3DT CNC Primer

From BenningtonWiki
Jump to: navigation, search

Cutting Basics

In practice CNC milling boils down to a few important factors.

1)Hold down and Fixturing. This how you hold the material while you are cutting. This should be considered first before programming your toolpath.
2)Tool Type. Different materials and cutting operations require different cutters. The old saying applies here "The right tool for the job".
3)Feed Rate: This how fast the machine moves while cutting. This speed is programmed in CAM and is crucial for a successful and safe operation.
4)Cutting direction: Conventional cutting is cutting in an anti-clockwise motion, while Climb cutting is clockwise. Each direction has various advantages and disadvantages.
5)Strategy: The type tool path you are running.

These factors all work together to create a successful cnc milling operation.

Hold down

Your stock material (the material you are cutting to create your parts) needs to be fixed in position properly or the force of cutting will send it flying across the room. If your parts come free or vibrate to much they may bind or wedge the cutter and cause it to snap - sending bits of sharp solid carbide flying into the air. THIS is why we always wear safety glasses while running the machine

Options for holding down parts:

1)Fastening with screws to the spoil board
2)Blocking in or using clamps
3)Adhering with spray adhesive or double sided tape
4)vacuum hold down (not an option for us)
  • a combination of these

For us fastening with screws and double sided tape will be our main methods of hold down. You must carefully plan out your hold down to coordinate with your toolpaths. If using screws you have to make sure your toolpath will not cut into your screw. You can use the machine to drill pilot holes so that your screws are in exact positioning you can reference in your model. When using double sided tape and cutting through parts you may rip up the tape and thus your part.

Tool Type

"The right tool for the job". To get an idea of what tools are out there check out the ONSRUDonline catalog. But before that you need to understand some tool geometry and terms.

Cutter diagram.JPG

Tool parameters:

1)Overall length - this is important. If you have deep pockets or surfaces you will need a long tool to reach those areas without haveing the router collide with the surrounding material. Longer tools will break more easily.
2)Cutting diameter - the diameter of the cutting edge.
3)Shank diameter - usually the same as the cutting edge diameter, but not always. You need a the right size collet that will hold your shank diameter. We have 14" and 1/2" collets.
4)Flutes - The number of cutting edges.
5)Helix Angle - Spiral cutters (like drill bits) move chipped material from cutting vertically up the shank. Straight cutters are used primarily to cut edges where no plunging is needed A high helix angles are typically best for soft metals, and low helix angles for hard or tough metals.
6)Flute Length - the length of your cutting edge. Determines your deepest cut.
7)Shank Length - you need enough shank to properly collet.
9)Spiral direction - up cut or down cut. Upcut - anti-clockwise from tip upwards. Down cut - clockwise from the tip.
10)Material - High speed steel (HSS) cutters are the least-expensive and shortest-lived cutters. Cobalt steel is an improvement on HSS and generally can be run 10% faster. Carbide tools are more expensive than steel, but last longer, and can be run much faster, so prove more economical in the long run. HSS tools are perfectly adequate for many applications. The progression from HSS to cobalt steel to carbide could be viewed as very good, even better, and the best.


Upcut vs downcut: Chip (swarf) removal is important. It keeps the cutting area clean which reduces force,vibration, tool wear and overheating. It is especially important when cutting soofter materials that may melt or burn at low temperatures, such as plastics, aluminum, and MDF. Upcut bits throw your chips up and out clearing them from the cutting area. They however, want to lift parts upwards which may present a fixturing problem. They also will chip laminate tops,grainy wood,or composite materials. Downcut bits help hold down parts but have less chip removal. They can avoid chipping and tear off in some materials.


Calculating Feedrate

A starting point for understanding what feedrate you should use is solvable by a simple equation. In practice I will ask you NOT to use this equation. I'll explain why.

