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.
Let’s talk a bit about bits. I enjoyed writing “5 Things Students Should Know About CNC” and with a new semester quickly approaching, I felt a follow up article about bits was in order. Bits are a deep topic, but over the next several articles we will cover the basics about the different bit types, what they do and why you want them. In addition I will share a few of my favorite basic bits that will serve you well starting out.
One thing I should warn you about up front though is that bit selection is heavily influenced by not only the application but by the machine they are used in. Ridged machines with powerful spindles can handle anything including big bits with aggressive cutting profiles. Moderately ridged machines with spindles are great prototyping and limited production tools; they just use smaller bits or less and are run slower. If you use a machine that is equipped with a router instead of a spindle or is not particularly ridged, then drive gently and be careful with large tools. Things may take a little bit longer but you’ll still get your projects done.
There are several ways you can categorize router bits. For our purposes, let’s first divide them into two categories: bits you can use in CNC routers and bits that you can’t. Any router bit with ball bearing guides or roller pin tips cannot be used in CNC machines. The ball bearings exist to guide stock consistently along the bit when used in hand routers and router tables, but CNC routers have no flexibility to follow the stock. When used in CNC systems, bits go where you tell it to go so the entire bit must be able to cut through anything it encounters.
Some specialty tools exist that only cut in specific areas. Examples of these tools include joining bits, grooving cutters and other similar tools. Most common versions of these cutters cannot be used safely in CNC machines, however some CNC specific versions do exist. They are commonly used in the cabinet and furniture making industries to speed up production but they are not for use in the student prototyping environment. Many of these tools cost several hundred dollars and require professional level skill and more powerful and full featured equipment than we commonly have available.
Please view the following videos to see a few of these tools in action but don’t feel limited or cheated by not preforming these tasks with a CNC mill for your projects. Everything done in both videos can be accomplished as secondary operations using a table router with regular bits and a drilling jig for the side holes created by an aggregate tool head used in the second video.
In a later article we will discuss some of the capabilities of professional grade equipment and the impact that it can have on your designs, but for the moment let’s just focus on creating our own prototypes.
In addition to unusual specialty tools that cannot center cut, some seemingly simple straight bits also lack center cutting ability. Whenever purchasing a router bit for CNC application, be sure that it can center cut or “plunge cut”. This lets you know you can push the bit down into the work piece to start a cut. Any non-center cutting bits have to approach a work piece from the side to begin cutting and may not be able to change cutting depth while inside the work piece.
One final detail that you must take into consideration is how you will hold the bit. Most systems students have access to do not have automatic tool changers so there is no need to worry about tool holders, but you still have to be sure that the shank of your bits match an available collet for your machine. Some machines use highly flexible ER collet systems allowing you to order a wide array of collet sizes, but systems equipped with routers usually have between 3 or 4 available collet sizes based on the most commonly available router bits. If you are using a regular router bit, this is usually never a problem, but if you ever find yourself needing something odd sized like a specialty end mill, this can become an issue. If your machine uses an ER collet system, you will likely be able to order the correct sized collet but quality collets are usually at least $20. If you are going to use handfuls of this bit then this may be the way to go but, most end mills can be ordered with a closely matching standard shank size like .125” and .25” and they only cost slightly more than regular end mills.
Now that we have covered some of the bits that do not work in CNC applications, let’s talk about what we want to use. The bulk CNC work is done using straight plunge cutting bits. These come in two main classes, straight flute and spiral flute. These basic bits can be broken down even further by the cutting edge material, number of flutes, length and diameter. Spiral bits also have one additional property, because their cutting edges act like a screw they create upward or downward directional forces. Up cut bits pull material up towards the router and away from the cutting surface resulting in better chip extraction but this same action can cause tearing around the top of the surfaces of the hole. In addition up cut bits can exert a surprising amount of pull on a part. This pull can become a problem in thin materials or in some vacuum work holding situations. Downcut bits force the work piece down. This results in cleaner edges around the top edges of the hole but this also directs chips into the cut. Because chips are pulled back towards the cutting area, downcut bits must be run slower than upcut bits to allow time for the chips to be removed and to prevent overloading the cutter. A third class of spiral bits also exists called compression bits. Compression bits are used for composite materials like plywood and some laminates. They are comprised of both upcut and downcut sections which pull material into itself to help reduce chipping.
