• Waterjet cutting
    We will machine wireframe models using the contour2d cutting page. You may open the page using the machining, contour2d machining menu command. We assume that the drawing of the target model is already imported to the system by reading a dxf file.
    1. Make sure your tool has the same diameter as the waterjet diameter.
    We will arrange the Autotool as a 1 mm diameter cylinder tool. We will select the Autotool from the tool combo box.
    2. Set Zmax and Zmin values as zero.
    The maximum height of the part is introduced on the controller panel and the topmost position for cutting safely without colliding nozzle to material is assumed as Z = 0.
    3. Arrange the starting position of the toolpath.
    You can force the system to prompt for the start position every time you introduce a new contour.
    4. Choose entry and exit moves for the toolpath.
    You can add lead in, and lead out to the contour definition start and end positions. It is either circular or linear.
    5. Set tool offset direction whether.
    It is a hole or an outer cutting?
    6. Set the tool rotation angle during cutting. Is it a bevel cut or a vertical cut with no conic angle?
    If you need a vertical cut choose the Work plane Z direction option.
    If you want bevel cutting, select the option Rotate around the tangent direction and set the angle parameter as you need.
    If you check the Make taper interactor check box then for every operation created the taper angle parameter values will be added to the graphics window where you may click and change. After changing the angle value, the related operation will be updated.
    7. Decide how sharp corners are handled while the toolpath is formed.
    For waterjet cutting it is good to split the toolpath where there is a discontinuity in the target contour..
    However if the part is an artistic figure you may prefer a continuous toolpath even on corners.
    8. Feedrate definitions are not important because the speed of cutting is adjusted on the machine controller.
    SolidCNC post-processor outputs symbolic values for the feed rate like Feed1, Feed2, etc. So the speed definitions on the page are not used.
    9. Select the target geometries by the Geometry selection button.
    Pick models to cut from the graphic screen and finish the selection when the contours to cut are selected.
    10. Send operations individually or all together to the output folder in the tree view.
    The order in the output folder is important. The first operation is cut first and the cutting order of operations goes on as they are in the folder. You can simulate the operations one by one. Right-click on the operation you want to animate and give the menu command Simple animation.
    11. Once you think everything is as you want you can print out the g-code.
    Make sure the post-processor is set appropriately.
  • 6-axis waterjet cutting by advanced swarf machining
    We will show using Moduleworks swarf machining functions to make toolpaths.
    We will output the toolpaths to a waterjet machine with 6 degrees of freedom.
    All 6 axes can run simultaneously so the output is quite complex.
    We will simulate the machine and see the nozzle trajectory realized on the actual kinematic system.
    1. First we will import a 3-D model of the target part by an IGES file.
    2. Position the part to the right position.
    Its center line must pass through the origin and along the positive X-axis.
    This is because the divisor axis is along the machine X-axis.
    3. Open Moduleworks add-on for advanced machining functions.
    Select tool diameter as 1mm to represent the waterjet.
    Open the Swarf machining tab.
    4. Select swarf surfaces and let the system calculate a toolpath.
    We will change it as needed after we see the result.
    5. We can swap the toolpath direction.
    The result makes sense after swapping the directions, but there are problems again.
    We need to retract the nozzle so it will not plunge into the uncut cylinder material.
    We will use the collision detection and handling page. In this tab, we can introduce 3D models to avoid colliding.
    The toolpaths will be modified where there are collisions between the tool and the check surfaces.
    The system will retract the tool along its axis direction and make it safe.
    6. We will output our toolpath by a post-processor capable of handling 6-axis degrees of freedom.
    It will ask the user for each operation whether to use the divisor at a fixed B angle or rotate the divisor simultaneously during this particular operation.
    Once we want to print the g-code a pop-up window will appear.
    We will prefer simultaneous rotation instead of a fixed B angle for the first operation.
    We will prefer fixed divisor for the last cut off operation.
    7. To simulate this cutting process we should load our machine.
    This is possible by Insert, Make transformation group menu path.
    8. We will attach the part model to the divisor of the virtual machine.
    Select the surfaces to attach and create a group link on our treeview.
    Select the appropriate models and right-click on the graphics window.
    Give the command Group, insert tree link. Give a name to the selection group.
    For example part. It will appear on the tree view.
