What s New GibbsCAM 2016, v11.3 Q1, 2016

Transcription

1 What s New GibbsCAM 2016, v11.3 Q1, 2016

2 Proprietary Notice This document contains proprietary information of 3D Systems, Inc. ( 3DS ) and is to be used only pursuant to and in conjunction with the license granted to the licensee with respect to the accompanying licensed software from 3DS. Except as expressly permitted in the license, no part of this document may be reproduced, transmitted, transcribed, stored in a retrieval system, or translated into any language or computer language, in any form or by any means, electronic, magnetic, optical, chemical, manual or otherwise, without the prior expressed written permission from 3DS or a duly authorized representative thereof. It is strongly advised that users carefully review the license in order to understand the rights and obligations related to this licensed software and the accompanying documentation. Use of the computer software and the user documentation has been provided pursuant to a 3DS licensing agreement. Copyright DS. All rights reserved. The Gibbs and GibbsCAM logos, GibbsCAM, Gibbs, Virtual Gibbs, and Powerfully Simple. Simply Powerful. are either trademark (s) or registered trademark(s) of 3DS in the United States and/or other countries. All other trademark(s) belong to their respective owners. Portions of this software and related documentation are copyrighted by and are the property of Siemens Product Lifecycle Management Software Inc. Microsoft, Windows, and the Windows logo are trademarks, or registered trademarks of Microsoft Corporation in the United States and/or other countries. Contains PTC Creo GRANITE Interoperability Kernel by PTC Inc. All PTC logos are used under license from PTC Inc., Needham, MA, USA. 3DS is an independent Software Provider. Portions of this software Spatial Technology Inc. / Dassault Systèmes / Spatial Corp. Portions of this software Geometric Software Solutions Co. Ltd. Portions of this software ProAXYZ by Productec SA. Contains Autodesk RealDWG by Autodesk, Inc., Autodesk, Inc. All rights reserved. Mori Seiki Solid Models provided in conjunction with GibbsCAM Mori Seiki Co. Ltd. Contains VoluMill by Celeritive Technologies, Inc Celeritive Technologies, Inc. All rights reserved. This Product includes software developed by the OpenSSL Project for use in the OpenSSL Toolkit ( This Product includes cryptographic software written by Eric Young (eay@cryptsoft.com). Portions of this software MachineWorks Ltd. Portions of this software and related documentation are copyrighted by and are the property of Electronic Data Systems Corporation. Other portions of GibbsCAM are licensed from GibbsCAM licensors, which may not be listed here. 3D Systems, Inc. Modified: Saturday, February 06, :32 PM

3 Contents NEW IN GIBBSCAM 2016, V Overview 4 Thread Milling 6 New Tool Type: Full Profile Threadmill 7 Tapered Thread Milling 7 Multiple Contouring 8 Oriented Turning 10 Rotate Tab 10 Changes to Machine Manager 10 VoluMill 11 Technology Expert 12 5-Axis Simultaneous Milling 14 All Calculation Strategies 14 Calculation Based on Surfaces 15 Calculation Based on Triangle Mesh 16 Calculation Based on Wireframe 19 Calculation Based on Swarf Machining 20 Calculation Based on 3-to-5-Axis Conversion 20 Calculation Based on Port Machining 20 Calculation Based on Multiaxis Machining 20 5-Axis Drilling 21 Data Exchange 22 Graphical PMI 22 NX (*.prt) Files 23 Miscellaneous 24 3

4 New in GibbsCAM 2016, v11.3 New in GibbsCAM 2016, v11.3 Overview Highlights since GibbsCAM 2015 (September 2015) include enhancements and changes in the following areas. Thread Milling The Thread Milling process has an expanded set of capabilities, especially when using the new tool type, Full Profile Threadmill. Offers the ability to vary depth with geometry, just as in the Holes process. Understands and works with hole features. Connects between Z passes. Allows for multiple passes and spring passes. Choose whether to rapid or feed from the center to the clearance diameter. Full Profile Threadmill is a new tool type: Number of teeth can be 1 or more. Support for threadforms and for tapered-angle tools. Tapered Thread Milling, for multi-tooth threadmills, derives taper angle from the tool profile. For detailed information on all these enhancements, see Thread Milling on page 6. Multiple Contouring The Mill module now lets you cut multiple contours on geometry with user-specified cutter side offsets. Separate sets of controls handle closed shapes and open shapes. For detailed information on these enhancements, see Multiple Contouring on page 8. Oriented Turning GibbsCAM 2016 provides improved support for turning, including the ability to use a single tool at multiple B orientations, re-orient a toolgroup for use on a different spindle, and turn at arbitrary orientations on machines with redundant rotary axes. Rotate tabs for all Lathe processes Support for flash tooling and for cake turrets 4

