CNC manual

0.0 Policies
Overview
The CNC is a computer controlled router. It can cut computer generated 2d and 3d models out
of solid materials like wood and foam. The Shopbot Buddy CNC router can cut materials that
have the maximum dimensions of 24” x 48” x 3”. You must provide your own materials. It
is recommended that students schedule an orientation session with the CNC staff to become
familiar with the CNC, or attend the CNC Open House scheduled once a semester.
CNC Router
The Shopbot Buddy CNC Router located in Room 003, in the basement of 320 Newbury St. The
software required is available on all of the computers in the Coder Lab and Rm.401.After reading
this manual through, if you have any questions please email us at cnc@the-bac.edu.
Training
Each student must first complete a CNC Router Orientation. Orientations are held at Open
House events at the beginning of each semester or can be scheduled for individuals as scheduling
allows. For class or faculty orientations, teachers are asked to email cnc@the-bac.edu to
coordinate.
Scheduling
The CNC machine is scheduled via an online service: http://baccnc.youcanbook.me
Students can schedule 3 types of meetings:
• Orientation (1hr)- To learn about the machine and software
• Prep (1hr)- To review the toolpaths and get approved to cut
• Cut (1-3hrs) - To cut projects. Toolpaths must be approved first.
Students can schedule up to 3 hours total in one day. 2 missed or late appointments will result
in loss of CNC privileges for the semester. Appointments can be rescheduled/canceled up to 24
hours before a meeting time. If you are unable to make an appointment, please let us know, by
emailing cnc@the-bac.edu
Safety
Provided safety glasses and hearing protection must be worn at all times while the Shopbot is
in operation. While the machine is in operation, stay outside of marked areas. Only authorized
operators can operate the machine. Students are never to operate the machine unsupervised.
Students are expected to be present during the duration of cutting.
1.0 Materials + SoFTWARE
Students must supply their own materials. There is limited storage for material. 48 hours after cut
session materials will be disposed of.
Acceptable Materials
Foam, Wood, Plywood, MDF (Medium Density Fiberboard)
Prohibited Materials
Metal, Styrofoam, EPS, Glass. Ask first about anything not on either list.
Material Limitations
The maximum cutting area is 24” x 48” x 2”(X,Y,Z). However, the material maximum size is 30”
x 50” x 3” - this additional space can be used to fasten material to spoilboard. Minimum material
size is 12” x 12” x .25”. Make sure you have a method to secure your material to the table. If
material is to screwed down, then you need to leave a 2” border where no cuts occur. Any cut-out
piece require tabs or mounting to a substrate. Any materials that you laminate yourself must be
securely glued with the correct type of glue and dried for at least 48 hours prior to cutting.
CUTTING Limitations
Material can be cut only as a bit cutting length. The deepest bit cutting length is 1-11/16”. See
bit diagrams at the end of this guide for cut lengths limits. Interior 90 degree corners will be
rounded, unless a dogbone fillet or another trick is used. Each project has unique cutting and
finishing decisions to consider. Be sure to consult CNC operators or Design Computing Assitants
earlier rather than later in the process.
SOFTWARE - Importing Content
The CNC machine accepts “part files” from PartWorks 2D or PartWorks 3D. Partworks
and Partworks3D are the preferred software tools for creating part files. They convert 2D vectors
and 3D artwork to toolpaths that are saved as part files (.crv).
Partworks can import vector linework (2D files) in the following formats: dwg(2007 or
earlier), dxf, eps, pdf, and ai.
Partworks3D can import 3D files in the following formats:
3D Studio (.3ds, .asc, .prj), DXF/AutoCAD/Rhino (.dxf), LightWave (.lwo), VRML (.wrl), or
Wavefront (.obj). Most 3D design software can be used to create compatible files for either
Partworks or Partworks3D, as long as it can export to one of the above file formats.
2.0 2d Guide
design considerations
Consider the router capabilities: 2D design needs to be much more premeditated and thoughtful
than 3D design. There are 3 common toolpath types:
Profile toolpaths will create a cut line along your drawing’s vectors. Within the profile
toolpath option, there are 3 settings to choose from:
• Outside: (closed geometry only—ie. circle, square) moves the router bit along the outside
of your vector.
• Inside: (closed geometry only) moves the router bit along the inside of your vector
• On the vector: (closed and open geometries) cuts through the center of your vector—
make sure you have accounted for the diameter of the bit when using this method.
Pocket toolpaths (closed and simply-nested geometries) will clear an area
inside a closed polyline. These never cut all the way through your material.
