Loading contours and positions to NC programs with CAD Import (#42 / #1-03-1)

Application

You can open CAD files directly on the control to extract contours or machining positions from them. You can then store them as Klartext programs or as point files. Klartext programs acquired in this manner can also be run on older HEIDENHAIN controls, since these contour programs by default contain only L and CC/C blocks.

Requirement

  • Software option CAD Import (#42 / #1-03-1)

Description of function

To insert a selected contour or a selected machining position directly into an NC program, use the control's clipboard. Using the clipboard, you can even transfer the contents to additional software tools (e.g., Leafpad or Gnumeric).

Opening files with additional software

CAD model with marked contour

Icons in the CAD Import

With the CAD Import, the control shows the following additional functions in the menu bar:

Icon

Meaning

Set the transition tolerance

The tolerance specifies how far apart neighboring contour elements may be from each other. You can use the tolerance to compensate for inaccuracies that occurred during drawing creation. The default setting is 0.001 mm.

C or CR

You can select whether the control will output circular contours C or CR in the NC program.

Show connections between two positions

The control hides and displays the tool paths between the positions.

Apply path optimization

The control optimizes the tool traverse movement between the machining positions. When you select the icon again, the control will discard the optimization.

Find circles according to diameter range. Load center coordinates to the position list

The control opens the Find circle centers by diameter range window. You can filter by diameters as well as by depths.

Applying contours

The following elements can be selected as a contour:

  • Line segment
  • Full circle
  • Pitch circle
  • Polyline
  • Any curves (e.g., splines, ellipses)

Linearization

CAD Viewer linearizes all of the contours that are not in the working plane.

During linearization, CAD Viewer subdivides a contour into individual segments. From these segments, CAD Import creates straight lines L and circular arcs C or CR that are as long as possible.

Thanks to linearization, it is also possible to import contours with CAD Import that cannot be programmed with the path functions of the control, such as splines.

The higher you define the resolution by specifying decimal places, the lower is the deviation from the imported contour. In any case, the deviation is less than 0.001 mm or 0.0001 inches.

Screen layout

 
Tip

You can prevent the linearization of, for example, circles that are not in the working plane. Select the working plane in which the circle has been defined.

Applying positions

You can also use the CAD Import to save positions (e.g., for holes).

Three possibilities are available in the pattern generator for defining machining positions:

  • Single selection
  • Multiple selection within a range
  • Multiple selection using search filters

Selecting positions

The following file types are available:

  • Point table (.PNT)
  • Klartext program (.H)

If you save the machining positions to a Klartext program, the control creates a separate linear block with a cycle call for every machining position (L X... Y... Z... F MAX M99).

 
Tip

CAD Viewer also considers circles that consist of two semicircles to be one machining position.

Multi-selection filter settings

If you use the quick-selection function to mark positions, the Find circle centers by diameter range window opens. You can filter the diameter or depth values, referencing the workpiece datum, by means of the buttons below the displayed value. The control will only load the selected diameter or depth values.

The Find circle centers by diameter range window provides the following buttons:

Button

Meaning

  • The control shows the smallest diameter found.
  • The control shows the smallest depth found.

This filter is active by default.

  • The control sets the filter for the largest diameter to the value selected for the smallest diameter.
  • The control sets the filter for the largest depth to the value selected for the smallest depth.

  • The control shows the next smaller diameter found.
  • The control shows the next smaller depth found.

  • The control shows the next larger diameter found.
  • The control shows the next larger depth found.

  • The control sets the filter for the smallest diameter to the value selected for the largest diameter.
  • The control sets the filter for the smallest depth to the value selected for the largest depth.

  • The control shows the largest diameter found.
  • The control shows the largest depth found.

This filter is active by default.

Selecting and saving a contour

 
Tip
  • The following instructions apply to the use of a mouse. You can also perform these steps with touch gestures.
  • Common gestures for the touchscreen

  • Deselecting, deleting, and saving of elements works in the same way for applying contours and positions.

Selecting a contour with existing contour elements

To select and save a contour with existing contour elements:

    1. Select Contour

    1. Place the cursor on the first contour element
    2. The control shows the suggested direction of rotation as a dashed line.
    3. If necessary, move the cursor towards the more distant end point.
    4. The control changes the suggested direction of rotation.

