Feed

Tutorials:-Working with Power MILL "PART III" 3D Area Clearance.

Tutorial by Sourbh
Small

next here

  1. Step 1:

    Offset Area Clear example

    •Import the model WingMirrorDie.dgk from D:\users\training\PowerMILL_Data\models.
    • Create a Tip Radiused tool of Dia 40 tiprad 6 and Name d40t6.
    • From the Main toolbar open the Block form and Calculate a material block Defined by - Box to the full model dimensions.
    • Reset the Rapid Move Heights and set the Incremental moves to Skim.
    • In the Start and End Point form set the Start Point to Block Centre Safe and the End Point to Last Point Safe.
    • From the Main toolbar select the Toolpath Strategies icon
    • In 3D Area Clearance select the option Offset AreaClear Model to open the following form.
    • Enter Name D40T6_D1.
    • Select Ramping.
    • Select Ramping Options Entering;
    Max. Zig Angle 4,
    Follow Circle, and
    Circle Diameter 0.6
    • Input or modify the data as shown in the sections arrowed above and click Apply to create the Offset Area Clear toolpath shown below.

    The Offset Area Clear strategy using Type All follows both the contours of both the Model and Block then gradually Offsets into the remaining material at each Z Height.
    • RMB on the toolpath and select
    Simulate from Start to bring up
    the Simulation toolbar

    The toolpath simulation toolbar will open

    • Select the ViewMill On/Suspend icon. from the ViewMill Toolbar,
    followed by the Shiny Shaded image icon .
    • Press the Play button to start the simulation.

    The simulation of the toolpath will start with tool displayed, but this can be controlled by toggling the light bulb on the tool entity in the explorer pane.
    NB. Not drawing the tool will speed up the simulation.

    The finished result indicates that the current tool geometry is not suitable to fully access some features (arrowed) on the model.
    As a result a further Area Clearance strategy is required using a smaller tool to continue locally into the remaining areas.
    This technique is known as Rest Machining.
    • Suspend ViewMill
    • Switch off the shaded image


  2. Step 2:

    Rest Machining

    Rest Machining is localised removal of material that remains in areas not accessible by larger tools used in previous toolpaths. The 3D Area Clearance forms contain options to apply Rest Machining either based directly on a previously defined Reference Toolpath or a Stock Model.
    The following examples illustrate Rest Machining using a Reference Toolpath.
    PowerMill Pro is also able to use a Stock model for this purpose. That functionality is covered in the supplementary PowerMill Pro Course.

  3. Step 3:

    Rest Machining using a Reference Toolpath

    • Create a Tip Radiused tool of Dia 16, tiprad 3 and name d16t3.
    • Right mouse click over the Toolpath icon in the explorer
    • Select Settings to reopen the Offset AreaClear Model form.

    icon.

    Note; all associated items originally used to create the toolpath will be activated.

    • Activate the new tool, d16t3.

    Enter a new name D16T3_D1.

    Enter:- Thickness 0.5 Stepover 1.0
    Stepdown 5.0

    The options arrowed control the Rest Machining limits by comparison with the previously defined toolpath D40T6_D1.

    Type All is the only available option for the basic PowerMILL license.

    Untick Area Filter

    • Input or modify the data exactly as shown above and click Apply to create the new Offset Area Clear toolpath shown on the following page.
    • Cancel the form.

    • Save Project as
    D:\users\training\PowerMILL-Projects\Wing_Mirror_Die.
    • Turn ViewMill On
    • Select the Rainbow Shaded Image .
    • Select the toolpath D16t3_D1 and Play the simulation.

    The ViewMILL simulation shows this next toolpath shaded in a different colour where it has machined in areas the previous toolpath did not cover

    The Reference Toolpath finished to rough out material closer to the component form.
    This will reduce the risk of excessive wear or damage to tools used for the subsequent finishing operations.
    • Select the Suspend ViewMill icon to return to PowerMILL

  4. Step 4:

    General information on Area Clearance Machining

    The following is reference information for the many different options contained in the Area Clearance form. This can also be found by using Help.
    Clicking the Thickness button on the Area Clearance forms opens the Axial Thickness box allowing the user to set separate values for Radial and Axial thickness. This faclity is also available on the finishing forms.

  5. Step 5:

    Z Heights

    If Stepdown is set to Manual on The Area Clearance form, there are five ways of generating Z Heights; Number, Stepdown, Value, Intermediate and Flat.

    Number - divides the block equally into the defined number of Z Heights, the lowest of which will be at the bottom of the block.

    Stepdown - creates a Z Height at the base of the block and then steps up a defined Height in Z. The setting Maintain Constant Stepdown causes the distance between all levels to remain constant and will modify the stepdown to create evenly spaced levels as near to the specified value as possible.