Drill toolpaths drill a hole the diameter of the bit in the center of the chosen
object.
Measure your material’s width and height precisely, they are not always what they are named.
Material thickness should be measured with calipers (available in CNC Room). To maintain
precision, do not rely on your material’s original edges and corners as square or measured.
AutoCAD conventions
1. Check that your units are inches.
2. Draw a rectangle the same size as your material, and put it on a layer called ‘material’. The
bed is 24” wide in the x-direction and 48” long in the y-direction. You generally want to offset
any cuts ½” within the boundaries of your material’s edges. Also consider how material will be
fastened, if its screwed down, please leave a 2” border.
3. Consider the order of your layers: first, make cuts that don’t cut all the way through your
material (ie. etches), then make cuts that penetrate all the way through your material and organize
these cuts from interior to exterior.
4. Name layers according to order, type of cut, and depth to cut though: for example, op02_
profile_inside_675 would be the layer name for the following type of cut: the second operation
toolpath that is a profile cut to the inside edge of the line at a depth of 0.675 inches (note that
decimal points should be written as underscores). Solid organization in your drawing will save
you time later.
5. Move the lower left corner of your material box with all cut lines inside to position (0,0).
6. Turn only the layers on that are to be cut paths—turn all other layers off.
7. Run the ‘Overkill’ command to delete any duplicate lines.
8. Use the ‘Pedit’ command to convert all lines to polylines.NOTE: be wary of two-point control
splines—the ShopBot software might misinterpret their geometry.
9. Save as AutoCAD 2000 dxf or dwg.
>>>Steps Continue on Next page
Open Partworks 2D (Version 3.5)
1. Open Partworks software by going to Start --> All Programs --> Shopbot -->
Partworks 3.5
2. Once in Partworks, go to File --> Open and select the dxf file you just exported. Also, you can Tools->Import Vectors-->browse to file
3. Check that the x and y directions are the same as in your original file. Rotate if necessary.
Material Properties
1. The first step is to fill out the ‘material properties’ window: check that your units are accurate and
in inches, enter your material thickness using the caliper measurement, zero Z-axis at the top of your
material, zero x and y axis at the bottom left corner, hit ok.
2. After you hit OK, the next step is to check and edit vectors
NOTE: make sure to keep your layers intact—every operation you perform will
move the selected object into the active layer!
3. Select all vectors (CTRL-A)
4. Run the ‘Join Open Vectors’ command—this is especially useful for ellipses,
splines, etc.—be thoughtful about changing the tolerance distance if you need to.
5. Run the ‘Select Duplicate Vectors’ command, and delete any duplicate vectors
if needed.
Assigning Toolpaths
1. Assign toolpaths to your vectors by layer using the toolbox palette on the right. Use
the step-by-step conventions below to avoid glitches within the ShopBot software.
2. In the layer manager window, turn off all layers using the light bulb icon.
3. Turn on your operation 01 layer and make it your active layer by selecting it (it should
4. Select all (CTRL-A) or manually select the vectors in this layer to be cut.
5. From the tools menu on the right, choose the appropriate toolpath: refer to the
description at the beginning of this tutorial for the differences between toolpath
types (profile, pocket, and drill).
6. After you click on the toolpath to use, a specifications window will pop up. Fill this
out appropriately--see the spreadsheets and the end of this document to help determine values and bits.
NOTE: When using profile cuts that go all the way through, be smart about your cut depth and pass
depth values. To get the cleanest edge on the bottom side of your material, cut the same vectors in two
separate toolpath passes. For the first pass, adjust the cut depth to 0.05” less than the material thickness.
For the second pass, adjust the cut depth to 0.02” more than the material thickness. (you should get an
error message when cutting more than the material thickness—check the difference thoughtfully, and
then click OK.) The cuts that go all the way through should always be the very last cuts that the router
should make. For more information on techniques (bridging, pass depth tricks, brass screws) and when
cutting out smaller pieces, ask the CNC staff.
7. Hit calculate after completing each toolpath setup.
8. This will bring you to the preview toolpath window (material selection is just for visualization).
Double check the image to make sure you’re cuts will come out as expected.
9. Repeat the above steps, 1-8, for each layer.
NOTE: if possible, use the same bit for all of the layers so that you don’t have to change bits halfway
through—this will save you time.
>>>Steps Continue on Next page
Preview, double-check, and save your cut paths.
1. Thoughtfully reorder toolpaths if necessary.
2. View cuts in 2D preview mode and confirm it’s what you want—check for weird artifacts at corners or
complicated geometries by zooming in.
