NC-2D Milling-Contouring

Contouring combines several powerful milling functions to create an automated tool path. Select some geometry to be milled and then NC-2D Milling-Contouring:

Offset Curves

Contouring will permit offsetting of curves to permit tool center programming. This function creates geometry within the Vector drawing that is subsequently processed to create the CNC program codes.

In order to use offset curves or tool center programming, set Tool Correction to none, and in the Contour section select the side of the geometry to offset, either left or right, and enter a distance to offset. This will normally be the tool radius, but may be a tool radius plus a stock amount if creating a roughing pass (to be followed by a subsequent job step with a to-size contour).

Off set curves can only be created if the original chain of drawing elements are flat within the X-Y plane at Z=0. If the original chain of entities is not planar, no offset can be created. The chain can be contoured, but cannot be offset.

The offset curves function of NC-2d Milling-Contouring is identical to the Draw-Other Curves-Offset, and has infinite look ahead to prevent gouging of a geometry sidewall with a tool.

Connect at Z

Connect at Z is the Vector process of joining one or many chains of lines, arcs, points, and curves into a safe toolpath. With some geometry selected, clicking the Z-Connections button on 2D and 3D milling dialogs or NC-Connect at Z from the Vector Cad-Cam menu displays this dialog:

All values shown above are defaults, and should work for most kinds of milling and routing.

The different lines created by the Connect at Z function, cause different results in Vector

A to B - Starting point in Z. This is a vertical rapid from .8 down to .1. Represented by a short dashed line style and layer attribute DOWNFAST. Iso G00 output code

B to Depth - Plunge cut. This is the Feed-reduced value in the tool setup dialog. The lines are represented as long dashed style and assigned layer DOWN. ISO G01 output code

Cutting along the first contour at depth – the original layer names are preserved, generates G01, G02, G03 motions at Feed rate. Any short dashed lines will generate G00 rapids, and long dashed lines will generate as G01, at feed reduced.

End of first contour to point C – Retract move. After cutting the contour, the tool is retracted at G00 rapid speed, to a safe Z height determined by the Z-Movement Horizontal. In this case .4. The layer is set to UP, and the line style is short dashed.

If only one contour is selected, the retract move is to point D, “Last point in Z”, 1.6 above.

Contour connections - If 2 or more contours are selected; a rapid move is created from point C to the X-Y location of the start of the next contour. This is assigned a layer name of HORIZ, and the short-dashed line style, which generates G00 rapid movement.

Rapid to Point B at start of second and subsequent contours. a vertical rapid from .4 down to .1. Represented by a short dashed line style and layer attribute DOWNFAST. Iso G00 output code

Repeat B to Depth - Plunge cut. This is again, the Feed-reduced value in the tool setup dialog. The lines are represented as long dashed style and assigned layer DOWN. ISO G01 output code

Cutting along the next contour at depth – the original layer names are preserved, generates G01, G02, G03 motions at Feed rate. Any short dashed lines will generate G00 rapids, and long dashed lines will generate as G01, at feed reduced.

The final move is always a retract move to point D, “Last point in Z”, 1.6 above. The layer is set to UP, and the line style is short dashed.

The “connect at Z” heights are always set relative to the current location of the Coordinate axis. Be sure to locate it to the top of part, or Z=0 before creating a Z-connection. The “connect at Z” function creates a single continuous chain of drawing elements. These elements may be re-selected at any time by changing to a 3D-view( such as default, front, right side, etc) which shows the relative heights of the start and ending “tails”. Shift-Select the tall tail (point D on the dialog screen shot) to select the entire contour in the correct order and direction.

Z-movement, Fast to Z, Incremental is an advanced capability that permits the initial rapid to .1 above the start of the contour, rather than .1 above the Z=0 level of the coordinate axis location. Use caution in checking this box as no stock interference checking is done and if point B is below the surface of the material, the cutter may rapid into the workpiece.

Customization note: By default post processing the Connect at Z lines will result in the feeds indicated above. If additional customization of the action during Connect at Z code generation, a contour may be added to the Vector NC menu that will specifically cause additional code to be created. A common use of this feature is the addition of torch/laser/water on and off commands during the processing of DOWN and UP contour lines. If the contour has exactly the same spelling and case as the layer attributes, any scripted commands contained within its definition will be created when the NC code is generated.

Approach and Depart Contour

Contouring can be used with automatic Tool Compensation, utilizing the Cutter Radius Compensation routines built into most CNC controllers. Creation of tool compensation code is automated with the addition of Arc in and arc out teardrop approach anddepart geometry. This is directly accessible to the Vector 2D contouring function, by clicking the Approach Depart button, filling in the dialog above, and check the approach depart check box on the Contouring dialog.

For most Controllers, G41 (left-climb milling) or G42 (right-conventional milling), the radius must be at least as large as the cutter, and a small overlap of .010 or .020 will create a robust toolpath with removal of nearly all the tool marks created by the start and end of cutting. Select the side of the contour to place the approach and depart, and if selecting a closed contour it is advisable to check “break first entity”, if it is an open chain, do not check “break first entity”.

As a rule of thumb use at least 3 times the cutter radius as a distance from the contour for the Start point. A .25 cutter with a .125 radius would have a .375 distance from contour. Adjust this value to control interference with adjacent geometry. The approach and depart will always be constructed on the first and last entity selected. Use the Simulate button to determine which entity is first.

Tool Correction (Compensation)

Click “None” to remove any cutter compensation code from the post-processed CNC program. The tool path will follow the instructions entered in the Contour section of the dialog.

Click left for G41 and right for G42. Make sure that proper approach and departs are included for the size of the target cutter.

Note: On some controllers it is required that all contours have a radius at least as large as the cutter radius. This can be done with a Draw-Arc-Fillet modification to all sharp corners of the contour.

The Offset may be used to make a rough pass, or to set a standard cutter slightly oversize for a test pass on the part, then adjust for final size by changing the controller cutter radius size.

Additional Contouring Functions

Select the Tool needed to make the contouring cuts.

Set the total depth of cut “Z-depth” as a positive value.

Set the Step value as an incremental depth of cut. This can create multiple passes until the final depth is reached. Each pass will be this depth, except the last one which will be the depth remaining. To set a .010 finish pass preceded by 2 large cuts, .5 depth, .245 Step. The first pass will be .245 deep, the second pass will be .490 deep, and the third pass will be .500 deep.

To cut the contour to depth with no retractions, but multiple passes, click “alternate direction of contours”.

JOB Tab

The Job tab on the Contouring dialog permits naming of the job step and modification of the tool technology provided by selection of the tool.