Vector Cad-Cam XI Lathe Tutorial

 

This tutorial uses jobs, inch units and in front of center tool positions.  Sample file zipped .CCD

 

Vector is a 3D cad-cam system.  It permits the user to draw complex shapes in 3D, to display them and to use the shapes for creating complex toolpaths for CNC machining.  The lathe portion includes several powerful capabilities that permit automatic calculation of roughing passes and finish passes.  The software has automatic compensation for tool nose angle, tool tip radius, and interference checking between the geometry and the sides of the tool bit.  This tutorial covers the use of angled turning tools.  There are separate documents that cover the use to the JOBS functions, grooving tools, and right hand-left hand tool cleanouts.

 

1)      Drawing orientation.  Vector defaults to the TOP View of a 3D drawing.  This is similar to plan view, or paper space in many cad systems.  Later versions of Vector can create a surface of revolution and render the part to display the design in various 3D views.

2)      File import types Because many Vector users have existing designs, or have a large investment in training in other CAD systems, Vector is oriented to using that data as easily as possible.  All Vector lathe drawings are drawn in the X-Y plane.  The CAM portion of Vector Cad-Cam converts the output to the coordinate system needed by the target machine controller.   DXF and IGES File formats are used to import this data, using the File-Open dialog, and selecting the Files of Type to match existing files.

 

 

The Blue line in this drawing represents the outer contour of the part, the magenta (pink) dashed line is the centerline of rotation.  The part origin is located at the intersection of the contour and the centerline at the right.

 

3)      Tool orientation: Above shows the default orientation for Vector and is used for a CNC machine with the tool behind the centerline of the part.  This is the normal orientation for commercial slant bed CNC lathes.  The part is between the operator and the turning tool.  This tutorial will show how to create toolpaths with an in-front tool oriented machine.  In this type of machine, the tool holder is between the part and the operator.  To convert from one type of machine setup to another, the drawing contour can be either mirrored, or rotated.  To rotate the above part contour:

-Shift-Select the contour

The red arrows indicate the direction of selection

-Edit-Cut the selected geometry disappears

-Edit-Paste, Reset, Set X rotation to 180, OK

 

F2, to unselect all

 

Creating finish toolpaths

 

Select the portion of the contour that is to be cut.  If the flange end of the above contour is to be held in a chuck, it may be best to break the line that represents the flange OD into 2 or more pieces to precisely control where the cutting occurs.

 

To do this, click select the flange OD,

Then Change-Break-Divide, select 2, and OK

The right portion of the line can be shift selected to select JUST the portion of the contour to be cut when the part is chucked by the flange on the left.

 

With the geometry shift selected the chain turns red and direction arrows are shown.

NC-Lathe-Turn Profile Lathe

 

·        -Click Select Tool, then either select a tool from the library, or define a new tool:

Define a 55 degree tool with offsets =1, 0.0 radius .5 long, .25 wide, and .125 thick.  Set the angle to the bottom to 35 degrees.  This tool will then be able to cut up to a square shoulder (55 + 35 =90).  Ignore the tool holder settings, and set the feed for inches per revolution or inches per minute depending on your cnc controller requirements, and set the spindle speed in revolutions per minute, or surface feet per minute, depending on your controller.  Feed reduced is used when approaching the contour, not while cutting.

 

Click OK and make sure to select the tool from the tool list before clicking OK on the tool list dialog.

 

·        Next, after returning to the Turn Profile dialog, click Origin

 

 

This origin is used for turning tools with  offsets set on the diameter and shoulder.

Click OK when it is selected as shown.

 

·        Set all stock values to 0

·        Set Path-Safe distance to .25.  This will start the cut at .25 to the right of the drawn contour and finish .25 along a shoulder, after the last of the contour is cut.  This permits cutting from the original geometry without needing any adjustment for stock material sizes.

·        The X direction is Right to Left

·        The Y direction is Bottom to Top ( the default here is top to bottom for a behind center tool orientation)

·        The options will not affect this toolpath, but if a trailer hitch ball kind of shape is cut, non-descending will prevent any cutting of diameters that are smaller than the maximum diameter of the “ball”

Click OK.

 

This is a finish pass for a sharp pointed tool.  Click UNDO , then REPEAT  and change the tool radius to .015 (1/64), or .031(1/32) to compensate the tool for a radius rather than a sharp point.  NOTE: radius compensation will make the tool follow a path different than the original geometry and when cut the arcs and angles will ALL cut to the exact dimensions drawn, without using tool nose radius compensation in the controller.  This is an exaggerated view of the effects of tool nose on a finish tool path; a 1/16-inch nose radius was used:

NC-Insert NC, and choose the Lathe post processor.

The Vector NC editor will open next to the drawing

 

The first time that Vector is run, it is very important that a couple of settings be changed:

Options-Coordinates

 

·        Set decimal digits to 4.  This is a minimum setting for arcs to work on most controllers using inch units.  Check with the NC controller manufacturer to determine if a different setting is needed.

·        Set Scale Factor for the Y-axis to –1.  This is the setting that is needed to change from Behind tool machines to in front tool machines.  All plus diameter values are changed to minus values, and hence even though the drawing is made using minus values for Y, the output will have positive values.  This will also insure that the correct sense of Clockwise and counter clockwise is determined when creating G02 and G03 arcs.

