Get familiar with the feedrates.
The generic post processors included with Fusion have many features built into them. By default, some features are disabled because they may not be supported for all versions of a given CNC control, or they change the NC program code from how most programmers expect it to look. The feed parameter feature is one example of such a feature.
The generated NC programs should generally be ready for machining immediately after post processing and not require further editing manually. Choosing the best feedrates for a given setup can be quite difficult at programming time unless the setup remains consistent considering machining time, tool wear, part quality, and more. Only once the NC program is running on the CNC machine can you see if the feedrates are appropriate or need adjustment. The CNC operator often needs to prove-in the NC program, in particular for larger production batches, which makes it more convenient if the NC program allows easy editing during the process. The new found feedrates can then be updated within Fusion and a new NC program can be post processed again if required.
The generic Heidenhain post processor includes a feed parameter feature which allows the CNC operator to modify feedrates in the NC program itself with minimum changes. The Heidenhain post processor outputs feedrate tables using Q-values for each operation that can be easily modified. The feedrate tables are disabled by default, but can be enabled by setting the useFeedQ property during post processing. The feature can be added for any CNC control which supports parameters.
Note that only feedrates actually used for a given operation are output. Fusion supports many different movement types for increased flexibility, but a comment describes each feedrate so the user knows its purpose. Not all feedrates apply to all machining strategies, so the feedrate tables will likely be different for each operation. Feedrates not put into the feedrate table are output directly as values.
The program below shows an NC fragment for a pocket operation. First the feeds are setup using "FN0" and they are hereafter referenced using "FQ55" or similar.
10 * - #01: Pocket 32mm R1.25 / STEP 0.5 / TOL 0.05 11 L Z+0 R0 FMAX M91 12 TOOL CALL 6 Z S6000 13 TOOL DEF 5 14 M3 15 L X-4.741 Y-2.744 R0 FMAX 16 L Z+100 R0 FMAX 17 M8 18 FN0: Q50=7000 ; Cutting 19 FN0: Q52=6000 ; Entry 20 FN0: Q53=7500 ; Exit 21 FN0: Q55=4500 ; Ramping 22 FN0: Q56=600 ; Plunge 23 L Z+70.099 FMAX 24 L X-4.739 Y-2.734 Z+69.96 FQ55 25 CC X-18.483 Y+0 26 CP IPA+0.119 Z+69.824 DR+ 27 CC X-18.483 Y+0 28 CP IPA+0.195 Z+69.693 DR+.