Education‎ > ‎

CNC Router 101

Class presentation here: https://docs.google.com/presentation/d/1ZZJPgDvorbs5rYXwNcsdP4EbCp53vzvXbybJh5fe0TE/edit?usp=sharing

3DHubs CNC Design: https://www.3dhubs.com/guides/cnc-machining/

At the CNC Router

Basics of How It Works


ink_part_vcarve.png

     Design                                    Create Toolpath             Run the CNC

     ( CAD Software )                 ( CAD / CAM program )         ( Machining Software )



  1. Design a vector file  

  2. Create a toolpath from the vector file

  3. Cut it with the CNC

CNC = Computer Numerical Control
Specifically a Computer Numerical Controlled  Router


The computer controls the machine, telling the motors where to move the router and how fast it rotates




Parts of the CNC

  • Power switch (and emergency shutoff)

  • Power cord

  • USB connection to computer

  • Spindle

  • Collet

  • Collet holder

  • Spoil board

  • X-axis ( 24” desktop, 96” on 4x8’ shopbot )

  • Y-axis ( 18” desktop, 48” on 4x8’ shopbot )

    • There’s an extra 6” on x and y - it will stop at the stoppers and crash the program

  • Z-axis ( 4” desktop, 8” on 4x8’ shopbot )

  • Z-plate ( 0.125” )

  • Dust collector - turn on before cuts

  • Dust skirt

  • Spindle rpm control:

    • Router is anything that cuts sideways

    • Router has constant torque

    • Spindle has varied RPM - draws as much power as needed


How to Turn It On

  • Power ba


  • .r

  • Check all Emergency Stops ( 1 on the table and 1 on the ground )  

  • Turn on computer ( password: makersgonnamake ) and open Shopbot program

  • Only when you need the spindle to run:

    • Turn on the dust collector

    • Put in key and rotate to 2 o’clock


Spindle Warmup Routine

Needs to be done if you are the first one to use the machine that day

  1. Turn on CNC Router and computer

  2. Open Shopbot

  3. Click “[C]uts” -> “C5 - Spindle Warmup Routine”

  4. Ensure nothing (ie. bits, wrench)  is in the spindle

  5. Follow on screen instructions ( time 10 minutes )


Safety Considerations

  • Do not leave the room while the spindle is running

  • Do not put your hand or any other part of your body any closer than 6 inches to the bit when it is moving. The router will not stop and can cause severe damage.

  • If the bit breaks or something seems to be broken or misbehaving, hit the pause button on the computer screen. If it needs to be shut off immediately press the red emergency stop button on the front of the bed.

  • Make sure no screws are on the path of the router. The screw will break the bit and will normally stay embedded into the project, but is capable of flying off and hitting someone.

  • After use of the machine clean the floor and all of your excess material out of the room, the sawdust on the floor and scraps can be hazardous and cause an injury.

  • Check and empty the vacuum bag frequently.


In the Classroom

SlideShow

https://docs.google.com/presentation/d/1ZZJPgDvorbs5rYXwNcsdP4EbCp53vzvXbybJh5fe0TE/edit?usp=sharing



Workflow


ink_part_vcarve.png

     Design                                    Create Toolpath             Run the CNC

     ( CAD Software )                 ( CAD / CAM program )         ( Machining Software )



  1. Design
    Computer Automated Design (CAD) Software

  • Create your design of what you want to cut

  • Today we are designing in 2D to create 3D results

  • We use Inkscape (like Adobe illustrator) - open source and simple

  • To design in 3D you will have to use a 3D CAD program

    • AutoDesk Fusion 360 & Rhino are available at MakerLabs

  1. Create Toolpath
    Computer Automated Design / Machining (CAD / CAM)  Program

  • Converts the design into toolpaths for the CNC Router to follow

  • Choose how it will be cut and with what end mills / drill bits

  • We will be using VCarve

  • It can also be done with Autodesk Fusion 360



  1. Run the CNC
    Machining Software

  • Utilizes the toolpath created and controls the CNC Router machine

  • Our CNC uses Shopbot3

    • The software is very specific and proprietary to the machine


CNC Bits (show block with different bits in it)