Straight Flute Router Bits
Spiral Flute Router Bits
For further clarification take a look at these articles discussing the basics of spiral bits. While they are primarily directed at traditional woodworking applications the basics still apply to CNC machining.
Besides the common straight cutting profiles, a few other useful bits are also commonly used. Ball nosed bits are used to create rounded edges and to smooth out 3d forms and angled bits are used to create smooth mitered angles and champers. In addition to creating miter joints, angle bits are used to enable a powerful finished technique called miter folding to create tight seamless angles and in a simple method of adding fast 3D details often used by the signage industry called V Carving.
Ball Nose Router Bits
One final bit exists that can have the greatest impact on the accuracy of your project. They are called spoilbord cutters or spoilbord surfacers and while they almost never touch your project they are essential to accurate work. Spoilbord surfacers are used to plain down the spoil board. This is done to ensure that the spoilboard is parallel to the x and y axis across the entire table. It is also done periodically during the life of the spoil board to remove groves left by through cuts. With vacuum systems this is essential because these groves cause a loss of holding power but they can also cause accuracy problems with other hold down systems as well, especially when they build up in heavily used sections of the table. Spoilboard surfacers are also used to remove the hard coating from the surfaces of MDF when used in vacuum table applications because it blocks the flow of air through the material.
Spoilbord surfacers come in a variety of sizes and two main styles. The most common and efficient has replaceable knives, however some versions are constructed like traditional router bits.
Most Spoilboard cutters are expensive so don’t run out to buy your own personal cutter. Instead talk with your shop manager or technicians if you recognize problems in the spoil board and see if they can handle this for you. You only want to consider surfacing your OWN spoilboards which you KNOW are hardware free. In school shops, a lot of people still use screws for work holding and they frequently crack off leaving remnants in the spoil board. If they have not been removed or are broken off below the surface of the table, you will likely not know until you hit it with the spoilboard cutter which is both dangerous and will destroy or at the very least damage a very expensive bit. I am making this safety point very clear because when I was in school, we all used steel drywall screws for work holding and we had plenty break. I know that hitting a screw with a .25″ router bit is enough to be dangerous in the right conditions so I don’t want to imagine what hitting one with a 2 inch surfacer is like. I assume though that it will potentialy be far worse since the outside of large bits travel at much higher speeds and the bits themselves contain much more mass.
5 Rules Every Design Student Should Know About CNC Prototyping
1. CNC integrated manufacturing does not exist to eliminate the need for technical skills.
It can produce designs with greater accuracy and repeatability than we are capable of, but it is still just a tool that enables accurate production. Just because a CNC router comes with a price tag of $15,000+ and is hooked to a computer that moves the tool for you does not make it capable of magic. In the end thoughtful selection of tools, materials and planning has almost the same impact on output quality as they do with hand tools.
2. There is nothing rapid about rapid prototyping when you’re learning.
Rapid production is all about understanding technology and applying it efficiently. The first few projects have a steep learning experience paved in rejected prototypes and likely a bit or two. It is important to remember that although CNC is just there to make your life easier and your projects more accurate, it is often not the final objective when prototyping. If you only need to make one, some things are better done by hand unless there is a specific reason you need to CNC them. The learning process takes time and so does tooling orders. Sometimes you can get what you need locally, but sometimes your project will need something special. You will not find a tapered ball nose bit at Home Depot the night before you need it. Once you get used to the technology it gets faster but it is never a silver bullet that will save you on projects that should have been started weeks ago. If it ever does save you on one of those, count your blessings and make sure you never try it again. Some things don’t work twice.
You may have already heard or seen the quote, “This machine has no brain so use your own”. If you are familiar with this saying then most of the following will be a refresher course. If this is the first time you have heard it, burn it into your mind because it may just save your life and at the minimum will save you a lot of money, time and frustration. Both successful projects and safety are never an accident. Plan how things will be set up, how the tool will do it, test it, then set up your work and make sure it proceeds exactly as expected.
