Job Setup

When setting up a new file, VCarve Pro prompts you to set up the job size, material thickness, position, origin, units, scaling, and modeling resolution and color options. Because other operations actually depend upon these settings, VCarve Pro (helpfully) prevents you from going further until you verify that your file is set up to match your actual machine and material.

Next, you’ll begin to align your digital file with physical reality by setting up your workspace to match your sheet material and machine cut area.

Job Type

Selecting a Job Type (Single Sided or Double Sided) is the first step in setting up a VCarve Pro file. It also determines what settings are displayed. When you cut the AtFAB projects from this book you’ll be routing single sided jobs.

1. Keep the default setting, Single Sided, as shown in Figure 7-6.

Figure 7-6. Job Type

Figure 7-7. New file with default job setup options

Job Size

The Job Size matches the actual dimensions of your material; this exercise uses a 4′ × 8′ × ¾″ plywood sheet. The units should match the default units of your CNC machine. While Width (X) and Height (Y) can be generalized, Thickness (z) must be the actual measured thickness of your sheet material, or T^MAX from “Measure Your Materials”.

1. Enter 48.0 inches for Width (x) and 96.0 inches for Height (y), as shown in Figure 7-8.

2. Enter T^MAX in Thickness (z) field.

If you’re working through the exercise, without plans to machine immediately, enter T^NOM—the nominal value of 0.75 inches—in the Thickness (z) field.

1. Select inches, as shown in Figure 7-8.

Figure 7-8. Job Size

Z Zero Position

The default Z Zero option sets the z-axis origin to the surface of the material. It’s also possible to set Z Zero to the surface of the machine bed. (“Pocket Cutting: Top Down or Bottom Up?” elaborates on why you would do this.)

1. Keep the default Z Zero option selected (Material Surface, as shown in Figure 7-9.

Figure 7-9. Z Zero Position

XY Datum Position

A datum is a fixed starting point of scale or operation. The datum position is intended to correspond to the machine’s origin or (0,0), which is usually set separately using machine-specific control software, but can be offset in CAM. Offsetting shifts the origin of your CAM file by a specified (x,y) amount relative to the machine bed size. Since the digital files you’re using are mapped to a full sheet, you don’t want to offset.

1. Keep the default datum options selected, shown in Figure 7-10 (unless your CNC is configured differently); “Use offset” should be unchecked.

Figure 7-10. XY Datum Position

Design Scaling

Figure 7-11. Design Scaling

This option scales the entire size of your file relative to the Job Size (X & Y) values you entered in “Job Size”. That’s problematic for parts that were designed and scaled in CAD to be dimensionally accurate.

1. Keep the default, making sure the box is unchecked (Figure 7-11).

Modeling Resoluton

Figure 7-12. Modeling Resolution

The modeling resolution and appearance settings are purely visual and have no effect on the toolpaths themselves.

1. Keep the default settings shown in Figure 7-12.

Complete Setup

Figure 7-13. Click OK to complete the Job Setup

1. When finished, click the OK button at the bottom of the Job Setup panel, shown in Figure 7-13. The Job Setup options will automatically be replaced by the drawing panel.

After you configure your Job Setup once, VCarve Pro will remember your selections and entries. They’ll be there each time you create a new file—but you’ll still need to click OK to confirm them every time.

If you ever need to access the Job Setup menu after setup, you can reach it through the Edit menu→Job Size and Position.

Note that VCarve doesn’t prompt you to c lick the OK button. If at some point you find yourself unable to select any vectors or use any commands, it’s because you haven’t hit the OK button to close out the menu.

Importing Vectors

With the job setup complete and physical parameters defined, you’re ready to import the Rotational Stools SketchUp file.

Download the Rotational Stools files from the book’s website. You’ll need ATFAB_STL_D4CNC.skp for this exercise.

