CNC Router 101
Class presentation here:
https://docs.google.com/presentation/d/1z0J3msKjeNkzQOtDGowYq-WXv3sUo-WxrOoSAq3kXHk/edit?usp=sharing
3DHubs CNC Design: https://www.3dhubs.com/guides/cnc-machining/
CNC Router Fees
Drop-In Rate: $2/cutting minute
Member Rate: $1.50/cutting minute
At the CNC Router
Basics of How It Works
Design Create Toolpath Run the CNC
( CAD Software ) ( CAD / CAM program ) ( Machining Software )
Design a vector 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
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 bar
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
Turn on CNC Router and computer
Open Shopbot
Click “[C]uts” -> “C5 - Spindle Warmup Routine”
Ensure nothing (ie. bits, wrench) is in the spindle
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.
Sweep up the CNC room when you are done - DO NOT use the shop vac.
Do not use Fusion 360 to design your files. If you must use it, you must show your Fusion 360 file with the tool paths to a fabricator for approval.
Do not use router bits larger than 1/2" in diameter.
In the Classroom
SlideShow
https://docs.google.com/presentation/d/1ZZJPgDvorbs5rYXwNcsdP4EbCp53vzvXbybJh5fe0TE/edit?usp=sharing
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
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
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 (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, 3, 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 )
We do not allow use of downcut bits on the member CNC as this creates a significant fire hazard.
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 $30 (Double Flute Straight)
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 and length
It can’t fit in between two lines if they are too close together
You can't cut deeper than the length of the bit
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
To access the MakerSpace version of Vcarve 11.5, follow these steps:
Go to this link: https://portal.vectric.com/organization/shared-invite/LymN96Q71BjnsVkUK9aG
Enter your email address.
You'll be able to download version 11.5. This will allow you to build and save Vcarve files, but not export them to run on the CNC. These files will only be able to be exported to Shopbot using MakerLabs' master computers on the CNC Router, laptop, and desktop computer in the co-working space.
Any files generated will only be able to open using the version of the software using the link above, and not the trial version.
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 design size
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
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 5% ( a lot of stepover )
Because of the tip - the less stepover, the more wavy the result
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)
Cuts 3D meshes
Note: When cutting through material, set the depth of the cut to 0.02” deeper than the material (Z) thickness
**Special Note: For VCarve version 10.5, it will generate multiple pockets if multiple tools are listed.
IE. In the image shown, it will generate .04" pockets for both the .5" and .25" endmills listed. If you only need 1 pocket to generate, remove the tool from the list that is not applicable.
Feeds and Speeds
Spindle Speed
Determined by the material that is being cut
Wood - 12,000 RPM
Aluminum - 8,000 RPM
Acrylic - 6,000 RPM
Feed Rate
Calculate this based on the number of cutting edges and the material
Online calculator: http://www.freudtools.com/products/explore/router-cnc
Use the lower speed of the calculated range
If using the 1/4" double flute straight bit (MakerLab's standard rental bit) you can access the feed rate calculator here
(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. Can be found on Onsrud website.
RPM - spindle speed
Determined by the material that is being cut
Plunge Rate - the speed at which the tool cuts downward
Maximum at MakerLabs is 0.5 inch / sec or 30 inches/minute
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
Passes
The number of passes it will take the tool to reach the specified depth.
For details, click “Edit Passes ... “
When working with aluminum or brass, pass depth should be very shallow. No more than 0.02", regardless of the diameter of the bit.
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 used on acrylic or aluminum
Avoid climb cut with a hand or table router. It can be dangerous and your material has a better chance of getting away from you.
Conventional Cut: the rotation bit pulls off the material
Gives a nicer finish on wood
Can also be used for aluminum or acrylic.
Note: every material and end mill is different and they 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
Click “Edit Tabs ...”
