KLGA Test Probe

MasterCam X5 Quick Learning

• Config & Keyboard Shortcuts
• 3D Wireframe Design
• Stock & Toolpath Creation
• Generating G Codes
• Drill & Tap Toolpaths
• Contour & Pocket Toolpaths


Optical Multi Enclosure

MasterCam Kool Links

• Basic G Codes for Milling


Optical Test Chassis

MasterCam Contour The Outside Profile

Contour toolpaths remove material along a path defined by a chain of curves. Contour toolpaths only follow a chain; they do not clean out an enclosed area. 2D contour toolpaths cut geometry in a single plane (typically XY) at a constant depth (Z = absolute depth). 3D contour toolpaths cut geometry in XY and Z, where the Z depth can vary over the toolpath. 3D is used where the geometry for each cutting pass is not contained within a single plane (Z = incremental depth). Only available if you chain 3D geometry as part of the contour toolpath.

— Contour the Outside Profile: Select Toolpath Group-1 » right mouse click » Mill toolpaths » Contour » select Chain (chain the contour in a CW direction) » select the outside profile edge » select OK to exit.

• Toolpath Type » Contour »

— Tool » Select Library Tool » checked Filter Active » select Filter button » select None button to deselect any previous tool » select Endmill1 Flat » Tool Diameter = Equal (enter tool diameter in the yellow box) » select OK to exit » select the selected tool » select OK to exit Tool Selection » Tool # = 1 » Len. offset = 1 » Spindle Direction =CW » Comment = write "Contour The Outside Profile".

— Cut Parameter » Compensate Type = Computer » Compensation Direction = Left » Tip Comp = Tip » Roll Cutter around Corner » Sharp » check Infinite Look Ahead.

— Depth Cut » check Depth Cuts » Max Rough Step (enter value) » # Finish Cuts (enter value) = 0 if you are going to use a finish tool » Finish Step (enter value) = the last cut of roughing tool » Depth Cut Order = By Contour.

— Lead In/Out » check Lead In/Out » check Enter/exit at midpoint in closed contour » check Entry = Tangent » check Gouge Check » check Exit = Tangent.

— Break Through » check Break Through » Break Through Amount (enter value).

— Linking Parameters » check Clearance » checked Absolute » uncheck Use clearance only at the start and end of operation » enter clearance value in the yellow box (default = 2.0) » Retract = checked Absolute (enter value in the yellow box (default=0.25)) » Feed Plane = Incremental (default=0.1) » Top of Stock = checked Absolute (enter value in the yellow box (default=0.0)) » Depth = checked Absolute (enter - for value) » select OK to exit 2D Toolpaths – Contour..

To change the order in which the holes are spot drilled...

— Geometry » Drill Point Manager (right click) select Sort options » Sorting » select Point to Point » select OK to exit » select the center point of the first hole to drill » select OK to exit Drill Point Manager » Regenerate all dirty operations to update the toolpath.


MasterCam Pocket The Inside Contour

Drilling the part using spot drill toolpath above...

— Poket The Inside Contour: from the Operation Manager Tree highlight

— Toolpath Group-1 » right mouse click » Mill toolpaths » Pocket » select Chain (chain the contour in a CW direction) » select the outside profile edge » select OK to exit.

• Toolpath Type » Pocket »

— Tool » Select Library Tool » checked Filter Active » select Filter button » select None button to deselect any previous tool » select Endmill1 Flat » Tool Diameter = Equal (enter tool diameter in the yellow box) » select OK to exit » select the selected tool » select OK to exit Tool Selection » Tool # = 2 » Len. offset = 2 » Spindle Direction =CW » Comment = write "Remove The Material Inside of The Pocket".

— Cut Parameter » Machine Direction = Climb » Pocket Type = Standard » Tip Comp = Tip » Roll Cutter around Corner » Sharp.

— Roughing » check Rough » check Constant Overlap Spiral » Stepover Percentage (sets the distance between roughing passes in the XY axis as a percentage of the tool diameter and will update the stepover distance) = enter value (deafault=75.0) » Stepover Distance = enter value (default=0.28125) » check Minimize Tool Burial » check Spiral Inside to Outside (enable allows you to spiral from the center to the pocket wall) » check Display Stock for Constant Overlap Spiral.

— Entry Motion = Ramp (sets a ramp entry into the part) » If Ramp Fails » check Plunge » Entry Feed Rate » check Feed Rate.

— Finishing » Finish (last pass to clean up the wall) » Passes = 1 » check Finish Outer Boundary » Cutter Compensation = Computer.

— Linking Parameters » check Clearance » checked Absolute » checked Use clearance only at the start and end of operation » enter clearance value in the yellow box (default = 2.0) » Retract = checked Absolute (enter value in the yellow box (default=0.1)) ยป Feed Plane = Incremental (default=0.1) » Top of Stock = checked Absolute (enter value in the yellow box (default=0.0)) » Depth = checked Incremetal » Depth = enter value (depth = - value).


  Home Porfolio Contact Us Kool Links Sunshine State Kids Zone Viet Cali Site Map
   
  Santa Clara, CA:     Designed by De Coloures Studio — 2007 ViBaDirect.com — All Rights Reserved