The Advanced UI Surface Paths Tab : Advanced Planar

Introduction

This topic explains the Surface Paths tabs of the Advanced UI in the Advanced Planar operation, and provides links to the related topics.

The Surface paths tab

The Surface Paths tab of the Advanced UI contains many of the parameters used to define the feature toolpath.

Parameters

  • Closed - Clicking the ellipses button opens the Machining direction dialog, allowing you to adjust the orientation of the toolpath plane.

 

Machining direction

 

  • Top - leaved the toolpath plane parallel to the X/Y axis.

  • Other direction - allows you to define the toolpath plane vector by entering its X, Y, and Z, values, or by using the Select tool plane button to pick a line whose vector the normal of the toolpath plane should be aligned with.

 

 

Pattern

  • High speed - this pattern provides fast corner and fillet processing, but eliminates several other options, including the Machining surfaces, and DHC dialogs.

 

  • ClosedMachining surfaces... - this button launches the Machining surfaces dialog which allows you to add surfaces to consider for specific offsets (allowances).


Machining surfaces

New surface

Use the Machining and Fixture buttons to add items to the list.

 

  • Machining.. - adds another surface to the list.

  • Fixture.. - when using the Advanced Rough, this option becomes available, and adds another fixture to the list.

  • Delete - removes selected geometry from the list.

 

 

  • Machining surface - When a machining surface is highlighted in the list, clicking the ellipses button enables selection mode for you to assign geometry to the highlighted item.

  • Fixture surface - When a fixture surface is highlighted in the list, clicking the ellipses button enables selection mode for you to assign geometry to the highlighted item.

  • Offset type - This parameter determines the amount of material or stock that is allowed to remain on the drive surface after an operation.

    • ClosedGlobal - expands the machining faces in all directions.



    • Radial and axial

      • ClosedRadial offset - expands the machining faces in the X/Y direction.



      • ClosedAxial Offset - expands the machining faces in the tool axis direction.


 

 

  • ClosedHeights... - Click Heights... to open the Heights dialog. The heights define the height area to be machined. Typically you can set the heights manually by entering 2 values, the start and end height. This height will be measured along the machining direction. Another possibility is to use the 'Automatic heights' which will basically create a bounding height around the selected drive surfaces.

 

Heights

Heights

 

  • Automatic - does not require values, but allows you to choose between: 

    • ClosedMin/max from machining surfaces - Uses the selected machining surfaces to define the min/max height.



    • Min/max from stock - Uses the selected stock to define the min/max height.

    • Min/max from both - Uses the selected machining surfaces and stock to define the min/max height.

  • User defined - allows you to enter the values referenced from the machine setup to define the start and end heights.

    • ClosedStart - defines the uppermost area to machine.



    • ClosedEnd - defines the lowest point to machine.

 

 

 

  • ClosedDHC - opens the Dynamic holder collision avoidance dialog.

 

Dynamic holder collision avoidance

  • Closed Check with machining surfaces - Select this check box to enable the toolpath calculation to gouge check the tool holder against the selected geometry.




  • Closed Collision safe areas - This enables the system to automatically filter out all the cuts where collisions between entire tool including Holder, Arbor and Shaft and machining surfaces were detected.


 

Clearances

 

  • Shaft - allows you to define the clearance used for the shaft of the tool.
  • Arbor - allows you to define the clearance used for the arbor of the tool.
  • Holder - allows you to define the clearance used for the holder of the tool.

 

 

 

  • ClosedMachining angle in X,Y - defines the toolpath angle in the XY plane.

    • Multiple passes on full width cut - creates additional cuts in the vertical plane when the depth between the current and previous cuts is more than Step over value.

    • Depth step - determines the spacing between vertical cuts when using Multiple passes on full width cut.

  • Optimal machining angle in X,Y - allows you to have the system calculate the machining angle to use based on the geometry selected. This option is only available when using the High speed option, and disables the manual machining angle in X,Y value input option.

 

 


Area

  • ClosedTrim to flute length - trims the toolpath so that any cuts deeper than the flute length of the tool are trimmed.




 

Undercuts machining

 

  • Type - is set to 3+2 and enables detection and processing of undercut areas in the specified range.

  • Maximum tilt angle - defines the maximum amount of tilt allowed in the search.

  • Minimum undercut depth - defines the depth at which an undercut will be considered for machining.

  • Process both directions - allows for the processing of opposite machining directions.

