Trial Period or Updates Expiring? Email Trial ID to Support

Thank you for testing MillMage!

Release Candidate users who see a "Your trial period has expired" notice when opening MillMage can request an extension to the update period by emailing the MillMage Trial ID to the Support team.

Find your Trial ID in the License Management window. Email your Trial ID to [email protected] to start your request. The duration of the extended update period may vary.

Warning

The current version of MillMage is a Release Candidate — a stable version of software that is nearly ready for official release, but in need of additional public testing. Please report any unexpected behavior in the MillMage Software Questions section of our forum, including screenshots and as much detail as possible. Ask hardware compatibility questions in the MillMage Hardware Compatibility section.

Users new to MillMage should follow the Getting Started guide.

Video: How to Use a Release Candidate

This video features our sister software, LightBurn. While there may be slight differences in appearance and layout, the demonstrated processes are similar in MillMage.

Warning

This documentation is in active development and in a prerelease state. These documents are not complete and may include missing pages, broken links, and placeholders. Content is being updated as feedback is reviewed. Your patience is appreciated.

Bore

Bore operations tell your router to cut out the interior of a circular shape. They're a specialized form of Profile operation, and only work on circles or shapes that are recognized as circles by MillMage.

Bore Operations & Circles¶

The Bore operation will only work with circles. If you do apply a bore operation to a shape that isn't a circle, you will see the following warning when you try to preview or cut.

Bore operation warning screenshot — The bore operation 'Bore' contains one or more non-circle shapes, they will not be included. Do you wish to continue?

Select Yes if you want to continue with Previewing or cutting the operation. Select No if you want to go back and make changes

Identifying Circles¶

Circles (ellipses with equal witdth and height) will always be recognized as circles. In addition, MillMage will recognize the following as circles, assuming all nodes are the same distance from the center:

Paths that take the shape of a circle, whether or not they have extra nodes added.
Regular polygons with at least 16 sides.

Bore Mode Settings¶

Click any option in the image below to jump directly to the relevant section for that option, or scroll down for a list of options and descriptions.

Sections that have special settings for Bore operations are listed just below, while common settings that apply similarly to most or all other types of operations are listed toward the bottom.

Note

For information on options that are unique to other types of operations, see Other Operations, below.

Clearing Pattern¶

Cut Direction¶

Controls the direction your router will move while carving.

Conventional milling moves the router against the rotation of the spindle.
Climb milling moves the router in the same direction as the spindle rotates.

Cut Preview¶

The Cut Preview depicts the movement of the router and rotation of the spindle relative to the material, as determined by your current Cut Direction selection.

Conventional
Climb

Stock to Leave¶

Enter a value here to tell your router to leave a given amount of material uncarved.

Applying a Stock to Leave value is useful for roughing passes that will be followed up by a finishing pass that clears the remaining stock.

For Bore operations, this will shift the toolpath inward from the selected shape.

Depths and Entry¶

Equation Support and Automatic Unit Conversion

The Depths and Entry/Steps fields in the Operation Settings Editor support equations and automatic unit conversion.

For example:

To cut to a final depth of ¼ in, type 1/4 in the Diameter field, then click in another field, and MillMage will convert to the value to 0.75.

Addition (+), subtraction (-), and multiplication (*), are all also supported.
If your display units are set to metric but you've taken measurements in imperial, you can enter 1/4 in and MillMage will convert the value to 6.350 mm. This works in reverse as well, converting metric units to imperial

Multiple notations are supported, including ft, ', ", and mm.

Start Depth¶

The depth, relative to the surface of your stock, at which the operation will begin carving or cutting.

A value of 0 means it will begin at the top of your material — any value greater than 0 will tell your router to begin carving below the surface of the material.

Final Depth¶

The depth, relative to the surface of your stock, at which the operation will stop carving or cutting.

Final Depth is the total depth of the material that will be removed from your stock.

Depth Per Rev¶

Specifies the depth of material to be cleared with each pass around the circle.

Common Settings¶

Click here for information on settings that apply similarly to all types of operations

Name¶

Use this field to edit the display name of the operation in the Operations Window. By default, all operations will be named according to their type.

Paint Color¶

Click the Paint Color button to open the Select Color window, which controls the color by which the operation will be indicated in the Preview window, if Show paint colors is enabled.

You can choose from a number of Basic Colors presented at the top left of the window, or create a custom color.

To create a custom color:

Press Pick Screen Color to hover your cursor over any color on your screen. Click to select the color you're hovering over.
Use the color gradient and shading slider at the top right.
Adjust numeric or hexidecimal values at the bottom right to create a custom color.
After creating a custom color, click Add to Custom Colors to save it for future use.

