Post Processing NC-Code

Creating NC-Code For The Machine.

Post Processing is when you convert the image of the toolpath on your screen, into the language for a specific NC machine. This output is usually in the form of G-Code, an alpha numeric format used to drive the machine tool. Different machines will use variations of this G-Code format for their controls. So while there is some standardization of codes, not all machines use the identical G-Code format. Because of that, Fusion has a variety of Post Processors available. Think of the Post Processor as a language translator.

You can Post Process for any single toolpath or any combination of toolpaths. To select all toolpaths, click on Setup in the Browser. After selecting the toolpaths, you can right click over the operations and select Post Process. You can also access it by pulling down the Actions panel.

Access:

Ribbon: CAM tab

Toolpath panel

Post Process

Right Click over the operations.

Toolpath Panel.

On the Post Process Dialog page there are a number of things you can control. The main thing we're going to look at is selecting the correct Machine Post Processor. Pull down the list under the Post Configuration section of the Dialog and scroll to the Fanuc Generic Post. Inventor HSM includes a large selection of Post Processors for a wide variety of CNC Controls.

After selecting the Post Processor, press the Post button at the bottom of the page. If the "Open NC file in Editor" is checked, the default Editor will open and display the NC output.

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. Check the available switches to add or disable functions. Not Every Post Processor Will Have The Same Options.

Examples of what these switches can control.

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.

Important: Use all necessary safety precautions when testing the NC code from any new Post Processor.

Please note that the post processing time can vary greatly depending on the complexity of the post configuration and the size of the toolpath. Generally, post processing should complete within a few seconds. The post processor runs as a background task making it possible to keep working while the NC code is being generated. The post processor task is listed in the Task Manager. If the post processing fails (e.g. if the program name is not supported), the error message can be viewed from the task manager by opening the task log.