MAINTENANCE OUTAGE: The University Wiki Service will undergo maintenance on Wednesday October 16th from 7:00 a.m. until 8:00 a.m.
During this planned maintenance window, wikis.utexas.edu may be unavailable.
Users are advised to save content locally that may be needed during this time and save all edits before maintenance begins, as unsaved work may be lost.
Page tree
Skip to end of metadata
Go to start of metadata

PART 1: 2D software, VCarve Pro ShopBot Edition

Video:  CNC Training - Intro and 2D

2D CNC routing is accomplished by assigning 'toolpaths' to 2D geometries.  For the purposes of these instructions we are assuming that the user is creating these geometries in AutoCAD, although they can be produced in any application that can handle layers and export a .dxf file format.

There are essentially 2 types of geometries that you can draw:

  1. Open Geometries: e.g. line segment, arc segment, spline or any un-closed shape
  2. Closed Geometries: e.g. square, rectangle, circle, ellipse, or any closed shape (you must verify that shapes are closed, this can be done with the pedit command in AutoCAD or with the Join Open Vectors tool in VCarve Pro)

To these draw geometries you can apply three (3) basic kinds of toolpaths:

1. Profile toolpaths will create a cut line along or around your drawings vectors. Within the profile toolpath option, there are 3 settings to choose from:

  • Outside: (closed geometry only) moves the router bit along the outside of your geometry, preserving the drawn geometry in the object being cut out.
  • Inside: (closed geometry only) moves the router bit along the inside of your geometry, preserving the drawn geometry in the cutout from the surrounding material.
  • On the vector: (closed and open geometries) cuts with the center of the bit traveling along the center of your drawn geometry; in order to evaluate where the bit will cut you must account for the diameter of the bit, this can be done using an offset command in AutoCAD with the offset set to the radius of the bit and by drawing circles with the same radius as the bit at the ends of the geometry.

2. Pocket toolpaths (closed geometries only) will clear an area inside a closed geometry down to a specified depth. These should not be used to cut all the way through your material, profiles should be used instead.

3. Drill toolpaths drill a hole the diameter of the bit in the center of the chosen object (circles are recommended, although their diameter does not control the diameter of the hole, for that you would need a profile or pocket and a diameter larger than that of the bit). Drill toolpaths do not function on points.

Measure your material’s width and height. measure your materialthickness with calipers. To maintain precision, do not rely on your material’s original edges and corners as square or measured.

Things to be aware of:

  • Using 'inside' and 'outside' with any pocket or profile commands when you have 'nested' closed geometries:  When you have a simple closed geometry these work in a straightforward and easily predictable way, however, when you have nested closed geometries (i.e. a series of concentric circles on the same layer and therefore in the same selection set) then you need to understand how the software processes the inside/outside command w.r.t. nested geometries.  As shown in the example below, with pockets (inside) on the left and profiles (outside) on the right, the software pairs nested geometries from outside to inside, and then routes on the outside or inside of the 'object' created by the nested pair.  The top example is two circles, the middle is 3 circles, and the bottom example is 4 circles.  The black lines are the circles as drawn and the reddish lines are the machine toolpaths.
  •  
  • Dimension identical to router bit diameter - If you have dimensions in your drawing that are identical to the diameter of your router bit, these features may not cut reliably due to rounding error (every time you do a 'save as' or 'import/export' you are using math to translate from one coordinate/geometry system into another coordinate/geometry system - this inevitably produces rounding error).  In order to prevent this, introduce a 'fudge factor'.  For example, if you want to pocket a 0.25" shelf and you are using a 0.25" diameter bit, make the shelf 0.26" wide instead.  Similarly, it should be noted that the router will simply ignore any features that are smaller than the diameter of the router bit since it cannot cut the feature without violating the drawing boundaries.
  • Internal Fillets - Often in routing we need to produce a functioning interior joint (i.e. a shape that can 'receive' an orthogonal shape in a geometrically determined way).  The thing to remember in this context is that you need adequate surface contact on an appropriate number of orthogonal planes to make this happen.  One option is to use a hand chisel after CNC routing to remove the fillets and create sharp corners.  The other option is to produce a 'dog ear' that eliminates the fillet but retains enough reference planes to locate the object.  The drawing below illustrates the problem created by fillets (left) and the recommended method for creating dog ears (right) - the example uses 0.75" sheet material with a 0.25" router bit, please note that the dog ears have a diameter of 0.26" as discussed in the bullet point above.  

