How to Use EstlCAM for CNC Routing: Toolpaths, G-Code, and GRBL Control

Introduction

EstlCAM is a free (for personal use) CAM program designed specifically for hobby CNC routers and mills. Unlike Fusion 360 CAM which requires cloud processing and subscription fees, or Vectric which costs hundreds of dollars, EstlCAM runs entirely offline on your PC with a one-time paid license option. It specializes in 2D and 2.5D toolpath generation with an intuitive workflow: import DXF or SVG, define tools, create toolpaths visually, and export G-code. This guide covers the complete EstlCAM workflow from setup through advanced strategies for engraving, pocketing, drilling, and 3D relief machining on desktop CNC routers like the WolfPawn 4040 Pro, Shapeoko, and LongMill.

What You Need

EstlCAM (download from estlcam.de)
CNC router with GRBL firmware
DXF or SVG files of your parts
End mills appropriate for your material
USB connection to your CNC controller

Step 1: Installation and Setup

Download EstlCAM from estlcam.de (Windows only, but runs on Linux via Wine).
Install and launch.
On first run, configure your CNC machine:

Setup > CNC Program Settings:

Machine Type: GRBL
Post Processor: GRBL (mm)
Feed Units: mm/min
Clearance Plane: 5 mm (safe travel height above the workpiece)
Tool Change Position: X0, Y0, Z20 (where the machine moves for tool changes)
Rapid Feed: 5000 mm/min (your machine's max rapid speed)
Work Area: Set X and Y to your machine's travel (e.g., 400x400 mm for WolfPawn)

Step 2: Import Your Design

EstlCAM imports 2D profiles from DXF and SVG files.

File > Open > Select your .dxf or .svg
The design appears on the canvas
Use the zoom and pan tools to inspect the import

Common import issues and fixes:

Wrong scale: The import dialog shows units. If your DXF was in inches, select inches. EstlCAM converts to mm automatically.
Open contours: EstlCAM highlights open paths in red. Close them in your CAD program (Inkscape, LibreCAD) before importing.
Duplicate lines: These cause double-cutting. EstlCAM has a cleanup tool: Edit > Remove Duplicates.
Too many nodes: Complex curves with hundreds of nodes slow down toolpath calculation. Simplify in your CAD program first.

Step 3: Define Your Tool Library

EstlCAM manages tools in a library that you build over time.

Click the Tool button (looks like an end mill icon).
Click New to add a tool.
Enter tool parameters:

Name: "1/8 End Mill"
Type: End Mill (or V-bit, Ball Nose, Drill)
Diameter: 3.175 mm (for 1/8 inch end mill)
Cutting Length: 17 mm (flute length)
Number of Flutes: 2 (or 1 for plastics, 3-4 for metals)
Max RPM: 24000 (your spindle max)
Feed Rate: 1200 mm/min (starting point for wood)
Plunge Rate: 600 mm/min (half the feed rate)
Depth of Cut per Pass: 1.5 mm (conservative for 1/8 inch in wood)
Stepover: 40% of diameter (1.27 mm for 3.175 mm tool)

Suggested starting tool library:

1/8 inch (3.175 mm) 2-flute end mill — general purpose
1/4 inch (6.35 mm) 2-flute end mill — fast material removal
1/16 inch (1.5875 mm) 2-flute end mill — fine detail
60-degree V-bit — engraving
90-degree V-bit — larger engravings
3.175 mm ball nose — 3D contours
Drill bits (1-6 mm set) — drilling operations

Step 4: Create Toolpaths

EstlCAM creates toolpaths by selecting geometry and applying operations. Click an element (line, arc, circle), then choose the operation type.

1. Engraving (Part > Text or Line Engraving)

Select the lines or text you want to engrave.
Click Engrave.
Settings:

Tool: Select your engraving tool (V-bit or small end mill)
Depth: 0.2-0.5 mm for light engraving, 1-2 mm for deep engraving
Strategy: On the line (centered) or Left/Right of the line

2. Profile/Contour Cutting (Part > Contour)

Select the outer contour of your part.
Click Contour (the button with a profile icon).
Settings:

Tool: End mill
Cutting Depth: Full depth of material (e.g., 6 mm for 6 mm plywood)
Direction: Conventional or Climb milling. Climb produces cleaner edges on rigid machines.
Tabs: Enable tabs for through-cuts. Set tab width (3 mm) and height (material thickness - 0.5 mm). Tabs hold the part in place until you cut them free.
Multiple Passes: Enable to cut in multiple depth passes. Set Z step per pass (1-2 mm).

