CNC advanced topics
Work-In-Progress
Below we discuss different topics related to cnc-machining that help understand problems and difficulties related to the process along with potential solutions. This page will also be used as reference to explain CNC-related slang.
Dogbones
Types of milling bits
Tolerance & tool deflection
Milling direction
Issues & potential solutions from earlier projects
As you use a spinning tool (milling bit) to cut out pieces you will get round off corners in inner corners which have a radius equal to the radius of your milling bit. This means there's no way to get a perfect sharp corner when cutting out shapes that will need to slot together like a puzzle.
However, there is a way to make sure you can still put your pieces together: dogbones. Dogbones are adjustments to the corners to make sure the milling bit cuts a bit into the shape such that pieces will be able to slot together. This adjustment is an arc which gets added and has the same radius or higher as the radius of the milling bit. There are 2 different types which just depend on the location of the arc: T-dogbone and a regular dogbone. Have a look at the image below to see the difference between the two.
As you can see, the T-dogbone is more visible than the regular dogbone. So one might ask why would you use them? Well, depending on the way your pieces slot together these actually can become hidden when placed in the correct position, as shown in the image below.
Have a look at the image below. Left is drawn with radius equal to milling bit - right is drawn with a radius bigger than the milling bit. Note the changing offset allowence in case your material is not precisely the specified thickness in the way it has been drawn.
Flat bits mean they create a flat bottom surface when using them to cut and come in a variety of forms. The most commonly used ones at fellesverkstedet are the Upcut, Downcut and Compression bit.
Image showing the different flat milling bits.
-
Upcut: Multi-purpose tool which removes chips very well from the slots being milled, so higher speeds/pass depths can be used. The thread of the bit goes upward while rotating. Great for plastics, woodwork en metals. Does cause tear-out on the top side of plywood, as it pulls up the wood fibers up.
-
Downcut: Thread of the bit goes downward while rotating so it pushes the chips downwards. This can cause tear out on the bottom side of the plywood, if there are gaps below the material or slots in the sacrificial layer. Mainly used for woodwork. Advantage of this bit is that when cutting mdf (>9) or plywood (>12) it pushes the dust downward causing it to pack around the pieces. This side-effect can be used to avoid using tabs, if the pieces are not too small.
-
Compressionbit: Combination of Up-cut and down-cut, which gives a clean edge on both sides. Great for cutting of plywood. Not good for drilling though as you get burn marks and it heats the milling bit, thus making it less strong.
Check out this video for comparing these different types of bits (including a straight edge cutter) cutting wood in slow-motion.
Mostly used for 3D-milling. The tip of this milling bit is round off which makes it excellent for machining smooth surfaces as it can match the angle of the surface. Because of the geometry of the milling bit you might get a difference in finish, due to changing diameter influencing the speed at which the bit cuts in a particular spot. This is especially visible when milling Aluminium or (Transparent) plastics.
Great for engraving or putting a chamfer on edges. Since it's conical shaped
Shape tools
When you are cutting through the material at high rotational speeds there's obviously forces in place on the milling bit. These forces makes the milling bit slightly deflect (= bend). How much deflection you get depends on quite a few factors: How long the milling bit sticks out, which material you are cutting, which diameter milling bit you are using and which material it is made out of, How sharp the bit is, how fast you are cutting, how deep you are cutting, which direction you are cutting and finally the stiffness of the machine. It's good practice to minimize tool deflection as much as possible as this will influence how precise you are milling and how long your milling bit will last.
Milling direction is the direction the milling bit is cutting around your part. It's either Conventional or Climb. The milling bit always spins clockwise (when looking from the top) so the choice of milling direction will influence the way the finish on the material looks and which tolerance (see tolerance & tool deflection) you are getting. Which direction to choose mainly depends on which material you are cutting.
Usually used on wood and foam materials. The milling bit moves counterclockwise around the piece you are cutting (while it rotates clockwise). Therefore the milling bit will get deflected a bit more towards the piece you are cutting, so less tolerance is needed to get a perfect fit in comparison to climb milling.
Usually used on plastics and metals. The milling bit moves clockwise around the piece you are cutting (while it rotates clockwise). Therefore the milling bit will get deflected a bit away from the piece you are cutting, so you'll need more tolerance to get a perfect fit in comparison to conventional milling.
For assembling pieces you can include joinery in your drawings to be cut on the cnc. This joinery requires different problems and challenges than traditional manual woodworking joinery, while at the same time solving others. More info on this coming.
Hidden joinery
Jens Dyvik was kind enough to share his Rhino 3D example drawings showcasing different ways to solve hidden joinery using the cnc.
His example file can be downloaded here
Knowing and measuring the thickness of your material plays an important factor in most milling projects, so use the correct tools (calipers) and try to be as precise as possible, as this will avoid a few potential problems during machining or assembling.
Don't ever trust the thickness which the supplier of the material tells you it is. They might sell their material as 18 mm f.e. but from experience we've seen that this thickness can be somewhere between 17.5 and 18.5. (In some cases even more than a milimeter different!). If you have pieces that need to slot together or you're trying to engrave something relative to the top of the material, these differences can and will screw up your project and assembly process. Even if you're ordering 10 sheets of the same material you might end up with different thicknesses for different sheets, and in some cases this thickness even differs a lot from 1 side of the sheet to the other or to the center.
Tabs are bridges between the pieces you want to cut and the rest of the material. The reason for needing these is to make sure that your part doesn't come loose before it's finished cutting the shape.
The tool or "drill" that you put into the cnc-machine and which rotates and cuts through the material.
Top layer of the machine which is used to screw material onto. Gets worn over time since you usually cut a tiny bit into this layer, hence the name sacrificial layer. This layer needs to be planed regularely to make sure you have a flat surface to attach the material to.
Problem: Long thin piece came loose due to vibration and damaged the corner of piece.
Solution: We used a thin last pass (1mm + depth into sacraficial layer) to make sure there's less forces on the pieces while it's coming loose. We also increase tab size and moved the starting point to a different position, again to reduce forces on the piece while it's coming loose. The thin last pass might potentially be visible though, as the tool deflects less then it did on previous passes.
Problem: Material is bent and sticks up in different places.
Solution: Increase the distance from the top of the material so that the bit travels higher. (in Vcarve on the top right above toolpath operations "Page Setup" and then increase the value of clearance & plunge) Do make sure your milling bit sticks out long enough or the collet will plunge into the material that's sticking up.
Problem: 50 mm Foam melts around the 6 mm diameter milling bit when cutting to the full depth. The dust cannot be cleared away and is trapped in the gap created by the milling bit.
Solution: Make more space for the dust to be cleared. Create a first pass with a 2 mm offset of the actual shape to be cut to half depth (25 mm in our case). Then we decrease the amount of steps for cutting the final shape from 2 to 3. Another solution which we didn't explore could be to use a bigger bit such that chips have more space to be cleared away.