3. Re-check the depths of all your cuts in relationship to each other and to the material thickness.
4. Click the ‘Save Toolpaths’ button to save an .sbp file to use at the machine.
5. Also go to File --> Save to save a .crv file so that you can tweak parameters within Partworks
6. Save both files to a thumb drive for your prep or cut meeting.
Please remember to contact a CNC Operator via appointment or visit the Coder Lab to discuss your
project with a Design Computing Assistant.
...END OF 2D SECTION
3.0 3D guide
The 3D software is a little simpler than the 2D because you typically only have to assign one
toolpath for the entire surface. It does start to get complicated, however, when your file’s thickness is greater than 2-1/2” because of the 1/8” bit’s cut depth (see bit graphic). This forces the
user to horizontally slice their model to thicknesses less than 2-1/8” and then post-laminate. Additionally, inputs like stepover and bit size can be manipulated for a variety of finish effects.
NOTE: Cutting foam is much faster and much less risky than cutting wood so it is best to run a
few jobs with foam before you use other materials.
3D modeling conventions
1. Check that your surface geometry fits within the dimensions of your material and that it is a
single, logical solid.
2. Unlike the 2D version, do not draw a box to represent your material. Also, do not draw the
material itself, any surface geometry will be understood to be a cutting surface.
3. Export your surface as an .dxf file.
Open Partworks 3D
1. Open Partworks 3D software by clicking on Start--> All Programs--> Shopbot-->Partworks3D
2. Once in Partworks, go to File --> Open and select the .dxf file you just exported.
3. Check that the x and y directions are the same as in your original file and that it will fit on the
bed in that direction.
Enter Surface Properties
1. Check that your units are in inches—you can use the scale mm to inches button and/or rescale
your surface if needed.
2. You can reorient the surface if desired, but it is recommended that you do these type of
manipulations in your 3D modeling software instead. Assuming your model was imported
correctly (side to be machined is facing up), under Top Surface, select Top and under Sides to
Machine, select Top.
3. Hit ‘Apply’ button
4. Hit ‘Next’ button
Enter material properties
1. Fill out the material properties menu. Zero the X and Y axes to this corner. Enter your
material’s boundaries and the thickness. Zero the Z axis at the top. Configure your“ground zero
cut plane,” see below
2. ShopBot will assume material size based on the extents of your model, but you will need to
adjust this to your specific material
3. Change the thickness of material to actual thickness based on your caliper measurement.
4. Under Machining Margins, if you select ‘Symmetrical’ equal to zero the bit will cut
a rectangle the same dimensions as the extents of your model at a clipping plane depth so
that your surface will protrude above a ground zero cut plane. You can extend the margins by
increasing the number next to Symmetrical. If you select ‘Use Model Silhouette’, the bit will
leave the top surface intact so that your model is embedded within the original surface of your
material. You can also increase that margin, and it will offset the outline of your model.
>>>Steps Continue on Next page
5. ‘Depth of Model Below Surface’ set at zero will float the highest point of your model to the top of
your material. To be careful, however, it’s recommended to set that value at 0.02 in order to avoid height
variations of your material.
6. Set the Cut Plane thoughtfully depending on your bit and your desired thickness.‘Bottom’ is the most
common selection.
7. Click ‘Apply’, Click ‘Next’
Roughing toolpath
This is not needed for foam. After you have run a few jobs with foam, you can cut wood, and you will
most likely want to create a roughing toolpath (it saves time). You can adjust the pass depth to the
maximum cut depth for the bit. Alternatively, it can be used, as is, without a finishing toolpath to make a
stepped topography.
Finishing toolpath
1. Under Bit Selection, select an appropriate bit, pass depth, feed rate, plunge rate,
stepover, etc. See chart labeled Material Spreadsheet attached to back of this
tutorial for selection criteria.
2. Choose a raster angle that is perpendicular to the dominant grain of your surface.
3. Select Create an extra pass at 90-degrees for increased resolution.
4. Click ‘Calculate’ to preview the bit’s travel paths.
5. The time estimation is not accurate unless you keep track of similar projects and
establish a scale factor. Click Next.
NOTE: Increased resolution is highly dependent on the type of model and material
you are using. It can be achieved with a smaller stepover rate, a smaller bit, and/
or increased passes. All of these techniques will take more time. Creating an extra
toolpath at 90-degrees is generally the most effective method.