    1. Select the contour element
    2. The selected contour element is displayed in blue and is marked in the List View area.
    3. Other contour elements are shown in green.
    4.  
      Tip

      The control suggests the contour that deviates least from the suggested direction. To change the suggested contour path, you can select paths independently of the existing contour elements

    1. Select the last desired contour element
    2. All contour elements up to the selected element are shown in blue and are marked in the List View area.

    1. Activate the output of comments with workpiece information, if desired

    1. Select Save entire list content to a file
    2. The control opens the Define file name for contour program window.
    3. Enter the desired name
    4. Select the path to the storage location

    1. Select Save
    2. The selected contour is saved as an NC program.
     
    Tip
    • Alternatively, you can use the Copy entire list contents to clipboard icon to copy the selected contour to the clipboard and then paste it into an existing NC program.
    • If you select an element with the CTRL key pressed, it is deselected for export.

    Selecting paths independent of existing contour elements

    To select a path independent of existing contour elements:

      1. Select Contour

      1. Select Select, if necessary
      2. The icon changes, and the control activates the Add mode.

      1. Place the cursor relative to the desired contour element
      2. The control displays selectable points:
        • End point or center point of a line or curve
        • Quadrant transitions or center of a circle
        • Points of intersection between existing elements

      1. Select the desired point
      2. Select more contour elements
       
      Tip

      If the contour element to be extended or shortened is a straight line, the control will extend or shorten the contour element along the same line. If the contour element to be extended or shortened is a circular arc, the control will extend or shorten the contour element along the same arc.

      Selecting positions

      Individual selection

      To select individual positions (e.g., holes):

        1. Select Positions

        1. Position the cursor on the desired element
        2. The control shows the circumference and center point of the element in orange.

        1. Select the desired element
        2. The control highlights the selected element in blue and displays it in the List View area.

        Multiple selection within an area

        To select multiple positions within an area:

          1. Select Positions

          1. Drag a box around the area while holding down the left mouse button
          2. The control opens the Find circle centers by diameter range window. The window shows the identified diameter and depth values.

          1. Change the filter settings as needed
          2. Select OK
          3. The control loads all positions within the selected diameter and depth ranges into the List View area.
          4. The control shows the traverse distance between the positions.

          Multiple selection by search filter

          To select multiple positions using a search filter:

            1. Select Positions

            1. Select Find circles according to diameter range. Load center coordinates to the position list
            2. The control opens the Find circle centers by diameter range window. The window shows the identified diameter and depth values.

            Notes

            • Set the correct unit of measure so that CAD Viewer shows the correct values.
            • Ensure that the unit of measure used in the NC program matches that used in CAD Viewer. Elements that have been copied from CAD Viewer to the clipboard do not contain any information about the unit of measure.
            • The control retains the content of the clipboard only as long as CAD Viewer is open.
            • CAD Viewer also considers circles that consist of two semicircles to be one machining position.
            • The control also transfers two workpiece-blank definitions (BLK FORM) to the contour program. The first definition contains the dimensions of the entire CAD file. The second one, which is the active one, contains only the selected contour elements, so that an optimized size of the workpiece blank results.
            • CAD Import outputs the radii of the circular arcs as comments. At the end of the generated NC blocks, CAD Import displays the smallest radius to help you select the most suitable tool.

            Notes on Contour Transfer

            • If you double-click a layer in the List View area, the control switches to Contour Transfer mode and selects the first contour element that was drawn. The control highlights the other selectable elements of this contour in green. Especially in case of contours with many short elements, this procedure spares you the effort of running a manual search for the beginning of a contour.
            • Select the first contour element such that approach without collision is possible.
            • You can even select a contour if the designer has saved it on different layers.
            • Specify the direction of rotation during contour selection so that it matches the desired machining direction.
            • The contour paths available depend on the selectable contour elements that are shown in green. Without the green elements, the control will display all solutions available. To remove the proposed contour path, select the first green element by pressing the left mouse button while holding the CTRL key down.
            • As an alternative, select the Remove mode.