Tutorials:-Working with Power MILL " PART I" To Generate the Programs(G-coded & M-coded) For Various CNC Machines.

Let Start With Beginning..

  1. Step 1:

    Start PowerMILL
    • Double click the relevant Power MILL shortcut icon on the desktop:

    Note:- On the training pc the icon will be displayed as PowerMILL .

    The following screen is then displayed:

  2. Step 2:

    The screen is divided into the following main areas:
    1) Menu Bar - clicking one of the menu names on this bar (for example, File) opens a pull-down list of associated commands and sub-menus. A sub-menu is indicated by a small arrow to the right of the text (for example File - Recent Projects >). Highlighting this arrow generates a list of commands/names specific to that sub-menu (for example, File - Recent Projects displays a list of recently opened projects that will open directly when clicked).
    2) Main Toolbar - this provides quick access to the most commonly used commands in PowerMILL.
    3) Explorer - the Explorer provides control options and storage of PowerMILL entities created during the session.
    4) Graphics Window - this is the working area.
    5) View Toolbar - provides quick access to the standard views and shading options in PowerMILL.
    6) Status Bar - reveals information relating to the current display. This can, for example, be a brief help description of the item beneath the cursor or information about the calculation that is in progress.
    7) Information Toolbar - this area provides a reminder of some of the active setup options.
    8) Tool Toolbar - facilitates the rapid creation of tools in PowerMILL.

    The other toolbars are not factory defaults, and are therefore not shown at initial startup. To display any of these, select using the relevant option under View - Toolbar, for example View - Toolbar - Toolpath to display the Toolpath Toolbar:

  3. Step 3:

    To change the colours of the background, select Tools - Customise Colours and select View Background. The Top and/or Bottom colours can be changed independently and Reset using Restore Defaults to restore to the original settings:

    PowerMILL remembers Toolbar and colour selections from one session to the next, for example, if the Toolpath Toolbar is open when the session is closed, it will appear the next time that PowerMILL is opened.

  4. Step 4:

    View Spinning- Dynamically rotate the view and quickly release the mouse. The faster the mouse the faster it will spin. This feature is switched off by default.
    Mouse buttons
    Each of the three mouse buttons perform a different dynamic operation in PowerMILL.

    Mouse button 1: Picking and selecting

    This button is used for selecting items off the pull down menus, options within forms, and entities in the graphics area.

    Mouse button 2: Dynamics

    Zooming in and out: - Hold down the CTRL key and mouse button 2. Move the mouse up and down to zoom in and out.
    Pan around the model: -Hold down the SHIFT key with mouse button 2. Move the mouse in the required direction.
    Zoom Box – hold down the Ctrl and shift key, drag a box around the area to zoom into using the middle mouse button.
    Rotate mode: Hold down mouse button 2 and move the mouse, and the rotation is centered about the trackerball.

    View Spinning- Dynamically rotate the view and quickly release the mouse. The faster the mouse the faster it will spin. This feature is switched off by default.

    • Select Tools -> Options, select the View tab and tick the option Spin View.

    Mouse button 3: Special Menus & PowerMILL Explorer Options

    When this button is pressed it brings up a local menu relating to whatever the mouse is over, such as a named item in the PowerMILL Explorer or a physical entity in the graphics area. If nothing specific is selected the View menu appears.

  5. Step 5:

    Simplified PowerMILL Example

    This example provides a quick overview of the machining process. It shows how to create and output a couple of simple toolpaths on a model of a valve chamber (using default settings wherever possible).
    The basic procedure is:
    1. Start PowerMILL.
    2. Import a Model.
    3. Define the Block from which the part will be cut.
    4. Define the cutting Tools to be used.
    5. Define Set up options (Rapid Move Heights – Start and End Point).
    6. Create a Roughing Strategy.
    7. Create a Finishing Strategy.
    8. Animate and Simulate the toolpaths.
    9. Create an NCProgram and output as a post-processed ncdata file.
    10. Save the PowerMILL Project to an external directory.

  6. Step 6:

    Import a Model

    • From the main pulldown menus select, File - Import Model and browse for the model file:-

  7. Step 7:

    Definition of the Block

    • Click on the Block icon on the top toolbar.

