MeshCAM Day 3 - 2D Machining

(NOTE: This tutorial is for MeshCAM V9, if you’re looking for V8, click here )

MeshCAM has become increasingly popular for plain 2D machining. Normally, this is not the recomended application for a 3D CAM program but MeshCAM has a number of features to make this very easy.

We’re going to cut and iPhone stand from a 2D DXF file. If you choose to follow along, you can download the DXF file here

1. Load the File

Loading a 2D file in MeshCAM is slightly different from a 3D file as you’ve probably done up to now.

• From the top menu, click File->Open
• Select the Stand.dxf file that you downloaded above
• In the popup, select File is Inch.

When loading a DXF file, MeshCAM must be told what thickness to use since DXF files do not contain this information

• When propted for a thickness, enter .125 inches (If you’re using metric units, you can enter 3mm)
• Click Ok

You can now use the mouse to move the 3D view and inspect the file.

2. Modify the Stock

By default, MeshCAM sets the stock dimensions to the exact dimensions of the geometry and will keep the center of the tool within that boundary. In this case, we need to enlarge the stock so MeshCAM has room to move the tool all the way around the geometry.

• From the top menu, click CAM->Define Stock
• Under XY Position, enter .125 for all of the Front/Back/Left/Right margin values
• Click OK

In the 3D view, the white box representing the stock value will now enlarge by .125 inches on every side.

3. Create a Tool

MeshCAM needs to know what tool you plan on using to cut the geometry so it can properly calculate a toolpath.

• In the top left side of the window, click Setup
• Click List Tools

• Click Add to add a new tool

• Copy the settings shown above.
• Click OK
• Close the tool list window

4. Global Settings

The global settings part of the toolpath dialog defines a few items that affect every toolpath that is generated.

• On the left hand side of the screen, click on the Tolerance value
• Enter a tolerance value of .001 in
• On the left hand side of the screen, click on the Area to Machine value
• Click Geometry Only
• On the left hand side of the screen, click on the Distance Around Geometry value
• Enter a value of .25 in

5. Create a Toolpath

From the top menu, click the "Toolpaths->Cutout" button.

• Click Select Tool
• Double click on the #101, .025in End tool that you created at the start of this tutorial

Note that the speeds and feeds will automatically be set based on the machine and the material you have selected. These are just a starting point and you’re free to change them if you’d like.

• Click OK

6. Generate Toolpaths

You’ll now see your toolpath listed on the left pane of the app.

• Click Calculate Toolpaths to create the toolpaths

7. Preview the Toolpath

Once the toolpath apprears in the 3D window, you can shift the view to get a closer look at any area you want to see in more detail. The waterline toolpath is shown as a series of yellow lines, the pencil toolpaths are in purple.

8. Save the GCode

MeshCAM comes with a bunch of post processors that tell it how to format the gcode for your machine controller. When saving the file, it’s important to pick the right post processor for your machine. If you have any doubts, pick Basic-Gcode or Mach3. Both are fairly generic and work with most machines.

• Click Save Toolpath
• Pick the correct post processor in the Save as type drop down menu.
• Enter a filename
• Click Save
• Go load the gcode into your machine!