SolidCAM HAAS Lathe Startup Guide

From Mindworks
Jump to: navigation, search

SOLIDCAM HAAS LATHE STARTUP GUIDE[edit]

This tutorial details the process of producing a CAM code for the HAAS Lathe using SolidCAM by walking through the process for an example part.

Example Lathe Part SolidCAM Tutorial[edit]

  1. Design or import a part in SolidWorks.
    Example Part
  2. Save post processor files on the C: drive if they are not already present.
    • Post processor files are located on the shared drive at: Z:\Engineering\SeniorDesign\- Group Folders\IEW\Machine Shop\SolidCAM Post Processor\Lathe HAAS
    • Copy Postprocessor files to the local c drive at: C:\Users\Public\Documents\SolidCAM\SolidCAM2016\Gpptool
    • Once completed, close both SolidCAM and SolidWorks and reopen to reinitialize.
  3. Open New Mill Turn part under the SolidCAM Part tab in SolidWorks
    File:SOLIDCAMLATHE2.JPG
    Opening a SolidCAM Turn Part
  4. Set up part (Suggested Settings)
    Turn Part Option Settings
  5. Fill in Part Data
    • Under CNC-Machine Select: gTurn_Haas_2xUofIdaho
    • Select: CoordSys
    • Define an origin: click Select Face, then select Revolute Face.
    (The origin should be at the end of the part or a natural location to zero the tool. Z is in the direction of rotation)
    • Click Green Checkmark
    (The remaining fields should auto fill)
    Part Origin
    Turn Part Data Menu, All Data Entered
  6. Create a Tool
    1. Double Click Tool List in design tree
    2. Select New Lathe Tool
    New Lathe Tool Button
    1. Select the tool you plan to use for the current operation.
    2. Change the geometry of the Tool Insert as shown below.
    Tool Insert Geometry Settings
    1. Adjust the Shank Settings as shown below.
    Shank Parameter Settings
    1. Set Tool Parameters according to the material to be cut.
      • (In this case carbide cutting 0.5” brass is selected)
      • The HAAS lathe spindle's maximum speed is 1800 RPM.
      • This website provides a feed and turning speed calculator: [1]
    Tool Parameter Settings
    1. Select the Mounting >> button in the upper right hand corner. In this menu use the Z+,Z-,X+,and X- buttons to orientate the tool such that it is positioned as it would be on the actual HAAS lathe's tool holder.
      • The tools location in space is irrelevant. Pay attention to the axis orientation of the part.
      • The X-Axis should point towards the operator when standing in front of the machine.
      When the tool is properly oriented, save and exit the mounting dialog.
    Tool Coordinate System
    HAAS Lathe Coordinate System
  7. Make a Turning Operation
    1. Under Turning select the Turning Operation.
    2. Select the solid features to turn then click New Geometry in the Geometry Tab.
    Geometry Tab Settings
    1. Select the Start and End faces then the green checkmark to select a Chain.
    Tool Path Chain
      • The Lathe will sweep the tool from the starting face to the ending face as is cuts the part.
      • Care should be take to ensure that the tool, both the insert and holder, will not interfere with the part as it is swept along the part.
    1. Select the tool we previously defined.
    2. In the Levels menu, set the safety distance.
      • 0.1” is acceptable.
    3. In the Technology menu, select the operation as desired.
      • Technology refers to the machining styles / technique used. For example, if we were milling technology could refer to cutting a pocket using a spiral pattern or a level drilling followed by finishing sweeps.
    4. Under the Link menu, set the Lead InLead Out and the Approach and Retract settings.
      • (Default settings are usually fine)
      • Lean In and Lead Out refer to the x axis tool approach and retraction method.
      • Approach and Retract refer to the z axis approach and retraction method of the tool.