5 New in GibbsCAM 2016, v11.3 Changes to Machine Manager and tool setup for sub-positioning For detailed information on these enhancements, see Oriented Turning on page 10. VoluMill VoluMill 7.2 provides enhancements in the following areas: Technology Expert. Instead of using the standard Materials dialog to suggest RPM and feedrate, you can calculate recommendations for many other parameters, including depth of cut and speed/feed/angle for ramp or helix plunge types. Calculations are based on material type and hardness, current tool values, and other factors such as conservative or aggressive cutting style, and recommendations can be applied selectively. Spiral motion, especially in simple pockets like squares and circles. Side Milling is significantly more efficient, and Side Mill Only is now the recommended setting. The algorithm uses wider radii for higher-speed cutting and better chip clearance. Also, Side Milling uses zigzag motion in situations when it reduces cycle times. Open-Face Milling. Improved algorithms can reduce cycle time for open faces by 60%. Performance when regenerating TP. Infrastructure improvements make regeneration smarter and quicker. For detailed information on these enhancements, see VoluMill on page Axis 5-Axis provides numerous enhancements throughout. For detailed information, see 5-Axis Simultaneous Milling on page 14. Data Exchange Expanded use of Spatial Corporation translators (separate options) provide new capabilities: Graphical PMI. Product and Manufacturing Information (PMI), can now be imported and displayed from several types of CAD files. NX (*.prt) Files. Files of type *.prt (Siemens Unigraphics UGS/NX files) can now be imported using the Spatial translator. For detailed information on these enhancements, see Data Exchange on page 22. Miscellaneous Lathe. Process dialogs for Rough, Contour, and Thread have a slightly different layout. Macros. You can now create balloon help for controls in macro dialogs you create. Hole Manager and Hole Editor. Context menus and new controls offer increased usability and some new functionality. Geometry Properties. You can right-click elements to summon a Properties dialog to query properties like ID, type, workgroup, CS, Wall/Air, Rapid/Feed and wrap depth. For detailed information on these enhancements, see Miscellaneous on page 24. 5

6 Thread Milling The Thread Milling process offers a greatly expanded set of capabilities, many of which can be seen in the following comparison of the new process dialog with the previous process dialog: Before GibbsCAM 2016 In GibbsCAM 2016 The new capabilities are especially useful in conjunction with the new tool type, Full Profile Threadmill (see below). Offers the ability to vary depth with geometry, just as in the Holes process. Understands and works with hole features. Calculates how many Z passes are required for the thread's start Z and end Z, based on the tool's flute length. The process connects between Z passes: Uses tangent arc retract/re-approach between each pass. Arc length can be calculated automatically or specified by the user. For OD threading: Connects using rapid in Z/feed arc. For ID threading: Connects via center of hole. 6

7 Allows for multiple passes and spring passes: You can specify depth between passes. When using a multi-tooth threadmill, spring passes occur after all main passes are complete. You can specify how many spring passes should occur at the finish cut diameter. You can choose whether to rapid or feed from the center to the clearance diameter. New Tool Type: Full Profile Threadmill GibbsCAM 2016 provides a new tool type for multi-tooth thread mills. For a thread milling process using such a tool, the value for Pitch (metric units) or TPI (threads per inch) is defined by the tool, not by the process. Number of teeth can be 1 or more. Support for threadforms. Support for tapered-angle tools. Tapered Thread Milling For all thread milling processes, clearance diameter is constant throughout the cut, and a single cut diameter is specified for the start of the cut. For multi-tooth threadmills, taper angle is derived from the tool profile. For single-tooth threadmills, you can specify Taper Angle: Straight threading uses a taper angle value of 0. BSPT/NPT uses a taper angle of degrees. Or you can specify a custom taper angle. 7

