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].

3D Relief Roughing

MillMage can create three dimensional shapes with curves and detailed features with two special operations, 3D Relief Roughing and 3D Relief Finishing.

Import a 3D model into MillMage, create your Depth Map, and setup a fast 3D relief roughing pass with larger diameter tooling to remove a bulk of the material. Follow with a slower, finer 3D relief finishing pass with a smaller-diameter tapered ball nose mill to carve free the final fine details.

Creating Depth Maps in MillMage

MillMage can Import 3D models to create the grayscale depth maps used in 3D carving operations.

Reference: Creating Depth Maps →

Assigning 3D Relief Roughing Operations¶

3D Roughing With Carved Background¶

Select a depth map in the Workspace and in the Operations window select New Operation → 3D Relief Roughing to open the 3D Relief Roughing Operation window. Update the roughing settings to match your machine and tooling and select OK to finish assigning the operation. MillMage will carve the depth map and the area within the bounding box.

Preview window showing 3D relief roughing operation result — a 3D carving of a triceratops fossil with a carved rectangular background — Depth Map Only Assigned to 3D Relief Roughing Operation

3D Roughing Without Carving Background¶

Assign both the depth map and the depth map outline to your 3D Relief Roughing operation to limit the relief carving area.

Warning

Wider tools may impact and/or cut beyond the shapes assigned to the current operation. Always review the upcoming travel and cuttings moves in the Preview window.

Select the design outline and the depth map and in the Operations window select New Operation → 3D Relief Roughing to open the 3D Relief Roughing Operation window. Update the roughing settings to match your machine and tooling and select OK to finish assigning the operation to the two shapes. MillMage will carve the depth map only.

Preview window showing 3D relief finishing operation result — a 3D carving of a triceratops fossil — Depth Map and Outline Assigned to 3D Relief Roughing Operation

3D Relief Roughing 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 3D Relief Roughing 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¶

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. Choose between Raster and Offset.

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.

Selecting Raster mode enables the option Raster Angle.

Raster Angle¶

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

A default value of 0° equates to right to left X axis movement. A value of 90° is parallel to forward and backwards Y axis of movement.

Offset¶

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

Selecting Offset mode enables the option Cut Direction, and Use Initial Feedrate Scale.

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

Depth to Leave¶

Enter the extra amount of material to leave behind, allowing for a final cutting pass with a 3D Relief Finishing operation. This will effectively shrink the size of the carved area inward, cutting less by the amount you enter in the Depth to Leave field.

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.

Use Initial Feedrate Scale¶

Apply a scaling factor to reduce the Feed Rate during the first carving loop into the material without a stepover. After the first cutting loop and at the first stepover instance, MillMage resume moving at 100% of the set Feed Rate.

Initial Feed Scale (%)¶

Scale to apply to the Feed Rate during the first cutting loop without stepover.

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.

Depths and Entry¶

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

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.

The Final Depth field can accept values with units of measure or as percentages. Setting the Final Depth to 100% will cut to/through the current stock dimensions Thickness value set in Project Setup.

The Start Depth and Final Depth settings combined control the thickness of your 3D relief carving. Subtract the Final Depth from the Start Depth to determine the 3D relief carving thickness.

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.

Entry Type¶

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

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.

For Spiral entires, rather than lowering to a set height before proceeeding to the next pass, the router is continually lowered in a spiral pattern for the duration of the operation.

Spiral¶

Constantly lowers the router into the material in a spiral pattern in X, Y, and Z, for the duration of the Profile operation.

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

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.

Operation Preview¶

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.

Offset
Raster With Outline Pass

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 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.