Warning

MillMage is in active development and in a prerelease state. Many operations and functions are not feature complete. Please report any unexpected behavior by searching for and reporting the issue or question in the MillMage Beta User Forum. Please include screenshots and as much detail as possible.

Beta Users: Finding Help

Find help and download the latest release candidate of MillMage in the MillMage Beta User Forum.

Users new to MillMage should follow the Getting Started guide.

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.

Female Pocket

Female Pockets are a special type of Pocket operation that allow you to specify an Allowance value that increases the area to be carved by your router, without alterning the original geometry of your project.

Slightly increasing the size of the carved area allows you to more easily inlay fitted parts into the pocket.

You can use Male Inlay operations in conjunction with Female Pockets to create parts that fit together snugly but without difficulty.

As with standard Pockets, Female Pocket operations tell your router to clear an area that falls within the outlines of designated vector graphics.

If a single vector graphic is assigned to a Female Pocket operation, the entire area within that graphic will be cleared.

If multiple vector graphics are assigned to the same Female Pocket operation, and one of the graphics is inside another, the area between the outlines of both will be cleared instead.

MillMage will also adjust output intelligently, shifting the inner and outer paths in opposite directions, so the size of the final pocket is increased by the specified Allowance in both directions.

Open vs. Closed Shapes

Because MillMage must determine the inside and outside of a shape in order to determine the area to clear, Pocket mode only works with shapes that are closed. A shape is closed when it is a complete, continuous loop whose start and end points are the same. When a shape's start and end points are different, it is open.

See Open vs. Closed Shapes for more information on the difference between open and closed shapes.

Female Pocket 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 Female Pocket (and standard Pocket) 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¶

The dropdown menu in the Clearing Pattern section controls the type of path your router will take as it clears the area within your assigned shapes.

Offset¶

Select Offset to tell your router to carve concentric paths that follow the outline of the shape(s) assigned to the operation.

Raster¶

Select Raster to tell your router to carve parallel lines in a back-and-forth motion, within the outline of the shape(s) assigned to the operation.

Two additional options are available if you select Raster mode.

Raster Angle¶

Controls the angle of the back-and-forth movements your router will make across the shape(s) assigned to the operation.

Outline Pass¶

Select whether to add an additional pass along the edges of the carved area, following the contours of the shape(s), Before or After the Raster carving is completed. You can also select No Outline.

Without an Outline Pass, Raster carvings may have stepped or flattened edges.

Raster clear without an **Outline Pass**

A Raster pocket operation with an **Outline Pass** — Raster clear with an **Outline Pass**

Allowance¶

The amount by which to enlarge the pocketed area. Adjusting Allowance does not affect the size of the shapes in your Workspace, and is only applied when to your shapes when the project is saved in GCode format, or sent to your CNC.

Depths and Steps¶

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 Pass¶

Specifies the depth of material to be cleared with each pass of your router. The total number of passes is equal to Final Depth / Depths Per Pass.

For example, if you set Depth Per Pass to 1 mm, and Final Depth to 10 mm, your router will make 10 passes of 1 mm each.

Step Over¶

Step Over controls the distance between each path of your chosen clearing pattern. A larger Step Over leads to greater distance between each path.

Step Over (%)¶

Enter a percentage in the Step Over (%) field to apply a Step Over value as a percentage of your tool's diameter.

In other words, if your tool's diameter is 0.125", entering 50% in the Step Over (%) will set the Step Over value to 0.0625".

These values are linked in both directions — if you adjust the absolute value in the Step Over field, the value in the percentage field will change to indicate the Step Over value's percentage of your tool's diameter.

Entry Type¶

Entry Type controls the motion of your router as it lowers into your material down.

For Zig Zag Ramp and Plunge entries, the router lowers to the depth set in the Depth Per Pass, as it begins carving.

Plunge¶

Lowers the router straight-down along the Z Axis into the material, before the router moves in X or Y. The same Plunge movement is repeated as the router lowers for each subsequent pass.

Zig Zag Ramp¶

Lowers the router along the Z Axis into the material, while also making lateral movements along the X or Y axis, meaning the tool enters at an angle — the exact angle is determined by the Ramp Angle setting.

The same Zig Zag movement is repeated as the router lowers for each subsequent pass.

The router makes a straight down movement in Z before beginning the ramped entry.

Ramp Angle¶

Controls the angle at which your tool will enter the material, if you’ve selected Zig Zag Ramp as your Entry Type.

Step Over¶

Step Over controls the distance between each path of your chosen clearing pattern. A larger Step Over leads to greater distance between each path.

Step Over (%)¶

Enter a percentage in the Step Over (%) field to apply a Step Over value as a percentage of your tool's diameter.

In other words, if your tool's diameter is 0.125", entering 50% in the Step Over (%) will set the Step Over value to 0.0625".

These values are linked in both directions — if you adjust the absolute value in the Step Over field, the value in the percentage field will change to indicate the Step Over value's percentage of your tool's diameter.

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 User 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.

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 Rate¶

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

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.

Coolant and Vacuum¶

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.

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.

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

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.

Female Pocket

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.

Male Inlay

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.

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