8 Multiple Contouring GibbsCAM 2016 provides support for performing multiple contours on geometry with userspecified cutter side offsets. Accordingly, the Contour process dialog now has an additional tab, Offset: Inapplicable situations. Settings in the Offset tab are ignored, and the tab itself is unbolded, in the following circumstances: When the item selected for part machining is a body (solid or surface). When profiles are selected. When the Contour process is paired with a Pocket process. 8

9 Functionality. Note that the Offset settings provide controls for both Closed Shapes and Open Shapes. This allows you to select closed and open shapes together, knowing that the system will use the correct settings for the corresponding types. If multiple shapes are selected, they will be cut centerline and without extensions, since GibbsCAM does not support machining markers on multiple selected shapes. You can choose Centerline to cut each shape on the tool's center, without offset. Selecting this option disables incompatible controls such as Cut Inside or Climb / Conventional. For Closed Shapes: Cut Inside will offset the tool towards the inside of the closed shape. If Alternate Side for Nested Shapes is checked, then the tool will cut inside the outermost shape, outside any shapes nested in that shape, inside shapes nested within those, and so forth, following the same rules as Pocketing does by default. Cut Outside will offset the tool towards the outside of the closed shape. If Alternate Side for Nested Shapes is checked, the tool will cut outside the outermost shape, inside any shapes nested in that shape, outside shapes nested within those, and so forth, following the same rules as Pocketing does when Outermost Shape as Boss is selected. For Direction: Climb (Left) and Conventional (Right) will offset the tool to the left or right of the shape. Shape direction is determined from the shape, with one exception: If an open shape has only one end terminator selected, then it is considered the start point regardless of the shape's innate direction. For Open Shapes: Start Extension and End Extension determine the distance from the start point (or end point) of the shape to the start point (or end point) of the toolpath. If applicable, Start Extension and End Extension values are applied instead of Overlap values that are set the Contour tab, so as to retain consistency with legacy behavior where machining markers can disable Overlap values. 9

10 Oriented Turning GibbsCAM 2016 provides improved support for oriented turning, including the ability to use a single tool at multiple B orientations, re-orient a toolgroup for use on a different spindle, and turn at arbitrary orientations on machines with redundant rotary axes. Rotate Tab The Rotate tab is added to the Lathe process dialogs for Roughing and Thread, and replaces the B-Axis tab for Contour. Rotate tab Contour, Roughing, Thread Rotate tab with Variable B Contour only Controls on Rotate tabs for all Lathe processes: preview pane with view controls Holder Angle Face Relief / Diameter Relief Face up checkbox Changes to Machine Manager Interop Events tab: new checkbox Advanced Different First/Second Angle Events Toolgroup tab: new checkbox Use TG Change Value Modifiers (for toolgroups of type Turret and Slide only) 10

11 VoluMill GibbsCAM 2016 now includes VoluMill 7.2, which provides the following enhancements: Spiral motion for areas where spiral motion is more efficient, especially in simple pockets like squares and circles. In the pocket shown below, following the helical entry into material, smooth spiral motion opens up the right side of the pocket, followed by other motions, including side milling, to complete the machining. The left side of the pocket requires no spiral: As the area is opened up, a natural transition area is created for the tool to move from one pass to the next at high speed. Side Milling. Because of gains in performance, selecting the Side Mill Only checkbox is now the recommended setting. (However, slotting can still be more efficient than side milling in some cases, such as milling with large stepovers and shallow cuts in softer material.) One of the sources of increased performance is the use of wider radii when possible, allowing higher-speed cutting and better chip clearance. This is illustrated in the preceding image. In addition, side milling now uses zigzag motion in circumstances when doing so reduces cycle time, as shown in the following image: 11

12 Open-Face Milling. VoluMill now determines cut angle and order of cuts to minimize cycle time, and ensures full stepover for the last cut. Cycle time for open faces is reduced by up to 60%. Performance when regenerating TP. Infrastructure improvements make regeneration smarter. For example, a change with no effect on geometry or slicing, such as a change to feedrate, no longer triggers a complete recalculation. Technology Expert Because VoluMill operations generate a different type of toolpath, values for feeds and speeds and other parameters can be fine-tuned using Technology Expert. 12

