OK, you've designed your first model and completed your first toolpaths. Now you're wondering how to make your CNC machine cut the part. For that you need a Post Processor.
What is a Post Processor ? A Post Processor (also referred to as a "Post") is a translator that converts the picture of the toolpath you see on the screen, into the language that your CNC machine understands. In most cases this language is G-Code, even though some controls may use a more conversational format. We will refer to it as "G-Code".
What is G-Code? If you don't know what G-Code is and you need more information, you should review the documentation contained in the Autodesk CNC Handbook. Review the chapter on "CNC Programming Language".
|
Access: |
Ribbon:
CAM tab
Toolpath panel
Post Process
|
Overview of the Post Processing Dialog.
- Use Personal Post Library - Folder location of your custom Posts.
- Use Installed Post Library - Folder location of the standard Posts
- Open Autodesk HSM Post Library - Go and search the on-line Post Library
- Open Folder - Open the current folder location
- Refresh - Refresh the list of Posts in the folder
- Reset Output Folder - Restore default Post folder location
- Add Cascading Post
Setup
Post Configuration: This is where you can select the active Post.
- Type a key word that represents your machine/control. "Centroid", "Mazak", "Anilam", etc...)
- set the All filter to limit the type of machining (Milling, Turning, Mill/Turn, Cutting, etc) .
- set the All Vendor filter to the Machine Manufacturer or Control Type.
Filtering The Available Posts.
In the Post selection area, Posts that match your selections will be shown. If no Posts are shown, adjust your search filter options. If you still cant find a post that seems correct for your machine, go back to the Setup (shown above) and select "Open Autodesk HSM Post Library". The on-line library has a larger selection of Posts to choose from.
Output Folder - Is where you want you new NC Program to be saved.
NC Extension - Most of the time the NC file extension will be .NC. Some machines may require specific file extensions.
Program Settings: These are things that can be inserted into the NC program, or will effect the output format of the NC program.
- Program Name or Number - An ID number at the beginning of the NC program used to select or activate it
- Program Comment - Text to define what this program is for. It can be a part number, description or customer name
- Unit - Keep the units the same as the Document - force Inch output - force Metric output
- Reorder To Minimize Tool Changes - When checked, this groups together operations that use the same tool
- Open NC Editor - Opens the default NC Editor to you can view the NC Program
Most machines/controls can have several ways of doing the same thing. NC Programs can also vary based on the available machine options. The Post will usually have "switches" to turn on/off functionality. In the section highlighted below, there are a number of switches that can alter the output of the NC Program. If a Post doesn't seem like it's right for your machine, It might simply be that you have something turned on/off that's effecting the output. Not Every Post Processor Will Have The Same Switches.
- Allow Helical - Inventor HSM will always do helical. But this can reduce your program size .
- Set to Yes, you will get G2/G3 IJK Helical Arcs - No, it outputs many 3D linear moves.
- High Feedrate - Is the fastest your machine can move at a programmed feedrate (G1 F###)
- Maximum Circular Radius - Some controls have a limit of how big an arc can be
- Arc Format - Use IJ centers G2 XYIJ or use Radius G2 XYR
- Use 4th axis - Suppress 4th axis indexing/rotary output for a 3 axis program.
Examples of what these switches can control.
If you have a Post Processor and just want to generate NC Code, see the chapter on : Post Processing NC Code.