Back to Komo VR 510 Router
General Information To Consider
Materials Nominal Thickness vs. Actual Thickness
When we are talking about "Flat Stock Material", we are talking about sheet goods like plywood, MDF, or plastic sheets. These goods are specified by their 3 dimensions (Length x Width x Thickness), but like dimensional lumber (eg. 2 x 4's) there are some discrepancies. With sheet goods, the Length and Width are true to size but the stated thickness is not. With plywood's, a 3/4" nominally thick sheet (which = 0.75") can actually measure anywhere from 0.65" - 0.72" thick depending on the type, grade, and production method of a given sheet. Even within an individual sheet, the thickness could vary +/- 0.02". With the more highly engineered materials (such as MDF, Particle Board, and Melemine), their actual thickness' tend to be greater then the stated nominal.
So why does this matter to us? It matters because typically when we use flat stock material we are relying on the thickness of the sheet to establish the thickness of the parts we are creating and/or to fit into areas that have been machined. This means that the design should use the actual thickness of the material to be cut.
The following instances are some good examples of sheet thickness determining successful end results:
Rabbets and Dado's: Rabbet's and Dado's are woodworking joints in which 2 components come together in a perpendicular fashion. A rabbet is defined as a cut into the edge of a piece of material. When viewed in its cross-section, a rabbet is two-sided (1 vertical and one flat bottom plane) and open to the edge or end of the surface into which it is cut. A dado is a slot or trench cut into the surface of a piece of material. When viewed in cross-section, a dado has three sides (2 vertical sides and flat bottom plane).
Accurately modeled material thickness is important to these types of joints because again we are relying on the thickness of the material to establish not only the width of the rabbet/dado but its depth to. If for example we are using 3/4" nominal plywood with an actual thickness of 0.7" and we modeled our rabbet's and dado's to the nominal thickness the following issues would occur. The perpendicular fitting piece (cut from the same sheet) would have a 0.05" gap (if is was a dado) or a 0.05" protruding lip (if is was a rabbet). And if the rabbet/dado was designed to be in the middle of the 3/4" material (meaning 3/8" depth of cut and 3/8" bottom thickness) the depth of cut would be 0.05" shallower than what was designed. In the end, precisely modeled thickness is the key to having proper fitting joints.
- Laminated Assemblies: When making parts from flat stock material, one method to make bigger, more complex parts it to pre-laminiate sheets pre-machining, or post-laminate cut parts after post-machining. Accurately taking into account the actual material thickness at the design stage not only helps to ensure a proper fit, but also creates assemblies with correct laminated thicknesses.
If we go back to our 3/4" nominal thickness vs. 0.7" actual thickness example, a six layer lamination of true 3/4" thick material would yield a final thickness of 4-1/2" whereas a six layer lamination of 0.7" material yields a final thickness of 4.2". If a given design used the nominal vs the actual thickness there would be a nearly 5/16" thickness discrepancy between the physical artifact and the digital model. In the end, precisely modeled thickness is the key to having dimensionally accurate assemblies.
- Integration with 3D Elements: 3D elements such as edge rounds, chamfers, patterns, bevels, and general 3D surfaces have important considerations in regards to actual material thickness, especially elements that interact with the top planer surface. If modeled to a given materials nominal thickness, one runs the risk of losing some or all of the elements attributes depending upon the amount of discrepancy of the actual material thickness.
If we go back to our 3/4" nominal thickness vs. 0.7" actual thickness example, a 1/16" edge round on the top surface of a 3/4" nominal thickness part will loose about 85% of its curvature due to the 0.05" thickness discrepancy (will not even look like a round). With a 1/8" round you loose about 50% of the round; with a 1/4" round you loose about 25% of the round; and with a 1/2" round you loose about 10% of the round. This is detrimental to the visuals of the round because the tangent point of the round to the flat plane is never reached. This results in a hard edge which makes the round look incomplete. Thickness discrepancy is less of a visual issue when you have geometry that creates a hard edge to begin with, but there are still accuracy issues to contend with. In the end, precisely modeled thickness is the key to having complete and accurate 3D elements.
