Y, and Z axes, they are managed by separate commands. The U axis is common in a lathe machine. This axis allows the cutting tool to move perpendicular to the machine’s spindle, enabling the machined diameter to be adjusted during the machining process.

A Growing Industry

In summary, as the manufacturing industry has grown, so too have the abilities of CNC Machines. Today, tooling can move across nine different axes, allowing for the machining of more intricate, precise, and delicate parts. Additionally, this development has worked to improve shop efficiency by minimizing manual labor and creating a more perfect final product.

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.

Multi-Start Thread Reference Guide

A multi-start thread consists of two or more intertwined threads running parallel to one another. Intertwining threads allow the lead distance of a thread to be increased without changing its pitch. A double start thread will have a lead distance double that of a single start thread of the same pitch, a triple start thread will have a lead distance three times longer than a single start thread of the same pitch, and so on.

By maintaining a constant pitch, the depth of the thread, measured from crest to root, will also remain constant. This allows multi-start threads to maintain a shallow thread depth relative to their longer lead distance. Another design advantage of a multi-start thread is that more contact surface is engaged in a single thread rotation. A common example is a cap on a plastic water bottle. The cap will screw on in one quick turn but because a multi start thread was used there are multiple threads fully engaged to securely hold the cap in place.

multi-start thread

Figure 1 displays a triple start thread with each thread represented in a different shade. The left side of the image represents a triple start thread with just one of the three threads completed. This unfinished view shows how each individual thread is milled at a specific lead distance before the part is indexed and the remaining threads are milled. The right side of the image displays the completed triple start thread with the front view showing how the start of each thread is evenly spaced. The starting points of a double start thread begin 180° apart and the starting points of a triple start thread begin 120° apart.

multi-start thread

Figure 2 displays the triangle that can be formed using the relationship between the lead distance and the circumference of a thread. It is this relationship that determines the lead angle of a thread. The lead angle is the helix angle of the thread based on the lead distance. A single start thread has a lead distance equal to its pitch and in turn has a relatively small lead angle. Multi-start threads have a longer lead distance and therefore a larger lead angle. The graphic depicted on the right is a view of the lead triangle if it were to be unwound to better visualize this lead angle. The dashed lines represent the lead angle of a single start thread and double start thread of the same pitch and circumference for comparison. The colors represent each of the three intertwined threads of the triple start thread depicted in Figure 1.

Lead Angle Formula

multi-start thread

The charts below display the information for all common UN/Metric threads as well as the lead and lead angle for double and triple start versions of each thread. The lead angle represented in the chart is a function of a thread’s lead and major diameter as seen in the equation above. It is important to be aware of this lead angle when manufacturing a multi-start thread. The cutting tool used to mill the thread must have a relief angle greater than the lead angle of the thread for clearance purposes. All Harvey Tool Single Form Thread Milling Cutters can mill a single, double, and triple start thread without interference.

Machining a Multi-Start Thread

  1. Use the table or equation to determine the pitch, lead, and lead angle of the multi-start thread.
  2. Use a single form thread mill to helically interpolate the first thread at the correct lead. *The thread mill used must have a relief angle greater than that of the multi-start thread’s lead angle in order to machine the thread.
  3. Index to the next starting location and mill the remaining parallel thread/threads.

Click here for the full chart – starting on Page 2.

multi-start thread