Between the router control systems and the CAM software used to generate your tool paths, you have more computational power at your fingertips than was used to put men on the moon. You can harness this technology at will to create complex objects with the push of a button, but never let that entire high technology lull you into a false sense of security. A drunken squirrel has more accident avoidance logic than the most expensive CNC router or CAM system. This is why it is so important to always follow safety procedures, plan your projects in advance and watch closely for mistakes before they become problems.
The collision detection system on advanced cam programs is of little use to most beginning students. Software collision detection is a valuable safety system for advanced projects that can help avoid mistakes, but relying on it is dangerous because it relies on the data you give it and the assumption it is accurate to ensure safety. In professional production with a small number of highly trained operators ensuring proper setup these systems are reliable, but for our purposes they are at best an indicator of areas to watch. In the academic environment where equipment is shared and everyone is learning, it is never safe to assume anything. You never know who used the equipment before you and if they changed anything. Small changes like pushing a bit in more than you told the CAM software it would be or using slightly thicker than expected material can render these systems useless. They also do not track the movement of the dust collector, or the bottom of the spindle. Since dust collectors are adjustable, large and protrude below the collet, the router will happily crush one into the work piece if ordered even if the CAM software never saw any collisions. To avoid this, plan out your setup in advance, know your work area and know where the tool will go. Once your plan is verified with an air pass, you are as safe as you can be. Watch the first run extra attentively and be prepared to interrupt it if you spot any problems.
Software is not the only thing that can’t think for itself. Remember the CNC machine is just a machine, no different than a band saw or table saw, even though it is hooked to a computer. While you spend less time with your fingers near spinning blades and you don’t have the same kickback risks, CNC machines are capable of moving on their own and they have no idea what is going around them. Use your safety interlocks whenever you are with the CNC workspace or you are just inviting accidents.
The average low end CNC system you will likely encounter is an entirely dumb system with little or no two way communication. Even expensive machines only have limited feedback and will not do much to stop impending mistakes, crashes or accidents so the responsibility for safety rests firmly with the operator. While we use computer controlled mills and routers to create parts for mankind’s most precision dependent applications, CNC technology traces its lineage to the era of punch cards and the protocols used to control them are usually just about as advanced. They only focus on telling the machine where to go, how to go there and how fast to move. The only feedback commonly available from most CNC machines is the limit switches at the extent of each axis designed to stop the gantry from moving off its tracks or crashing the router into the side of the machine and some older machines do not even have these basic safety devices. Most machines cannot tell you if you’re pushing the tool too hard or even the true location of the tool. All the router usually knows is where the tool is supposed to be based on the commands that it has been given and the assumption they were successfully carried out accurately. Your only method of ensuring you get the result you expect is planning, tests and careful observation.
4. Never leave automated machines alone…EVER!
You may hear stories about professionals doing this, but remember you are not a professional yet and that expensive hardware your using is not yours either. If they want to risk thousands of dollars of their money it is their choice, but this is never acceptable in the academic environment. Advanced machines running proven programs are at best capable of semi attended operation and even this is a calculated risk. The programs we run as industrial designers are used to create prototypes. They are often only used once and there is no way to know they will run error free and the machines we run them on are not usually particularly intelligent. In addition, things just happen from time to time and if you’re not there to see it how will you stop it from destroying your work or the machine?
This happened when a collet loosened unexpectedly while cutting a finishing pass on a proven file. The error was caught within a minute and and the machine shut down. If the machine was left unattended, how would this have been stopped? All it takes is a programing mistake or hitting the edge of a hold down screw to damage a cutter and cause it to run hot enough to start a fire.
If this sounds like extreme paranoia, please see these pictures I am borrowing form a Woodweb article located here that you really should read.
This was not a freak occurrence… it happens. Do you know where your fire extinguishers are?
5:Garbage in, garbage out!
Prototyping can get expensive and we’re usually working on projects we need done yesterday, so we are always looking for places to save both money and time. When we start out it is hard to know what you need to invest in and what is just a waste of money or time to get. Bad choices on materials and tools can ruin an otherwise successful project or require enough redo’s to make you wish you had invested in higher quality materials to begin with.
