The RPC uses Delcam PowerMill to process and program for the DAAP CNC milling machines. The tutorials on this and subsequent pages are being made available to students who wish to learn how to be more self sufficient in toolpath programming. This tutorial will cover basic interaction with PowerMill and the general premise of 3-axis CNC programming.
Additional information for machine specific programming:
All DAAP CGC computer labs should have PowerMill 2010. From the Windows7 environment type powermill
on the "Search for programs and files" prompt line or navigate through the Applications folder, Delcam, PowerMILL, PowerMILL 2010 and run the following executable:
Make sure that you do not run PowerMill in training mode, you will be unable to save your files!
The PowerMill Interface
- Explorer Pane
- Viewport Pane
- Viewing Toolbar
- Main Toolbar
- ViewMill Toolbar
- Simulation Toolbar
- Tool Toolbar
- Status Toolbar
Similar to many Adobe programs, PowerMill tools are grouped in toolbars
that can be added to and subtracted from the interface at the user's will. If the interface that you see when opening PowerMill does not match the above, navigate to the toolbar list through: View, Toolbar
. It is recommended that you select Main, Explorer, Viewing, ViewMill, Status, Tool and Simulation
The explorer pane allows you to browse through the elements of your project. Right-clicking any of the headers in the explorer menu will allow you to create new elements in your project.
header for instance, allows you to import new .IGES
geometry exported from a CAD program.
The Explorer pane is also used to run the Set DAAP PowerMill Session
macro. It can be accessed on PowerMill's User Menu, simply right-click in the empty space of the Explorer pane to show the DAAP CAM User Menu 10A
Running this macro configures the software with several important presets and user settings that enable you to connect to the RPC's centralized resources. PLEASE NOTE: Other tutorials will not work as described if you skip this step.
The Viewport area in the center of the PowerMill interface operates on a similar premise to many other CAD programs. Mouse controls for the Viewport are:Left-Click
to pick individual elements or click and drag to window pick multiple elements.Shift-Left-Click
to add to selection.Ctrl-Left-Click
to subtract from selection.Middle-Click
and drag to rotate the model view.Shift-Middle-Click
and drag to pan the model view.Ctrl-Middle-Click
and drag to zoom the model view. Drag up to zoom in, down to zoom out.Right-Click
on any surface, wireframe or toolpath to call up a menu for that element.
The white wireframe corner in the center of the Viewport is the origin
(X 0 Y 0 Z 0) for the active project. Align your CAD model near the origin in the positive quadrants before exporting as an .IGES
The Viewing toolbar on the right hand side of the interface contains buttons that control the viewport and model shading. From the top of the bar, the icons control orthographics, isometrics, zoom to fit, block view, shading, wireframe and selection. Holding your cursor over an icon with a
opens a jump list of additional viewing tools.
toolbar is home to most of the common and necessary buttons used in CNC programming.
button will call up the Block dialogue.
The block is a virtual representation
of the piece of material you plan to mill. The dimensions entered in the Limits section of the dialogue should match the measurements of your physical stock
. In the viewport the block is displayed as a translucent box.
The Rapid Move Heights
button will call up its accompanying dialogue.
Rapid Move Heights define a value on the Z axis where the mill will not collide with your block
during the program. This allows the mill to move quickly across the model between cutting paths and operate more efficiently. The Safe Z
field defines the maximum height that the tool will pull up to move across the block, the Start Z
field defines height at which the toolpath will slow down as it prepares to encounter the block. Setting accurate rapid move heights is an important step in creating a safe and functional program.
The Toolpath Strategies
button opens the Strategy Selector.
The Strategy Selector contains templates for various methods of milling. Several of the tabs at the top of this window contain templates made for the specific machines
of the RPC. Use these preset templates in PowerMill to generate toolpaths that can be successfully run on RPC CNC machines. More information on toolpath selection will be provided in the general strategies section.
The Toolpath Verification
button opens its respective dialogue after a toolpath has been calculated.
Clicking the Apply button on this dialogue calculates whether or not an active toolpath will collide with the model it is cutting around. This can occur in cases where a tool attempts to reach a depth that is too steep and/or deep
or if settings such as the rapid height have not been correctly input. Keep in mind that as the diameter of a mill decreases, the reach is also compromised.
It is also important to keep in mind that PowerMill saves project folders
rather than individual files. Opening a project only requires that you browse to the project folder that you saved to. When submitting a PowerMill project to the RPC online it is necessary to compress the project in a .ZIP
button will call up a small dialogue that allows you to pick points on your imported geometry. The dialogue will calculate point to point differences in the X, Y and Z axis, total distance between points, and can be used to find the exact diameter of a circular or semicircular object. This can be useful when organizing your model parts to accommodate mills or when deciding what type of tool to use.