Layout of Imported Data

Think back to when you were organizing the last step of “Save as SketchUp 2014”; after all the “part components” were laid out onto the cut sheet, you grouped them all into a final, single group. The Rotational Stools file has also been organized this way.

All project files in this book have been organized this way, just like the Chair example.

Grouping components prevents VCarve’s Auto Orientate feature from automatically re-laying out parts. When factors like grain direction and alignment matter, as explained in Chapter 3, manually arranging parts onto the sheet is preferable to depending on Auto Orientate to do the job alone.

1. Choose Exploded Flat Layout and Auto Orientate under Layout of Imported Data.

Figure 7-14. SketchUp File Import window detail

Vector and Layer Adjustments

Importing one file format into another is always a little tricky, and as you’ve seen from all the conversion settings, there are many things that can go wrong. Once you’ve imported your SketchUp vectors, it’s helpful to check over all of the settings, vectors, and layers.

Distinct parts should appear, just as they did in SketchUp. Ensure that the vector layout in the main VCarve window matches the screenshot shown in Figure 7-15. The cut file outline should match the Job Size and orientation.

The workflow from SketchUp into VCarve typically requires a few additional adjustments. These next steps will walk you through these adjustments of aligning the cut file to the material stock, ungrouping vectors, and joining open vectors.

Align Cut file to material stock

1. If the sheet material outline does not align with the sheet in the main VCarve window, select all vectors in the file (either with the cursor or Ctrl + A).

2. Click the Align Tools option from the Drawing Toolbar→Transform Objects→Align Selected Objects icon, shown in Figure 7-15. This will align the entire cut file with the material stock that you just defined in the Job Setup.

3. Close the Alignment Tools by clicking the Close button at the bottom of the palette (Figure 7-17). You may need to scroll down to the bottom to see it.

4. Save your file as a VCarve file or CRV. Name it Rotational-Stools.crv.

When working in the blue sidebars, you’ll need to click a “Close” button at the bottom. Just like you had to click “OK” to get out of the Job Setup menu, you’ll need to click “Close” to deactivate the Drawing palettes that open up.

Figure 7-15. Rotational Stools file in VCarve Pro, use Alignment Tools to correct sheet misalignment.

Figure 7-16. Alignment Tools palette open, vectors aligned to material

Figure 7-17. Alignment tools “Close” button

Ungroup Vectors

The technique of combining all 2D components within a single overall component in SketchUp preserves your cut sheet layout during import, but all parts will be grouped into a single layer as a result. On initial import, you’ll find that SketchUp layers will be black, rather than distinct toolpath layer colors, distinguishing inside cuts from outside cuts and holes.

If your file imports without its layer colors, you’ll need to release the group so that each part is placed onto its originally assigned cut layers. To ungroup parts back to their original layers:

1. Select all vectors, then from the Drawing sidebar go to Edit Objects → “Ungroup objects onto their original layers,” as shown in Figure 7-18.

2. Select only the parts; not the outside cut sheet border. Click the Zoom Selected icon, Drawing→2D View Control→Zoom Selected, to enlarge your view of the parts.

   You can also ungroup by right-clicking and selecting Ungroup Objects→Ungroup objects back onto original object layers.

3. After ungrouping, the vectors take on the color of the SketchUp toolpath layers: blue for outside profiles, green for inside profiles, and red for holes (Figure 7-20).

Figure 7-18. Ungroup objects back onto their original layers

Figure 7-19. Select only the stools vectors and then Zoom Selected

Figure 7-20. Ungrouped vectors return to their SketchUp layer color

Join Open Vectors

VCarve toolpaths work best when they’re created from closed vector shapes. Diligently grouping vectors while in SketchUp usually ensures that your imported file will have closed vectors, but sometimes things don’t go as planned.

It’s possible that your part vectors are not joined together, but are individual lines in places. Luckily, VCarve has a “Join Vectors” operation that lets you quickly identify open vectors and close any open, unjoined vectors that you may have imported.