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
If tabs are placed in an awkward area, they're more difficult to remove later on
Ramps
Always select “Add ramps to toolpath”
Type: ”Smooth”
Distance: At least twice the distance of the end mill's diameter
Exporting your File
Before exporting toolpaths, double check the order they are listed in. The CNC will run the toolpaths in order from top to bottom. If you need to adjust the order that they run, either click and drag them through the list, or use the up and down arrows to move them. Generally, pockets are run first, and profits that cut all the way through the material are run last.
Hit the Save Toolpaths button to export your files for the shopbot
Make sure Export all Visible Toolpaths is selected
Select the Post Processor (Should be Shopbot mm or inches)
Save toolpath “.sbp” file
Save vCarve file ( for personal use )
Step 3: Clamp Down Methods
Material can be secured in a variety of different ways. If you can rip material off the bed, so can the machine.
Screws
Use screws through a sacrificial part of your material. Make sure the screws will not get hit while running the job. You can damage or break a bit if hitting a screw.
Clamps
Material can be clamped directly to the bed using regular wood clamps. Be careful with clamp placement to avoid running the tool into the clamps.
Cleats
Wood cleats can also be made from scraps of wood. Cleats are a block of wood with a rabbet (groove on one side), and can be used to hold down material on each side. The rabbet height should be slightly less than the material height, allowing it to pull down tightly when screwed in place.
A thin, slightly flexible strip of wood can be used on varying material thicknesses. Glue a smaller strip across it, which will butt against the material to prevent slipping.
Jigs
Press-Fit Jigs
A press-fit jig provides good holding power and can be made quickly and accurately using the Shopbot.
This is a good solution for holding small work pieces, extra-thick stock, or if the material has already been cut to its final size and there is no room for screws.
Shown here: two pieces of MDF have been glued together and pocketed out to hold this piece of hard- wood. The jig is screwed to the table, then the work- piece is pressed in.
A similar method can be used where blocks of wood are tightly screwed to butt up against each edge of the material to hold it in place.
Door Stop Jig
This method is good for repetitive processes where you need to switch out materials of the same shape and size.
Blocks of wood are butt up against two edges and screwed into place. A third block of wood is screwed into another edge at and angle, and a door stop shaped piece of wood is wedged between the material and the angled block. This allows for quick and easy removal of the material, while keeping it secure.
The ideal angle for the wedge is 110 degrees.
Step 4: Run the CNC - ShopBot
Open ShopBot
Run the Spindle Warmup Routine if you’re the first to use the machine that day
Make sure nothing is attached to the spindle
(Go to Cuts> Spindle Warm Up Routine)
The spindle warm up routine will take about 10 minutes and will stop automatically when finished.
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
Move accurately using the commands “mx #” or “my #”
Or press “k’ to open the keypad control
Zero the router vertically ( Z direction ) with respect to your material
Move using the keypad so the bottom of the bit is in line with the top of the material
Turn on the dust extractor
Load your toolpath “.sbp” file
“Cut Part”
Follow on screen instructions
Log your cutting minutes: https://airtable.com/shr9hFYq5LBUSHKWw
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.
Using the Desktop CNC
- Bring RED computer + connect CNC to it through USB. Make sure the connection is stable.
- Connect both to a power source, that is not being shared with the big CNC
- Turn the CNC on with the switch on the right corner by moving it upwards. The control box on the side will light up.
- Open Shopbot in the RED computer
- Clamp your material and zero axes
- Feed rates cannot be greater than 2"/second on this machine. The Desktop CNC cannot move as fast as the CNC Router table, and will skip steps if it is pushed to move too fast.
- Spindle speed is set manually through the dial on the control box .
F is frequency (revolutions per seconds) = RPM/60.
ie. F200 will be 12000RPM
- Proceed to run file.
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”
How do I change from mm to inches and vice versa in Shopbot?
Go to Values > Display Values
Use the dropdown menu to switch from mm to inches.
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.
Resources
Free project files:
https://www.toolstoday.com/t-tool-videos
https://www.shopbottools.com/explore/projects
More Feeds and Speeds:
http://www.harveytool.com/cms/GeneralMachiningGuidelines_17.aspx