• How to use the sawblade cutting page:
    Sawblade cutting page produces tangential motion of a disk geometry for a given 2D geometric model.
    Disk geometry definition comes by tool selection. The tool must be a cylinder. Its diameter and height values should be the same as sawblade diameter and thickness.
    2D geometric model selection is called contour selection on this page. A contour is a connected set of 2D geometric elements such as lines, circular arcs, splines, conic arcs, etc. A contour is always on the X-Y plane of the active coordinate system.
    1. Open the sawblade cutting page.
    You can do this by menu command sawblade cutting under machining. Clicking the same icon on the toolbar will open the page, too.
    2. Select a contour geometry.
    If you do not select any geometry then the last selected set will be used when you press calculate.
    After selection, define a start point for contour ordering. Be careful! Complete the selection! Otherwise, calculations may fail or use the previous selection.
    Contour selection is done by selecting curve objects or Solid2D objects.
    Solid2D objects can be created from Shapes 2D or macro tables.
    Imported DXF or IGES files add curve entities. You may convert these to Solid2D objects.
    3. Select your tool.
    Use a tool with the same dimensions as your sawblade. If not available, create it using the Tool Dialog page.
    4. Enter the part height.
    This is the plate thickness.
    5. Enter safe Z value.
    Must be higher than part height to avoid cutting in the air move phases.
    6. Define cutting parameters.
    Enter max cutting depth for arcs and lines. Define separate feed rates for circular and linear moves.
    Cutting feed rate is used while the tool is cutting. Entry feed rate is used during plunge moves. Link feed rate is for fast air moves (G00 if set to 0). Exit feed rate is for retraction after cutting.
    Spindle value is the RPM of the sawblade.
    7. Enter plunge height.
    This is added to the first cutting Z position. Must be greater than max cutting depth.
    8. Define liftup value.
    Moves the entire tool path along Z+. Different from Z overcut, which can also move angularly if bevel cutting is applied.
    9. Set stock to leave.
    Offsets toolpath on X-Y plane. Positive makes it larger, negative makes it smaller.
    10. Trim and extend tool trajectory.
    Use drop list options to control start and end trimming.
    11. Select machining side.
    Choose correct side for outer boundary and inner holes.
    12. Taper angle parameters.
    Used for bevel cutting (e.g., 45° side walls). Select "some edges" if not all walls are inclined. Then assign taper values to specific edges.
    Set taper height equal to part height to cut entire wall angularly.
    13. Set type to Segment.
    Common for stone and ceramic cutting.
    14. Tool rotates CCW option.
    Used if your controller supports M codes for rotation direction. Affects post-processor output.
    15. Geometry filter options.
    You may choose to machine only lines or arcs in complex parts.
  • Stone cutting from DXF drawing with saw and milling combination
    1. If you have a 5-axis bridge cutting machine with a milling spindle alongside the saw, you can generate g-code as in this example.
    2. Open your design's DXF file in SolidCNC.
    3. The curves from the drawing may include a closed outer contour and holes inside.
    If they form a watertight closed geometry, you can convert them to a 2D solid.
    To create a solid 2D, go to the Geo menu tab, then select the Make command under 2D Solid. You can also find the same command on the toolbar.
    Select the curves belonging to the part body on the screen and confirm.
    When the solid is created without any issues, the color of the drawing will change.
    4. When you cut the outer contour with a saw, the part will appear. If desired, saw cutting can be added for internal hole.
    5. Add operations with 2D Contour cutting page for places you want to cut with the milling machine.
    6. Send the saw paths to the output folder.
    7. Also send the milling operations to the output folder.
    8. Print the G-code.
  • Macro Page
    1. Opening the Macro Page.
    1.1. Clicking on the "View" element on the toolbar opens a tab, where you can select "Macro tables diolog" to open it.
    2. Changing Macro.
    2.1. Choose the desired macro from the dropdown box at the bottom of the Macro Page. A sample representation of the selected macro will appear.
    3. Editing Macro Dimensions.
    3.1. Modify the dimensions of the opened macro either directly on the shape or through the macro table.
    4. Adding a New line to the Macro Table.
    4.1. Select a row on the macro table, then click the "Make new line" button to add a copy of the selected row as a new one.
    4.2. Make changes to the added row.
    5. Deleting a line from the Macro Table.
    5.1. Choose the row to be deleted in the macro table and click the "Delete line" button to remove the selected row.
    6. Saving the Macro Table.
    6.1. Click the "Record table" button at the bottom of the Macro page to save the current macro table to disk.
    7. Running a Macro.
    7.1. Select the desired row for drawing, then click the "Run" button at the bottom of the Macro Page to execute the drawing of the selected row.
    7.2. Place the drawing in the desired area.
    8. Creating a Saw Path.
    8.1. After drawing the shape, the saw page opens automatically or can be opened by clicking the saw icon on the toolbar.
    8.2. Make necessary adjustments on the saw page, (with crucial settings being part height and tool selection).
    8.3. Click the "Select Contour" button to choose a starting point and define the processing line.
    8.4. Adjustments are made on the saw page, and the calculation is performed by clicking the "Calculate" button. Re-calculation can be done with the "Recalculate" button.
    9. Process Simulation.
    9.1. Access the desired operation by right-clicking on the "Operations2.5" folder in the application's left panel.
    9.2. Start the simulation.
    9.2.1. Adjust the simulation speed on the opened page and start or stop the simulation.
    10. Part Positioning.
    10.1. Parts can be moved later by selecting them with the "" button in the middle of the shapes and positioning them to the desired location.
    10.2. Part positioning allows connecting cutting operations.
    10.3. If cuts enter the part after it's moved, shapes turn red as a warning.
    11. Output Process
    11.1. To output, right-click on the button, select "Lock Button" from the menu, and the button will turn blue. Locked parts are positioned together.
    11.2. Right-click on the blue button, select "Edit reorder operations" from the menu, and a page opens.
    11.3. Click the "Send to Optimize" button at the bottom of the opened page to determine tool paths. Toolpaths that align merge into a single toolpath.
    11.4. The selected tool paths are shown colored in the diagram. Adjust their order with the "Move Up" and "Move Down" buttons.
    11.5. Click the "Output Folder" button to send toolpaths to the output folder. Simulation can be performed again from the output folder.
    11.6. Right-click on the "Output Folder" node in the tree view, select the print option in the menu, provide a name in the opened window, and save the file.
Back to the Menu