Solids Tab
The Contouring and Roughing process dialogs have a Solids tab which contains information specific to machining solids and sheets. The tab is bolded when a solid is selected and the settings found here will only be effective if a solid is used in the operation.
Cutting Direction
Note that the user must select the Cutting Direction only in the Contouring Process dialog. The selection made for the cutting direction determines whether the tool will climb cut or conventional cut during a contouring operation. When geometry, profile or solid is selected for a contouring operation, machining markers appear on the selected geometry, allowing the user to indicate the direction of the cut by selecting the appropriate arrow. If the cut direction is indicated with the machining marker arrows, the setting for the cutting direction contained in the Contouring dialog will match the selection indicated by the arrows. Likewise, if a selection is made for the cutting direction, the machining markers will be updated to match that selection. One does not supersede the other; the system uses the last selection made before the operation is processed. These options are especially useful when only a solid or sheet is selected for a contouring operation, because when that is the case, machining markers do not come up on the screen, providing the user with a method to designate the direction of the cut.
Tolerance
When Use Global Settings for Solids is checked in the Document Control dialog, use these radio buttons to toggle between a Rough and Finish tolerance (applicable only to the specific process). Using this setting speeds up toolpath and minimizes G-code.
Advanced Settings
Use the Advanced Settings to override the tolerances set in the Document Control dialog on a process-by-process basis. Click the Advanced Settings button to access the Advanced Settings dialog and then select the Override Global Settings checkbox to apply the clearance and tolerance values to the process. A blue checkmark will appear on the Advanced Settings button if the global settings are being overridden.
Clearances:
This section allows the user to set the interaction between toolpath and fixtures that are to be avoided. A fixture may be defined as a sheet or a solid designated as a fixture.
There is a text box for the clearance value from a Fixture. This value is the additional distance the toolpath will be offset from the object.
Tolerances:
These are the machining tolerances for the toolpath, or the margin of error. The toolpath may deviate by up to these amounts. A looser tolerance will require less memory and creates shorter output. To provide as much flexibility as possible, there are separate settings for Cutting, Stock, and Fixture. The Cutting tolerance is the tolerance of the toolpath over the selected face or faces-the area to be cut. The Stock tolerance is the accuracy of the toolpath's interaction with the stock definition. The Fixture tolerance specifies the accuracy of the toolpath's interaction with areas that are to be avoided. The default value for all selections is 0.005" or 0.127mm.
Project 2D Toolpath:
The system will trim toolpath to a specific area when a solid and 2D geometry are selected for contouring. The toolpath will be bound within the selected geometry and will not go beyond the bounds of the stock if the geometry overlaps the defined stock. The behavior of the toolpath within the geometry is optional based on the Project 2D Toolpath option.
When this option is disabled, selected geometry acts as a boundary that the toolpath will not cross. The tool will take successive 2D passes in Z, using the solid as a shape to follow and the geometry as a boundary. When this option is on, the toolpath will be projected over the solid, creating 3D toolpath while following the shape of the geometry (that is, the tool will take a pass around the geometry). If viewed from the top, the toolpath will look like toolpath for a regular 2D pocket. If viewed from another angle, the difference is apparent. By projecting the toolpath, an adequate finish is left on the part and the tool always moves in the same direction. However, this toolpath creates extra cut time and can re-machine the surface of the part on multiple passes. An example of using Project 2D Toolpath is illustrated in Figure 40.
Surface Stock
The Surface Stock setting specifies the amount of material that will be left by the toolpath on any sheet or solid machined by the process. The toolpath will be offset by the Surface Stock amount in X, Y and Z. The Stocką amount entered in the Contour tab only adds stock in the cutting plane (machining CS X,Y). If both Stocką and Surface Stock are entered, they will be added together; one does not override the other. Surface Stock can be less negative up to -0.00005 less than the corner radius of the tool.
Z Step
If Desired Z Step is selected, the step in Z will be constant based on the value entered. The Ridge Height selection will create variable steps in Z resulting in a uniform ridge height on the cut part, generating a smoother finish on the part. The Ridge Height (also called scallop height) is calculated from the tool's corner radius cutting a flat surface. It is an approximate value.