Often when we think of CNC routers, the first thing that comes to mind is sheet goods like plywood and MDF. This is not accidental since at least half of what we cut on CNC routers is usually sheet materials. I am not going to start an exhaustive lecture on choosing the right plywood today as that is an essay in itself, and instead I am simply going to say that all plywood is not created equal. You can safely get your MDF at the home improvement store and nothing bad will usually happen, however the same thing does not hold true for plywood. Good plywood is expensive and usually purchased at a dedicated lumber vendor. It has a consistent core with good adhesion that will handle fine details and CNC cutting with less chipping or weak spots. This is where the standard home improvement store plywood tends to fall short. You might be able to get away with it on large parts but if you try producing an intricate design in it, you run the risk of finding a weak point in the lower grade core and having delamination or cracking occur. It is a fine material for cutting cabinet sides out of on a table saw, but it doesn’t hold up when you start cutting it in 2” strips and routing pockets ¾ of the way through it like we tend to when designing highly refined objects that push the potential of plywood to the limits. For this kind of performance, high quality plywood like Baltic Birch or ApplePly is essential. Don’t be afraid to ask questions to your vendors since they are specialists in what they do and they can be an important component in successful projects.
Just because wood is the first thing we often think about with CNC routers does not mean you should limit your imagination. You can also use routers to cut Renshape and some modeling foams. These materials take time to acquire and usually cost more than alternatives such as creating a large lamination of MDF, but they have properties that make them extremely useful in some applications. Renshape for instance will hold mold details much better than MDF, require less finishing and is less sensitive to moisture.
Not only do materials count, but so do the tools. Bits are an important part of CNC success, not an afterthought. Bits need to be paired appropriately with both the material they are cutting and the application they are used for. If you rely on only home improvement stores for your bits, you are limiting yourself to a small selection of spiral and straight flute tools intended for use in hand and table routers. This is OK for simple projects but you will quickly find that you need specialty bits and more data. If you do buy your bits from a home improvement store, buy the big name brands only and stay away from bargain bits and combo packs like they are the plague. Under no circumstances should you buy your router bits from bargain suppliers like Harbor Fright. They are great to use for the pack of forester bits you use once every blue moon or for the digital calipers you always have with you but not your router bits. CNC routing is hard on bits since you cut at high speeds for long periods of time with no breaks. Additionally there is no change in pace between cutting with the grain or cross cutting and you don’t feel the router so you can’t slow down when encountering excessive resistance from dull tools or hard spots in the material. Don’t take chances with your projects; buy good bits from trusted suppliers.
Good bit suppliers and manufacturers open up a new world of possibilities. The options available are extensive and deserve their own essay, but suffice it to say that you can choose from hundreds of bits tailored for specific materials and applications. Ball nosed bits will enable you to create curved 3D designs, angled bits are produced to create mitered corners and you can even find special form bits to produce edge details.
Take your time when ordering your supplies in between projects and try to leave room in project schedules to get the good stuff. The right materials can make your projects shine and good bits last a while if you take care of them.
Remember that at the end of the day, CNC technology is there to enhance your prototyping capabilities and free your mind to crisp, detailed and innovative designs. As long as you’re working to push the envelope, there will be a learning curve and resistance but that is just a sign of progress. Stay with it and see the places your mind can take you.
Behind all the data in callouts on plans and bills of materials are the real features that hold our designs together. While final selection is often an engineering decision, understanding fasteners makes creating practical designs and prototypes possible. It also helps us to understand why existing products are designed and produced the way they are and to understand the reasons for engineering modifications. Please bear with me if some portions of this are a bit dry. Fasteners are an expansive topic full of concepts and terms most of which were coined by engineers and machinists. Once we get through the basics, we will begin to discuss how to exploit them to make our designs stronger.
It is not my goal to turn designers into engineer, but to give us a window into the reasoning behind their decisions so we can better anticipate their needs. There is no reason that hardware must be shown, but there is also no reason we have to hide it if it is well managed. With integration and care, fasteners can become an integrated part of designs from furniture to electronics.
The beginning of fastener selection begins with a simple set of questions:
1. What are you holding together and does it have any special properties that will limit your fastener choice?
Common examples of limiting factors include materials being too soft or thin to hold threads. In these instances it may be necessary to add threaded inserts, through bolt or use another fastening method.
