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 )

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 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

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.
- Sweep up the CNC room when you are done - DO NOT use the shop vac.
- We do not recommend using Fusion 360 to design your files. Please note that the consult and ongoing support will not be available for files designed with Fusion 360.
- 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 )

1. Design
2. 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
2. 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
2. 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 12 to run on MakerLabs' CNC Router, follow these steps:

Step 1: Sign up for a free account with Vectric at https://portal.vectric.com/login if you do not have one already
Step 2: Enter your email address here to register your email under MakerLabs with Vectric:
https://portal.vectric.com/organization/shared-invite/LymN96Q71BjnsVkUK9aG
Step 3: Download and install the Free Trial of VCarve 12 from vectric.com 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.
Step 4: Open VCarve 12 and login with the Vectric account you made in Step 1
Step 5: Program your design, save the .CRV project file to a USB stick, and take it to the MakerLabs CNC Router. (Ensure you are logged in when you save your file, or else you'll run into problems at the MakerLabs computer)
Step 6: Open your file on the CNC router computer using the VCarve 12 Makerspace Edition. Login with your Vectric account, double-check your settings, and export your toolpaths as a .sbp file
Step 7: Open your .sbp file in Shopbot to cut your part

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.
        Aluminum
        Soft Plastics
      - 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

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
- 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

1. 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.
2. Hit the Save Toolpaths button to export your files for the shopbot
3. Make sure Export all Visible Toolpaths is selected
4. Select the Post Processor (Should be Shopbot mm or inches)
5. Save toolpath “.sbp” file
6. 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

1. Open ShopBot
2. 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.
3. 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.
4. 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”
5. 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
6. 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
7. Turn on the dust extractor
8. Load your toolpath “.sbp” file
9. “Cut Part”
10. Follow on screen instructions
11. 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?

1. Click the Question Mark
2. A window will pop-up
3. 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

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.

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

Page updated

Google Sites

Report abuse