Introduction to Broaching - Strategies and Illustrations

Strategies and Illustrations Three strategies are provided for linear broaching in order to cater for different tool types and cutting scenarios. Please view the sample files provided to see examples of broaching strategies. Reference Hole Reference hole options Options and diagrams change with type of Tool selected. Hole Diameter (All tools) Enter the diameter of the start hole. This is used as a reference for the clearance and first pass positions. Use Circle diameter where available (All tools) Check this box to use the diameter of selected circles for the start hole diameter. Adjust for Chord Height (Key, Cham) When checked, adjusts the clearance position and first pass to allow for the chord height between the flat edge of the tool and the edge of the start hole. This is used for Keyway tools. T Dimension (Key, Cham) Distance from center to keyway flat. Across Flats/Across Corners (Hex) Used to calculate the final diameter. Final Diameter (Com, Lob, Form tools) Reference Hole Strategy This is the preferred strategy for Linear Hexagon, Chamfer and Hexalobular tools, but it may also be used with Keyway tools. Your tool data should include a manufacturers’ recommended predrilled hole dimension. This hole should be large enough to fit the tool into, but smaller than the final broached shape. We recommend that you draw a circle of this pre-drilled diameter. First, create a process to pre-drill the hole, then create your linear broaching process. Select the circle for this process group. On the broaching process dialog, check the Use Circle Diameter where available option. If you did not create a circle, then select a point at the center of the hole. Make sure the Use Circle Diameter option is un-checked, and enter the pre-drilled diameter on the broaching dialog. Next, specify the final size to be broached. For a hexagon tool this can be specified as the distance Across flats , or across the sharp corners. For other tools it will be the finished diameter. The stock dimension can be used to adjust the final size: A negative stock amount will broach the part under size. A positive amount will cut it oversize. The Clear Amount is the distance from the pre-drilled diameter where you can rapid to before starting to broach. A positive value will position the tool inside the pre-drilled hole. The First Step value is the distance outside of the pre-drilled diameter where you want to make the first broaching stroke. The Desired Stepover value is an incremental distance between each broaching stroke, and the Final Step value is the amount of material to be removed by the final stroke. For the broaching process, the tool will move across to the hole center, rapid down to the Entry Clearance height Z (if it is above this value in Z). It will then move down to the start Z depth (either at feed or rapid, according to the Rapid In checkbox). This will be followed by a rapid move across to the Clear Amount (3). There will now be a series of 4 moves for each broaching stroke. It will then move to (2) the hole center and down to the (3) start position. It will complete the first cut (4) and return to the clear amount. The first cut is important as the hole may not be exactly the correct size. The next cut will be the Desired Stepover amount, the exact size of which will be calculated in conjunction with the first and final steps, dividing the distance and rounding it to make a whole number of steps. This stepover cut will be repeated until the tool reaches the final finishing cut just short of the Across Corners measurement of the final diameter, where it cuts the Final Step amount. After the final stroke, the tool will retract in Z to the exit clearance height. The broaching process dialog requires an orientation angle, where zero degrees will result in the tool pointing along the X axis direction. The tool definition includes a setup angle. If this setup angle does not match the broaching orientation, then either the tool or the part will be rotated to achieve the required alignment. (Your MDD will control which is rotated.) If your machine does not have any axes that rotate around the Z direction, then the broaching orientation and tool setup angle must be the same, because no rotation is possible. For machines that are able to rotate the tool relative to the part, you can define a series of broaching strokes at different orientations (for example, to create a complete hexagon). Check the Multiple Orientations option and enter the number of duplicates together with the required angle. Note: When the toolpath requires a change of orientation, this rotation can be output either before a linear move, with a move, or after it. Your choice between these three options is set in the DCD Machining Preferences tab, using the Oriented Toolpath pull-down menu. Center Point Center point options Across Flats/Corners (Hex) Distance across flats/corners used to calculate the final diameter. Distance to Flat (Key Cham) Distance from center to keyway flat Final diameter (Com, Lob, Form tools) Center point strategy Center point strategy might possibly be more appropriate for Keyway tools as you may not be cutting into a circle. You pick the center point and the known distance is from this point to the top of the keyway. End Point End point options No tool-specific options required. All dimensions entered would be negative as you are working back from the known end point. End point Strategy End point Strategy would be used primarily for cutting sharp corners with Corner Tools. Pick a point to be machined, enter the clear amount (negative distance) and the First Step, also a negative amount. Multiple Orientations can be programmed, but will only work with a regular shape, such as a square or hexagon, because a center must be defined as a rotation point. Below is an example of broaching using a corner tool. Stock Controls Stock Amount of stock to leave after the final pass Clear Amount Clearance position measured as a distance from the end point First Step Position of the first broaching pass measured as a distance from the end point Final Step Amount to remove by the final broaching pass. Desired Stepover Distance between each broaching pass. Common Controls 1. 