12
July
2012

Feed Table in NC Programs

Sometimes the user wants to be able to modify feedrates in the NC program itself. This is often desired for production to optimize programs for reduced machining time, part quality, and tool wear. However, editing NC programs manually is normally not recommended unless supported/intended by the used post processor configuration.

The generic Heidenhain post now includes sample code showing how to output feedrate tables using Q-values for each operation which can be easily modified. The feedrate tables are disabled by default but can be enabled by setting the "useFeedQ" property during posting. The same code can be used for any control which supports parameters.

Note that only feedrates actually used for a given operation are being output. HSMWorks supports many different movement types for increased flexibility but a comment describes each feedrate so the user knows it´s 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+.
...

  • Tags: Post Processing

Categories: HSM Tips and Tricks

Leave a comment

You are commenting as guest.