    The Block Form is used to define the 3D working limits. This could be the actual raw material size or a user defined volume, localised to a particular part of the component.

    The Block Form default is Defined by - Box around the model dimensions on clicking the Calculate button. Individual values in the form can be edited or locked (greyed out) as required in addition to being calculated to include an offset by entering a suitable value in the box marked Expansion.

    • Click on the Calculate button.
    • Click on Accept.

  8. Step 8:

    Cutting Tool definition

    The Tool definition forms are accessed from the icons accessed from the Tool toolbar located to the bottom left corner of the graphics area.
    For use with this example, 2 tools will be created, A Tip Radiused for roughing out and a Ball Nosed for finishing.
    •Click on the down arrow to display all of the Create Tool icons.
    All of the tool types appear as icons.
    Placing the cursor over an icon will open a small box containing a description of the tool type (Tool tips). Note the unavailable, greyed out tool definition icons are only available in PowerMILL Pro.
    • Select the Create a Tip Radiused tool icon.
    The Tip Radiused Tool form opens ready for the user to input the required values. When a diameter value is input the tool length automatically defaults to five times this value. This value can be edited if required.
    It is highly recommended to input a more appropriate Name for the tool. In this case the tool has been renamed as Name D12t1.
    If appropriate, a specified Tool Number can be output to the NC program. If the machine has a tool changer this number will represent the location in the carousel.
    •Enter a Diameter of 12 a Tip Radius of 1.
    •Enter D12t1 in the box marked Name before Clicking on Close.

    •Repeat the Tool Definition operation, this time selecting ‘Create a Ball Nosed tool’ and in the form entering a Diameter 12 with a Tool Number 2 before and enter the name BN12 before Clicking on Close.
    •In the explorer panel on the left of the screen, open the tools and right mouse click on the D12t1 tool to raise the local menu. Select Activate.

  9. Step 9:

    Rapid Move Heights

    The Rapid move heights form is essential to allow the user to safely control rapid tool movements across the workpiece. Safe Z is the height above the job at which the tool can move at rapid feedrate, clear of any obstructions such as the workpeice or clamps. Start Z is the height to which the tool will descend, at rapid feed rate prior to applying the plunge feed rate. PowerMill displays rapid moves as dotted red lines, plunge as pale blue and cutting as green.
    •Click on the Rapid Move Heights icon.
    •In the resultant form select the Reset to Safe Height button.
    •Click on Accept.

    This will automatically set absolute SafeZ and Start Z values to be above the block by the distance in the incremental height fields shown at the bottom of the form.
    An absolute setting will always cause the tool to feed down from the same height.

    In the section of the form labelled Incremental Heights, in addition to Absolute, two additional options are available Plunge and Skim.

    Plunge will enable the rapid feed rate to continue to a specified distance above the full plunge depth before the plunge feed rate cuts in.

    Skim will operate in a similar way to Plunge but with the addition of applying rapid horizontal moves, at a specified distance above the highest point across the component to the next plunge position.

  10. Step 10:

    Tool Start and End Point.

    • Click on the Tool Start and End Point icon.

    The Start and End Point form allows the user to define a position where the tool travels to before and after a machining strategy. By default the tool Start Point is set at Block Centre Safe. Other Start and End Point definitions are achieved by selecting different options in the Method area on the form.
    These include First/Last Point Safe, First/Last Point, and Absolute.

  11. Step 11:

    • Accept the form with the default settings.

    The D12t1 tool is positioned at the Block Centre Safe position ready for the user to create the first toolpath.

  12. Step 12:

    Creating a Roughing Strategy

    • From the Main toolbar select the Toolpath Strategies icon.

    •Select the 3D Area Clearance Tab.
    •Select the option Raster AreaClear Model to open the following form.
    •Input the new Name D12t1-a1 for the toolpath that will be created.
    •Edit the Thickness value to 0.5. This is the amount of material that will be left on the job
    •Edit the Stepover value to 10. This is the distance between each raster pass (the width of cut).
    •The Stepdown value (depth of cut) is left at the default of 5 mm.
    •Click the Apply tab to process the machining strategy.