2. How strong does the joint need to be?
The first step in considering how strong a joint needs to be is to consider the force that will be applied to it. Force comes from several sources including shear forces, compressive force, and torsional forces. While accurate calculations are best left to the engineers, it is not hard to guess the forces being applied to parts of a product such as a chair seat, pad holder or first aid kit bracket and adjust your fastener selection accordingly. This section is really just a reality check to help avoid surprises down line when things are translated into real objects.
3. How will we make the joint meet the required strength?
This question really boils down to how many fasteners do we need and how strong do they need to be. To achieve this we have a wide range of fasteners available to help us. The hard part is choosing the right ones. Optimal selection is often an engineering decision, however for our purposes there are four main factors for us to consider.
What is the fastener made of and how strong is it for our application?
Fasteners are made from everything from plastic and common steel to aluminum, precious metals and exotic high strength alloys.
How large does the fastener need to be? This is often the primary variable we adjust within a given fastener style since the price difference between smaller sized fasteners is often minimal. In mass quantities, optimization here will save money but it requires analysis outside of our capabilities. It is not hard to assume that for an example in a prototype, we think a few 6-32 machine screws will be sufficient to hold the baseplate of a lamp in place. If the base was heavy and we were nervous our screws might not be enough, we could either add additional screws or simply switch to 8-32 machine screws without any significant changes being made.
How strong is the material that the fastener is being secured into?
Often the fastener may be far stronger than the material it is inserted into. Common examples of this are screws threaded into plastic or wall hooks mounted in drywall. If a child hangs from a towel bar it is not usually the fasteners holding it to the wall that fail but the fasteners themselves being pulled out of the wallboard that causes failure. The same sort of failure can be seen in threaded joints when tightened excessively in low strength materials like plastic. The behavior is called thread tear out and can significantly compromise the holding strength if it is allowed to occur. To counteract this, coarse threads with large bearing areas and a high percentage of thread engagement are used. It is often a good idea to manage the torque used to install fasteners if there is a risk of tear out. This can be as simple as the clutch on a power driver or simply requesting that screws are simply installed “snug tight” in installation instructions.
How many fasteners will be needed?
Very few things are held in place with a single bolt or screw. It may be possible but it is often desirable to spread the load out over several fasteners. This both reduces the stress on a single fastener allowing for smaller components to be used and also provides redundancy.
Once the fasteners are selected, the hard part is done and all that remains is simply locating and implementing them. When it comes to fasteners it never usually hurts too slightly over engineer in the concept stages. Later on things will likely change based on engineering analysis and calculations but it is often easier to start with a shell that assumes there will be fasteners of some sort involved. Simply omitting or modifying a few fasteners later is usually easier than trying to hide extra screws in a basically finished design. Another benefit of planning for fasteners early on in products is that it allows greater control in aesthetically motivated placements and an opportunity to explore options that not only are low in cost but also low in visual impact or that embrace or enhance your intended design.
As you begin to become aware of fasteners and how they are used, it is easy to begin to take note of the common products around you and how they are assembled. This observation is actually one of the most important reference materials available to designers since similar products already on the market can be evaluated quickly and used for inspiration.
To make a joint with a bolt or screw two options exist.
Through bolting is accomplished by simply boring a clearance hole through two or more pieces of material then securing them with a bolt and nut. While machine screws may also be used in the same manner, all bolts technically need a nut to fasten them. The common hex bolt and square head bolt can also be treated like a screw to further confuse things since they feature externally wrenching heads but they are the exceptions to the rule since other bolts such as carriage bolts and plow bolts rely on a nut for tension.
The clearance hole is simply a hole large enough to pass the threads of the fastener through without interference. Many modern software packages have included clearance numbers built in as an option but they can also be looked up in good tap and die charts.
As an example, a .25-20 bolt may fit through a .25 inch hole with some resistance. To achieve a smoother fit a letter F bit could be used to drill a tight fighting hole .2570 inches in diameter that allowed easy fastener travel and held tight tolerances.
You may have noticed the bit used to bore the clearance hole was not a common size you likely have in your tool box and it was specified with a letter. This is not a mistake; there are three series of drill bits in common usage. The one used most often in general fabrication are the fractional sizes. They are called that because they are based on common fractions. 3/32”, 1/8” and 1/4″ are all examples of fractional bits. Lettered bits also exist in sizes A-Z and numbered drill bits ranging from #1-80 or so. These bits in many cases exist specifically to allow for a class of fit for either clearance holes of threaded holes and are essential for getting tight professional fits.