Vacuum Hold Down Method
The KOMO CNC router utilizes a vacuum hold-down method in order to hold flatstock material rigidly in place during machining/cutting operations. This is a fairly effective holding method do to the fact that the programmer/operator doesn't have to work around, hold-down clamps or screws (methods of mechanical hold-down). Vacuum hold-down allows for higher material efficiency though closer part spacings, no dedicated mechanical hold-down areas, and no dedicated material edge perimeter. The entire 5' x 10' bed of the KOMO is vacuum hold-down capable which enables a highly versatile machining strategy. Typically the KOMO is setup for 4' x'8' or for 5' x 5' flat stock.
Vacuum hold-down is accomplished through the use of a "Spoilboard" (alternatively known as a bleeder board) which acts as a mediator between the aluminum plenum table and the material being cut. The spoilboard is a sacrificial sheet of MDF which has been faced on both sides (which removes the hardened faces) and is porous enough to allow some air to flow through which enables the material to be cut to be sucked down. This means that the higher the air flow rate through the spoilboard the lower the vacuum hold-down; where as the lower the air flow rate through the spoilboard the higher the vacuum hold-down. How well materials/cut parts are sucked down to the table is dependent on the following criteria:
- Material Porosity: Some materials are more porous than others (such as MDF and OSB (oriented strand board)) due more to their manufacturing method than their material choice. The more air that can make it through the material to be cut, the less effective the vacuum hold-down becomes.
- Material Flatness: How much a sheet/piece of material has deformed from flat (ie. warped, cupped, twisted, distorted, checking,...) effects vacuum hold-down mostly by the deformation being to much for the vacuum to overcome with out the aid of some assisted hold-down (such as screws or taping the boundaries). Issues with severe material deformation is seem primarily in the "cheaper" types/grades of plywood and "sawn lumber" (rough sawn, S-2S, S-4S, dimensional or otherwise). With plywood, how well or how poorly sheets remain flat has primarily to do with the overall quality of the wood used, and the quality of the manufacturing process. Typically with "cheaper" plywood's, manufactures are prone to use poorer (i.e. cheaper) qualities of wood with lots of voids and knots for the core of the plywood and slap on a nice veneer on the outer surfaces. This sort of approach tends to create unbalanced constructions which in turn makes the material distort into a convex/concave shape or if we are really unlucky the dreaded "S" bend. These sorts of materials are great for testing or prototyping intial ideas, but higher quality materials should be used for final designs. If the material is to warped, then it can't be cut.
With sawn lumber, the amount of distortion one gets is impossible to predict because there are so many different variable to consider. What species of wood is it? How was it cut (through sawn, quarter sawn, or radial cut)? Where in the tree did the lumber come from (towards the heart or the bark)? Was it air dried, or kiln dried? Whats the woods current internal humidity? What is the atmospheric humidity? Did the tree grow with any particular internal tensions?
Luckily, most sawn lumber distortions can be rectified through cutting selective cutting away of material by means of a joiner, planer, or facing; this is called "Truing".
- Material Rigidity: Highly flexible materials (like thin "soft" plastics) have a hard time staying sucked down during cutting operations. They tend to want to peel back from the spoilboard.
- Part Geometry: The amount of vacuum an individual machined part experiences is based primarily upon the the amount of surface area said part has. Typically any part that has 100 square inches or less should be treated as potentially being thrown off the KOMO during machining operations. Of course the shape of this 100si part is extremely important. The more the part resembles an elongated rectangle the less vacuum per square inch the part will experience.
The amount of vacuum hold-down any part has is less on the perimeter and more on the interior of that part. So as the circumference of a part increases, the less interior vacuum it will have. So as an example, if we have three parts that all have 100si of surface area and the first part measures 10" x 10", and the second measures 5" x 20", and the third part measures 1" x 100"; the first part will experience the most vacuum hold-down, than the other two having the least circumference (40 linear inches), and the third will have the least vacuum due to its having the most circumference (202 linear inches).
- Amount of cuts per sheet: As we cut through our particular material, creating the physical parts developed in a digital medium, we are creating leaks for our vacuum; the more leaks we have, the lower our vacuum hold-down will become. The amount of cuts any particular sheet has is dependent on our part layouts, part shape(s), and the efficiency of our material utilization.
