Education‎ > ‎CNC Router‎ > ‎

CNC Router 3D

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 3D 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





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.



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

  • Use Fusion 360 or Rhino to develop your 3D file and need to save the file as a .stl

  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 for 3D

  • End mills are designed to cut sideways

  • 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 for 3D

    • Roughing Pass

      • Something that take away a lot of material quickly

        • Square / flat bottom - standard cuts

    • Finishing Pass

      • Bull-nose

        • Tapered tip

      • Ball-nose

        • Completely rounded tip

  • Bits at MakerLabs:

    • Bring your own bit

    • Buy one for $40

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




Scalloping

Scalloping is the material left in between passes


The larger the scallops that are left behind, the more sanding you have to do to make it smooth.

Flat End Mill

  • To reduce scalloping (increases time) you can have a smaller cut depth

Ball Nose

  • To reduce scalloping (increases time) you can increase step over


.

Step 1: Design - CAD Software


The CNC Router 102 we will be taking a 3d file and learning how to cut it.



Design Considerations

  • The router bit is limited in its width (Hole)

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

  • The router bit is restricted in the z-direction (Undercut)

    • It can’t get underneath


  • How 3D paths are calculated is by the centre of the tip, this can alter the output of your 3D file







  • An example of what the CNC will cut

  • “Machining Allowance” - shift the designed path to cut less

    • This can be used to offset the difference between the designed and actual path



Step 2: Create Toolpath - VCarve

Starting a 3D Project

  1. Start a New File
        See Job Setup

  2. “File” -> “Import…” -> “Import Component / 3D Model…”

  3. Find the 3D model.  **Use “.stl” for best results
        See Orientate 3D Model

Job Setup

Job Size (X & Y)

  • Manually enter the size


Material (Z)

  • The thickness of your material

  • Accurate up to 0.01”


Units

  • Always in inches (for best compatibility)


Z Zero Position

  • Determines what zero is in the z-direction


XY Datum Position

  • Where the machine calls zero in the XY plane


Leave everything else as the default


Orientate 3D Model

Initial Orientation

  • Flip and rotate the 3D part


Model Size

  • Scale the model

  • Double check that the size is correct

  • Center the model


Zero Plane Position in Model

  • To include your entire model, set depth below top the maximum (slid to the bottom)


Types of Cuts

  • Roughing Machining Toolpath

    • Roughly cuts the the 3D profile

    • Cuts quickly

    • Do this first

  • 3D Machining Toolpath

    • Accurately cuts the 3D profile

    • Cuts slowly

    • Do this second


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



Machining Limit Boundary

Where the edge of the cut should be

  • Model Boundary

    • The most useful   

    • Only the XY area of the model will be cut

  • Material Boundary   

    • The XY of the entire job page will be cut

  • Selected Vector(s)

    • This uses any selected vector or vectors as the machining boundary.

  • Selected Level

    • Levels or layers of the design can be chosen to cut

  • Boundary Offset

    • Extra space added on the edge of the boundary

Machining Allowance

Used to add extra material to the design to be cut.
Can be used to offset differences in designed and actual cuts.


Roughing Strategy ( Roughing Toolpath )

The process in which the tool will travel.
This can drastically affects how long the cut will take.
It’s best to experiment and check the estimated time.

  • Z-level

    • Usually faster

    • Looks like a terrain view in steps

    • It will take steps in the z-direction at the maximum pass depth for the tool and raster in the specified direction ( X or Y )

    • Profile…

      • Outline the edge of each layers ( to remove scalloping in the XY plane )

  • 3D Raster

    • Rasters along the X or Y direction changing height as it moves


Area Machining Strategy (Finishing Toolpath)

The process in which the tool will travel.
This can drastically affects how long the cut will take.
This affects the scalloping left behind.
It’s best to experiment and check the estimated time.

  • “Offset” versus “Raster “

    • Circular designs tend to be faster with “Offset”

    • “Raster Angle”

      • Adjust the direction in which it is rastered

      • Two finishing passes at different angles will remove a lot of the scalloping

  • Stepover Retract - Lifts of z between stepovers, slightly removes opposite direction marks


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
        When using multiple bits, it is best to save a toolpath for each different bit

  3. Save vCarve file ( for personal use )



Step 3: Run the CNC - ShopBot

Cutting a 3D Project

  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

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

  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



Zeroing Z-Axis

When changing bits during one cut, it can be very challenging to keep the zero for the z-height. A noticeable height difference will be seen if it’s not set well.

Be consistent. For each bit:

  1. Put the bit loosely in the collet and let the bit fall down onto the material - this will be the zero for the z-height.

  2. Lower the z-height until an appropriate amount of the bits shank is in the collet.

  3. Tighten the bit.

*** Note: If the entire top surface of the material will be removed so this cannot be done with the next bit, then set the “Z Zero Position” to the “Machine Bed”


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.



Comments