SheetCam Quick‑Start: Load a File → Create Toolpaths → Generate G‑Code for CommandCNC

A friendly, repeatable workflow for new operators. Plasma‑focused; router notes included.

Before you start

• Launch the right profile so the correct Machine & Post load automatically.

  • Windows: your shortcut like SheetCam TNG.exe -c Plasma or -c Rotary.

  • Linux: launcher Exec=/opt/SheetCamTNG -c Plasma (or your path).

• Have your drawing ready (DXF/SVG/DWG). Keep geometry clean, closed, and layered.

• Know your material (type & thickness) and have a matching tool set up (kerf, feed, pierce, heights).

1. Create/confirm the Job setup

1. File → New job (or open an existing job if you use templates).

2. Options → Job options

   • Size: set your working area for preview/layout.

   • Thickness of Material: pick type/thickness if you track it here.

   • Origin: usually lower‑left (X0,Y0). Adjust if your shop prefers another corner.

   • Rapid Clearance: set a sensible rapid height over clamps/warp.

   • Click OK.

   

    

2. Import your drawing

1. File → Import drawing… (DXF/SVG/…)

2. In the import dialog:

   • Scaling: match the file’s units to avoid scale surprises.

   • Drawing position: Center on table or Lower‑left as you prefer.

3. Click Open. You should see the part on the table.

Quick checks:

• If the part is microscopic/huge → unit mismatch. Re‑import with correct units.

• If lines don’t connect → fix in CAD or use SheetCam tools (next step).

3. Create the Operation (Plasma Cut)

1. Operations → New operation → Plasma Cut.

2. In the operation dialog:

   • Contour method: usually Outside for outer profiles, Inside for holes/slots, No Offset for marking. 

      

   • Layer: Select the layer you want to cut with this tool.

   • Tool: choose the tool for your material.

   • Leads: pick Lead‑in shape (arc or straight) & length (often 1–1.5× kerf). Optional Lead‑out.

   • Cut direction: CW/CCW as needed (inside features often CW for right‑hand torch swirl; follow your charts/post).

   • Rules: (optional) add small hole rule to slow feed or disable THC below a diameter.

3. OK. You’ll see red arrows/leads indicating entry points.

Tip: Use multiple operations if different layers or features need different tools/speeds (e.g., marking vs cutting; small holes vs perimeter).

4. Refine start points, leads & order

• Start points: Mode → Edit start points then click a contour to move its pierce point to a better location (avoid corners, tight pockets, aesthetic faces).

• Leads per feature: right‑click a contour to override default lead length/type.

• Cut order:

  • Inside features (holes/slots) before outside profiles.

  • Operations → Move up/down to reorder, or use Automatic ordering and then tweak.

  • Enable Cut small parts last to reduce tip‑ups.

Router note: add Tabs/bridges in the operation so parts don’t move. Place tabs on straight runs, not corners.

5. Simulate & sanity‑check

• View → Show simulation (or the simulation/play icon).

• Watch for:

  • Leads piercing into adjacent parts.

  • Missed holes (open contours won’t cut).

  • Z moves clearing clamps (check Safe Z).

  • Reasonable total time & number of pierces.

• Fix issues by adjusting start points, leads, or operation order and re‑sim.

6. Post the G‑code

1. Click Post process (the G‑code icon) or File → Post process.

2. Confirm the Post (should match your machine via profile/Machine).

3. Choose an output filename and folder (your machine’s “Drop” folder if you use network transfer).

4. Click Save. SheetCam writes the NC file and usually opens it in the Code window.

Final checks:

• First lines show the post name & units.

• Skim the pierce count vs expected.

• Transfer to your controller (USB/network) and run your shop’s dry‑run routine.

7. Save for reuse

• File → Save job as… to keep your part, operations, and settings together.

• Consider a template job with table/material defaults to start future parts quickly.

Common mistakes & quick fixes

• Part wrong size: Re‑import with correct units.

• Holes not cutting: Contour is open—heal in CAD or use Join with a small tolerance.

• Torch diving / rough cut on small holes: Add a small‑feature rule to reduce speed and/or disable THC for holes under a threshold.

• Lead pierces a finished face: Move start point to a hidden edge; use Lead‑out off where needed.

• Warp hits: Increase Lead‑in length, raise Clearance/Safe Z, or cut small parts later in the sequence.

• Router parts fly loose: Add tabs, increase tab thickness/length, cut internals before externals.

Handy tools & views

• Mode → Show intersections to spot bad geometry.

• View → Show rapids / Show leads to verify motion.

• Operations list: toggle eye icons to enable/disable operations during testing.

Appendix A: Simple profile setup (so the right Post loads every time)

• Create two launchers:

  • Windows: "C:\\Program Files (x86)\\SheetCam TNG\\SheetCam TNG.exe" -c Plasma and -c Rotary.

  • Linux .desktop Exec: /opt/SheetCamTNG -c Plasma and -c Rotary.

• Launch each once, go Options → Machine → Load machine…, pick the correct machine, OK, then close to save. From now on, just click the right launcher.

Router differences (at a glance)

• Tool: endmill/bit with diameter, step‑down, RPM, feed & plunge.

• Operation: Contour with Tabs; use multiple passes (step‑down) for thick stock.

• Hold‑down: confirm clamps/fixturing; plan clearance accordingly.

You’re set. Run this checklist for a week and it becomes muscle memory.