With a vacuum hold-down method comes two machining strategies that one needs to utilize, especially when producing prototypes (NOTE: If you are only cutting one, then it's a prototype): the Onionskin
and the Tab
- Onionskin: An onion skin is a thin (typically 0.08" thick for wood based based flat stock, 0.03" for plastics, 0.15" for aluminum and 0.15" for sawn lumber) piece of material that connects cut parts together until they are ready to have their final cut. This turns "Perimeter Cuts" (see 2-1/2" Axis and 3 Axis programming tutorials) into a two stage process. The first being the cut down to the Onionskin level the programmer has specified, and two, cutting through the Onionskin thereby cutting the part free. The reason we use the Onionskin method is two fold. One is to keep our 4' x 8' sheet of material acting like a full sheet even though 90% of an individual part has been cut. This is an important consideration due to the lateral stresses cutters exert during the machining process due to the fact that the Onionskin acts as a shear membrane which is able to counter the lateral forces. Since the Onionskin is typically only 5% - 10% of the original thickness (if we assume 3/4" nominal material) there will be substantially less lateral stress on the part when we cut through it.
The second reason to use the Onion skin method is that it prolongs substantial vacuum leaks a sheet of material experiences until the very end of the program. Unlike vises and mechanical methods, vacuum hold-down only creates downward pressure of the material to the spoilboard. It is this pressure in conjunction with friction between the material and the spoilboard that keeps the material to be cut and the parts being cut in place. If we prematurely lower the vacuum pressure before we are finished machining parts, we run the risk of losing (i.e. throwing) parts. This means that cutting through the onionskin needs to happen as the last machining operation of any program.
- Tabs: Tabs are connections that tie machined parts to other machined parts/waste material to prevent unintentional movement and are a result of the onionskin machining process. They work by triangulating lateral forces back to anchor points, a full onionskin does this automatically whereas tabs are much more selective. They are used on parts that are typically 100 square inches and smaller and/or on parts that have a high surface area/circumference ratio. Since they are a result of the onionskin machining method, tabs are the same thickness as the onionskin, a good portion of the time, the thickness of the onionskin is determined based upon tabbing needs and requirements.
Due to the fact that we are cutting the majority of the part free from the rest of the material, proper tabbing method is a very important aspect to consider. Because it is not just understanding where to put tabs for successful machining, but understanding best locations for post process removal. For a more in-depth explanation on tabbing strategies see programming tutorials.
Unlike the laser cutters or 3D printers, all 3 Axis CNC machines that use endmills (like the Bridgeport and the KOMO), have "issues" with inside corners. This is due to the rotating action that these machines use in order to cut material, it is like trying to put a cylindrical peg into a square hole, you can get most of it but not all of it. The reason that inside corners can be such an issue is when you want other parts (machined or otherwise) to fit within the machined aspects. But there are ways to help minimize the impact of this constraint such as:
- Restmachine: One method of reducing inside corner woes is to use a smaller tool and minimize how much of it is there. The smallest cutter that can cut the full thickness of 3/4" nominal material is 1/8" which would leave a 1/16" inside corner fillet. The drawback to this method is that it can take a large chunk of time (and time = $) to cut a large amount of inside corners. It is a method that should be used with extreme discretion.
- Chisel out left over material: This is the only method that completely takes care of the inside corner fillet. This is a completely post-process method that involves a sharp wood chisel (the sharper the better) and a whole bunch of patience. As with "Restmachining" this method should be used with discretion as it can take a large amount of time to complete if you have a lot to do. This method is also material specific, and can not be done (very easily) on metals and plastics.
- "Dog Bone" Method: (Click Here for "Dog Bone" Example Images) Another method to deal with the inside corner is to machine the inside corner away so that a sharp cornered receiving part will fit. The result bears some resemblance to cartoon dog bones (hence the name). This method requires some forward thinking on what cutting tools will be used to complete the necessary cutting action. It is extremely easy with this method to cut away to much material and not leave enough surface area for joint strength let alone any glue or fasteners. But this method does allow for immediate assembly of parts right off the machine.
