Warning

This documentation is in active development. Content is being updated as feedback is reviewed. Your patience is appreciated.

Submit documentation feedback with the widget at the bottom-left of this window or by emailing [email protected].

Open a support ticket with the widget at the bottom-right or by emailing [email protected].

Texturing

Add depth to your backgrounds and embellishments to your designs with the Texturing operation. Texturing operations use a tool path that is a series of cutting moves that ramp in and out along the cutting raster path within the closed shape. Texturing options include adjusting the density, vector, depth, and lengths of cutting paths.

MillMage Pro Feature

If you are currently using MillMage with a Core license, head to Help → License Management and click the Trial Pro button to get access to all Pro features for two weeks.

Assigning Texturing Operations¶

Open vs. Closed Shapes

Similar to Pocket operations, Texturing 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.

Assign a closed shape to a Texturing operation to fill the shape with the texture paths. Include an additional enclosing shape to define specific areas for texturing.

Texturing Operation Settings¶

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

Sections that have special settings for Texturing operations are listed first, while common settings that apply similar to most or all other types of operations are listed toward the bottom.

Note

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

Clearing Pattern¶

Raster Angle¶

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

Stock to Leave¶

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

For Pocket operations, this will effectively shrink the size of the carved area inward by the amount you enter in the Stock to Leave field.

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.

Min Length¶

Specify the minimum length of each cutting segment. Each cut segment will be at least this long within the cutting path.

Max Length¶

Similar to Min Length, set a maximum length to each cutting segment.

Discard Below¶

Specify a segment length lower limit where the tool will skip spans smaller than that value and will then resume carving along the path. Texturing segments smaller than the Discard Below value are not cut and instead replaced with a travel move up out of the material to the Fast Retraction height and will move to the next texture segment along the same raster path.

Set the Discard Below value to zero to produce fully carved paths within the assigned closed shape.

Line Overlap (%)¶

Adjust the overlap of the beginning and ending entry points along the cutting path to make the entry cutting move occur over a previously carved area.

Offset Alternate Lines¶

Add increasing complexity to Line Overlaps by enabling offset Alternate Lines.

Ramp Style¶

Use the dropdown to set the ramp style to Linear, Fall, Arc, Ogee, or Smooth.

Linear

Carves into/out of the material along a straight path until it reaches the final depth.

Fall

Carves into/out of the material along a concave-curved path.

Arc

Carves into/out of the material along a convex-curved path.

Ogee

Carves into/out of the material along a concave curve at first, and finishes the path along a convex curve.

Smooth

Carves into/out of the material with a slight convex curve near the top of the cut, transitions to a smooth path, and finishes with a gentle convex curve at the bottom of the path.

Ramp % of Line¶

Ramp % of Line represents the percentage of the current texturing line segment that consists of ramping moves.

Depths and Entry¶

The Depths and Entry section allows you to adjust the depth of the toolpath and affect the resulting width.

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.

Screenshot of example settings — Starting at 3 mm Deep, Carve Texture at Least 1 – 3 mm Deeper Than Start Depth

Screenshot of Preview window showing resulting path — Resulting Texturing Path, With Cuts 4 — 6 mm Deep

Start Depth¶

The depth at which to start cutting. Generally the top of your material. The total cutting depth of a Texturing operation is the Start Depth + the Max Depth.

Min Depth¶

The Min Depth field controls how deep the tool will cut at least. When set, the deepest point within the texture cut will be at the Min Depth or deeper.

Max Depth¶

Max Depth is the total amount of material that will be removed from your material stock as measured from the start depth, and can be entered as a value, an equation, or a percentage of the material thickness.

Stepover¶

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

Stepover (%)¶

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

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

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

MillMage will use a cutting path of varying depth along the midline of the shape when possible before using the Stepover value to begin clearing larger areas.

Stepover Variance (%)¶

Vary the location, direction, and stepover spacing of the cutting path within the texturing area.

Pattern Preview¶

The Pattern Preview depicts the path (in purple) your router will travel on an example shape, based on your Clearing Pattern selections.

The gray area indicates the overall space that will be carved.

Raster Without Outline Pass

Common Settings¶

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

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 Feed¶

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.

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 hexadecimal 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 without 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.

Quick Tip Video: Auto Use Layer

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.

Tool Number¶

The unique number assigned to the tool to support automatic tool changers.

Tool Diameter¶

The diameter of the cutting edge of your tool.

Tool 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 Feed¶

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.

V-Carving

V-Carving dynamically adjusts the height of an angled V-Bit to perform variable-width carvings with precise details unachievable with standard end mills.

Drill

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

Bore

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

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.

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.

Fluting

A special type of operation that uses shaped tools and ramped paths to create decorative effects.

Texturing

Carves patterns into your material with controllable type, depth, length, and angles of carving.

3D Relief Roughing

3D Relief carving utilizes a grayscale depth map to quickly clear out the material around a three-dimensional object.

3D Relief Finishing

3D Relief carving utilizes a grayscale depth map to slowly and precisely carve the fine details of a three-dimensional object.

Surfacing

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

Face

A special type of operation that works similarly to Pocket and is intended for ensuring the surface has a flat top surface and the desired thickness.

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