13 Instead of using the standard Materials dialog to suggest RPM and feedrate, you can calculate recommendations for up to ten parameters not just spindle speed and feedrate, but also depth of cut, stepover, and speed/feed/angle for ramp or helix plunge types. Recommendations are calculated based on not just material type but also hardness, current tool values, tool coating and holder choice, how well the part is held, the degree of taper. After you choose a machining style (conservative or aggressive) and calculate the recommendations, you can choose to apply some or all of the recommendations to your VoluMill process. 13

14 5-Axis Simultaneous Milling All Calculation Strategies All calculation types: For roughing cycles, safe links are now created much closer to the part. This reduces machining time and air move travel, especially when retract distances are set to Current Z-Height. All calculation types:gouge tab offers a new substrategy for Retract Tool, Along tool plane, to avoid collisions while retaining tool orientation and height. All calculation types: Link tab: Default Lead-In/Out now provides automatic extension or trimming until arc is tangent with tool axis. All calculation types: Link tab: Retracts dialog offers new ability to retract to an incremental clearance area, as illustrated below. Retract to an incremental plane Calculation based on Existing Toolpath: Surface Paths tab offers a new strategy, Dropping, that lets you project an arbitrary toolpath onto a surface, along a direction you specify, as illustrated below. 14

15 Dropping toolpath onto a surface: Before Dropping toolpath onto a surface: After Calculation Based on Surfaces Calculation based on Surfaces, pattern Project curves, type Spiral: Surface Paths tab now offers the ability to define the start point of the projected spiral. Calculation based on Surfaces: Tool axis control tab offers a new capability, Smoothing, that lets you apply smoothing parameters for the rotary axis and cutting direction either globally or individually. Calculation based on Surfaces: Surface Paths tab offers a new strategy, Flowline. Flowline toolpath will be aligned or mapped to the U or V direction of a single machining surface according to your choices, as illustrated below. This lets you avoid having to select additional bounding geometries like wall surfaces or edge curves, and the maximum stepover can be maintained with a constant distance even if the surface topology is very complex. Calculation time is very fast. 15

16 Calculation based on Surfaces:Roughing tab now offers a new capability, Mirror, that creates a mirror image of a toolpath by reflecting it symmetrically with respect to a defined axis and point. This is an extension to the Transform/Rotate capability. Calculation based on Surfaces: Surface Paths capabilities for Extend/trim have been expanded to allow Side extensions beyond the actual drive surface at the start or end, resulting in additional cuts before the first cut or after the last cut. Calculation based on Surfaces or Triangle Mesh, pattern Rough: The Roughing tab now offers a new capability, Transform/Rotate, that lets you copy toolpath by translation along a direction or by rotation around an axis. This allows you to create fully rotation symmetric operations for such purposes as impeller machining, or to apply a pattern multiple times on a surface. Calculation Based on Triangle Mesh Calculation based on Surfaces or Triangle Mesh, pattern Rough: The Roughing tab now offers a new capability, Transform/Rotate, that lets you copy toolpath by translation along a direction or by rotation around an axis. This allows you to create fully rotation symmetric operations for such purposes as impeller machining, or to apply a pattern multiple times on a surface. Calculation based on Triangle Mesh, pattern Parallel Cuts: Surface Paths tab, Stepover section, now offers new controls, Detect threshold distance and Pass extension. For areas steep enough to meet the criteria you specify, the system creates regions with passes that are perpendicular to the regular ones. Calculation based on Triangle Mesh: The Surface paths tab offers additional capabilities for Depth step (Advanced): For Intermediate Slices, you can now choose Constant depth step and define intemediate slices by the depth distance between them. Calculation based on Triangle Mesh:Utility Options tab now offers an option, Intermediate slices feedrate, that lets you specify feedrate for intermediate slices as a percentage of the 16

