Mill Turn – Main Spindle Programming

July 7, 2021

ckopecky

Main Spindle Programming, mill turn parts, nx, NX CAM, NX CAM how-to, nx cam tutorial

Blog, NX CAM

0

Mill Turn Programming – Main Spindle Programming

This blog is titled “Mill Turn Programming – Main Spindle Programming” and is a continuation of Mill Turn Part Setup.  In the previous blog we created a mill turn setup file.  In the mill turn setup file we positioned the part on the main and sub spindle, defined workpiece geometry, avoidance, and containment planes.  In this Mill Turn Programming demonstration, you will learn the following: 

  • Retrieve tooling from the library. 
  • Create Main spindle turning and milling operations. 

Importing Tools from the Library 

With the setup file from the previous blog opened, we will retrieve the following tools from the out of the box tooling library. 

 Class to SearchLibrary ReferenceTool Description
Turning – OD TurningUGTI0101_011OD Turning Left 80 Deg.
UGTI0101_013OD Turning Left 55 Deg.
UGTI0102_008ID Turning Left 80 Deg.
Turning – ID GroovingUGTI0112_1001ID Grooving Tool 0.236″
Turning – Face GroovingUGTI0113_001Face Grooving .25 in
Turning – OD GroovingUGTI0111_004OD Grooving 0.157″
Drilling – Spot DrillUGTI01321_013NC-Center Drill 1/4″
Drilling – Twist DrillUGTI0301_553Carbide Drill 1/4″
UGTI0301_536Carbide Drill 1″
Milling – End Mill (non indexable)UGTI0201_012End Mill 1/2″

The steps outlined below will be used to import each too. I will demonstrate retrieving UGTI0101_011, follow these steps and retrieve the rest of the tools in the list.   

  1. From the Home tab on the ribbon bar, select Create Tool 
  2. Select Retrieve Tools from Library 
  3. Expand the Turning parent group > Select OD Turning as the Class to Search > OK 
  4. OK Search Criteria dialog  
  5. Alternatively, you can copy the Library Reference name from the list above and paste into Libref to narrow your search to that specific tool.  With this method you do not need to specify a class to search.
  6. Browse to UGTI0101_011 
  7. OK 

Append to Mill Turn Part Setup

Before we create the turning operation, we will make a setting change to Avoidance Main that was done from the previous blog post.  We will add a motion type for the engage and retract for the turning operations.

  1. Switch to the operation navigator – Geometry view on the resource bar > double click to edit AVOIDANCE_MAIN
  2. Motion to Start of Engage > Motion Type=Direct

Create Main Spindle Turning Operations – “Mill Turn – Main Spindle Programming”

We will now create rough & finishing turning operations on the face, OD, and ID.

Rough Facing

  1. From the Home tab on the ribbon > select Create Operation
  2. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Facing
    3. Program = TURNING
    4. TOOL = UGTI0101_011
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_ROUGH
  3. OK
  4. Main > Axial Trim Plane 1 > Limit Option = Point
  5. Select a point on the face of the part.
    1. Select Specify Point and change the selection type to Inferred Point.
  6. Generate

Rough OD

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Rough Turn OD
    3. Program = TURNING
    4. TOOL = UGTI0101_011
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_ROUGH
  2. Once in the Facing operation dialog > Switch to Strategy
  3. Toggle off Allow Undercut to avoid cutting into the face groove.
  4. Generate.

 

An Axial Trim Plane was not specified in the operation, it was inherited from the CONTAINMENT_MAIN.

Finish Facing

    1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > Match the settings in the Create Operation dialog > OK
      1. Type = turning
      2. Operation Subtype = Facing
      3. Program = TURNING
      4. TOOL = UGTI0101_013
      5. Geometry = CONTAINMENT_MAIN
      6. Method = LATHE_FINISH
    2. Main > Axial Trim Plane 1 > Limit Option = Point
    3. Select a point on the face of the part.
      1. Select Specify Point and change the selection type to Inferred Point.
    4. Generate.

Finish OD

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Finish Turn OD
    3. Program = TURNING
    4. TOOL = UGTI0101_013
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_FINSIH
  2. Main > Toggle on Omit Reversals. This will avoid cutting any grooves or material below the max OD.
  3. Strategy > Toggle off Allow Undercut to avoid cutting into the face groove.
  4. Generate.

Drill Center Hole

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = centerline
    2. Operation Subtype = Centerline Drilling
    3. Program = TURNING
    4. TOOL = UGTI0301_536
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_AUXILIARY
  2. Main > Toggle on Omit Reversals. This will avoid cutting any grooves or material below the max OD.
  3. Main > Distance > Enter a value.
  4. Generate.