Toolpath Generation
Use these radio buttons to toggle between using the Gen 3 or the Gen 2 Engine. The system is set to use Gen 3 by default for contouring operations. The user must specify a tolerance for the constraint faces as well as the Create 2D Toolpath settings (described in the section below) if using Gen 2.
Constraint Faces Tolerance
This value specifies the tolerance for constraint faces. Note that this value should be smaller than the Constraint Faces Clearance value to avoid gouging.
Constraint Faces Clearance
This value specifies the clearance for constraint faces, or the distance by which you wish tools to clear these faces.
Create 2D Toolpath
The purpose of the Create 2D Toolpath settings is to produce toolpath from what might otherwise be a 3D toolpath. The system has multiple options on how to achieve this toolpath for contouring operations. This allows more control over the results of toolpath generation.
The term "2D toolpath" is used to identify a toolpath of the type desired for machining a 2D prismatic part and "3D toolpath" to identify a toolpath typical of machining a complex surface. Strictly speaking, the system's 3D toolpath methods frequently produce toolpaths that are mathematically 2D, as they only move in X and Y. These are not, however, optimal for the machining of 2D prismatic parts. "Prismatic" refers to parts that can be constructed by extruding XY shapes along the Z-axis.
A 2D toolpath contains lines and arcs and does not vary with surface tolerance. A 3D toolpath is usually a large number of small line moves that vary from the true surfaces by the surface tolerance. A 3D toolpath is created when solids and surfaces are being machined.
Create 2D toolpath is useful when a solid or single surface is being machined and most useful when the solid being machined has 2D elements such as planes and cylinders. The selected faces of a feature must be stitched together into a single surface. Create 2D toolpath is recommended primarily for use on solids, but if sheets must be machined, then they should only be used to machine a collection of surfaces if each surface is a single feature (for example, if each of the surfaces was a single pocket).
None of the choices available from Create 2D toolpath will approximate complex surfaces with arc moves. Any of the options may fail to produce a toolpath. This is why multiple choices may be selected. They are attempted in the order in which they are listed. When one fails, the next is attempted. If they all fail, a 3D toolpath is created. An informational message box will appear listing the status of each of the 2D methods attempted. Even if a method creates a toolpath, it may nevertheless be an invalid toolpath. Several of these methods have protection limitations that are different from the standard 3D toolpath. They are documented below and are noted as they apply to each option.
Stock Body
By activating this option, the system will attempt to create 2D toolpath from a stock body for the outermost loops of a roughing operation. The 2D toolpath can come from geometry, solids, and stock definitions. Solid stock body definitions do not inherently produce 2D toolpath but instead produce a large number of small line moves. Selecting the Stock Body option will apply the Slice Offset Body only to the stock body. Since the stock can be used as the outer loop of pocket, a 2D toolpath here will improve all the roughing passes in a pocket. This function will produce better toolpath with 2D and 2.5D prismatic shapes, and will work better with the Material Only option.
There is no undercut protection if the Create 2D Toolpath option is selected for stock. If a stock definition gets smaller as you go down in -D, then the area to be machined at D= -2 can be smaller than the area at D= -1. We only see the area at the level being machined; this can lead to a rapid Z move into an area we think is clear, only to discover that uncut material from a higher level is bigger, resulting in a crash. To avoid this, you can either avoid using the Create 2D Toolpath options for your stock, or else you must be sure to visually check your entry plunge moves.
Part Body:
This option allows the system to generate optimized toolpath based on the selected body. There are four Part Body options for how the toolpath is generated. Any combination of these options may be selected. The system will start with the simplest, quickest one, try to generate toolpath, then move down the list of selected items to the next option if the current option fails. When this option is inactive, the system produces 3D toolpath from all solids.
The model to the right is ideally suited for 2D toolpath. The next four examples will show the toolpath generated using the various Part Body options on the same model. Without Create 2D Toolpath, standard 3D toolpath is created as shown. A similar image will be used for each of the four options.
