Toolpath Objects

JTS Jobs-Tooling-Simulation Process

Toolpath Objects

The creation of toolpaths using Tool definitions results in a complex entity that we call a toolpath. This is a single entity with many properties defined by the creation of the toolpath. These properties include the geometry that defines the tool motion, the tool itself, feeds and speeds, and information needed to create the CNC program or to run a simulation.

Even though all the individual vector directional arrows are shown, a single click selects the toolpath in the defined order and direction, which is fixed for a toolpath object. NC toolpaths can be copied and multiple copies can be pasted into a drawing.

Toolpath objects (rather than the classic Vector toolpath which consisted of a chain of entities), are created by selecting the Tool/job button on NC- Drilling, 2d-Milling, 3d-Milling, and Lathe dialogs:

Clicking the Tool/job button will access the tool library for the selected NC process. Click Select tool to see the list of available tools. Pick the desired tool from the list, and click OK. If the desired tool is not present, import a tool library, or create a new tool by clicking the NEW button.

Enter a descriptive Name that describes the job step and change the default technology values from the tool table if desired. Clicking OK returns you to the process dialog where you can change other values to finish the creation of the toolpath object.

Tool Library

The tool library or tool table is a listing of all the tools that are available for selection from the various NC machining functions. Selecting NC-Tool Lib-Tool Table will list all defined tools, including drills, end mills, lathe turning and grooving tools. Selective groups available to the various processes can be viewed by selecting the Mill, Drill, Turn, and Groove Tool Tables independently. i.e. NC-Tool Lib-Tool Table Drill to see just the tools defined with NC-Tool Lib-Define Drill Tool

Predefined tool libraries can be saved for reuse in later sessions of Vector. To save a Tool library for reuse: NC-Tool Lib-Tool Table Export

The tool data in the table will be saved as a .ttd file extension. By default exported libraries are saved to a directory named \VECX\ttd

Selecting multiple tools using CTRL or SHIFT select will enable a mass delete of all items selected.

Use NC-Tool Lib-Tool Table Import to reopen a previously saved tool library. Once a tool library has been imported, all tools contained in that library will be displayed with NC-Tool Lib-Tool Table. Tools may be added to an existing library that has been imported and any changes such as feeds and speeds, size, etc, to the list will be permanently saved if the tool table is re-exported as a new library file name, or optionally as the same name if you choose to overwrite the original file name. If a drawing has previously defined tools, importing a tool table will merge the imported table with the existing tools.

Use Delete and Change to alter the contents of an existing Tool Library. Select/highlight the name of the tool and then click the Delete or Change buttons to perform the action. See Tool Definitions for instruction in using the Change button.

Tool Definitions

The tools used in the JTS fall into several categories. Flat, Ball and Bull nosed end mills for 2d and 3d milling operations, drills for drilling operations, turning tools for lathe roughing and profiling, and grooving tools for Lathe grooving and contouring.

Clicking the NEW button on a tool table listing will open this dialog:

Select the type of tool you wish to define, and click OK.

Each of the different types of milling cutters and drills has a dialog to precisely define the tool geometry, associated tool offsets, and the default feeds and speeds.

Tool Section, common to all milling tools:

Name – enter a name to describe the tool. The tool table is sorted by this name so it is a good idea to keep the names consistent. The name above would be a 1/8 diameter, 2 flute end mill, with feeds and speeds set to cut aluminum.

Number – the location of the tool holder within a tool holder magazine,

Correction D – the offset memory location within the controller in which the radius of the cutter is stored. This is used for G41/42 cutter compensation.

Correction L – The offset memory location within the controller in which the length compensation value is stored. This value is used in most multiple tool setups.

Depending on the tool type definition, the dialog will vary slightly in the next section

Flat End Mill , used for bottom and side cutting.

Diameter – Enter the actual diameter of the tool. This value is used for pocketing and other milling dialogs that request tool diameter. It is also used to represent the tool size during simulation.

Length – Enter the length of the flutes of the end mill. This value is only used in the simulation representation.

Technology, the technology settings are the same for all the milling cutter types.

Feed – normal “cutting along” feed rate for this cutter. Usually specified in units per time, inches per minute, inches per second, mm per minute, etc.

Feed Reduced – a reduced feed rate to be used when plunging the end mill straight vertically into the work piece material. Same units as Feed

Speed – Spindle speed to be used with this specified tool and material. Specified as RPM.

Variations for the other types of milling cutters follow:

Filleted Cylinder Mill, This tool shape has a radius or fillet on the cutter corners, also known as a bull nose cutter.

Length – Enter the length of the flutes of the end mill. This value is only used in the simulation representation.

Radius Fillet – This is the corner radius of the bull nosed cutter.

Ball End Mill. This tool has a full radius cutter end. A woodworking tool is the cove bit.

Length – Enter the length of the flutes of the end mill. This value is only used in the simulation representation.

Conic Mill cutter, also known as a V-cutter.

This tool has a tapered tip and a small flat on the end. The angles are indicated in the drawing. This tool may be used for simulation, but is not implemented in 3D surface machining.