1. Check for open vectors by Edit → Select All Open Vectors. If any are open, it’s easiest to fix them one layer at a time.

1. Turn on the blue layer, Profile Outside, and turn off all other layers.

2. Select all elements on Profile Outside choose Drawing → Edit Objects → Join Open Vectors.

3. Repeat this process with the Inside Profile and with other layers.

Figure 7-21. Joining the open outside profile vectors

You can also select all by using Ctrl + A and then hitting J to bring up the Join menu.

If you find discrepancies with orientation, origin, or scale, it’s best to go back to your CAD file, check the origin and units, and re-import into the file.

Creating Profile Toolpaths From Vectors

Each profile toolpath has a unique combination of cutting attributes. “Toolpaths” explained how a tool could be programmed to cut inside, outside, and on the vector. Depending on where the tool cuts, relative to the vector, the kerf shifts position, and, in turn, changes the dimensions of the part.

Before you create the toolpaths for the Rotational Stools, take a look at Figure 7-22, which contains three identical squares drawn with identical dimensions. Each square is cut with a 1⁄8″ profile toolpath, each toolpath having a different relationshp to the drawn vector.

Figure 7-22. The same size, equally spaced boxes with outside, inside, and on line profile toolpaths applied

In Figure 7-22, the red line with black arrows visually represents the path the tool will travel to machine the part. Figure 7-23 shows a 3D machining simulation of the toolpaths.

Figure 7-23. 3D machining simulation of outside, inside, and on line toolpaths in Figure 7-22

The outside toolpath creates a dimensionally accurate part, while the inside toolpath cuts a correctly sized slot. The on vector cutting option is not dimensionally accurate as a slot or a part. Avoid cutting on the vectors, unless you are etching or cutting decorative embellishments.

Rotational Stools Toolpaths

ATFAB_STL_D4CNC.skp has three toolpathing layers. The vectors that outline each part are assigned to the Profile Outside layer, the square shapes centered in each of the seats are assigned to the Profile Inside layer, and the vectors that form the fastener holes are assigned to the Profile Hole layer.

Up to this point, you have been working with virtual vectors organized onto layers—let’s turn them into actual, physical toolpaths!

To cut out the Rotational Stool’s outer profiles, you need to assign the tool to cut on the outside of the vector, creating dimensionally accurate parts that will fit together well. Conversely, to machine the Stool’s inside profiles and fastener holes, the inner dimension is important, so you’ll assign an inside toolpath that will cut on the inside of the vector.

In addition to defining the relationship between the cut path and 2D vector, toolpaths also require four other inputs: tool diameter, cut depth, pass depth, and toolpath type.

In the following steps, you’ll be using the Toolpaths menu, shown in Figure 7-24 to create three different toolpaths to handle these different cutting requirements. As you define each toolpath, it’s helpful to take advantage of your layer organization. Use the Layers List palette to isolate and assign definitions to each toolpathing layer.

The Toolpaths menu is on the right; the Layers menu is on the left.

Figure 7-24. Layers List palette on the left side, and Toolpath Operations on the right

Seat Inside Profile Toolpaths

Next, you’ll define the Stool’s inside profiles on the seat parts. Return to the main VCarve window, to turn off the Profile Holes Layer and turn on the Profile Inside layer.

Next, you’ll create a second inside profile toolpath for the seat slots in the same way you created the fastener hole toolpaths.

Select Profile Inside Vectors

1. Close the Preview Toolpaths menu (there’s a Close button at the bottom, just like in the Drawing menu options).

2. Uncheck the 000 holes toolpath in the Toolpath List. The hole toolpaths will disappear. Unchecking a toolpath hides it from view, but it is still there and can be reselected at any time.

3. Open the Layers tab (bottom of the left Drawing menu).

4. Turn on the green inside profiles layer and hide the holes layer (shown in Figure 7-37).

5. Select all vectors on the Inside Profiles layer, Ctrl + A.

Toolpaths, once calculated, are distinct entities from the vectors used to create them. Unchecking the toolpath name from the Toolpath List will hide the toolpath, but it’s often helpful to leave it on so that you can see the relationships.