  • End mills are designed to cut sideways

  • Drill bits are designed to only cut up and down

  • Shank - clicks into the collet ( we have ⅛”, ¼”, ½” collets )

  • Important Dimensions

    • Diameter of the cutting head - how much it will cut ( ⅛” - 2” )

    • Length - how deep it can cut ( 1” - 4” )

    • Flutes - number of cutting edges ( 1, 2 or 4 )

  • End Mill Styles

    • Profile

      • Square / flat bottom - standard cuts

      • V-bit - engraving

      • Ball-nose - 3D detailing

    • Flute direction

      • Straight

        • Safest but not durable

      • Upcut

        • Pull chips up but more risky can pull up material too

        • Can blow out top edge

        • Don’t use on thin material <¼” or cheap layered plywood

      • Downcut

        • Avoids burring and creates clean top surface

        • Heats up quickly ( can melt plastic )

      • Compression ( Combination ) Bit  

        • Upcut and downcut - best of both

        • Need to cut lower than the upcut portion of the end mill  

  • There are hundreds of specialty bits for each material and effect

  • Bits at MakerLabs:

    • Bring your own bit

    • Buy one for $40

    • Rent one for $5 / day (note: if you break it you buy)



Step 1: Design - CAD Software


The CNC Router 101 class goes over 2D Design using Inkscape.

With a 2D design, a 3D part can be created by controlling the depth of the cut.


Design Considerations

  • The router bit is limited in its width

    • It can’t fit in between two lines if they are too close together

  • Ensure all lines are closed paths

  • To create a snug fit, the difference between the male and female offset is 0.05 inch (ie. box and lid)

Step 2: Create Toolpath - VCarve

Open your vector file in VCarve

Job Setup

Job Size (X & Y)

  • When opening up your vector file this should be automatically set to your desig

  • Double check this is correct


Material (Z)

  • The thickness of your material

  • Accurate up to 0.01”


Units

  • Always in inches (for best compatibility)


Leave everything else as the default



Types of Cuts

  • Pocket

    • Cuts the inside of a closed vector

  • Profile

    • Cuts along a closed vector line - either inside, outside or on the line

  • Drill

    • Drills the specified circles

  • 3D Cuts (Rough and Fine)

    • Cut’s 3D meshes


Note: When cutting through material, se the depth of the cut to 0.02” larger than the material (Z) height


.Tool Setup

Cutting Parameters

  • Pass Depth - how deep each pass will go

    • Less than the end mill’s diameter

  • Stepover - the amount each pass overlaps itself

    • Usually ~50%

    • Ball-Nose Bits: Stepover 95% ( a lot of stepover )

      • Because of the tip - the less stepover, the more wavy the result

Feeds and Speeds

  • Spindle Speed

    • Depends on the cut and material

    • For plywood we use 12’000 rpm at MakerLabs

  • Feed Rate

    • Calculate this based on the number of cutting edges and material

    • Online calculator: http://www.freudtools.com/products/explore/router-cnc

      • Use 12’000 RPM unless you have a good reason not to

      • Use the lower speed of the calculated range

    • (Feed Rate) = (Number of Flutes) x (Chip Load) x RPM

      • Feed Rate (

      • Number of Flutes (unitless)

        • The quantity of cutting edges of the bit

      • Chip Load

        • The amount of material which should be removed by each tooth of the cutter as it rotates and advances into the work. Chips help remove the heat produced by the cutting process.

        • Find this value online

      • RPM - spindle speed

        • Determined by the material that is being cut

        • Use 12’000 RPM unless you have a good reason not to

  • Plunge Rate - the speed at which the tool cuts downward

    • Maximum at MakerLabs is 0.5 inch / sec

Tool Number

  • If you’re cutting using multiple end mills / bits, specify a different bit and it will need to be changed during the cut when specified to


Passes

  • The number of passes it will the tool to complete the specified depth.

