06.Nov.2012 A Bit About Bits: Why Size Matters
One important consideration when choosing the right bit for a job is bit size. Size matters with router bits because many important properties are directly related to the size of the router bit. Larger bits are more ridged and they can cut faster, but they also require more power, have larger kerfs and have larger minimum corner radiuses. On the opposite side of the spectrum, you can get nice tight corners with a small bit but you can also break them much easier or turn a 1-2 hour job into a 6 hour marathon. The key to success is to understand the best place to use each type of bit so you can play to their strengths and avoid their limitations.
The most obvious bit size variable is diameter. Bit diameter has great implications for almost all aspects of bit performance. Larger diameter bits are more ridged allowing them to withstand greater cutting forces. Being ridged also helps them resist vibrations and deflection and enables more accurate cutting. Deflection is minute flexing the bit undergoes as it is resisted by the material it is cutting. Deflection is usually undetectable in wood working because by the time it gets bad enough to notice or measure, your bit is either in several pieces or other easy to notice problems have surfaced. In metal milling where tolerances are tighter, errors caused by deflection may be measurable.
In addition to larger bits being more ridged, they also have room for larger cutting edges and deeper flutes. These large cutting edges enable the bit to remove more material at a time allowing you to cut faster. This is possible because the chip load capacity of each cutter has increased. Chip load is a key component of the formula used to determine chip load and will be covered in depth when we talk about feeds and speeds. Because of these reasons, we often try to use the largest bit we can in a given situation. Big bits have one weak point though; they limit the minimum inside radius possible.
The minimum inside radius of any design is limited to half the diameter of cutting bit. Outside radiuses have no limitations because they are created by the software guiding the tool. This same principal applies to both 2D features such as pockets and profile cuts as well as 3D forms created with ballnose bits.
The minimum inside radius that can be created by a .5” diameter router bit is .25”. On comparison, a .25” bit can create a .125” radius. Because this smaller radius is often either considered acceptable to leave in corners or easy to minimize with a few layout tricks, .25” bits are frequently used for versatile profile cutting. If you need even more precision, jumping down to a .125” bit will give you a .0625” radius. That’s just 1/16th of an inch and usually more than enough for most wood related applications. One tradeoff is that it is easier to snap bits smaller than .25” in profile cutting applications. In addition the cutting length of the bits get short and the small chip handling capabilities make them a little slow. To counteract this, they are often saved for high precision areas or as part of a secondary process to speed things up. It is also common to order these bits with larger diameter shanks such as .25” increasing their rigidity. In this case, we commonly refer to these bits by their cutting diameter and the shank diameter is listed separately.
As you can see here, the minimum inside radius produced by a cutter can have an impact on the potential resolution of 3d work as well. As long as the bit can reach inside the smallest part of an interior feature and move around freely, it can reproduce it as accurately as the stepover used will allow. It can also radius top edges if desired or leave them crisp depending on the desired effect. External curves are different; they will always have a point of minimum radius where they contact another part of the model of a spoil board. This will create a fillet like feeling in the model that is determined by the minimum radius of the bit. In product design, these transitions and small groves are the most common reasons to employ smaller bits.
If you desire a sharp transition at the end of an external radius, a secondary pass needs to be taken with a regular bit to square off the edge. You can also overcut with your ballnose bit to complete the curve if you are on the perimeter of your part. This technique is good for high accuracy patterns and hard materials because the computer can control the entire surface of the curve or when no other bits reach the bottom of the job.
Resist the urge to overcut with the ballnose bit unless there is a good reason because it tears up spoil boards. A good through cut with a bottom zeroed router bit will leave around .05” or less of spoil board damage regardless of bit size. If you cheat it with a ball nose bit, you need to reach a depth equal to the radius of the bit or greater. In the case of a .25” ballnose bit, this is at least .125” deep. That’s more than double normal overcutting damage and it gets worse with large bits. If you want to over cut with the ball mill, consider adding a sacrificial temporary spoil board so the users after you don’t have to deal with the groves.
Now that we have covered how small diameter bits can increase resolution, let’s talk about speeding up our pocket clearing with large bits. When pocket cutting or clearing large areas of material from above a 3d design, speed is our friend. Since CNC machining is a subtractive process, the amount of material that needs to be removed from around a model may be as much or greater than the actual volume of the final model. We will try to leave as much waste material as possible alone in places like large holes or around the edges of the work piece to reduce cutting time but sometimes this does not work out. If we can’t leave tabs to hold the material in place, the material is too small to be held securely to the table by vacuum pressure or the remaining material will interfere with dust collector or spindle travel, then it has to go.
The amount of new material a bit removes on every clearing pass is called stepover. Stepover can be referred to as either an absolute distance or more commonly as a percentage of the bit diameter. It is easy to keep track of stepover since it simply is how far the centerline of the tool is offset for each pass
This illustration shows two common pocket clearing strategies implemented in a square hole with a 50% stepover. Small stepovers are used for hard materials and large steppovers are used for rapidly clearing large areas in soft materials. The best way to know what works with your material is to test it. As a general rule of thumb, I consider 50% to be maximum cutting capacity for tools. There are times when you can run them with larger stepovers but these are specialty cases and require testing. Usually there is a bigger time savings in getting things done on the first try than trying to push the envelope and running into problems.
If you need to think about running big steppovers, then it’s usually time to switch up to a larger bit. At 50% stepover, a .25” bit will remove .125” of material per pass and a .5” bit will remove double that. By doubling the horizontal material rate, you will significantly reduce cutting times. Larger bits also have larger chip loads so you can feed them slightly harder and save a little more time. They are also stiffer and can usually handle cutting deeper per pass. By increasing the pass depth per cut, machining times often rapidly drop because you also eliminate both time spent positioning the tool and the time spent cutting. While you can often save time by increasing the pass depth of any bit to some extent, this is most effective with larger diameter bits. This is because the maximum recommended chipload per cutter begins to drop anytime you cut deeper than the bit diameter.
Most CAM software allows for large diameter roughing passes to clear out large holes. In addition, advanced software has features like rest machining. Rest machining is particularly valuable in 3D model development because it allows us not only to use large tools for roughing passes but also for finish passes. We then return to high detail areas that need additional finishing with smaller bits to remove the remaining material. This helps us concentrate our focus on the majority of the designs requirements instead of being forced to use a small bit for an entire project or settle for less detail.
This video is an example of the power gained by constraining bits to small working areas where their strengths can best be utilized. To create tight corners in this vacuum forming buck a .125” ballnosed router bit was used to tighten up corner detail. A long shanked .25” ballnose bit was used to finish the most buck where it would have been impossible to use the 1/8” bit. If tight details were demanded at a lower point in the design, a bit extension, or tapered bit would have been used.
Your ability to utilize multiple bits is primarily limited by your CAM program. Easy to learn CAM programs like Cut 3D will get you started with 3d carving in an afternoon and are something every student should know how to use. They are a great place to start learning the ropes and can be integrated with other Vetric programs like VCarve to create decent models quickly. After you become comfortable with the concepts of machining, it’s time to move up to professional 3D CAM software. Most of this software is aimed at the metal machining industry so it tends to be powerful, expensive and a bit hard to pick up. Select the best package you can afford or use whatever is available in your school shop and learn it well. Once you get the hang of your CAM programs, you will be able to push your hardware to its physical limits and unchain your prototyping potential.