 

These changes need only be made the first time Vector is used.  After clicking OK on the above dialog, any subsequent use of the Vector Lathe configuration will retain these settings.

 

For some controllers additional slight modifications to the setup may be needed.  Click Options-Driver if special settings are needed.  This is unlikely unless the machine is more than 10 years old, or a non standard/ non g-code controller.

 

When using jobs, the radius values are automatically doubled to create G-code with diametric values.  If this is not desired, or if not using jobs and creating lathe output, there is an option to use radial values as well.  THE DEFAULT IN ALL CASES IS TO DIAMETER.

 

Click OK after making any changes to the above dialogs to apply the changes to the lathe configuration.

 

1)      Start and end blocks for jobs are not in the default lathe configuration.  These need to be added.

 

In the NC editor, click Options-Macro.  There are several items listed in the large box on the bottom left.  Among these are Start and End.  These two macros are used for manual code generation.  For automated code generation with jobs, we will add two more macros, “start” and “end”.  Note that the only difference is the lower case beginning letter.  These two macro names are reserved for use by jobs to insert beginning and ending code in an automatically generated CNC program.

 

To add the start and end blocks:

 

Click on the bottom line of the Menu List of the Options-Macro dialog, it is highlighted in blue below, then Click in the Macro Text box and type start.

 

Click Change to add start to the list of macros.

 

 

Repeat the same process to add end to the list of macro menu items.

 

Select start from the list and click Edit

 

Enter the desired Start Blocks for your lathe program.

 

For some controllers the first line MUST be a % sign without any line numbers.

 

@! Adds a line without permitting line numbers

 

@!% places a percent on the first line without permitting line numbers.

 

The next line is usually a program name or number

Vector has a symbol ( variable) that stores this value.  It can be entered directly within the job table.  To include it in the start blocks enter  @programnumber

 

 

Following is a sample of some codes that should be included:

 

G90 Absolute Mode

G18 X-Z planar arcs

G80 Cancel drilling cycles

G40 Cancel Cutter Compensation

G70 Inch Mode programming ( may not be required, and may vary by machine)

 

Enter these codes as shown, followed by a single blank line.  Press enter to create a blank line.  Use the arrow keys on the keyboard to check that only one blank line is entered.  Some controllers require these codes be on separate lines, if required enter them in that manner.  Place a space as the first character on each line except the first one.

 

Click OK to save the data

 

Click end on the list of menu items and Edit.

Again a blank macro dialog box appears.

 

In the ending blocks, at a minimum a program end is usually added.

 

M02 - Be sure to enter space M-zero-2, and not M-oh-2

 

 

Depending on the controller and your methods for programming, additional ending blocks can be added.  Be sure to check for a single blank line after the last line of code, just as with the Macro-start.

 

Click OK and then be sure to also click OK on the Change Macro Menu dialog.  This applies all your changes.

 

If you click on Macro on the NC-Editor menu, the new items added, start and end, will now show on the list.

 

 

To create the lathe CNC program from the finish pass that we have developed, with the toolpath selected/active, click the Generate NC from JOBS button .

 

 

Comments, tool change info, work offsets, etc can also be used with this technique.  See the documentation on the jobs system for additional options.

Creating multiple roughing passes.

At the point that we created the finishing toolpath:

Change-Attributes, click blank.  The finish tool path disappears.  Reselect the part contour that was used for creating the finish pass.

NC-Lathe-Turn Horizontal Area Lathe

 

All the same settings as for finishing, except Stock distance in X (shoulder) .002, Stock distance in Y (radius) .006. A composite “offset” can also be used, but generally with shoulders and diameters, it is better to leave a very small amount on the shoulder and slightly more on the diameters.

 

Toolpath Step distance .25

Toolpath Safe Distance .125

 

The roughing passes are shown.  Short dashed lines are rapids, solid lines are programmed feed rate.  Note that at the end of each horizontal pass, the tool is programmed to follow the contour back to the previous pass.  This eliminates the stair steps that occur if only horizontal passes were made.  Following this roughing technique with a single finish pass will result in a uniformly smooth surface contour.

 

Open the Job table by clicking the  button.

Click on the Turn Profile Lathe job step , and then activate it by clicking the activate button on the left. 

 

Next Move it down below the roughing, (turn horizontal area-Lathe) job step by clicking the move down button.

 

Your job steps should now look like this:

 

Insert a new NC object, or open the previous one by double clicking on the icon inside the drawing.  Select all the text inside the editor and delete it.

 

Generate NC as with the finishing path described previously.

 

Click inside the editor at the beginning of the program.  Use the keyboard arrows to move through the program.  Note that a red arrow follows the line of code to the end of each corresponding line or arc of the toolpath in the CAD window.

 

A few additional notes about Lathe turning geometry:

 

-I hate deburring parts.  With that in mind I have developed a few rules that I use when constructing lathe geometry.

 

Never leave a sharp corner, unless the part design requires it ( like a punch edge).  Add a small fillet to break the corner, and make sure that your feed rate permits about 3 turns of the spindle to cross the filleted corner.  If feeding at .006 inch per rev, make your fillets at least .018 inches.  .025-.030 will even feel even nicer.

 

 

Always add fillets to a chamfer’s corners, using the same sizing rule.

 

Always try to start a diameter by coming around the corner from a face: