Contour process
The contouring process is used to make a passes along a shape or multiple shapes. The toolpath can be set to either side of the geometry or on center. When multiple shapes are selected the toolpath is automatically on center, which is typically used for engraving.
Material
Clicking this button will open the Materials dialog where you can select and edit materials. Refer to the Common Reference Guide for a full description of the material database.
Speed: RPM
The value entered is the rate of the spindle measured in revolutions per minute. Clicking the button will load a recommended speed from the Material Database based on the part material and tool composition.
Entry Feed
The value entered designates the rate measured in feet per minute or meters per minute that the tool will be moving when it enters the material. Clicking the button will load a recommended speed from the Material Database based on the part material and tool composition.
Contour Feed
The value entered is the rate measured in feet per minute or meters per minute that the tool will be moving when cutting. Clicking the button will load a recommended speed from the Material Database based on the part material and tool composition.
Depths Diagram
The items in this section of the dialog define the clearances and depths for the toolpath. Additionally, the Wall Control option lets you make 2 1/2 axis cuts.
Entry Clearance Plane
Entry Clearance Plane specifies the location the tool will make a rapid move to before feeding to the start point of the toolpath.
Exit Clearance Plane
The Exit Clearance Plane specifies the location the tool may rapid to after completing the toolpath.
Surface Z
The Surface Z specifies the top level of the material.
Floor Z
The Floor Z specifies the finished depth of the pocket.
Rapid In
When this item is checked, the move from the Entry Clearance Plane position to the Z start point of the toolpath will be a rapid move rather than a feed move. The Rapid In option should be used with caution, as it can create rapid moves directly into the part material.
Wall Control
The Wall Control button brings up a dialog which provides for the creation of 2 1⁄2 axis surfaces (tapered or swept wall shapes) on contouring processes. If the wall is tapered the button will show the angle of the taper and if the wall is a swept shape the button will say "Swept".
The three radio buttons at the top of the dialog determine the type of wall that will be created by the contouring process. The available choices are Straight, Swept shape and Tapered w/Fillets. The Straight option is the default, and when it is selected no information needs to be entered in this dialog. The information necessary for tapered and swept walls is described below. Additional information is found in this dialog if the contouring process is combined with a roughing process in the Process list. Refer to "2 1⁄2 Axis Surfacing" on page 118 for an example of using this feature.
Swept Shape
When the Swept shape option is selected, a designated drive curve will be swept around the base curve shape. The drive curve is the shape of the wall. The DC EP Left (Drive Curve End Point) and DC EP Right selections are used to indicate which side of the base curve cut shape the end point of the drive curve will be located on. This depends on the cut direction. The cut direction is determined by the Machining Marker arrows. Visualize looking down the base curve along the cut direction; the drive curve will be attached to the left or right of the base curve. When the Contour process is a part of a multi-process operation you can also specify whether to apply the sweep to the Pocket walls, the Island walls or both.
Tapered Shape
When the Taper w/Fillets option is selected, the walls of the shape will be created with the designated side angle and any radii specified for the top and bottom fillets. When the Contour process is a part of a multi-process operation you can specify different settings for both the Pocket and Island walls.
Top Down / Bottom Up
These selections indicate whether the toolpath will start at the top of the shape and cut down (Top Down) or start at the bottom of the shape and cut up. The Bottom Up selection creates the smoother surface finish.
One Direction / Back & Forth
If One direction is selected, the tool will always cut in the same direction. The tool will make each pass from the start point to the endpoint of the toolpath, moving back to the start point for each additional pass. The move from the end point back to the start point will be a rapid move if Depth First is turned on in the Process dialog. If it is turned off, the move will be a feed move. If Back & Forth is selected, the tool will alternate between climb cutting and conventional cutting. The tool will begin cutting at the start point of the toolpath and cut to the end of the toolpath, then reverse direction and cut from the end point to the start point.
User D Step
This option creates a depth step of a specific value. This is an absolute distance in Z that determines the depth of cut on each pass.
Shape Step
This option generates a parametric step based on the drive curve or taper. This specifies a distance along either the drive curve or taper angle that determines the depth of cut on each pass.
Ridge Height
This parameter is available when creating a tapered wall. The Shape Step and Ridge Height text boxes are interactive; either value can be entered and the other will be calculated. The Ridge Height (or "scallop height") is an approximate calculation of the material left on the tapered wall between each pass of the tool.
Z Step Section
The items in this section help you define the toolpath behavior when stepping down in Z and transitioning between shapes.
Desired
This is used to specify the depth of each pass. The system uses the Desired Z Step value and the Floor Z value to calculate the Actual Z Step and the # Passes that will need to be made.
Retracts
Retracts becomes active when multiple passes are being taken when contouring a given shape and the Depth First option is activated. When it is turned on, the tool will rapid up to the entry clearance plane after taking each pass and rapid to the start point of the next pass. When Retracts is off, the tool will feed from the end point of one pass to the start point of the next pass without retracting up in the Z axis.
Depth First
This option allows the user to specify a preference for how multiple contours with more than one Z Step are to be machined. Activating Depth First will cause the toolpath to completely machine the first item to the final Z depth, then move onto the next item. By deselecting Depth First, the user has told the system to first machine all selected items at the first Z step. Once the first level is complete on all selected items, the operation starts over at the first pocket or contour and begins to cut at the second Z step. This will continue until the operation is complete.
Prefer Subs
This checkbox provides the user with the option of using subprograms in the posted code. Activating this item produces shorter G-code output.
Hit Flats
This option modifies the Z Step so that a contour pass is taken at each flat surface, such as a boss top or the pocket floor. The Z Step gets recalculated for this option and the step will vary to hit the flats and therefore the Z step will not match the value shown under Actual.
Entry and Exit
The items in the Entry and Exit section let you create additional moves to add to the start and end of the toolpath. There are three options, Line and 90° Radius, 90° Line and Advanced. Entry/Exit lines are useful when using Cutter Radius Compensation (CRC) because CRC is typically turned on and off on the first and last line moves of the toolpath.
Line and 90° Radius
This option will generate a 90° arc (you specify the radius) will be added at the beginning and end of the toolpath. This arc will be tangent to the start feature at the start point and the end feature at the end point. If a value is entered in the Line text box, a line of the specified length will be created tangent to the arc as the first and last move in the toolpath.
90° Line
When this option is selected a line of the specified length will be added to the toolpath. This line will be perpendicular to the start feature at the start point and the end feature at the end point.
Advanced
Use this option to create a custom entry and/or exit move. When this option is selected the Entry/Exit tab is bolded. Define the custom entry and exit in the Entry/Exit tab. Use an advanced move as described in the Entry / Exit tab. Refer to Entry/Exit Tab for more information.
Stock ±
The value entered specifies the amount of material left on the part geometry after the completed toolpath. A positive value will offset the tool away from the geometry, leaving material on the wall. A negative value will move the toolpath into the geometry. If you are cutting the geometry on center this option will have no effect.
Z Stock
This is the amount of stock in the Depth you wish to remain or remove. A negative value will cut deeper into the stock by the amount specified. A positive value will leave material.
Overlap
An Overlap value extends the end point past the start point by the specified amount. This is very useful when using CRC.
Spring Passes
The number entered is the number of extra times the final pass will be made. In operations with multiple Z depth passes, the tool will retract to the entry clearance plane defined in the contouring process.
Stay In Stock
Toolpath generated by the system can be optimized in various ways by using the Stay in Stock, Material Only and Ignore Tool Profile options. These options are hierarchical - one depends on another being active. If Use Stock is active, then Material Only is available and if Material Only is active, then Ignore Tool Profile is available.The Stay In Stock option will confine the toolpath of any Contouring operation that goes beyond the bounds of the stock. The operation will be trimmed to the edge of the stock, causing the tool to retract and rapid to the next entry point.
Material Only
Material Only depends upon Stay In Stock being active. Material Only optimizes toolpath by limiting the toolpath to areas that have material. If a part has already been partially machined, Material Only will optimize the cut areas and ensure there will be no "cutting air." For an extended discussion on Material Only see Material Only.
Ignore Tool Profile
Ignore Tool Profile will cause Material Only operations to ignore the shape of tools in preceding operations. This is useful when re-machining with a tool that has a corner radius equal to or greater than that of prior tools. When Ignore Tool Profile is activated, Material Only pretends that all mills are sharp endmills. When a part is defined by 2D geometry only, it is recommended that Ignore Tool Profile be activated as material left on 2D walls can be easily visualized by the system.
Deselecting Ignore Tool Profile makes things a bit more complex. First of all, the remaining material is more accurate, factoring in all tool tapers and corner radii of the tools in prior operations. If you have a roughing tool with a large corner radius and a finishing tool with a smaller corner radius that will be cleaning up material left on the floor by the larger tool, be sure to turn off Ignore Tool Profile. Leaving this option off is also best for machining non-2D parts, such as a pocket in a solid with bottom fillets.
Feed Entry Type
This menu allows you to select how the tool will feed into the part. By default the tool plunges (Auto Plunge) but you may select a Ramp or Helix entry.
Ramp
Selecting this option will let you define a ramping motion when entering the part.
Z Start Point
This is the Z position at which the ramp will start. If this position is lower than the Surface Z the tool will plunge to this position.
Cut
This value is the maximum Z step that the tool can take. The value is equal to twice the Z depth of a single ramping move, i.e. it is the total depth of the zig and the zag in a ramping move. This value controls the Ramp Length based on the current Slope and Ramp Angle.
Slope Z per Inch/MM
This value specifies the slope of the ramp. A value of 1 will move the tool down 1 unit in Z for every unit of movement in XY. A value of 0.25 will generate a slope where the tool will move down 1 unit in Z for every 4 units of movement in XY. Specifying the Slope will calculate the Ramp Angle and Ramp Length values based on the current Cut value.
