MeshCAM Day 2 - Image Machining

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

Yesterday you got a walkthough of the most common MeshCAM workflow, machining a 3D STL file. Today we’ll look at something a little non-traditional: machining an image file.

If you choose to follow along, you can download the PNG file or get it as a ZIP file.

1. Load the File

From the top menu, click File->Open
Select the image file that you downloaded above and click OK
In the Image Settings dialog, uncheck Allow Resize
Under Pixels/inch, enter 300.
For the Z Size, enter .1
In the Height Mapping section, click Black is Z-

The 3D view now shows the image converted to a height map with the lighter parts of the image set at a higher Z level and the darker set to a lower Z level.

2. 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

3. Set Machine

MeshCAM has a number of machine configurations built-in to help calcualte starting values for speeds and feeds.

Click Setup->Set Machine
Click Shapeoko

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 Material value
Pick Wood - Hard
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

MeshCAM will attempt to pick sensible speeds and feeds for your project based on the machine and material you pick. It’s fine to pick your machine or something closer to your machine and material instead of Shapeoko and hard wood. Just be aware that if you do so, you’ll end up with different values for speeds and feeds below.

5. Create a Toolpath

Since this project is a low-relief, without a great deal of material to be removed, we have the option to skip the roughing toolpath. To be complete, we’ll include it here but it’s not always necessary.

From the top menu, click the Toolpaths->Roughing button.

Click Select Tool
Select the #1 Ball Mill that you created above
MeshCAM will fill in approximate speed and feed values based on the machine and material you’ve selected. Feel free to change these as necessary.
Set the “Options” section to match the image above.
Click Ok
From the top menu, click the Toolpaths->Parallel Finishing button.

Click Select Tool
Select the #1 Ball Mill that you created above
Set the “Options” section to match the image above.
Click Ok

6. Calculate Toolpaths

On the left pane you’ll see your roughing and finishing toolpaths listed.

Click Calculate 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 part for the geometry.

8. Save the G-Code

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
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!

Conclusion

You may have never considered using an image as the source for a CNC machining project but the feedback I’ve gotten over the years is that this is one of the most popular features in MeshCAM.

If you’re one of these people then you may want to open up your favorite image editor and see what you can come up with. As you play with it more you may think of projects that would take much longer to complete with a traditional CAD workflow.