17 feedrate for the main machining cycle. Because the tool load on such slices is usually low, you can set the feedrate higher, thus reducing machining time. Calculation based on Triangle Mesh: Surface Paths tab offers a new control, Offset type, that lets you specify a virtual offset to machining surfaces (such as for material or stock allowance) for radial and axial directions either globally or individually. Calculation based on Triangle Mesh pattern Rough or Wireframe pattern Parallel Roughing: The Roughing tab offers a new parameter, Link length threshold, that lets you specify maximum allowed length of hard links between parallel cuts. Calculation based on Triangle Mesh, pattern Constant cusp: Surface Paths tab now offers a new capability, Exclude undercut areas, that avoids air cut generation for undercut areas, resulting in reduced overall machining time. Calculation based on Triangle Mesh, pattern Rough: Surface Paths tab offers a new Intermediate slices capability, Start point, that lets you indicate a start position for Roughing toolpath. Actual start position will be located on the cust closest to the user-defined point. Calculation based on Triangle Mesh, pattern Trochoidal: Surface paths tab now offers a new capability, Start point, that lets you specify a desired start position for trochoidal toolpath. The actual start position will be located on the cut closest to the user-defined point. Calculation based on Triangle Mesh, pattern Constant Z: In the Surface paths tab, the Depth Step dialog box now provides a new capability, Adaptive depth step, that offers parameters to control the conditions for adaptive depth cuts: the additional slices can now be constrained with a Minimum depth step distance and a Maximum stepover distance, helping you to create only the minimum necessary amount of adaptive slices. Calculation based on Triangle Mesh, pattern Constant Z: In the Surface paths tab, the Depth Step dialog box now provides a new capability, Machine vertical walls, that lets you machine only vertical areas of the machining surface selection. The main benefit is that the Constant Z pattern works most effectively on vertical areas. Shallow areas always need special treatment, and this feature makes it easier to separate the areas. Calculation based on Triangle Mesh, pattern Rough, type Adaptive: Improvements to algorithms have made Adaptive roughing significantly faster (up to 50%), with smoother lead-in motions and improved ability to reach into narrow slot areas. Calculation based on Triangle Mesh, pattern Rotary: The Surface paths tab offers a new capability, Axis of rotation, that frees you from having to align the part to the Z axis and instead lets you specify a line or vector as the rotary axis for the toolpath, as illustrated below. 17

18 Calculation based on Triangle Mesh, pattern Rough: In the Roughing tab, the Stock definition dialog (for stock types Surfaces and Bounding box) offers a new set of Area parameters that allow you to define a certain machining area within the stock material. This is particularly useful for rest machining when you want to machine only one area from the rest material. It differs from 2D stock containment in that the containment is not considered as a hard boundary, or pocket; instead, it is a soft boundary where the tool can engage from outside and does not need to ramp in. Calculation based on Triangle Mesh, pattern Trochoidal: Surface paths tab now offers several parameters for Entry and Exit that let you add lead-in and lead-out motion to the trochoidal toolpath pattern, as illustrated below. 18

19 Calculation Based on Wireframe Calculation based on Wireframe, pattern 2-Axis Rough: Surface paths tab offers a new capability, Fixture curves, that lets you specify a fixture contour that must be avoided, so as to prevent collisions between tool and fixture during the machining process, as illustrated below. Calculation based on Wireframe: When an input contour contains arcs, 2D profile cycle calculations provide arc segments in the toolpath rather than a set of polygonized linear cuts. Calculation based on Wireframe: You can now specify a unique start point on each curve to be, as illustrated below. 19