From 2D Body
This option will generate 2D toolpath (lines and circles) without the surface tolerance deviation, provided that all of the faces selected are 2D. It makes high-quality 2D toolpath very quickly. Note that a horizontal chamfer or fillet is not 2D.
In order for the From 2D Body option to work, either the entire body or all faces of a pocket must be selected. No passes above the part will be generated and all Z steps will be uniform-there will not be a variable step. The From 2D Body has limited undercut protection, no constraint face protection, no fixture protection and can fail due to complex face edges. If a partial body selection is made, (faces are selected instead of the entire body), it is recommended that Use Stock be turned off.
Slice Offset Body
This option will accept any shape body with 2D or 3D elements. It is relatively fast and produces high-quality 2D toolpath. This option will work on all selected faces including 2D, 2.5D and 3D but only 2 and 2.5D faces will produce optimized toolpath. Note that this is the only choice that produces 2D toolpath from 2D and 2.5D faces. A 2.5D face is a face that can result in a 2D toolpath from an XY plane slice at a specific Z level. This 2D toolpath may be different at each Z level. Examples include spheres, cones, Z-axis revolved bodies, and some swept bodies.
In order for the Slice Offset Body option to work, the entire body or all faces of a pocket must be selected. Additionally, all selected faces must be able to offset by the tool's corner radius amount. If the selected faces fail to be offset by the tool's corner radius, Slice Offset Body will not work. The probable cause is that faces at concave corners are smaller than the offset amount. If Slice Offset Body succeeds in its offset calculation, it will generate all toolpath and will skip any other Create 2D Toolpath choices. Slice Offset Body does not protect against undercutting, constraint faces or fixtures. If a partial body selection is made (faces are selected instead of the entire body), it is recommended that Use Stock is off.
2D on Top, Replace on Bottom
This is intended for bodies that have a top Z range that is entirely 2D but then transition to 3D below this range. The 2D on Top, Replace on Bottom option will use From 2D Body methods for the top Z range and Replace TP with 2D Sections below that. This option is intended to improve performance in pockets that are primarily 2D with a complex floor. This option does a good job of cleaning up slow 3D toolpath where 2D and 2.5D faces have failed.
Replace TP with 2D Sections
This will produce a combination of 2D and 3D toolpath. There are no restrictions on the shapes the option can work from.
The Replace TP with 2D Sections option will produce a 2D range down to a depth where 3D toolpath will be needed. The From 2D Body optimization option will be used to within the tool's corner radius in Z of the start of the 3D range. 3D toolpath will be generated from this Z level down. This may produce some 3D toolpath on 2D faces near the transition area in Z, but is safer than gouging the part.
This option works best with single pockets as opposed to a large and complex group of faces that may transition from 2D to 3D at different Z depths in different areas. This option can significantly reduce toolpath generation time as the From 2D Body option is extremely fast but slowed on toolpath requiring many moves.
Limitations of Create 2D Toolpath
Undercut protection
3D toolpath has undercut protection and will not allow the tool to cut a section of the part if doing so violates a higher area of the part. This includes a wall with grooves, a mushroom-shaped part, or blind features such as a pocket on the backside. This is why it is a good idea not to select backside faces when using Create 2D toolpath options. Some of the 2D methods do not have this protection. Undercut protection on a stock body has a different effect than undercut protection on a part body. On a part body, undercutting will gouge the part. Undercutting on a stock body may fool a tool into plunging into overhanging material, because it thinks there is no material at the Z level being machined; this does not cause a part gouge. Undercut protection eliminates both potential problems.
Constraint Face Protection:
3D toolpath will not gouge an unselected face on the same body. Some of the 2D methods do not have this protection. Without this capability, you cannot cut one face of a square pocket, as starting at the face's edge will cut into its unselected neighbor.
Fixture Protection:
3D toolpath will not cut into a fixture body or face. Some of the 2D methods do not have this protection and will ignore fixtures.
Despite these limitations (listed on the following pages with the appropriate function), there are many parts that do not need this protection, and the advantages of a 2D toolpath for prismatic solids are significant.