Lathe Basics Tutorial

Introduction

This tutorial is designed to highlight some of the key areas of the lathe module. In this example, we will be working on both the OD, and the ID. Operations will include Turning, Grooving, and Threading.

Example File

If you are connected to the Internet, the part file for this example can be downloaded automatically by clicking the following link: Lathe_Basics_Tutorial BBCD.zip

Once you download and saved the zip file, extract the files on your system in an easy place to remember. You can then open the file to use with this tutorial. All files for the tutorials in this help system available for download can be found by clicking on the following link: http://www.bobcad.com/helpfiles.

 

This tutorial highlights the following features of the BobCAD-CAM software:

 

  • Create a Turning Job
  • Creating Stock and Adjusting Visibility
  • Creating Lathe Features
    • Lathe End Face
    • Lathe Turning (OD and ID)
    • Lathe Groove (OD and ID)
    • Lathe Thread (ID)
  • Creating Feature Settings
    • Adding Extensions
  • Selecting a Tool
  • Adjusting Parameters
  • Blanking Toolpath
  • Selecting Geometry
  • Setting Machining Strategies
  • Setting Parameters
  • Setting Patterns
  • Opening and Closing Simulation
  • Posting the Program

Part 1) Open the Example File and Create a Turning Job

For every turning part that is created, you will need to open or create the lathe part and then create a Turning Job. In this case, we will be opening an existing CAD file to create a Turning Job.

 

 

 

Important: The wireframe geometry is flat in the X/Y plane and in the X-/Y+ quadrant. When creating a Turning Job, this is the quadrant in which your geometry should be located.

 

  1. Open the Lathe_Basics_Tutorial.bbcd file.

  2. Click the CAM Tree tab.

  3. Right-click CAM Defaults, and click New Job.

  4. Under Job Type, select Turning and click Stock Wizard. 

    The Stock Wizard displays.

Part 2) Creating Stock and Adjusting Visibility  

The first page of the Stock Wizard allows you to define a Workpiece for the Turning Job and the subsequent pages handle shape, size and clearances. In this example, we will not define a Workpiece, but will define the shape, size and clearances for our stock. Once the stock has been defined you can adjust the visibility of the stock.

 

  1. Click to skip assigning a Workpiece.

    For more information on assigning a Workpiece, see the Assigning Workpiece Geometry topic.

  2. In the Stock Type page, leave the selection on Cylindrical.

  3. In the Size group, type in the following values:

    1. Stock Diameter = 5.125
    2. Internal Diameter = 1.000
    3. Length = 6.000
    4. Stock Origin = 0.125

  4. Click .

  5. Leave the Clearance values as they are and click OK to finalize the stock and exit the wizard.

  6. In the CAM Tree tab in the BobCAM  CAM Tree, right-click Stock and select either Transparency or Blank. These choices will allow you to, either adjust the transparency of the stock or blank it out completely.

 

Higher Transparency

Blank

Part 3) Facing the Part

For most every Turning Job, you will need to face off the stock. By selecting a Lathe End Face feature, we will automatically create toolpath up to the machine zero without the need to select geometry. The only time geometry will need to be selected for the Lathe End Face feature is if the desired toolpath needs to end before, or, continue beyond the machine zero.

 

Add the Feature

 

  1. In the CAM Tree, right-click Machine Setup - 1 and select Lathe End Face.

    The Lathe End Face feature launches with the Geometry Selection page active. Since our target geometry is already at the machine zero, we do not need to select geometry.

  2. Click Next>> to continue to the Feature page.

 

Create Feature Extensions


  1. Select the Extension check box and, in the End Distance box, enter a value of 0.1000.

 

Tip: Since the Lathe End Face feature ends at the inner diameter of our stock, we use a small extension so our tool radius does not leave any material.

 

  1. On the left side of the Lathe Wizard, click Rough.

 

Tip: We select page options in the tree on the left side of the Lathe Wizard to skip pages with options we are not interested in adjusting.


Select a Tool


  1. Click Tool Crib at the top of the Lathe Wizard.

    The Tool Crib launches.