  • Check surfaces - opens geometry selection for check surfaces to be chosen.

 

 

  • ClosedRound corners - smooths cutting segments based on the maximum deviation used in the dialog, as seen in the image below.




  • Closed 2d Containment - contain the toolpath within a selected curve.

 

2d Containment

 

  • 2d containment - opens the select geometry dialog to allow you to select the boundary geometry.

 

Trimming criteria

 

  • ClosedTool tip point - defines the boundary in relation to the tip of the tool.



  • ClosedTool contact point - defines the boundary in relation to the point of contact between the tool and the machining surface.



 

  • ClosedTool - allows you to choose the relationship between the tool and boundary.

    • ClosedInside - forces the entire tool to stay inside of the boundary. (This offsets the toolpath to the inside of the boundary by the tool radius.)




      • ClosedAdditional Offset - is used to add an additional offset to the location of the tool at the boundary. Note that positive or negative values are supported.




    • ClosedCenter - forces the center of the tool to cut directly on the specified boundary.




    • ClosedOutside - forces the entire tool to go outside of the boundary. (This offsets the toolpath to the outside of the boundary by the tool radius.)




      • ClosedAdditional Offset - is used to add an additional offset to the location of the tool at the boundary. Note that positive or negative values are supported.




 

  • ClosedExclude flat areas - opens the Exclude flat areas dialog allowing you to set the flat tolerance factor and define minimum and maximum widths.


 

Exclude flat areas

 

  • ClosedFlat Tolerance Factor - This can aid in recognizing flats in models with poor mesh quality. While this value can normally be left at the default value, increasing it will loosen the definition of what is considered a flat area in the mesh, which can result in toolpath being applied to areas previously not considered flat.




  • ClosedMinimum Width - Areas under this width will have toolpath applied, thereby ignoring the Exclude Flat Areas feature.




  • ClosedMaximum Width - Areas over this width will have toolpath applied, thereby ignoring the Exclude Flat Areas feature.




    - No maximum width is set, and the Minimum Width and Tolerance will control the areas the feature is applied to.

    - A maximum width is set to work along with the Minimum Width and Tolerance to control the areas the feature is applied to.


  • Filtering - click the button to open the Filtering dialog. This gives you access to the Minimum segment length in % of tool diameter value. This option lets you filter toolpath segments according to a minimum segment length defined as a percentage of the tool diameter. All toolpath contours shorter than the value are eliminated which improves machining time and reduces air moves.

  • ClosedRest finishing - opens the Rest finishing dialog.

 

Rest finishing

 

  • Based on

    • ClosedTool - calculates a toolpath that will remove all the non-machined areas left be previous bigger finishing tool.



      • Big tool diameter - Enter the previous tool diameter here and BobCAD-CAM will calculate what stock would be remaining in order to compute tool path for the current tool. Be sure to enter a diameter larger than the tool used for this operation.

      • Big tool corner radius - Enter the previous tool radius here and BobCAD-CAM will calculate what stock would be remaining in order to compute tool path for the current tool.


    • ClosedStock - calculates a toolpath that will remove all the non-machined areas by analyzing an stl file of the stock remaining from the previous operation.



      • Detect thicker than - allows you to enter a value to ignore. For instance, if an allowance has been left for finishing by another operation, entering that amount will have this operation leave that allowance.

      • Rest stock... - opens the File Open dialog allowing you to select the stl file.


  • ClosedExpand rest area - allows you to manually extend the area to be rest roughed, in order to ensure overlap.


 


  • Closed Silhouette containment - limits the machining area by the silhouette of the machining surfaces projected along the machining direction. This applies to the Advanced Planar, Advanced Z Level Finish, Equidistant, and Advanced Rough operations.


 

Silhouette containment

 

  • ClosedOffset - extends the containment by the specified value.


 

Defined by

 

  • ClosedPart silhouette - is the default setting. The machined area is limited to the tool center line which follows the actual part silhouette. The tool does not reach beneath the containment. For shallow areas the tool does not reach the outer edge.




  • ClosedPart end height - is offset outwards by the tool radius to get to full depth.




  • ClosedTool contact - adjusts the boundary as needed so the contact point between the tool and machining surface is what stops at the boundary.




  • ClosedTop of vertical walls - stops the machining at the top of vertical walls.




  • ClosedBottom of vertical walls - stops at the bottom of the vertical walls.