Length (L) – Enter the length of the tool to be used for simulation.

Diameter (Ø1) – Enter the actual diameter of the tool tip. Set to 0.0 for a sharp tipped tool.

Diameter (Ø2) – Enter the actual diameter of the tool. This value is the maximum diameter of the conical tool, it is used for pocketing and other milling dialogs that request tool diameter. It is also used to represent the tool size during simulation.

Angle ( Degrees) – The side angle of the tool in degrees.

Job Table

Selecting NC-Jobs-Job table from the Vector 11 menu toggles the display of the job table. The hot key to display the Job Table is the letter “J”. Clicking the J button will also toggle display of the tool table.

The Job table is a listing of all the process steps of a job. Drilling, milling and turning jobs can all be defined simultaneously. Each time a Tool/job selection is made for a machining process, a new item is added to the Joblist. Macro Start and End are automatically supplied.

Click the + symbol (plus) on the Job table to expand the levels below a particular table entry on the left. The – symbol (minus) will compress the listing.

Select a process from the JobList (Job<Contouring> above) and click the Deactivate Job Step button to keep the process, but ignore it for purposes of simulation and generating NC. The process will be shown on the list in a lighter gray color, rather than the black text of the rest of the table. Select the process and click Activate Job Step to access the process again. If a process is selected in the drawing and it is blanked through the Change-Attributes dialog, it will become inactive. Press the Del key, to permanently remove a job step from the table. Deleting a selected toolpath from the CAD drawing will also remove a process from the job list. This can be undone with the Edit-Undo function.

Values with a white background can be retyped and the changes applied by clicking the Tab key, or by selecting the job step and then the Change Job Step button. Some values cannot be directly accessed, such as @toolDiam above. To modify this value, click the Change button, modify the tool size on the Create tool dialog and click OK to apply it to the table.

Selecting a process step that is out of order, and then using the Move Up or Move Down buttons to rearrange the job step order will place the steps into the desired order. Click the check boxes next to several job steps to activate, deactivate, or delete multiple items at once.

Click the Simulate button to run a simulation of the active job steps listed in the job table. The NC button will generate the CNC code. NC-Insert Machine must be completed prior to clicking the NC button, and an NC object must be open.

Use the Macro button to add NC-Macro execution steps to your job steps.

Click the small triangle to see a list of available macros. Click the desired macro and then OK to add the desired macro execution to the job steps. A macro execution is ignored for simulation purposes, but will be executed in job step order when the NC code is generated.

Custom variables can be defined with the Symbol button. @programnumber is a default symbol that is available to provide communication of program number to the CNC program when the code is generated.

Use the Format button to format numeric information for output to the NC file:

String is any valid text string of characters. Place the @mysymbol in a macro that is listed on the Job list and when the NC code is created, the value assigned to the @mysymbol will be entered into the NC code.

For existing files from older Vector versions, "jobs" can be created. For this there are several functions in the job menu. Select the tool path previously defined and NC-Define Job Mill, turn, groove, etc. A tool selection dialog will be displayed and the multiple entity tool path will be turned into a toolpath entity with tooling parameters, and it is then listed on the Job list, and can be simulated.

Stock Definition

Stock definition is used to define a volume from which machining is to be simulated. It is roughly equivalent to the size of the stock that will be used for the machining job. With the toolpaths selected, NC-Jobs-Define Box Stock

The default coordinates are the X-Y-Z extents of the selection. For many milling jobs, the Zmax will be 0 to display machining below the top of the part, set = Z0. It may also be advisable to add an incremental amount around the X and Y extents to show ( in the simulation) the pockets, etc as machined from a solid shape. The Offset values will automatically add this amount in each direction. .25 in the example above.

A red, enclosed volume of space is defined around the extents of the selected toolpaths.

Simulation

After toolpaths and job stock have been defined, and the order of operation has been reviewed and adjusted if necessary, it is often desirable to visualize the program. This can be accomplished with the simulation tool. A simulation can be run only for jobs.

To run a simulation, click the simulation button on the job tool bar this will atart the simulation and display the simulation controls toolbar.

Leave it floating on the screen area, or drag the simulation tool bar to the open space next to the tool bars and it will dock at the top edge of your screen. Point to the various symbols to see tool tip with each button function. From left to right they are Play, Stop, Pause, reset, Single Step, Faster, slower, and Visible. While a simulation is running these buttons can be used to change the behavior of the activity so that faster and slower processing can be observed, single step is very handy when you want to closely observe planned tool motion in congested tool paths. Normally pressing play on this toolbar does not start the job simulation. Rather start the simulation by pressing the Simulate button on the job toolbar. (NC-Jobs-Job Table). Individual job steps can be simulated by selecting the desired toolpath, and then the Job stock. During simulation the D hot key can be pressed and the view can then be dynamically rotated to view the simulation from different perspectives. Press ESC after the simulation is completed to hide the 3D rendered part. The ESC key can be pressed again to show the rendered part.