Click OK to apply the color to your operation, or Cancel to exit the window thout applying the color.

Output¶

Controls whether the operation will be sent to your CNC when you Preview your project, press the Start button in the Job Control Window, or save your project in GCode format.

Auto Use Layer¶

Enable this switch to automatically apply this operation to all shapes set to a given layer. Designate the layer by clicking the button to the right of the switch.

Note

When Auto Use Layer is enabled, you can still Assign Operations to graphics set to any other layer, as normal, but all graphics assigned to the chosen layer will also have the Operation applied to them.

Tool Setup¶

Select Tool¶

Press the Select Tool button to open your Tool Library and select a tool to assign to the operation.

MillMage will automatically filter for appropriate tools for the type of operation you've selected. Some operations require specific tool geometries — if a tool's geometry is not appropriate for the type of operation you've selected, it will be unlisted and not selectable.

Tool Information¶

The remaining fields in this section display information about your selected tool, as entered in the Tool Library.

Tool Name¶

The name you gave the chosen tool in the Tool Library.

Diameter¶

The diameter of the cutting edge of your tool.

Cut Length¶

The length of the cutting edge of the chosen tool, from the top to the bottom of all flutes.

# of Flutes¶

The number of flutes on the chosen tool.

Feeds and Speeds¶

The Feeds and Speeds saved to a given tool from your Tool Library are automatically entered in the Operation Settings Editor when you select that tool.

To enter speeds in units other than what's set in Device Settings, enter the measurement including in/" or mm to specify the units you want. MillMage will automatically convert to the appropriate units as shown in the example below.

What Feeds and Speeds should I use?

The proper Feed and Speed settings depend on your tool, machine, material, and use case. In short: there's no easy answer to that question.

For specific recommendations, the best resource is usually the manufacturer of your machine or tool.

Feed Rate¶

Controls the speed at which your CNC will move laterally (along the X and Y axes) during operations.

Ramp Rate¶

Controls the speed at which your CNC will move vertically (along the Z Axis) during ramp movements.

Spindle Speed¶

Controls the speed at which your router will rotate your tool.

Note

Not all CNCs allow Spindle Speed control through software. Some have routers which must be adjusted manually.

Plunge¶

Controls the speed at which your CNC will move vertically (along the Z Axis) during plunge movements.

Chip Load¶

The Chip Load calculation shows the thickness of material removed by each cutting edge of a tool, during a single revolution of the spindle.

Chip Load = Feed Rate / (Spindle Speed (RPM) x # of Flutes)

The optimal Chip Load varies according to your tool and material. For specific recommendations, the best resource is usually the manufacturer of your machine or tool.

Excessively low Chip Loads produce dust, wear out bits more quickly, and risk overheating the tool and burning the edges of cuts. Excessively high Chip Loads produce chips that clear inefficiently, and may overstress and break the bit.

Vacuum and Coolant¶

Enable Vacuum¶

Enable this setting to automatically turn on your vacuum system when this operation begins.

This option requires a vacuum system that is connected to your CNC's controller.

See Controlling Vacuum Accessories With Custom GCode for more information.

Enable Coolant¶

Enable this setting to automatically turn on your coolant system when this operation begins.

This option requires a coolant system that is connected to your CNC's controller.

See Controlling Coolant Accessories With Custom GCode for more information.

Other Operations¶

All types of operations are listed below. Select an operation to learn more about the settings available for that type of operation.

Pocket

Tells your router to carve the entire area inside the outline of a single closed shape, or between the outlines of multiple closed shapes that are set within one another.

Rest Pocket

Tells your router to carve only the space within a single closed shape, or between outlines of multiple closed shapes that are set within one another, that a larger Clearing tool could not reach in a previous Pocket operation.

Profile

Tells your router to carve a path along the outlines of geometry in your project.

Chamfer Profile

Tells your router to carve angled edges along the outlines of closed shapes in your project. This operation require use of a V-Bit.

Dogbone Slot

A special type of operation that works similarly to Profile mode, but adjusts the geometry of your shapes to allow interlocking CNCed parts to fit together.

Drill

Tells your router to carve directly down, at the center of the shape the Drill operation is assigned to.

Inlay Female

A special type of operation that works similarly to Pocket mode, but adjusts the geometry of your shape to be slightly larger, to allow fitted inlays to fit more easily.

Inlay Male

A special type of operation that works similarly to Profile mode, but adjusts the geometry of your shape to be smaller, to allow fitted inlays to fit more easily.

Surfacing

A special type of Pocket operation used for leveling your CNC's work table.

Bore

A special type of Profile operation used for making holes in your parts.

For more help using MillMage, please visit our forum to talk with MillMage staff and users, or email support.