3. Pocketing (Part > Pocket)

Select a closed contour (the area to be cleared).
Click Pocket.
Settings:

Tool: Largest end mill that fits in the pocket
Max Depth: How deep to pocket
Stepover: 40-50% of tool diameter
Strategy: Zigzag (fastest) or Spiral (better finish)
Multiple Passes: Enable with Z step per pass

4. Drilling (Hole > Drill)

Select circles (holes).
Click Drill.
Settings:

Tool: Drill bit matching the hole diameter
Depth: Through (material thickness) or specific depth
Peck Depth: How deep each peck goes (0.5-1 mm for soft material, 0.2 mm for hard)
Dwell: Pause at bottom (0.2 seconds to break chips)

5. Thread Milling (Hole > Thread)

Select a hole.
Click Thread.
Select thread standard (M3, M4, M5, UNC, etc.).
EstlCAM generates a helical toolpath that cuts threads.

6. 3D Relief (3D > Relief)

For 3D surfaces:

Import a heightmap (grayscale image where white = high, black = low) or an STL.
Click 3D Relief.
Settings:

Tool: Ball nose end mill
Stepover: 10-20% of tool diameter for fine detail
Strategy: Parallel (straight passes) or Spiral (circular from center)

Step 5: Set Up Stock Material

Click Setup (the gear icon).
Set Material:

Dimensions: Width, Depth (X, Y), Thickness (Z)
Position: Set the workpiece origin (usually bottom-left corner, top surface)

Set the Workpiece Origin:

X0, Y0: Typically the bottom-left corner of your stock
Z0: The top surface of the material (or the spoilboard if using bottom-Z)

Step 6: Simulate and Verify

Click Simulation (the play icon).
EstlCAM runs a visual simulation of the complete G-code.
Watch for:

Tool crashes into clamps or fixtures
Wrong cutting depths
Uncut areas (pockets that are not fully cleared)
Rapid moves through the material (bad clearance plane)

Use the slider to scrub through the simulation.
Check the estimated machining time at the bottom.

Step 7: Save Toolpaths and Export G-Code

File > Save Toolpaths
Select the operations to export
File > Save CNC Program
EstlCAM generates the G-code file
The G-code is saved as a .nc file

Direct GRBL control (optional):

EstlCAM can control GRBL machines directly via USB:

Connect your CNC to the PC via USB.
Select the correct COM port in EstlCAM.
Click Connect.
Use the jog controls to position the machine.
Zero the axes (set work coordinate origin).
Click Start to run the program directly from EstlCAM.

Step 8: Advanced Strategies

Trochoidal Milling (for deep pockets and slots):

Trochoidal toolpaths use circular milling motions instead of straight plunges, reducing tool load and enabling deeper cuts:

Select a pocket or slot.
Click Pocket.
In the strategy settings, enable Trochoidal.
Set the step width (0.5-1 mm) and arc diameter (5-10 mm).
This lets you cut slots up to 3x the tool diameter in width with a single tool.

Adaptive Clearing (for aggressive material removal):

Select a large pocket.
Use a large end mill (1/4 inch or 6 mm).
Set a deep depth of cut (up to 1x tool diameter).
Set moderate feed rate and high RPM.
Use climb milling for chip evacuation.

V-Carving (for signage and decorative work):

Import text or line art as DXF.
Select the vectors.
Click Engrave with a V-bit selected.
EstlCAM calculates the depth based on line width: narrow lines = shallow, wide lines = deep.
This creates dimensional lettering and artwork with a single tool.

Inlay Cutting (for decorative inlays):

Create a pocket toolpath for the female (recessed) part.
Create a contour toolpath for the male (insert) part with slight oversize.
Cut the female part from the base material.
Cut the male part from the inlay material.
Glue the insert into the recess.

Tips for EstlCAM Success

Start conservative. Use shallow depths and slow feeds on your first attempt with a new material. Increase gradually.
Use tabs for through-cuts. Parts will fly off the bed if not held. Set tab width to 3-5 mm.
Verify with simulation. Always watch the full simulation before running G-code on the machine.
Save the project file (.ecp). This stores the toolpaths and settings. You can regenerate G-code without re-doing the CAM.
Use the largest tool possible. A 1/4 inch end mill removes material 4x faster than a 1/8 inch end mill.
Organize toolpaths by tool. Do all operations with one tool, then change tools. Minimizes tool changes.
Zero Z on the top surface. This is the most common approach. Use a Z-probe or paper method.
Preview the G-code in another simulator. Open the saved .nc in NCViewer.com or CAMotics for a second opinion.

Conclusion

EstlCAM is the ideal CAM program for hobby CNC routers. The workflow of import DXF > select geometry > choose operation > set tool > simulate > export G-code is intuitive and fast. The built-in tool library, visual toolpath creation, simulation, and direct GRBL control eliminate the complexity of industrial CAM software. For 2D cutting, pocketing, drilling, V-carving, and 3D relief work on desktop CNC machines, EstlCAM provides everything needed at a price point — free for personal use — that makes it accessible to every maker. Master the contour, pocket, drill, and engrave operations and you can machine any 2.5D part your CNC can handle.

Related Guides

Loading_