If you don’t have a favorite tap and die chart of your own or a mechanical reference book you use for tidbits like drill sizes and tap selection, this free chart is highly useful: http://www.physics.ncsu.edu/pearl/Tap_Drill_Chart.html . It is hosted by North Carolina State University and well laid out. I frequently refer to this one over any of my printed versions simply because it’s always there at your desk when you need it. If you find yourself getting deeper into the selection of drill bits, taps and other mechanical bits as part of the design and prototyping process, investing in a copy of the Machinery’s Handbook is a good idea. This several thousand page shop book is filled with mountains of information on machining operations, lubricants and all things mechanical you will likely run across and plenty of things you hopefully never will. While the most recent edition is always a good idea, most of the basics never change so it is Ok to save a few dollars and go used on one of these if you find one from the last decade or so for a good price.
Almost any hole can be tapped provided it is deep enough to both hold threads and allow the tool to pass. Tapped holes come in two main styles. Through tapped holes are the simplest form of tapped hole. In a through tapped hole the piece receiving threads is drilled smaller than the fastener and threads are cut through the entire hole using a tap with a tapered nose. These tapers help to both align the hole and push chips ahead of the cutting head reducing clogging. In high speed tapping machine, spiral point taps are used to accelerate the process. Through tapped holes are used because they are easy to produce and allow the fastener to protrude to the other side in adjusting applications such as set screws and levelers.
Blind tapped holes are tapped holes that do not entirely go through material. These blind holes allow screws to be used without being visible outside a product or allowing the possibility of leaks. To create a blind tapped a hole smaller than the tap is drilled and the hole is then threaded with a bottoming tap. Bottoming taps have a flat face allowing them to thread closer to the bottom of a hole. Because bottoming taps cannot push chips ahead of them and out of the part, they must feed chips back up the hole behind the cutting faces of the tap. This allows for a greater possibility of chips clogging the tap resulting in poor cutting results or causing the tap to stick and break. In hand applications this is solved by frequently backing the tap out to break and remove chips. To help taps cut it is desirable to over drill blind tapped holes where possible. This extra clearance passed the required threaded depth of the hole allows space for chips that fall to the front of the tap. If space is available for a deep enough over drill it is often possible to use a traditional tap to create blind holes instead of a blind tap. This allows for faster production of blind tapped holes with fewer stuck taps and problems. In general practice it is a good idea to allow at least 1-1.5 times the diameter of the hole passed the intended threaded depth of holes where possible to allow room for chips and the tap body itself.
Because the actual depth that allows for efficient production tapping varies on material selection, tap choice and many other variables it is best to give as much freedom to the engineers and manufacturers of parts as possible. Sadly few definitive formulas guarantee trouble free tapping in all situations so it is best to err on the side of caution where possible. To give manufacturers room to work within the specifications, it is best to only specify minimum threaded depth required and any maximum drill depths. Manufacturing optimization will then work within these constraints to produce that feature with the shortest over drill practical to allow reliable and rapid production.
It is useful to be able to read and produce proper engineering style thread notations. This formal style of referring to threads is commonly used in component data sheets, for communicating with manufacturers and in a shortened form when shopping for fasteners.
The basic components of a thread call out are the major diameter of the fastener and the thread pitch. Additional information such as thread form and class of fit are also commonly added.
In inch fasteners, the major diameter may be referred to by either a decimal number or a fraction.
Additionally small sized inch fasteners are referred to by number series. The even numbered sizes between #0 – #12 are commonly used but odd numbered and larger numbered screw sizes exist. After #12, most modern fasteners now jump up to .25 inch major diameters and continue with standard fractional sizes.
To prevent confusion, metric fasteners are preceded by the letter M.
Thread Forms: A wide range of threads exist with different uses. Some threads such as acme thread are optimized for load transferring and used in lead screws in CNC applications. The majority of threads are either Unified National or metric.