- Design Integration: The last option to consider is to integrate the inside corner fillet into the design and production of your part(s). This option requires the most forward thinking and planning, could require extensive post-machine process (depending on the design and part complexity), but one of the "cleanest" looking methods. There are two potential methods to use; let the intended cutter give you a inside corner fillet, or model one. With the first method, you simple need to plan out what tools will do what operations for what aspects of your part(s). If you know what cutter you want to use for a particular operation, then you know what radius will be in your inside corners. For example, a 3/8" (=0.375") diameter cutter will leave a 3/16" (0.1875") inside corner fillet, since 3/16" is the radius of a 3/8" circle. The drawback to the method is that it is possible to lose track of what tools were used, and then correspondingly what fillets you will be getting. The second method of modeling inside corner fillets allows for a more selective fillet size and a broader range of usable tools. This means that you are guaranteed any radius fillet as long as you use a tool with the same radius or smaller. For inline assemblies
What cutting tools you use for your machining operations matters, but one of the major hurdles to overcome is knowing which tool to use for particular operations. There are many different types that can be broken down into the following categories:
- Drills: Used to created diameter specific holes in specific increments depending on type (Imperial, Metric, Lettered, or Numbered). Drills are only meant to move inline with the axis of rotation, NOT FOR LATERAL CUTTING. Drills can be put into standard collet's IF that collet is for that particular diameter. For drills that do not meet this requirment, they will need to go into a CNC grade drill chuck.
- Finishing Cutters: The most diverse tool category that has multiple subset groupings and frequent combinations such as:
- High Helix: Good for non-wood based materials
- Low Helix: Good for wood based materials
- Up Shear: Pulls waste chips out of the cut
- Down Shear: Pushes waste chips back into cut
- Straight Flute: Neutral shear, and lowest cost (mostly used in hand held routers
- Compression Cutters: These cutters have both "Up Shear" and "Down Shear" flutes which is great for veneer materials such as plywoods and melamine. The different "shears" help to prevent chip out at the cut edge on both the top and bottom faces.
- Roughers: Used primarily for aggressive material removal where finish is not an issue.
- Ball Mills: Used to create 3D surfaces, contours, and machining artifacts. The half hemisphere end cuts tangentially to the 3D surface, so depending on the diameter tool used in conjunction with amount of toolpath stepover, a highly accurate physical representation of a mathematically defined surface can be created.
- Insert Cutters: Uses replaceable inserts and a holder to accomplish cutting tasks. The advantage insert cutters have over solid endmills is that when a cutting edge gets dull on a particular insert, that insert is simply replaced with a new one; the whole cutter doesn't have to be replaced. Great for facing, or cutting custom profiles.
Cutters come in an almost limitless variety of types, diameters, length of cut, number of flutes, and materials. What cutters you use is dependent on any number of variables but there are some rules of thumb to keep in mind:
- The bigger the diameter cutter used, the cheaper the cut can be: The bigger the diameter of the cutter, the more lateral stress' that tool can take. The more stress a cutter can take, the higher that tool's feed rate can be. The higher the feed rate, the less time it takes to complete the cut. The less time it takes to cut, the cheaper the cutting cost will be
- Different tools are better at different things: Unless a particular project is designed to be fully cut using just one tool, the use of multiple tools (different lengths, diameters, ball mills vs. flat mills) can open the range of machining options, and physical details you may want. A general rule of thumb is to use the biggest tool you can for any machining operation you are performing, then move down in size as you need to. See tutorials for Material Specific/Machining Type Tool Sets. Some more specific examples, you want to use a flat endmill to cut "Flat Surfaces" (flat being perpendicular to the Z 0 plane), and ball mills to cut angled, and "3D" surfaces.
Tool Feeds and Speeds
Using the proper cutting feed rate through material, along with how fast a tool is spinning as it goes through material also is an important aspect to consider due to lateral stresses and friction created during machining operations. For specific Feed and Speed information see Material Specific/Machining Type Tool Sets
Tolerances for "Fits"
As much as we would like to think that our machined parts fit will fit perfectly together, this is usually not the case. Parts that have to go together with large amounts of "persuasion" (i.e. taking a large hammer and forcing two parts together) tend to have other problems of parts breaking or deforming under the hammering process. To aid in this issue, we can introduce tolerances into areas that require them. The following are aspects that require further consideration:
- In-Line Assemblies vs. Perpendicular Assemblies: With In-Line assemblies (where part faces are parallel to each other) the amount of tolerance required to get a good "fit" will be less due to the fact that all mating surfaces are machined surfaces. This means that the resulting surfaces have been cut by the CNC process and are therefore more accurate than factory/raw edges.