2. 3. 4. 5. Entry clearance plane Entry clearance plane Exit clearance plane Rapid in feature Start position End position Tool will move to this Z level before beginning the operation. Exit clearance plane Tool will move to this Z level when the operation is complete. Rapid in feature Check this box if you require the tool move to be a rapid instead of a feed move from the clearance area. Use caution with this option as the rapid move will be made directly into the part material. Start/End position The start and end positions are measured along the depth axis of the machining CS. Entry/Exit Feed Feed speed. Feedrate Broaching Feedrate per minute. Ramp out When checked, exit at 45 degrees. 1. Unchecked 2. Checked Orientation Tool orientation angle. CW/CCW Check to indicate if the orientation is measured clockwise (CW) or counterclockwise (CCW) from the 12 o’clock position. Multiple orientations If duplicate moves are required, check this box and indicate the orientation angle, and if this is measured CW or CCW from 12 o’clock. Rotary Broaching Process In rotary broaching, a broaching tool is held in a toolholder that allows the tool to rotate inside it. The tool is also held with a slightly misaligned axis of rotation so as to create a slight wobble as it rotates. Internal or external broaching of a part is possible. Internal broaching requires a starting hole or opening in the workpiece so that the broaching tool can be pushed or pulled through. The broach is completed in just one pass. The entry point is totally random and the process is therefore best suited to cylindrical parts. Rotary Broaching Process Dialog Broaching tab 1. Feeds and Speeds 2. Clearance Diagram Rotary tab For details, see the Mill guide's discussion of the Rotate tab. 3. Machine controls 4. Face Broaching When cutting an internal broach, a pilot hole should be pre-drilled. It is also advisable to cut a 90degree countersink at the start of the hole that is greater than the across-point (OD) of the broach. If necessary the part should be made longer and faced off after broaching. For external forms, a 90-degree chamfer should be added that is less than the ID of the feature being broached. Again, this can be faced off afterwards. Feeds and Speeds Entry/Exit Feed Feedrate as defined in units per revolution. Feedrate Broaching Feedrate in units per revolution. Spindle Fwd/Rev Click the required radio button. Entry RPM Check to specify a different RPM for the entry spindle speed. Broaching Spindle Speed Tool/Part Spins Check the radio button as required. Clearance Diagram 1. 2. 3. 4. 5. Entry clearance plane Exit clearance plane Rapid in feature Start position End position Entry clearance plane Tool will move to this Z level before beginning the operation. Exit clearance plane Tool will move to this Z level when the operation is complete. Rapid in feature Check this box if you require the tool move to be a rapid instead of a feed move from the clearance area. Use caution with this option as the rapid move will be made directly into the part material. Start/End position The start and end positions, measured along the depth axis of the machining CS. Machine controls Coolant Specify the coolant method, Flood or Through spindle if required. Part Station (Appearance depends on MDD used) Select the part station to machine on. Selection here will set all processes in the process list, because they must all machine the same part. Machining CS (Appearance depends on MDD used) Select the Coordinate System to be used when generating toolpath for this process. Output of all operations will be based on the specified CS. This CS will determine tool and rotary head orientation. Face Broaching Check box to create a Face Broaching process. Conventions Conventions GibbsCAM documentation uses two special fonts to represent screen text and keystrokes or mouse actions. Other conventions in text and graphics are used to allow quick skimming, to suppress irrelevancy, or to indicate links. Text Screen text. Text with this appearance indicates text that appears in GibbsCAM or on your monitor. Typically this is a button or text for a dialog. Keystroke/Mouse. Text with this appearance indicates a keystroke or mouse action, such as Ctrl+C or right-click. Code. Text with this appearance indicates computer code, such as lines in a macro or a block of G-code. Graphics Some graphics are altered so as to de-emphasize irrelevant information. A “torn” edge signifies an intentional omission. Portions of a graphic might be blurred or dimmed to highlight the item being discussed. For example: Annotations on a graphic are usually numbered callouts (as seen above), and sometimes include green circles, arrows, or tie-lines to focus attention on a particular portion of the graphic. Faint green borders that outline areas within a graphic usually signify an image map. In online help or a PDF viewer, you can click a green-bordered area to follow the link.