    9. Your virtual machine kinematic tree rests under the tree view VTransformationGroup node.
    Expand it to reach the PartHolderB node of this particular machine model.
    Right-click on this node and give the command Add part by link name.
    This will attach the part model to the divisor model and an increment of B angle will rotate the part together with the divisor model.
    10. We will load the simulation file on the Control panel page.
    Right-click on any node of your VTransformation group and give the menu command Control panel.
    Select the process file printed by the post-processor using the Read button.
    You can run the simulation step by step for each line on the Control panel page.
  • Waterjet cutting by advanced machining pages wire-frame functions
    Using advanced machining functions by the Moduleworks add-on we will prepare tool paths and output these as g-code programs to run on our simultaneous multi-axis waterjet machine.
    1. Import your 3D or wireframe models that define the part.
    2. Move the part model to the correct position which will conform to the reference position on the CNC waterjet machine.
    Make sure the maximum Z coordinate of the part model is Z = 0. All part positions must have negative Z coordinates in the CAD system for a safe cutting trajectory.
    You can make an axis-aligned enclosing box for moving the part model easily. That box will enable you to pick corner positions correctly. The corners of the box are the maximum and minimum points of the model along the coordinate axis. Geo, the Make Box menu path will open the page to make the axis aligned box. And as soon as the page appears you can select models for the box from the graphics window. When you finish your selection, the axis-aligned box will appear. Then you can move a corner point of this box to the origin of the coordinate axis together with the part models.
    3. Make wireframe curves out of surfaces.
    You will use the Surface, Extract surface edges menu path.
    4. Make the lines that will represent nozzle direction on important points.
    We will use the Direction, point, and length function of the Make Lines page to draw the nozzle direction lines. Nozzle direction on some specific points can be defined using the side walls.
    5. Now you have all geometric data ready for making the toolpath operations.
    Open the advanced machining pages. The menu command path is Advanced Machining, Show GUI.
    6. Define a cylindrical tool that represents waterjet.
    We will make its diameter 1mm.
    7. Select the wire-frame machining tab.
    8. First select Drive curves for the tool path.
    9. Select Orientation lines.
    These lines represent nozzle directions relative to part geometry at those positions. The nozzle axes vectors between these given definitions are calculated by linear interpolation.
    10. Select a machining side for the offset of 1mm waterjet.
    11. Define the lead-in and lead-out types.
    12. Check retract plane definitions for safe link moves.
    13. Check the toolpath by animating and if there are any changes needed you may give the menu command See parameters by right-clicking the operation on tree-view.
    14. We will copy-clone the operation for other pockets.
    We need to click on the Transform toolbar icon and give the copy repeat no as 14 for this particular example.
    15. After cloning we will send all the operations to the OutputBox on the tree-view and print out our program g-code to run on the 5axis simultaneous CNC waterjet machine tool.
  • Water Jet Entry, Exit, and Angled Cutting
    In this video, we will work on an example for the entry and exit distances for each edge of the part for the water jet and angled cutting.
    1- You can select the machining side of the tool as right.
    In this case, there will be a tool offset similar to a car moving from the starting point and shifting to the right as it progresses. If, after calculating the toolpath, the offset is not on the desired side, select left instead of right and press the "Recalculate" button.
    2- There are three different options for entry and exit.
    Ramp pitch is used to determine the movement of the tool in the Z-axis during entry and exit.
    Direct: In this option, the tool enters and exits the cut directly.
    Arc: In this option, the tool enters and exits the material using a defined circle diameter and angle.
    Line: In this option, the tool enters and exits the material using a defined line length and angle.
    3- The start and end cutting allowance shortens or extends the selected cutting path.
    Positive values shorten the path and are used to leave a holding allowance to prevent the material from breaking.
    Negative values extend the path in its own direction. The circular or linear extensions defined in the entry/exit page are added to the calculated path, including the holding allowance or the extended path.
    4- Angled cutting:
    The A angle value is displayed, and you can click on it to set the angle.
    If the A angle value is not active, check the option Rotate around tangent line in the Tool Axis menu. When the Add conic angle editor option is active, after calculation, a drawing of the tool rotated by the specified angle and the angle value will appear on the screen. You can click on the angle value in the graphic display to modify it.
Back to the Menu