  2. Click ROUGH to select the insert type, and then click Add From Tool Library.

    The Tool Library launches.

  3. Select tool number 263 to highlight the CNMG - 3/64RAD - ROUGH TURNINGtool.

  4. Click OK to exit the Tool Library and return to the Tool Crib.

  5. Click OK to exit the Tool Crib and return to the Lathe Wizard.

  6. Select Parameters.

Adjust Parameters and Compute


  1. Select the Rough Allowance check box.

 

Tip: In this case, we use our roughing tool to rough and finish the face. Since we use the same tool for the rough and finish, the need to create a separate finish operation is avoided by utilizing the Rough Allowance. The Rough Allowance ceases the roughing operation at the values entered and creates an additional semifinish pass up to the Finish Allowance specified next.

 

  1. In the Finish Allowance group, change both the Z and, X value to 0.0000.

Tip: By setting our Finish Allowances to 0.0000, the semifinish pass we take acts as a final finish.

 

  1. Since no other options need to be adjusted for this operation, click Compute.



Blank Toolpath

 

  1. So that we can focus on one toolpath at a time, right-click the new Feature Lathe End Face in the CAM Tree and select Blank/UnblankToolpath to hide the toolpath.

Part 4) Turning the Part

In this step we create a Lathe Turning feature, assign Rough and Basic Finish operations, and define the parameters of those operations.

 

Add the Feature and Select Geometry

 

  1. In the CAM Tree, right-click Machine Setup - 1 and select Lathe Turning.  

    The Lathe Wizard launches with the Geometry Selection page active.

  2. Click Select Geometry.

    The Lathe Wizard hides and the Feature Geometry Picking dialog opens to allow geometry selection.

  3. In the graphics area:

    1. Left-click the end of the first entity to be turned.

      The geometry is added to the list.

    2. Going to the end of the last entity to be turned, hold Shift on your keyboard and left-click again to select all the entities between the two.

    3. Click OK to confirm the geometry selection and return to the Lathe Wizard.

 

Tip: To confirm geometry selections, you can also click the icon in the toolbars or simply press Spacebar.

 

Left-click

Shift + Left-click

Result

 

  1. In the Lathe Wizard, click Next>> to continue to the Feature page.

 

Adjust Feature Settings


  1. In order to avoid cutting the grooves with these operations, select the Remove Primary Undercut check box in the Undercut group.

  2. To continue beyond the selected geometry, select the check box for Extension and enter a value of 0.2500 into the End Distance box.

  3. Click Next>> to continue to the Machining Strategy page.

 

Set the Machining Strategy


  1. Select Rough / Finish in the Machining Strategy section of the Machining Strategy page to assign a Rough and Basic Finish operation to the feature.

  2. Select Parameters.

 

Adjust Parameters


  1. Adjust the Z value of the Finish Allowance to 0.0010.

  2. In the Bounds group, select the Trim to Stock check box.

  3. Click the Apply to All Operations button to apply the trim to the finish pass as well.

  4. Select Finish.

 

Tip: In this case, our stock has already been faced off. In order to avoid unnecessary feed movement, we use the Trim to Stock option to set trim the toolpath to the Operation Stock.


Select a Tooland Compute

 

  1. Click Tool Crib.

    The Tool Crib launches.

  2. Click FINISH and then click Add From Tool Library.

    The Tool Library launches.

  3. Select tool number 277 to highlight the VNMG - 1/32RAD - FINISH TURNINGtool.

  4. Click OK to return to the Tool Crib.

  5. Click OK to return to the Lathe Wizard.

  6. Click Compute.



Blank Toolpath

 

  1. Right-click the new Feature Lathe Turning in the CAM Tree and select Blank/Unblank Toolpath.

Part 5) Grooving the OD

In this case, we have two grooves that need to be completed on the OD of the part and one groove on the ID. Right now we will focus on the two OD grooves.


Add the Feature and Select Geometry


  1. Right-click Machine Setup - 1 in the CAM Tree and select Lathe Groove.  

    The Lathe Wizard launches.

  2. Click Select Geometry.

  3. In the graphics area:

    1. Left-click and hold to the left of the grooves.

    2. Drag a window around the lower half of the grooves.  

      Both grooves are highlighted.

