How do I set up a new job in VCarve Pro & Aspire: Job Type, Job Size, Z Zero Position, and XY Datum explained?

Overview

Job Setup is the first form you see when creating a new project (File > New). Every setting here has direct consequences for how your toolpaths are calculated and how your machine behaves. Getting these right before you start designing saves you from having to redo work later. The same form reopens for an existing job through Edit > Job Size and Position. This covers the fields in the 12.5 Job Setup form for VCarve Pro and Aspire.

---

Job Type

Three options. Choose before you do anything else, because this affects everything downstream.

Single Sided

The default. Your design is cut from one side of the material only. The CNC machines the top face, and the bottom is the spoilboard-facing side that stays flat.

• Use for: Signs, plaques, wall art, decorative panels, most standard CNC work
• Simple, no registration required

Double Sided

Design and machine both sides of the material. You create separate designs for Top and Bottom, then flip the material on the CNC.

• Use for: Thick carvings (bears, fish, figures) that need detail on both sides, double-sided signs, furniture components with detail on front and back
• Requires a flip jig or alignment pins to register the material accurately after flipping
• Switching sides: use the Top and Bottom icons on the View toolbar above the 2D view

Rotary

Designs are wrapped around a cylindrical blank. The rotary axis of the CNC turns the material while the other axes carve.

• Use for: Columns, balusters, barley twists, fluted spindles, engraved cylinders, round signs
• Requires a CNC with a rotary axis
• The software calculates toolpaths in flat XY space and wraps them around the cylinder using a post-processor set up for wrapping. It does not do true 4-axis machining.
• Job dimensions: the form asks for the Length and Diameter of the material. With the rotary axis along X, Length runs along X and Diameter takes the place of the job Height (Y).

---

Job Size

Width (X)

The dimension of the material along the X axis (left-right on the machine).

Height (Y)

The dimension of the material along the Y axis (front-back on the machine).

Thickness (Z)

The full thickness of the material stock. This is the total material height, not the carving depth. The software uses this to:

• Display the material block correctly in the 3D preview
• Calculate safe Z travel heights (rapid height above material)
• Determine how deep toolpaths can go before hitting the spoilboard

Pro tip on job size: Set the job size to match your MODEL dimensions, not your full machine bed. The 3D modeling resolution is spread across the whole job area, so a smaller job area gives more resolution per square inch and much better 3D detail. If your sign is 12" x 8", set the job to 12" x 8" even if your machine can cut 48" x 96".

---

Units

Inches is standard for North American shops. All dimensions, feeds and depths are in inches.

mm is for metric users and metric-calibrated machines.

Units can be changed later in Edit > Job Size and Position.

Important: The post-processor must match the units your controller runs in, not the units of the job. The job can be drawn in either unit, and the software converts when the toolpath file is saved.

---

Z Zero Position

This is one of the most critical settings. It must exactly match how you touch off and zero your machine's Z axis.

Material Surface (recommended for most users)

Z=0 is at the top face of the material. The tool touches the top surface of the material, you zero Z there, and all depth calculations go downward from that point.

• Advantage: Consistent depth regardless of material thickness variation. Even if your material is slightly thinner or thicker than specified, your carving depth stays correct relative to the surface.
• Most common setting. Use this unless you have a specific reason not to.
• How to zero on the machine: Lower the tool to touch the material surface and set Z=0 at that point

Machine Bed

Z=0 is at the machine table or spoilboard surface. All Z depths are measured from the bottom of the material.

• Advantage: Useful for through-cuts. The profile cut depth is exactly the material thickness, so you cut all the way through regardless of surface variations.
• Disadvantage: If the material thickness varies (which it always does slightly), your carve depth relative to the surface varies too.
• How to zero on the machine: Lower the tool to touch the spoilboard or table and set Z=0 there
• Use when: Doing precision joinery where bottom registration matters, or when your machine has a fixed table reference

The mistake beginners make: Setting Z Zero to Material Surface in the software but zeroing the machine from the spoilboard (or vice versa). This causes all Z depths to be off by exactly the material thickness. Always match these two.

---

XY Datum Position

This sets where X=0, Y=0 is on the material. The datum can be set at any corner or the middle of the job, so there are five positions: the four corners and the center. A red square is drawn in the 2D view while the form is open to show the selected position.

Common choices

• Lower-left corner: Most common. Machine X=0, Y=0 is at the lower-left corner of the material. Intuitive for most gantry CNC setups.
• Center: Useful for symmetrical designs, rotary work, or when your machine zeros at center of travel
• Other corners: Match whatever your machine and fixture setup requires

The golden rule: The XY datum position in Job Setup must exactly match where you physically place X=0, Y=0 on your machine for every job. Inconsistency here shifts your entire design relative to the material.

Use Offset

Allows the datum position to be set to a value other than X0, Y0. Used when your material is not at the absolute machine zero, or when you are referencing from a fixed point that is not the corner of the stock.

---

Design Scaling

Design Scaling option, which matters when you edit the Job Size of an existing job:

• Checked: If you later change Width or Height in Job Setup, your drawings are re-sized to stay in the same proportion and relative position within the new material extents
• Unchecked: Your drawings keep their existing size even after the job size changes

Leave it unchecked unless you specifically need to resize your design by resizing the job.

---

Modeling Resolution

This sets the quality of the 3D model. Standard (fastest) is acceptable for most parts. High (3 times slower) and Highest (7 times slower) are for large parts with small details. The better the resolution, the slower the computer works, and the resolution is applied across the whole job area. See the Modeling Resolution entry for more detail.

---

The Correct Order to Fill Out Job Setup

1. Choose Job Type first (Single Sided / Double Sided / Rotary)
2. Set Units (inches or mm)
3. Set Width and Height to match your material (or model size if optimizing for resolution)
4. Set Thickness to your actual, measured stock thickness
5. Set Z Zero Position to match exactly how you will zero your machine
6. Set XY Datum Position to match exactly where you will place machine X=0, Y=0
7. Set Modeling Resolution appropriate for your job size and detail requirements
8. Click OK to create the job