ViewMill and Simulation
The ViewMill toolbar is used to test Toolpaths and NC Programs prior to execution in a mill to ensure that it will function as intended. Viewmill is inactive by default until the On/Supsend
button is clicked. Starting ViewMill will enable the Simulation bar as well.
These toolbars work in conjunction. ViewMill controls the simulation environment and the Simulation bar allows you to select a specific toolpath to view. When ViewMill has been activated, the shaded block for the active toolpath will become solid. Selecting a toolpath from the Simulation menu and using the Play/Pause controls will show a virtual representation of your toolpaths milling the virtual block. Using the Rainbow Shade mode as shown activated on the ViewMill Toolbar above, the toolpaths will be color coded as they are played.
The Tool Database
The Tool toolbar and the Tool Database Search are important tools in managing and exploring the catalog of mills that the RPC has in its inventory. The Tool Database Icon
will call up the Database Search dialogue.
The standard tools used on the Bridgeport and Autoprofiler can be easily imported to a project without involving the Tool Database, but for specialized programming with non-standard Bridgeport tools and most Komo work
, the Database Search is a much easier way to navigate the catalog.
The simplest way to pick out a tool set is from Stock Material
list. All of the materials in the drop down Stock Material
list have preset cutting data for a group of mills. Check the Use Stock Material
box and use the material list to refine your search. By picking a material such as Styrofoam and clicking the Search
button the Search Results
field will be populated with a list of all the tools programmed to cut styrofoam, more importantly, when you import the the tools by picking them from the list and clicking the Create Tools
button, the cutting presets will be loaded automatically.
PowerMill's Tool Database Search engine also allows advanced users to call out specific parameters for tools including the tool Name, Diameter, Length, Number of Flutes and Type (the profile of the cutting edge)
. Using these guidelines you can easily narrow down your results to find a specific tool or tool set.
When searching based on tool names it is important to understand the naming convention
used in the database. Each tool is named with the following convention (Type)(Features)(Flutes)(Diameter)(Tag)
. Every tool has a unique name that describes it, as shown in the search results in the image above that can be used to quickly identify groups of tools. The 3 letter tag
at the end of every tool's name describes the machine it belongs to. Use any of these tags in the Search String
field to find a corresponding group:
||Bridgeport Machining Center
||KOMO CNC Router
General 3-Axis Strategy
The RPC CNC mills and router operate on similar 3-axis systems. This strategy has its pros and cons: it can be adapted to a wide range of materials
and fabricate accurately on small or large scale
models yet lacks the ability to produce "undercuts"
or any shape that wraps under a vertical slope.
CNC programs are created from a number of "toolpaths", mathematical linework that defines the motion of the tool, specifically the tip of the cutting edge. PowerMill displays toolpaths as green wireframes
The pattern of toolpaths are spaced depending on the type of machining taking place. There are multiple general strategies for toolpaths.
The Roughing strategy is aimed at removing the greatest amount of material
from the raw block. Roughing is usually associated with large, flat mills
that can quickly and efficiently clear away large spaces. This will leave a terracing effect on the block in the general shape of the final model.
Because roughing can be a very destructive process, a shell thickness of 0.05 inches
is added around the model to shield the final surface.
Depending on the amount of detail in a model, several roughing paths may be run with progressively smaller mills in order to remove material in small spaces. This is called Rest Machining
as it removes the rest of material left by the preceding tool.
Finishing strategies are used to further refine the block after roughing. A Semi-Finish
path is used to remove more of the terracing and added thickness from the roughing path. Semi-finishes are done on objects that are sculptural in form (having surface data being being convex or concave). Objects that are 2.5 axis in behavior (meaning a top view profile that does not change), will not require a semi-finish.
, then a Final Finish
mills down to the surfaces of the CAD model.
Notice that the finishing toolpath is tightly knit across the surface of the model, and that this path uses a ball mill
in order to achieve a clean result.
As with the Roughing strategy, Corner Picking is a type of rest machining
for finishing. Because larger tools are limited by their radius, smaller diameter mills must be used to clear out detailed pockets and corners
In addition to the 3 main strategies of CNC, there are also several used for unique modeling situations.
In cases where a model has significant flat faces positioned horizontally or vertically
, Flat Finishing and/or Vertical Finishing may be employed to create an even plane. This type of path resembles the Roughing strategy in that a large tool is used to clear a wide area.
Drilling with CNC is very similar to manual drilling. In instances where a simple hole must be made drilling can sometimes be the best option.