 

 

Sorting

  • ClosedReverse cutting order

    Select the check box to swap the cutting order, from inside to outside, to outside to inside.
    Clear the check box to retain the original cutting order.



  • ClosedCutting method - controls the cutting method or the toolpath pattern. Select either:

    • ClosedZigzag - the tool alternates the cutting direction with every new cut. This means the cut starts at one side and then moves to the other side. Once it reaches the other side, the tool cuts back in the opposite direction. The cuts are joined by the parameters set up in the Links page.



    • ClosedOne Way - the tool cuts in one direction. This means that each cut starts on one side and ends on the opposite side. The cuts are joined by the parameters set up in the Links page.



    • ClosedUp / Down - is designed for tools which can only machine in an upward/downward direction. This toolpath moves along the defined machining angle, but moves lifts up and moves to locations to reengage in a manner which will continue to engage material in an upward (or downward) manner as seen in the animation below.



      • Advanced - launches the Advanced options for up and down machining. Which gives you access to: 

        • Overlap distance - defines an amount of overlap between the points and which the toolpath disengages, and then reengages to maintain the up, or down, cutting.

        • Minimum height change - defines the height difference defining the up/down range.

  • ClosedStart corner - determines in which of the four corners the operation should begin. This option is available when the High speed option in the Pattern group is not selected.

    • • Lower Left - defined as the corner with the smallest value position in the X,Y axes.
    • • Lower Right - defined as the corner with the smallest Y value, and largest X value along the axes.
    • • Upper Left - defined as the corner with the largest Y value, and smallest X value along the axes.
    • • Upper Right - defined as the corner with the largest value position in the X,Y axes.



  • ClosedDirection for one way machining - controls how the tool cuts into the material.

    • ClosedClimb - tool movement and the spindle rotation have the same direction.



    • ClosedConventional - tool movement is opposite to the spindle rotation.



  • ClosedStart Point - allows you to define desired start position for roughing toolpath. Actual start position will be located on the closest cut to user defined point. Available for 'Offset' and 'Adaptive' roughing types.

    Select the check box when specifying a toolpath starting point. Click Start Point to open the Start Point Parameters dialog box, and enter the coordinates or select a point to act as the start point.
    Clear the check box when not specifying a toolpath starting point.

 

Surface Quality

  • ClosedCut tolerance - determines how accurate the toolpath must be in relation to the selected geometry.

 

Tip: You can reduce the cut tolerance value, for example from 0.0005 to 0.005, to speed up the toolpath calculation while creating and modifying your toolpath. Once your are happy with the result, you can then set it back to the original tolerance to calculate the toolpath before posting the output.

 

  • ClosedAdvanced - opens the Advanced options for Surface Quality dialog allowing control over the output type, arc fits, and point distribution.

Advanced options for Surface Quality

 

  • ClosedOutput type - determines how the surface quality is controlled.

    • Fit arcs and point distribution - allows for control over the arc output and point distribution.

    • Polygonize and point distribution - allows for control over point distribution.

    • High surface quality - handles control of the surface quality without user input.


  • ClosedPlanes - determines the planes in which toolpaths arcs will be fitted.

    • ClosedAny - arcs are fitted in all planes.




    • ClosedCoordinates - arcs are fitted in XY, XZ and YZ planes only.




  • Arc fit - select to output arcs in the toolpath.

  • ClosedArc fit links - allows for the reduction in the number of points on blend splines by arc-fitting the blend spline links.




  • ClosedArc fit factor - determines the tolerance of the arc fit.




Point distribution

 

  • ClosedMaximum distance - Selecting this check box allows you to set a maximum distance between toolpath points, as well as control over the maximum angle deviation between points.




  • ClosedMinimum distance - Selecting this check box allows you to set a minimum distance between toolpath points, as well as control over the allowable deviation, or tolerance, between points.




 

 

 

 

Stepover

 

  • ClosedMaximum stepover - controls the maximum distance between toolpath cuts.



  • ClosedAdaptive - creates additional toolpath passes on the steep areas considering the specified minimum stepover value.



    • ClosedMinimum stepover - defines when additional passes should be added.



    • ClosedTrim adaptive passes - removes additional toolpath from areas of the part that do not necessitate the additional passes.



  • ClosedPerpendicular - creates regions with passes which are perpendicular to the regular cuts.


 

Related Topics

The Multiaxis Wizard