Why is my CNC cutting in the wrong position or wrong depth, and how do I troubleshoot Aspire-to-machine errors?

Overview

The CNC is cutting in the wrong place, at the wrong depth, or the design is offset from where it should be. These are among the most panicked questions on the software maker's user forum, but every case has a specific, diagnosable cause. There are four main categories: Z depth errors, XY position errors, scale errors, and mirrored or rotated results.

Z Depth Errors (Cuts Too Deep or Too Shallow)

Cuts exactly [material thickness] too deep

Cause: Z Zero mismatch. The software is set to "Machine Bed" but the machine was zeroed from the material top (or vice versa).

Fix: Match Z Zero in Job Setup to how you physically zeroed the machine. Use Material Surface for V-carving and relief work.

Cuts slightly deeper than designed (0.02 to 0.1")

Cause: The material is thicker than the Thickness value entered in Job Setup.

Fix: Measure the actual material with calipers. Real 3/4" plywood is typically 0.700 to 0.720". Enter the measured value, not the nominal.

Cuts shallower than designed, or does not cut through on profile passes

Cause: The material is thinner than specified, or Z Zero was set slightly above the material surface.

Fix: Re-measure the material and re-zero Z. To make sure the profile goes all the way through, set the Cut Depth slightly deeper than the measured thickness. In the Cut Depth box you can type a calculation using the letter Z or T for the material thickness, for example z+0.02=, and press the = key to evaluate it.

Do not use a negative Allowance for this. The Allowance on a profile toolpath is a sideways (XY) offset from the vector, not a depth. A negative allowance cuts the part smaller on every edge and does nothing for depth.

XY Position Errors (Cuts in Wrong Location)

Design is offset from the correct position by a consistent amount

Cause 1: The XY Datum position in the software does not match where you set X=0, Y=0 on the machine.

Fix: In Job Setup, set the XY Datum (the red square that shows the origin position) to match exactly where you physically set machine X=0, Y=0. Lower-left is most common.

Cause 2: The design was not centered on the job, or was created at a different position than expected.

Fix: Use Center on Job (Align tools) to reposition the design, then recalculate toolpaths.

Design cuts in the correct area but each pass shifts slightly (backlash)

Cause: Mechanical backlash in the machine's X or Y axis. The axis "slips" after reversing direction.

Fix: This is a machine hardware issue, not a software issue. Check drive belt tension, set screw tightness, and anti-backlash nuts. Consult your machine manufacturer.

Design cuts at the correct position but is mirrored

Cause: The machine's Y axis (or X axis) runs the opposite direction from what the software assumes, through hardware wiring, controller setup or post-processor setup.

Fix: Check the hardware wiring and controller axis directions first. If the machine itself cannot be corrected, a post-processor setting may be able to compensate, but that is only recommended if you are confident in your machine configuration. A wrong datum corner shifts the job but does not mirror it.

Scale Errors (Design Cuts at Wrong Size)

Design cuts at 25.4 times the correct size (or 1/25.4 of it)

Cause: The post-processor units do not match the units your controller runs in. For example, the controller expects inches but the file is output in mm, or vice versa.

Fix: Jog the machine from X=0 to X=1. If it moves 1 inch, use an Inch post-processor. If it moves 1 mm, use a mm post-processor. The post-processor must match the controller, not the job. The job can be drawn in either unit, and the software converts when the toolpath is saved.

Design cuts at approximately correct size but slightly off

Cause: Machine calibration error. Steps/mm (or steps/inch) is not set correctly in the machine controller.

Test: Command the machine to move exactly 10.000" in X. Measure the actual movement with a digital caliper.

• If it moves 9.9": steps/inch too low, so increase steps/inch by about 1%
• If it moves 10.1": steps/inch too high, so decrease by about 1%

Fix: Adjust steps per unit in your machine controller (Mach3, Grbl, Centroid, etc.). This is a machine calibration issue, not a software issue.

Orientation Errors (Rotated Output)

Design cuts rotated 90 degrees

Cause: The machine's XY axis orientation does not match the software's assumption. Some machines have X as the long axis, others have Y as the long axis.

Fix: Either rotate the design 90 degrees before saving toolpaths, or change which axis of the machine is wired as X vs Y in the controller firmware.

Design cuts correctly but on the wrong side of center

Cause: XY Datum mismatch. The design was set up with a center origin but the machine was zeroed at a corner (or vice versa).

Fix: Match the origin position exactly. Set the center origin in Job Setup AND zero the machine at the center of the material.

Pre-Cut Verification Checklist

Before any cut, verify:

1. Post-processor: the correct one selected for your machine?
2. Units: do the post-processor units match the units your controller runs in?
3. Z Zero: Material Surface or Machine Bed? Does it match how you will zero on the machine?
4. XY Datum: which corner is 0,0 in the software? Does it match where you will zero on the machine?
5. Toolpath Preview: does the 3D simulation look correct BEFORE cutting?
6. Air cut first: run the file with the spindle off and Z raised 0.5" to verify XY motion without cutting.
7. Material Thickness: measured with calipers, not nominal?