Use the Centre Line Feature option on the Feature Machining panel to create a centreline engraved feature from a selected vector, usually vector text, which you can then machine using the Feature Machining toolpath.
The boundary of a selected vector represents the centreline of the cutting tool. The engraved feature has no diameter other than that of the tip of the cutting tool.
To create a centreline engraved feature:
- Select the vector from which you want to create a raised feature.
- In the
3D Toolpaths area, click the
Create Feature Machining Toolpath
button to display the
Feature Machining panel.
- Select Centre Line Feature.
- Enter the depth of the centreline engraved feature you want to create in the Feature Depth box.
- To perform the machining strategy that you have selected as a series of passes in the Z direction, select
Do Multiple Z Passes.
- Enter the number of Z passes you want to make in the Num Slices box.
- Click Linear Spacing. This distributes the Z passes through the feature material.
- Click Add to add a new slice.
- Highlight a value in the box on the left of the Do Multiple Passes area and click Delete to delete an individual value.
- Select how the cutting tool reaches the depth you have defined.
- Drop Tool — If selected, ArtCAM checks for collisions between the tool geometry and the machined relief. This reduces the possibility of gouging.
- Project Tool — If selected, ArtCAM ignores the tool geometry and the centreline of the tool is projected onto the relief.
- Select the
Cut Direction you want to use.
- Climb — Select the option to rotate the cutter in the same direction as the feed motion. The option is selected by default.
- Conventional — Select the option to rotate the cutter in the opposite direction to the feed motion.
Note: Set the default cutting direction on the Options panel. - Enter a value in the Tolerance box to specify how closely you want the cutting toolto follow the shape of the selected feature.
- If you want to change the height at which the tool makes rapid moves between toolpath segments and define the Home position for the tool, click the
Machine Z control bar to expand its settings.
- Safe Z — Enter the height at which your selected tool makes rapid moves between toolpath segments. This value must be sufficient to clear any clamps used to hold your material block or sheet in position.
- Home X, Y and Z — Enter the X, Y and Z coordinates of the tool's start and end position. This should be a safe distance away from your material block or sheet.
- Click Select next to Feature Tool to display the Tool Database dialog, from which you can select the tool you want to use.
- Click Setup next to Material to define the size of your material block.
- In the Toolpath area, enter a Name for the toolpath. If you leave this box blank, the toolpath is named after the type of toolpath you are creating. For example, if you create three Feature Machining toolpaths and do not rename them, they are named Feature Machining, Feature Machining 1 and Feature Machining 2.
- Ensure the vectors along which you want to create the
Feature Machining
toolpath are selected, then:
- Click Calculate Later if you want to calculate the toolpath at a later time either by itself or as part of a batch. The toolpath is added to the Project Tree under the Toolpaths item, but is red to indicate it has not been calculated.
- Click
Calculate Now to calculate the toolpath now. A progress bar is displayed in the
Status Bar area during calculation, then the toolpath is added to the Project Tree under the
Toolpaths item. It is black to indicate it has been calculated.
A wireframe representation of calculated toolpath is displayed in the 3D view.
Note: You can edit a toolpath's settings either before or after it has been calculated.
After you have calculated the toolpath, you can simulate it.
Note: The availability of this feature is license dependent.