Ramp Angle
This is the angle of descent for the ramping motion. Specifying this value will calculate the Slope and Ramp Length based on the current Cut value.
Ramp Length
This value specifies how long the ramp is from the Z start to Z end position of a single stroke. This value controls the Cut based on the current Slope and Ramp Angle.
XY Ramp Angle
The ramp angle determines the starting angle for ramping into the part. You can let the system choose, specify to start along the X or Y axis or specify a particular angle.
Helix
Selecting this option will let you define a helical motion when entering the part.
Start Point
This is the Z position at which the helix will start. If this position is lower than the Surface Z the tool will plunge to this position.
Cut
This value is the maximum Z step that the tool can take. The value is equal to the Z depth of a fill 360° helical revolution. This value controls the Diameter based on the current Slope and Angle.
Slope Z per Inch/MM
This value specifies the slope of the helix. A value of 1 will move the tool down 1 unit in Z for every unit of movement in XY. A value of 0.25 will generate a slope where the tool will move down 1 unit in Z for every 4 units of movement in XY The XY distance is measured along the circumference of the helix. Specifying the Slope will calculate the Angle and Length values based on the current Cut value.
Angle
This is the angle of descent for the helical motion. Specifying this value will calculate the Slope and Length based on the current Cut value.
Diameter
This value is the diameter of the helix. This value controls the Cut based on the current Slope and Angle.
Helix Location
This setting specifies where the helix should be situated relative to the tool's entry position. Center at Entry SP creates the helix so its center is at the start point and an additional move from the helix end to the start point will be generated. Helix End at Entry SP generates the helix so its endpoint is at the same position as the start point for the rest of the toolpath. This eliminates the move from the helix center to the start point.
Round Corners
This checkbox allows the user to designate how the system will handle the external corners of a contour. When the Round Corners option is selected, the system will add a radius move to the toolpath at every external corner of the cut shape. The tool always stays in contact with the finished shape and does not create burrs at the corners. Sharp corners can be created when this option is on by entering a corner Break of zero. When the Round Corners option is off, no radius move will be created.
Break
The value entered in this text box specifies a radius that will be put on every external corner of the selected cut shape. It will only be available only if the Round Corners option is active. Operations that include a corner break value should not be used prior to a Material Only operation. Material Only assumes the part shape is always equal to or smaller than the material at all times. This will be true unless the corner break is used because corner break cuts a radius onto a sharp corner, which can cause inaccurate Material Only calculations.
Cutter Radius Compensation On
A checkbox that indicates whether Cutter Radius Compensation is turned on or off. Most CNC machines require that CRC be turned on for Entry line moves and turned off for Exit line moves.
Coolant
A checkbox which indicates whether coolant is turned on in a process. Flood is the standard coolant option. Additional coolant options are available with custom post processors.
Pattern
When Pattern is on, the process will create identical toolpaths in different locations on the part. The toolpath generated will be cut once for each point in the selected pattern workgroup. The pattern workgroup, which is chosen from the adjacent pop-up menu, contains unconnected, plain points that serve as origin points for the placement of the toolpaths created by the process. The original toolpath will NOT be cut unless the origin point for that toolpath is included in the pattern workgroup. Posted output will create one subprogram for the primary toolpath and call that subprogram once for each point in the pattern workgroup. For more information, See "Pattern" on page 123.
Machining CS
The Machining CS appears on this tab when a 3-axis MDD is active. See Machining CS for information on this option.
Solids Tab
This item is bolded when a solid is selected. The items found on this tab only apply to machining solids. Please refer to the SolidSurfacer manual for information on the contents of this tab.
Open Sides
This tab is always available. The settings found here affect the toolpath when there is one or more open sides or "Air" geometry.
Minimum Cut
This is the smallest amount of material left behind that the system will target for machining. Extra toolpath will be created to cut areas that have this amount of material or more remaining. Areas with this amount of material or less will not be targeted for machining though they may incidentally be cut due to normal process parameters. A value of 0 would cut all around the part (because everything has at least 0 stock) while a large value, such as the tool diameter, may not cut anything.
When using the Material Only machining option the Minimum Cut value is very important. A value of "0" will attempt to find all possible Material Only situations while a value greater than the tool radius is unlikely to find much to cut. This function helps you maximize the efficiency of Material Only so that you can ignore really small bits of material and better focus your Material Only operations.
Entry / Exit Tab
This tab contains advanced movement for entry and exit cycles. It is available when Advanced is selected as the Finish Entry/Exit style. Refer to Entry/Exit Tab for more information.
Rotate Tab
This tab is available when using a Mill/Turn MDD or a 4- or 5-axis MDD. The settings found in this tab allow you to create rotate the part or create rotary operations. Refer to Rotate Tab for more information.