CNC Router 3D
Basics of How It Works
Design Create Toolpath Run the CNC
( CAD Software ) ( CAD / CAM program ) ( Machining Software )
Design a 3D file
Create a toolpath from the vector file
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
Design Create Toolpath Run the CNC
( CAD Software ) ( CAD / CAM program ) ( Machining Software )
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
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
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
Start a New File
See Job Setup
“File” -> “Import…” -> “Import Component / 3D Model…”
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
Calculate all the toolpaths of the project
Save toolpath “.sbp” file
When using multiple bits, it is best to save a toolpath for each different bit
Save vCarve file ( for personal use )
Step 3: Run the CNC - ShopBot
Cutting a 3D Project
Secure your piece to the bed
Use screws through a sacrificial part of your material
Or develop a jig to hold secure the material
Make sure the screws will not get hit!
Warning: If you can rip material off the bed, so can the machine
Open ShopBot
Run the Spindle Warmup Routine if you’re the first to use the machine that day
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.
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”
Zero the router horizontally ( X & Y directions ) on your material
Zero the router vertically ( Z direction ) with respect to your material
Turn on the dust extractor
Load your toolpath “.sbp” file
“Cut Part”
Follow on screen instructions
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:
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.
Lower the z-height until an appropriate amount of the bits shank is in the collet.
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?
Click the Question Mark
A window will pop-up
At the bottom, select “Switch to FULL”
Strange Error messages you do not recognize and google doesn’t help
Reload default configuration file
Select on the ToolBar “[U]tilities” -> “[R]eset default Settings, load a Custom Setting File, or clear System Log”
Select and Open the file “ShopBot_PRS96x48alpha.sbd”
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.
If spindle stops in the middle of cutting and the following message appears:
ShopBot No Longer Being Recognized!
"An error is occurring that could not be corrected. You will need to exit, check all cables, then restart the software. Tool Location may no longer be accurate."
Take a photo of where your zeros are
Restart the Shopbot software. Zeroes should still be accurate.
Modify your Vcarve file if necessary to start where the machine left off.
Parameter Error:
Parameter Value Above Range for VS -- Setting to Upper Limit (304.799995422363)!
This error means the file is set so the jog speed is greater than 300mm per second. This is faster than the CNC can safely move and the speed will need to be adjusted to a lower speed. If you do not click OK on the error message within 20 seconds the application gets stuck and you have to restart the whole ShopBot and start over.
Fees
Drop-In Rate: $2/cutting minute
Member Rate: $1.50/cutting minute ( the first 60 minutes of CNC time each month is included in membership )