FR = RPM x T x CL

FR = the calculated feed rate in inches per minute or mm per minute.
RPM = is the calculated speed for the cutter.
T = Number of teeth on the cutter.
CL = The chip load or feed per tooth. This is the size of chip that each tooth of the cutter takes.

chip load can be calculated using the cutter diameter and a chipload % which changes for different materials. A simplified breakdown below.
soft materials 4%:

aluminum, MDF, particle board, extruded acrylic, polycarbonate, foams

hard materials 2%:

Brass, Hardwood, cast acrylic

ChipLoad = chipload % x diameter of cutter

Why you shouldn't use the above formula. The primary reason is that the speeds calculated will be a lot faster than our machine can travel. Our machine is a little slow, but slow is alright. When the machine travels too quickly it doesn't have enough torque to accelerate and the motors bind and not complete the motion. Steppers motors (vs. Servo motors) do not have encoded feedback, so the machine will assume it traveled the distance it was meant to without any knowledge of the actual distance traveled. This causes big problems moving forward.
The maximum travel speed for our machine in the X&Y is 150 in/min. Without load 200 in/min will work, with loads you have to stay under 150 in/min. If you are making a full width cut into a hard material you probably wont cut anything above 75 in/min because of the load. Our Z axis has maximum speed of 15 in/min, which again decreases with load. You wouldn't want to drill much faster than that, so in the end it that limitation only comes into play with 3d surface milling. The secondary reason is that you still learning to program toolpaths, so mistakes and poor decisions are inevitable. In this case, slower speeds are safer and will minimize risk and increase time you have to react to a situation. We're not manufacturing, so we can afford inefficiencies in milling. Your patience is required. For our proposes you can use approx. 25% to 50% of a calculated feedrate from teh above method - as long as it's under our maximum speed. You can always start slowly and increase the feedrate as you mill, with caution. In general feedrates are determined by your experience with your machine, materials, cutters, and trial and error.

Cutting Direction

Like feedrate calculation determining your cutting direction is not an exact science. It has to do a bit with experience, preference, your machine, and your material. CNC forums such as [www.cnczone.com]are a wealth of information on such topics in cnc machining. Machinist LOVE to talk shop. I often browse forums for opinions on technique and make a cautious decision on who's advise to try for myself. Below are some great comments on cutting direction from forums. They illustrate the nature of the problem.

Conventional Milling 01.png Climb Milling 01.png

"A milling cutter can cut in two directions, sometimes known as conventional or up and climb or down.
Conventional milling (left): The chip thickness starts at zero thickness, and increases up to the maximum. The cut is so light at the beginning that the tool does not cut, but slides across the surface of the material, until sufficient pressure is built up and the tooth suddenly bites and begins to cut. This deforms the material (at point A on the diagram, left), work hardening it, and dulling the tool. The sliding and biting behaviour leaves a poor finish on the material.
Climb milling (right): Each tooth engages the material at a definite point, and the width of the cut starts at the maximum and decreases to zero. The chips are disposed behind the cutter, leading to easier swarf removal. The tooth does not rub on the material, and so tool life may be longer. However, climb milling can apply larger loads to the machine, and so is not recommended for older milling machines, or machines which are not in good condition. This type of milling is used predominantly on mills with a backlash eliminator." - wikipedia

"Climb milling is my "preferred" direction in wood and most other materials. There are a lot of reasons for any particular choice in many milling/routing operations. Speed, chip clearing, finish, shear direction, material, bit construction and personal preference are but a few." - Ron (rgBrown) shopbot talk forum [1]

Climb vs conventional - wood.JPG

"Climb milling leaves the chipped corners on the finished job while "conventional" milling removes its own chipped corners as it goes along." - Gerald D shopbot talk forum [2]

"Also, excepting Gerald's example, climb cutting usually causes less tearout with heavy cuts but for a cleanup pass, conventional often leaves a cleaner finish." - sheldon shopbot talk forum [3]

"When cutting wood, conventional cutting will almost always give a better cut. The only time I climb cut is when the cutter breaks the edge of the workpiece, and tearout is a problem." Gerry CNCZONE.com forum [4]