    • For details, click “Edit Passes ... “

  • If the the last pass is very small (ie. <0.03 inches), set the number of passes manually to one less to save a lot of time


.

Climb vs Conventional Cut

Climb Cut: the rotation of the router bit pushes into the material

  • Usually makes a better finish

  • Never climb cut with a hand or table router

Conventional Cut: the rotation bit pulls off the material

  • Better than a climb cut on softwoods and aluminum

Note: every material is different and hey should be tested to determine the best finish



Tabs

Tabs are pieces of material left behind in profile cuts when the material is cut all the way through. Tabs should always be used and ensure that the pieces will not move, break, or fly away throughout the rest of the cut.

Tab Sizes

  • Length: 0.25 inches

  • Height: 0.25 inches

  • Select “Create 3D tabs” - gives them a ramp

Tab Placement

  1. Click “Edit Tabs ...”

  2. Click on the selected vector to place each tab

    Note:

  • Minimum 3 tabs

    • 1 tab isn’t enough

    • 2 tabs can create an axis for the material to rotate about

  • Don’t place a tab in a corner


Ramps

  • Always select “Add ramps to toolpath”

  • Type: ”Smooth”

  • Distance: At least twice the distance of the end mills diameter



Save File

  1. Calculate all the toolpaths of the project

  2. Save toolpath “.sbp” file

  3. Save vCarve file ( for personal use )



Step 3: Run the CNC - ShopBot

  1. Secure your piece to the bed
        Use screws through a sacrificial part of your material  
        Or develop a jig to hold secure the material

    1. Make sure the screws will not get hit!

    2. Warning: If you can rip material off the bed, so can the machine

  2. Open ShopBot

  3. Run the Spindle Warmup Routine if you’re the first to use the machine that day

  4. Put the appropriate bit in the spindle
        Remember: the bit is already specified in the toolpath “.sbp” file
        Change with a one hand, or two hand squeeze
        Ensure the bit is clicked into the collet
        Tighten as hard as possible.

  5. Check the RPM of the machine and ensure it’s the same to your designed toolpath “.sbp” file
        The RPM can be found under “Tools” -> “Spindle Control”

  6. Zero the router horizontally ( X & Y directions ) on your material
        Move accurately using the commands “mx #” or “my #”
        Or press “k’ to open the keypad control

  7. Zero the router vertically ( Z direction ) with respect to your material
        Use the Z-Plate

  8. Turn on the dust extractor

  9. Load your toolpath “.sbp” file

  10. “Cut Part”

  11. Follow on screen instructions

  12. Log your cutting minutes: https://goo.gl/forms/LjrlJ3MjG5NSDdD53


Quality Assurance - Air Pass

An air pass is where the CNC follows the motions of your toolpath “.sbp” file but does not cut the material. The X & Y directions are properly zeroed with respect to the material but the Z direction is zeroed above your material so that the lowest point does not touch the material.

Run an air pass in between steps 6 & 7 above.

.FAQ’s

Where is the larger, detailed command window of Shopbot?

  1. Click the Question Mark

  2. A window will pop-up

  3. At the bottom, select “Switch to FULL”

Strange Error messages you do not recognize and google doesn’t help

Reload default configuration file

  1. Select on the ToolBar  “[U]tilities” -> “[R]eset default Settings, load a Custom Setting File, or clear System Log”

  2. Select and Open the file “ShopBot_PRS96x48alpha.sbd”

  3. If ShopBot is an easy mode, switch to Full mode (see above)


Runtime Error 13:

Delete C:/ProgramData/Shopbot/Shopbot 3/shopbot.ini
Reopen Shopbot
In pop-up asking for configuration, select file (in folder alpha) for ShopBot PRSAlpha 96x48 - double check the z-height settings

The toolpath is cutting inside & outside the line

Check if all the vectors are a closed path. If not, "weld" or "join" all the lines together.




More Feeds and Speeds:

Subpages (1): CNC Checklist
Comments