    Value - creates a single Z Height at the defined value. You can specify as many Z Heights as is required, but when using Value you must do so one at a time.

    Flat - Identifies flat areas of the model and creates a Z height (+ thickness) at these values.

    Intermediate - adds the specified number of Z Heights between existing Z Heights.

    Appending Z Heights
    Z Heights can be also be used from saved Area Clearance Toolpaths. When a toolpath is activated the Append button becomes active.

  6. Step 6:

    Profiling
    A profile can be performed at each level to remove steps that will be left by the cutter Before, During, or After a Raster - Area Clearance strategy. Additional profile passes can be applied when machining either on either Every Z, or the Last Z level with Offset, Profile or Raster strategies. Note: Offset and Profile strategies inherently follow the component profile.

  7. Step 7:

    When
    This determines when the profile pass takes place during machining. There are 4 options

    None – No profiling pass is performed
    Before – PowerMILL will perform the profiling first and then the raster path.
    During – As the raster path is generated it will find profile paths as it goes.
    After – PowerMILL performs the profile pass last.

    Cut Direction
    This determines the direction of the tool. Choosing a single direction will more than likely lead to more lifts generated.
    Any – this allows the cutter to travel in both directions allowing it to climb mill and conventional mill.
    Climb – this will force the cutter to only travel in one direction so that it is always climb milling.
    Conventional – this will force the cutter to only travel in one direction so that it is always conventionally milling.

  8. Step 8:

    Final Profiling Pass
    This option is held in the profiling area of the main area clearance toolbar and allows the user to make an additional, final profiling pass to further reduce tool wear.
    Allow tool outside block
    The Allow tool outside block tick box is located in the Expert Area Clearance form, which is opened by selecting the tab midway down the right hand side of the main form.
    This enables the first pass of an Offset or Raster pass to be performed to the specified Stepover, rather than the full radius of the tool.

  9. Step 9:

    Ramping
    This provides a way to lead down onto a tooltrack where it is impossible to approach from outside the Block at the full machining depth (eg within a pocket).

    The Zig angle is the angle of descent along the machining direction as the tool ramps into the material. There are 3 different types of ramp move following the geometry of the Toolpath, a Circle, or a Line. If the length of the Zig angle is limited to a finite distance a ramp move in the opposite direction, Zag angle can be applied.

    The Ramp Length is defined as ‘Tool Diameter Units’ (TDU). For example, with a 10mm diameter tool, A Ramp Length of 2 TDU’s would equal 20mm. Normally the Ramp Length should be greater than the tool diameter to allow swarf to clear from beneath the tool.

    Zag Angle
    If a finite ramp length has been specified, then PowerMILL will insert Zag moves. The default setting for Zag angle has the Independent flag set - which means the angle, is defined manually. The default angle is 0 degrees. When unset, it will be the same value as the Zig angle.

    If Approach Outside is set, and where it is practical for it to operate without gouging it will take priority over Ramping.

    If the defined geometry for a Ramp move is such that it would cause a gouge then it will be replaced by a Plunge move.

  10. Step 10:

    Machining Flats
    The area clearance strategies in PowerMILL have an option that allows the user to control the way in which flat areas of the model are rough machined. These are found on the area clearance form under Machine Flats.

    • Import the model ….\PowerMILL_Data\Models\Flats.dgk
    • Create a 12mm diameter End Mill tool and name it EM12
    • Calculate the Block using the default settings.
    • Set the Rapid Move Heights and check Start/End Point is set to default; Start Point - Block Centre Safe and End Point - Last Point Safe.

    • From the Toolpath Strategies form, select Offset Area Clearance.
    • Apply and then Cancel the form

    It can be seen that with Machine Flats - Off the toolpath has ignored the flat surfaces of the model. It has maintained a constant Stepdown value and completely performed area clearance across the material Block at each Z Height.
    • Right mouse click over the Active toolpath and in the local menu select Settings
    • Select make a Copy of the toolpath.
    • Change the Machine Flats option to LEVEL (This is the default).
    • Change the name to Flats_Level.
    • Apply and then Cancel the form

  11. Step 11:

    The Area Clearance toolpath now removes material from the Flat surfaces leaving just 1.1mm this is equal to the thickness plus the tolerance set in the form. Where new slices have been added, the toolpath clears all the way to the edge of the block.

    • Right mouse click over the Active toolpath and in the local menu select Settings
    • Select make a Copy of the toolpath.
    • Change the Machine Flats option to AREA.
    • Change the Name to Flats_Area.
    • Apply and then Cancel the form.

  12. Step 12:

    The Component is fully area cleared at the general Stepdown heights and locally to the edge of the component Flat areas. This provides a shorter toolpath compared with using the Level option.
    • Save Project as:- D:\users\training\Projects\AreaClearFlats

  13. Step 13:

    //Thanks//

Comments

Please log in to add comments