20 Calculation Based on Swarf Machining Calculation based on Swarf machining:surface paths tab offers a new control, Guide tool at, that lets you specify whether the tool should follow the surface's upper curve or lower curve. Calculation based on Swarf machining:multi cuts tab offers a new control, Direction, that lets you create mutiple cuts for stripe milling that follows the actual curvature of the machining surfaces. This is most useful for convex shapes, such as gear flanks or the pressure sides of impeller blades. Calculation based on Swarf machining:utility tab now offers a new capability, Maximum angle step, that limits the rotation angle of the machine head to a specified value measured from last toolpath point. If the rotation angle is too large due to kinematic properties of the machine, then the distance between two toolpath points will be refilled with additional points. The number of points is calculated by division of rotation angle and maximum angle step, resulting in small staps for angle changes. Calculation Based on 3-to-5-Axis Conversion Calculation based on 3-to-5-axis conversion:utility tab now offers a setting, Maximum angle step for rotation axis, to recalculate interpolation points when rotary or tilting angle exceeds the maximum defined the Tool axis control setting for Maximum change. Calculation Based on Port Machining Calculation based on Port Machining: Surface paths tab offers a new checkbox, Automatic spine, that ensures the minimum distance between spine and port is always larger than the tool radius. The toolpath is extended automatically to the end of the port so that the tool can roll over the edge. Calculation based on Port Machining: Surface paths tab offers a new checkbox, Roll over edge, that creates a toolpath extension so that the tool approach and entrance is smooth and gradual. The flute cuts out material step by step from the tip and is not in full contact with the material on full diameter. Calculation based on Port Machining: Link tab now offers the ability to calculate the radius and direction for the Connection cylinder automatically, using the minimum clearance cylinder as the boundary. Calculation Based on Multiaxis Machining Calculation based on Multiaxis Machining: Surface Paths tab now offers the capability of defining a floor consisting of multiple surfaces, as illustrated below. 20

21 Using multiple surfaces to define a floor Calculation based on Multiaxis Machining: In the Roughing tab, Stock definition for Stock type of Surfaces offers a new option, Stock has undercuts, that lets you avoid air cuts in certain stock materials, such as a castings that have pre-machined or undercut areas. 5-Axis Drilling For Drilling, when the Link tab choice for Large gaps is Retract to incremental clearance area, you can specify clearance area using two traversing types: Direct and Step. With Direct, the tool retracts to the incremental clearance area value using a connection that is a direct line to the next position; for example, the line can diagonally connect the two cuts in the shortest and fastest way. With Step, the retraction distance is never less than the incremental clearance value, using a connection that is a horizontal line to the next cut; because the line is horizontal, the incremental clearance area value of the lower point will be extended until the upper incremental clearance area distance is reached, for a greater safety distance while traversing. 21

22 Data Exchange Expanded use of Spatial Corporation translators gives GibbsCAM 2016 several new capabilities. Note that readers for NX (Spatial), STEP (Spatial), and CATIA v5+v6 are separately purchasable options. Graphical PMI Product and Manufacturing Information (PMI), such as the exact color, shape, and positioning of Geometric Dimensioning and Tolerancing (GD&T) information like notes, dimensions, datums, and information on roughness and tolerances, can now be imported and displayed from CAD files of the following types: NX (Unigraphics or UGS/NX) STEP (ISO 10303: AP203 and AP214) In STEP, Graphical PMI has also been called PMI Presentation. CATIA v5 R2x and above When an imported GibbsCAM model contains PMI, you can click and hold the Show Dimensions button for menu options relating to dimensions and PMI. PMI-related options under the Show Dimensions button; PMI Manager; and GibbsCAM solid model with PMI displayed 22

23 NX (*.prt) Files Files of type *.prt (Siemens NX files, formerly called Unigraphics or UGS/NX files) can now be imported using the Spatial translator, which offers the ability to import Hole features and to recognize and preserve their threading. As with translators for CATIA v5 and STEP, you can specify whether to use Datakit or Spatial as the translator for Siemens NX files. Separate licensing is required. 23

24 Miscellaneous Lathe. Lathe process dialogs for Rough, Contour, and Thread have a slightly different layout. Macros. You can now add balloon help for controls in macro dialogs you create. Hole Manager. The context menu (right-mouse menu) has some new items: Fit Columns has been moved from a button, and Hole Groups lets you see the groups that the selected hole belongs to, or add it to a group or remove it from a group. Hole Editor. Now provides at-a-glance information on hole ID (the title bar now reads, for example, Edit Hole H5) and segment ID and count (the left column now tells you, for example, Segment 3 of 4). Two new buttons have been added: Reset Hole Definition (to undo all unsaved changes) and Profile to WG (to save the hole silhouette as geometry in a workgroup; this is especially useful for form tool definition). Plug-Ins. The Contour Trace plug-in is moved out of GeoTools and into the Geometry submenu. Geometry Properties. When you right-click a selection of one or more elements (points, lines, curves), you can summon a dialog that shows you the most important properties of each element and allows you to toggle Air/Wall or Rapid/Feed status and to supply or modify a value for wrap depth, as illustrated below. 24

25 25