Cut Out Toolpath
1. If you want the Router to cut out your model after it has routed the surface, select Create Cut Out
Toolpath
2. Enter the properties similar to all other toolpaths (bit selection, pass depth, etc.)
3. Click ‘Calculate’. Click ‘Next’
Preview and check toolpaths
1. Click the Finishing Toolpath Preview button and confi rm that the toolpath is doing what you want
2. If it looks correct, click ‘Next’
3. If something looks wrong, click the icons at the top to navigate to previous screens and change
applicable settings. After you have made changes, be sure to hit Calculate, and proceed until the
Finishing Toolpath Preview looks good.
Save your files
1. Select ‘Finishing Toolpath Save’ to save a .sbp fi le for use at the machine.
2. Also go to File --> Save to save a .3dv fi le so you can go back and tweak parameters
in Partwork 3D.
Please remember to contact a CNC Operator via appointment or visit the Coder Lab to discuss your
project with a Design Computing Assistant.
...END OF 3D SECTION
4.0 DIAGRAMS + REFERENCE
CNC ShopBot Buddy
Router Track
Router
Router Bit
Material
Y-axis
Z-axis
X-axis
Spoil Board
Feed - the rate at which the machine travels along the
X & Y axis.
Router Track
Router
feed rate inches/sec.
Material
Spoil Board
Plunge - the rate at which the machine travels along
the Z axis.
plunge rate
inches/sec.
Cut Length
Cutting bits:
Diameter
1 11/16”
Bit Selection
1/8”
FLUTE GEOMETRY
77-102 1/8” Upcut Spiral Taper
• Straight flute: Offers a neutral cutting action - highest
force.
1”
• Upcut flute: Provides the best surface finish and
allows for good chip extraction. May cause part
1/4”
lifting if vacuum or fixturing is not sufficient.
• Downcut flute: Provides a downward force which
65-025 1/4” One Flute Upcut
helps eliminate part lifting. Chip rewelding MAY
7/8”
occur if there is no space below the part for chip
expansion.
1/4”
NUMBER OF FLUTES
48-005 1/4” One Flute Straight
• Single Flute: Allows for larger chiploads in softer
materials.
1 5/16”
• Double Flute: Allows for better part finish in harder
materials.
1/4”
52-910 1/4” Two Flute Upcut
1 3/16”
1/4”
57-910 1/4” Downcut
1”
1/2”
48-072 1/2” Two Flute Straight
1/2”
1 1/2”
1”
1 1/4”
91-000 1-1/4” Spoilboard Cutter
37-82 60 degree Flute
CNC TERMINOLOGY
Part File:
The file that Partworks creates to guide the Shopbot through milling the material.
Material:
The substance (foam, wood, mdf, etc.) from which the Part will be milled.
Part:
The desired finished piece(s) that is(are) being milled by the Shopbot.
Waste:
The left-over material including sawdust, border material, tabs, intermediate material.
Border:
A border of 1” minimum is required for fastening the Material to the substrate.
Tabs:
Small (but substantial) bridges of Material that are purposely left in order to keep
secure parts that would otherwise not be secured to the substrate after milling.
Substrate:
A flat, approved scrap material that is placed between the Material and the CNC bed.
The substrate will reduce the effective throat (z-axis available height)
Router:
The router is attached to the z-axis carriage and rotates the bit for cutting. It has five speeds, from10,000RPM to 18,000RPM which are manually controlled by the operator.
The collet secures the bit in the router. The bit shaft must be seated deeply enough to make full
Collet:
contact with the interior end of the collect tube.
Bit:
The bit is the cutting tool that makes contact with the material. Bits have 1-4 cutting edges (or flutes), a cutting diameter, and recommended chip loads.
Chip Load: Feed per tooth - the amount of material removed by EACH cutting edge of the bit.
Chiploads are also used to directly calculate feed speed.
Feed Speed: The speed that the bit is moved along an axis.
Stepover:
Stepover is the distance a bit should moves between adjacent toolpath tracks.
The recommended stepover distance for flat-ended bits is 75% to 80% of the bit’s diameter.
For rounded bits (e.g. ball nose cutter) the stepover should be much smaller to reduce cusp.
Stepdown:
The distance the cutting tool moves in the z-axis between cuts. Stepdown should never be more than 1.5x the diameter of the bit’s diameter.
Toolpath:
The contour path that the bit will follow to cut out the part while making Climb Cuts or Conventional Cuts.
Climb Cut: Where direction of bit rotation is the same as the feed direction.*Better for final surface finish for components cut out of material.
Conventional Cut: Direction of bit rotation is counter to the feed direction.
*Better for final surface finish for the cut edge of the stock material
Cusp:
The peaks/raised areas left between passes on round-ended bits.