With Perpendicular Assemblies (such as you find with Rabbet and Daddo joints), we run into issues of material thickness variations (especially with engineered flat-stock material such as plywood). The problem being that the width of a machined slot is more accurate and consistent that the nominal thickness of the part fitting into it. We may have measured the thickness of the sheet and designed the assembly around this "Actual Thickness". But if we took multiple measurements we would see that their is a range that the actual thickness falls in (see the example in the Materials Nominal Thickness vs. Actual Thickness section). All "raw" materials have variations in their thickness, it is a fact that one needs to accept. But their are work arounds we can utilize:
- Slot Enlargement Method: This method is simply make the slot fit to the worst case scenario. Take the largest thickness and a design your slots to that thickness. This method works best if the material consistently has this thickness vs. being a singular outlier.
- Facing Method: This method involves cutting the face of the material down to a known thickness (such as what one would do with a planer). One issue with this method is that it can not be used on all materials. Hardwoods, softwoods, high density urethane foam, opaque plastics, solid surface, aluminum, particle board, and (to some extent) MDF all have consistent "materiality" throughout their respective thicknesses which is essential to understand because when we cut the top surface we are revealing new material. We want to know with some certainty that this new material will be just as good/consistent/aesthetically pleasing as what was their before. We can't make these sort of assumptions with plywood's due to the fact that the faces of plywood's (especially veneer plywood's) are so thin we run the risk of cutting through them and revealing the core which in most cases is of much poorer quality/consistency/aesthetic value.
- Shoulder Method: This is a more localized version of the facing method to where only the portion that is going to fit into the joint is cut down to a known thickness. This way any "revealed" aspects of the material will be concealed in the joint, and any variations in the material thickness is of no consequence.
- Permanent Joints vs. Joints for Dis-assembly: Joints for permanent assembly need to be snug but not too snug; we want to be able to tap the parts together, not pound. The purpose being that we want the parts of the joint to take and transfer stresses vs. the joint reinforcing method (i.e. glue and/or nails and/or screws and/or bolts). The amount of tolerance required depends upon the type of assembly the joint is (In-Line vs. Perpendicular) and the material used.
Joints for Dis-Assembly however need to come apart as easily as they go together and visa-verse. Naturally these joints require more tolerance to make assembly/disassembly easier.
- Actual Thickness vs. Machined Thickness: (I think I have already covered these aspects in the previous sections.)
- Modeling Tolerance vs. Programming Tolerance: There are three ways to introduce fit tolerance into joint assemblies, we can either program those tolerances within the individual toolpath strategies of our CAM software (in our case Delcam PowerMill) and model the parts with 0 tolerence , or we can model necessary tolerances in within our CAD software, and program parts with 0 tolerance; or the third option is the combination of these two methods.
The amount of parts that can be put onto a given piece of material (from a board of Hardwood to a sheet of Plywood to a block of foam) is an aspect one should consider with much contemplation because it has direct bearing on the overall cost of a given project. The more parts that can be put onto a given piece of material, the lower the overall cost will be. Here are some general rules of thumb:
- Orthogonal parts allow for better nesting: Squares, rectangles, and triangles are the most efficient types of shapes to produce because when they nest together there is no wasted space between parts.
- Curves Kill: Circles, ellipses, and curvilinear shapes have a lower efficiencies due to the void spaces created when two parts are situated next to each other
- "The Same Parts" vs. "All Parts Are Different": If you are cutting alot of the same part(s), grouping them together within your nesting strategy is a good idea. Most parts present opportunities for nesting patterns when thought of in singular contexts.
If however you have a wide range of part sizes/types to produce, you start to lose efficiency from void/leftover space created when parts don't nest very well.
- Layouts: Nice and Tight vs. Wide and Vast (I think I have a
- Wood Grain: To follow or not to follow: (I think I have a
- Large Parts vs. Multiple Subparts: (I think I have a
Position Pin Locations for Post Laminating Parts
Wood Dowel Rod: McMaster-Carr Link
Wood Dowel Pin: McMaster-Carr Link
Metal Dowel Rod: McMaster-Carr Link
Plastic Dowel Rod: McMaster-Carr Link
Metal and Plastic Dowel pins: McMaster-Carr Link