AutoCAD conventions (Here is a sample file: test-door.dxf - also available on the Shopbot share.)

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 60” wide in the y-direction and 96” long in the x-direction. You generally want to offset any cuts ½” within the boundaries of your materials edges.

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, 2_hinge_profile_inside_0_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).

5. Move the lower left corner of your material box with all cut lines inside to position (0,0). (This will require you to use the move command in AutoCAD by grabbing the lower left corner of your material layer and enter #0,0 as your destination.)

6. All layers and geometries that are not intended to be cut (except the material layer) should be deleted from the production drawing.

7. If you are using multiple sheets of material for one production, we recommend making a master file that contains all sheets then do a 'save as' and save each sheet (i.e. sheet-1, sheet-2).  In each of these sheet files, relocate the material to (0,0) and delete the other sheets.  You need a 1:1 correspondence of files to sheets of material (unlike the laser cutter).

8. Run the ‘Overkill command to delete any duplicate lines.

9. 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

10. Save as AutoCAD 2000 dxf.

Open VCarve Pro Shopbot Edition

  1. Open VCarve Pro software by going to Start --> All Programs --> VCarve Pro - Shopbot Edition 7.0 --> \VCarve Pro - Shopbot Edition 7.0
  2. Open the 'partworks license code & install instructions.txt' file in the Shopbot Share (\\arch-data.austin.utexas.edu\shopbot - open to all UTSOA users) - copy and paste the license code into the license window.
  3. Once in VCarve Pro, go to File --> Open and select the .dxf file you just exported.

Check that the x and y directions are the same as in your original file.  The window should look like this with the sample test-door.dxf file:


Job Setup

  1. Check that your x and y dimensions are accurate and in inches
  2. Enter your material’s thickness from the caliper measurements 
  3. Zero the Z-axis at the top of your material
  4. Zero the X and Y axes at the bottom left corner (0,0)
  5. hit OK

Check and edit vectors: If you were unable to pedit all your vectors into closed shapes, you can use the ‘Join Open Vectors’ command---this is especially useful for ellipses, splines, etc.---be thoughtful about changing the tolerance distance if you need to.

Duplicates: You can also check for duplicates with the ‘Select Duplicate Vectors’ command, please be aware that misapplication of this command can result in deletion of intentional duplicates (i.e. ones on different layers) - this is why using overkill inside AutoCAD with 'search across layers' turned off is the preferred method.

Assigning Toolpaths  - We will be using a by-layer process for assigning toolpaths to geometries (this is why we place these geometries on separate layers within our drawing application).

  1. Open the Toolpaths menu by mousing over the Toolpaths tab in the upper right corner and then click on the 'thumbtack' to hold the menu in place.
  2. Select the 'Layers' Tab on the bottom left of the screen.
  3. Turn off all layers except for the first one you want to process - make sure the light bulb icon is on and that the current layer is highlighted in bold.
  4. Click in the drawing space and Select all (CTRL-A) - this will select all of the vectors in this layer.
  5. From the tools menu on the right, choose the appropriate toolpath: profile, pocket or drill.
  6. After you click on the toolpath to use, a speci?cations window will pop up. Fill this out appropriately--see the attached material spreadsheet to help determine values.
  7. Start Depth is typically 0.0, and your Cut Depth varies.
  8. Click on Select and choose the bit you intend to use in the next menu. Make sure all of your settings (pass depth, stepover, feed rate, plunge rate, etc.) are all appropriate to your material type and appliaction--see attached spreadsheet for settings selection.
  9. If you are using a Pro?le Toolpath, select one of the three options as described previously in the tutorial.
  10. Almost always select Climb if using wood or other hard materials; use Conventional for soft & spongy materials like foam.
  11. Name your toolpath.
  12. Click Calculate.

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) when cutting out smaller pieces, ask SOA-IT 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.
Toggle back to vector view with this tab.
Your completed toolpaths are listed here. You can edit them, delete them, rearrange their order by selecting the toolpath, and then clicking on the desired icon below.
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.
Preview, double-check, and save your cut paths.
1. Thoughtfully reorder toolpaths if necessary.
2. View cuts in 2D preview mode and con?rm 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 ?le 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 Charles or a thumb drive, go down to the shop and follow instructions there.

Next: Bits and Speeds 

        Using the CNC

  • No labels