Figure 7-37. Selected seat inside profiles; the green inside profiles layer is on, and all other layers are hidden

Create Seat Inside Profile Toolpaths

1. Create a new profile toolpath by keeping the vectors selected and then clicking the profile toolpath icon under the Toolpaths menu→2D Profile Toolpath.

2. Open the Toolpath Database by hitting the Select… button under the Tool section, Toolpaths menu→2D Profile Toolpath→Tool.

3. Select a 0.25 inch end mill (¼″), Tool List→Imperial Tools→End Mill (0.25 inch).

4. Enter the settings shown in Table 7-1. Any settings not specified will be left as the VCarve Tool Database default.

Table 7-1. Seat Inside Profile Settings

Tool Diameter	0.25 inch (¼″) end mill
Passes	3
Cut Depth	0.76”
Machine Vectors	Inside/Left
Direction	Conventional
Toolpath Name	000 Inside Profiles

Figure 7-38. Selected 0.25-inch tool from the Tool Database

Simulate Inside Profiles

When VCarve automatically opens the 3D Window and Preview Tab, you will see this new toolpath added to the Toolpath List at the bottom of the right-hand menu.

1. Ensure that 000 Inside Profiles is turned on (checked) and review the animation and visuals of the vectors, and the actual cuts made by the ¼″ end mill.

2. Check that the material is cut all the way through, that the cut shapes match those in the original cut file, and that no details are obliterated by accidentally selecting a tool that’s too large.

Figure 7-39. Machine paths for inside cuts

Outside Profile Toolpaths

Now it’s time to cut out the parts by creating outside profiles. You’ll repeat the same process of selecting vectors and then programming the toolpaths like you did previously with the inside seat toolpaths, using the same ¼″ end mill.

Create Outside Profiles

1. Enter the settings shown in Table 7-2. Any settings not specified will be left as the VCarve Tool Database default.

Table 7-2. Outside Profile Settings

Tool Diameter	0.25 inch (¼″) end mill
Passes	3
Cut Depth	0.76”
Machine Vectors	Outside/Right
Direction	Conventional
Toolpath Name	000 Outside Profiles

Figure 7-40. Isolate Outside Profiles

Simulate Outside Profiles

VCarve automatically adds this third toolpath (000 Outside Profiles) to the Toolpath List at the bottom of the right-hand Toolpaths menu.

As before, review the animation and visuals of the vectors, spindle path, as well as the actual cuts made by the ¼″ end mill. Ensure that kerf matches the end-mill size, that material is cut all the way through, and that the cut shapes match those in the original cut file.

Figure 7-41. Run Simulation of Outside, Inside, and Hole toolpaths

Toolpath Order

After programing these three toolpaths, it’s probably obvious that the CNC machine must make many multiple passes to complete a job. The CNC performs each toolpath operation separately, in a predefined cut sequence. Logically, one operation will need to go first, with the second and third to follow.

When assigning a cut sequence, it’s ideal to cut holes and interior cuts situated within larger parts first and then follow up with cutting outside profiles. Small, inside, self-contained cuts within larger parts are generally less likely to shake loose once they’re cut. Some overall parts, on the other hand, have the potential to shift or vibrate out of position, once cut from the sheet. By cutting the outside profiles last, you eliminate this risk for misalignment.

Define Cut Sequence

1. Turn all toolpaths on. Go to the Toolpath List at the bottom of the Preview Toolpaths menu and check all the boxes.

2. Use the up and down arrows to move the three toolpaths into the correct order:

   1. 000 Holes,

   2. 000 Profile Inside,

   3. 000 Profile Outside.

Figure 7-45. Toolpath cut order is important; always cut holes first, then inside profiles, and then the outside profiles—otherwise the parts may move around, causing problems