Unified National Threads are often called out with the following abbreviations: UNC: Unified National Coarse UNF: Unified National Fine UNEF: Unified National Extra Fine
Metric has two primary thread pitches, fine and course. Since all metric standard fasteners are governed by a uniform thread standard, only the thread pitch is called out. In practice, it not uncommon for the thread form to be omitted from documentation involving common hardware unless it is an odd thread form such as Acme or pipe thread. In these cases it is usually assumed that the thread form is either Metric or Unified National.
While noting the thread form may often seem like a redundant step, this practice has its roots in the drafting standards which trace their origin to the industrial revolution where several competing and non compatible thread forms were in common production. Additionally specifying the thread forms is a simple insurance policy against mistakes and miscommunication which can be extremely costly in the production environment.
Class of Fit: The class of fit is the tolerance to which the fasteners are produced.
In inch fasteners 3 primary grades exist.
Class 1 is loose fitting and reserved for low tolerance applications. Class 2 is the most commonly used grade of hardware providing consistent fit and tolerances at a reasonable price.
Class 3 fasteners are high precision fasteners used when tolerances are extremely critical such as in machine tools and engines.
Metric fasteners use a slightly different grading system that divides hardware into general usage or high precision. Metric Fasteners with a class of 6H for internal threads and 6G for external applications are for general usage. High Precision applications commonly use two designators such 5H6G which refers to the tolerance of the internal thread and the external thread.
Precision fasteners and high strength fasteners are rarely seen in design applications and included for completeness only. When the stresses and tolerances demand this level of consideration, engineers need to be actively involved in the decision making process.
How we hold things together matters. While final fastener choice is usually an engineering and manufacturing decision, a few basic rules about fasteners and understanding how they work helps us to create plausible designs and communicate effectively with other disciplines. Being able to create logical designs on our own is also essential when working on small projects with startups and on tight deadlines where the bulk of initial design engineering tends to land on the designer who creates the initial digital models.
Basic Thread Vocabulary:
External Thread: A thread that protrudes outwards from a part. Examples include bolts and the ends of bottles.
Internal Thread: A thread that protrudes inward towards the center of a part. Examples include nuts and bottle caps.
Major Diameter: The distance between the outer most extents of a thread.
On external threads this is be measured between crests.
On internal threads this is measured between roots.
Minor Diameter: The distance between the inner most regions of a thread.
On External Threads this is measured between roots.
On internal threads this is measured between crests.
Pitch: The distance between parallel points on a thread.
When inch fasteners are used, pitch frequently referenced in terms of threads per inch. To get the actual measurement of thread pitch in these cases, divide by 1.
When using metric threads, the actual pitch is stated after the major diameter of the fastener.
Angle of Thread: The angle between threads measured along a plane that runs through the center of the threads .
Vocabulary is important in communicating technical details with accuracy. Almost everything has a name and it is helpful to be able to explain and discuss key concepts without pausing to explain every tool, feature function or fastener along the way. I will be posting weekly vocabulary focusing on specific themes or questions I ran into during the week.
Kerf: The width of grove made by a cutting tool. (The American Heritage Dictionary)
The width of a kerf varies depending on the cutting tool being used. The kerf can be less than 1/16” inch when cutting with jeweler’s saws or as large as ¼” or more when utilizing CNC routers. Depending on the process used and the precision required, offsetting the cut to prevent removing excess material may be necessary. Nesting patterns are especially sensitive to the effect of kerf because material is removed symmetrically from both parts. As a result it is often impossible to simultaneously cut tight fitting interlocking parts when they share the kerf of a cutter.
One tool capable of cutting tight fitting nesting parts is laser cutters. This useful link shows how to determine the kerf of a laser cutter.
Rip Cutting: Rip cuts are cutting operations made parallel to the direction of the grain.
Table saws and band saws are frequently used for rip cuts.
Cross Cutting: Cross cuts are cutting operations made parallel to the grain. As the cutter encounters the fibers of the wood at their strongest, slower feed rates are required for quality cuts.
Miter saws and radial arm saws and band saws are frequently used for cross cuts. Table Saws are also used for cross cutting when fitted with cross cut sleds and blades. It is also worth mentioning that when cutting plywood, due to the alternating grain directions of the plys, any cutting direction will behave like a crosscut.