    3. Click OK.

Left-click + Hold

Drag Window and Release

Result

 

  1. Click Next>> to continue to the Feature page.

Adjust Feature Settings and Select a Tool


  1. In the Feature page, under the Constraints section, select From Geometry.

  2. Select Groove.

  3. Click Tool Crib.

    The Tool Crib launches.

  4. Click GROOVE and then click Add From Tool Library to enter into the Tool Library.

    The Tool Library Launches.

  5. Select tool number 281 to highlight the 1/8 WIDE - 1/64RAD - OD GROOVE tool.

  6. Click OK.

  7. In the Tool Crib, click OK.

  8. Select Patterns.

 

Set Patterns, Parameters and Compute


  1. Select Center Out under Sorting and click Next>> to continue to the Parameters page.

  2. Select the check box for Rough Allowance and adjust the X value to 0.0050.

  3. Under Semifinish Pattern, set the Overlap value to 0.0050 to ensure that each of the downward semifinish cuts will go slightly beyond center.

  4. Set the Finish Allowance values to 0.0000.

  5. Click Compute.


  1. Right-click the new Feature Lathe Groove in the CAM Tree and select Blank/Unblank Toolpath.

Part 6) Boring the ID

Now that we have completed the outer diameter of the part, we need to begin working on the inner diameter. The first thing we will work on is a basic Rough and Finish.

 

Add the Feature and Select Geometry

 

  1. Right-click Machine Setup - 1 in the CAM Tree and select Lathe Turning.

    The Lathe Wizard launches.

  2. Click Select Geometry.

    In the graphics area:

    1. Left-click and hold to the upper left of the ID groove.

    2. Drag a window around the entire groove. The groove and connected entities highlighted.

    3. Press confirm the geometry selection.

Left-click + Hold

Drag Window and Release

Result


  1. Click Next>> to continue to the Feature page.

Set Feature Settings


  1. In the Feature page under Material Approach, set the Rapid Plane to 0.0500.

  2. Under Feature Parameters, select ID from the Feature Type list to set the orientation of the feature.

  3. Under Undercut, select the Remove Primary Undercut check box so that our rough does not try to complete the ID groove feature.

  4. Select the check box for Extension and enter a value of 0.4500 into the End Distance box.

  5. Select Rough.

Select a Tool


  1. Click Tool Crib.

    The Tool Crib launches.

  2. Click BORING and then click Add From Tool Library.

    The Tool Library launches.

  3. Select tool number 500 to highlight the CNMG - 1/32 RAD .750 BORING BARtool.

  4. Click OK.

  5. In the Tool Crib:

    1. Notice the orientation of our ID boring tool in the graphics area in the top right corner of the Tool Crib.
    2. In order to have this tool orientated properly, select under Mounting Orientation.
    3. Notice the tool and its holder is now in the proper orientation.
    4. Click OK.

  6. Select Parameters.

Set Parameters, Leads and Compute


  1. In the Parameters page, select the check box for Rough Allowance and adjust the Z value to 0.0010.

  2. Set both Finish Allowance values to 0.0000.  

  3. In the Bounds group, select the Trim to Stock check box.

 

Tip: In this case, our stock has already been faced off. In order to avoid unnecessary feed movement, we use the Trim to Stock option to set trim the toolpath to the Operation Stock.

 

  1. Select Leads.


  1. Under Lead-out, set the Length value to 0.0500.

  2. Click Compute.



Blank the Toolpath


  1. Right-click the new Feature Lathe Turning in the CAM Tree and select Blank/Unblank Toolpath.

Part 7) Grooving the ID

Now that we have cleared out the ID with our ID Turning feature, we can work on the ID groove.

 

Add the Feature and Select Geometry

 

  1. Right-click Machine Setup - 1 in the CAM Tree and select Lathe Groove.

    The Lathe Wizard launches.