Rough ID

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Rough Turn ID
    3. Program = TURNING
    4. TOOL = UGTI0102_008
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_ROUGH
  2. Main > Reversal Mode =
  3. Non Cutting Moves – Departure > Motion Type = Axial – > Radial. This setting will change the departure motions to avoid a rapid motion through the part.
  4. Generate.

Finish ID

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Finish Turn ID
    3. Program = TURNING
    4. TOOL = UGTI0102_008
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_FINISH
  2. Main > Toggle on Omit Reversals
  3. Non Cutting Moves – Departure > Motion Type = Axial – > Radial.
  4. Generate.

Finish OD Groove

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Groove OD
    3. Program = TURNING
    4. TOOL = UGTI0111_004
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_FINISH
  2. Profiling > Toggle on Additional Profiling. This will add a finish pass after roughing the groove.
  3. Stock, Tol. & Clearance > add 0.01 Rough Stock to both Face and Radial.
  4. Generate.

Finish ID Groove

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Groove ID
    3. Program = TURNING
    4. TOOL = UGTI0112_1001
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_FINISH
  2. Profiling > Toggle on Additional Profiling. This will add a finish pass after roughing the groove.
  3. Approach > Motion to Start of Engage > Motion Type=Radial – > Axial. This will avoid collision when entering the part.
  4. Departure > Motion to Return Point / Clearance Plane > Motion Type=Automatic. This will avoid collisions when retracting out of the part.
  5. Stock, Tol. & Clearance > add 0.01 Rough Stock to both Face and Radial.
  6. Generate.

Finish Face Groove

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = turning
    2. Operation Subtype = Groove Face
    3. Program = TURNING
    4. TOOL = UGTI0113_001
    5. Geometry = CONTAINMENT_MAIN
    6. Method = LATHE_FINISH

The tool retrieved from the library is too large to cut the face groove, we will edit the insert width from the operation.

  1. Main > Edit/Display Tool
  2. Insert Width=0.125
  3. Generate.

The main spindle turning is complete, we can now hide the spun outline of the part and show the solid model to create milling operations.

  1. Switch to Part Navigator on the resource bar > Hide Blank & Part Spun Outline.
  2. From the ribbon bar select the View tab > layer Settings
  3. Toggle on Layer 2.

Finish Mill Flats

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = mill_planar
    2. Operation Subtype = 2D Profile Wall without Floor
    3. Program = TURNING
    4. TOOL = UGTI0201_012
    5. Geometry = MCS_MILL
    6. Method = MILL_FINISH_POLAR
  2. Main > Select or Edit Wall Geometry
  3. Select the 4 flats and 4 radius on the flange area. 8 total face. > OK
  4. Generate.

 

Drill 0.25 Holes

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = hole_making
    2. Operation Subtype = Drilling
    3. Program = TURNING
    4. TOOL = UGTI0301_553
    5. Geometry = MCS_MILL
    6. Method = MILL_FINISH_POLAR
  2. Main > Select or Edit Feature Geometry
  3. Select the 4 holes > OK
  4. Generate.

Spot 0.25 Holes

  1. From the Home tab on the ribbon > select Create Operation. Match the settings in the Create Operation dialog > OK
    1. Type = hole_making
    2. Operation Subtype = Spot Drilling
    3. Program = TURNING
    4. TOOL = UGTI0321_013
    5. Geometry = MCS_MILL
    6. Method = MILL_FINISH_POLAR
  2. Main > Select or Edit Feature Geometry
  3. Select the 4 holes.
  4. Change Machining Area to FACES_TOP_CHAMFER
  5. Generate.

And the main spindle operations are complete and you’ve finished reading our latest “Mill Turn Programming – Main Spindle Programming” post!  In the next installment of this blog post series, we will create the remaining sub spindle turning and milling operations – stay tuned in the next few weeks. We publish a new tutorial and/or industry article every Friday.

Can’t wait that long? Check out my previous blog on setting up mill turn parts in NX CAM or click here for our other blog posts.

Sign Up for Our Newsletter!

Post by Collin Kopecky

Hi, I’m Collin, and I’m a CAM Engineer at Swoosh Technologies. For over 15 years, I’ve programmed various 3-, 4-, and 5-axis machine tools, as well as multi-channel mill turn machines. My experience in the manufacturing industry has given me insight and knowledge in mold making, high volume production, and process improvements.

Leave a Reply

Your email address will not be published. Required fields are marked *