Just an FYI to to all Post-Processor Developers regarding SIEMENS 840D Posts for Mills. Please stop treating G17, G18 & G19 as if they act just like FANUC codes! THEY DO NOT! G17, G18 & G19 have different in-feed directions for the application of Tool Offsets. Treating
G18 or G19 just like FANUC will cancel the current tool length offset
in G17 and will cause the tool to take a dive directly into the part! I'm
now repairing a machine because of a crash caused by someone editing a
post and not having a proper understanding of the control. If G18& G19 are to be supported, then the proper application of G18 &
G19 is crucial. Since the infeed direction changes when a new plane
code is encountered, the machine must be told which direction to apply
the tool length offset using the TOFF or TOFFL command. While
this will work if you actually want to see G18 & G19 and cut arcs in
those planes, it is unnecessary. For anyone who wants to cut 3D arcs
with SIEMENS, your choices are use CIP arcs for everything, (Brute Force
but it will work) or simply insure that arcs in the G18 & G19
planes are formatted as shown below. Make sure treat axis addresses and arc centers as non-modal. G02/G03 X---- Z---- I---- K---- F G02/G03 Y---- Z---- J---- K---- F No
G18/G19 code required at all as SIEMENS will automatically process the
arcs for the proper planes while the active plane is still G17! Helical
Arcs in the G17 XY plane must have all 3 addresses (XYZ) present in the
line of code. Modality of the axis addresses is not supported for
Helical Arcs. Sections 8.2 & 5.8
of the SIEMENS Fundamental Programming Manual (6FC5398-1BP40-3BA1) deal
with Plane Selection and programmable tool offsets. Paying attention to this basic code formatting information will eliminate costly machine crashes and down time. |
↧
FYI to Post-Processor Developers regarding SIEMENS and G17, G18 & G19
↧