  2. Click Select Geometry.

    In the graphics area:

    1. Left-click and hold to the upper left of the ID groove.

    2. Drag a window around the entire groove. The groove and connected entities highlighted.

    3. Press confirm the geometry selection.

Left-click + Hold

Drag Window and Release

Result

 

  1. Click Next>> to continue to the Feature page.

Set Feature Settings


  1. In the Feature page, under Material Approach, set the Rapid Plane to 0.0500.

  2. Under Feature Parameters select ID from the Feature Type list.

  3. Under Constraints, select Custom and then click Pick since the material has already been removed for a portion of this geometry, we can change where the toolpath begins.

    The Lathe Wizard hides and the dialog opens allowing geometry selection.



  4. Highlight the connecting entity to the right of the groove, and left-click.

  5. Confirm the geometry selection.

    The Lathe Wizard returns.

  6. Select Groove.

Select a Tool


  1. Click Tool Crib.

    The Tool Crib launches.

  2. Click GROOVE and then click Add From Tool Library.

    The Tool Library launches.

  3. Select tool number 280 to highlight the 1/8 WIDE - 1/64RAD - ID GROOVE tool.

  4. Click OK.

    In the Tool Crib:
    1. Select under Mounting Orientation.

    2. Click OK.

  5. Select Parameters.

Set Parameters and Compute


  1. Select the check box for Rough Allowance and adjust the X value to 0.0500.

  2. Set both Finish Allowance values to 0.0000.

  3. Click Compute.




Blank Toolpath


  1. Right-click the new Feature Lathe Groove in the CAM Tree and select Blank/Unblank Toolpath.

Part 8) Creating the ID Thread

Now that the ID has been cleared out, we will need to create the threading operation on the ID.

 

Add the Feature and Select Geometry

 

  1. Right-click Machine Setup - 1 in the CAM Tree and select Lathe Thread.

    The Lathe Wizard launches.

  2. Click Select Geometry.

    In the graphics area:

    1. Select the entity to the right of the ID groove.

    2. Drag a window around the entire groove. The groove and connected entities highlighted.



    3. Press confirm the geometry selection.


  1. Click Next>> to continue to the Feature page.

Set Feature Settings


  1. In the Feature page, under Feature Parameters select ID from the Feature Type list.

  2. Select the check box for Extension:

    1. In the Start Distance box enter a value of 0.3750.
    2. In the End Distance box enter a value of 0.0300.

  3. Select Thread.

Select a Tool

  1. Click Tool Crib.

  2. Click THREADING and then click Add From Tool Library.

  3. Select tool number 505 to highlight the 60 DEG - LAY DOWN - ID THREAD .IC  tool.

  4. click OK.

  5. In the Tool Crib:

    1. select under Mounting Orientation.
    2. Click OK.

  6. Select Parameters.

Set Parameters and Compute


  1. Under Parameters, set Threads Per Unit to 5.0000.

  2. Select the check box for Override and set Thread Height to 0.1190.

 

Important: The Thread Height that is calculated in BobCAD-CAM is the theoretical sharp height. Depending on the thread being cut, you may need to adjust this value.

 

  1. Click Compute.



 

Blank Toolpath


  1. Right-click the new Lathe Thread feature in the CAM Tree and select Blank/Unblank Toolpath.  

Part 9) Simulation

The next step is to simulate the program to look for any necessary changes.

 

Open and Close Simulation

 

  1. In the Modules menu, click Simulation.

 

For help with simulation, view Getting Started with Simulation.

 

 

Tip: The Simulation contains a CutSim tab. Clicking on the Advanced Properties button will launch the Parameters dialog box allowing you to select the Enable check box in the Section plane group. This will put the stock in the section plane view seen in the image above. Leave the values as they are and click OK.

 

  1. To close simulation, click Modules> Exit Simulation.

Part 10) Posting the Program

Once the lathe result has been finalized it will be time to produce the code to send to the machine.


Post and Save or Edit

 

  1. In the CAM Tree, right-click Turning Job and select Post.

    The code is posted in the Layer-UCS-Post Manager.

  2. Right-click the code in the Layer-UCS-Post Manager to select Save As or Edit CNC.

    With this method, you can either save to a particular file location or open the NC code in Predator Editor respectively.
  
This concludes this tutorial.