G83 cycle not behaving exactly as expected

[Denford Admin]

A customer has asked if there is a problem with the G83 peck drilling cycle in v5 milling.

Their example program was:

Code: Select all

G21
[billet x50 y50 z20
G00x0y0m03s2000
G90G1Z50.h01F2000
G83g98r3.z-3.q1.f600x0y0
G80g00z50.
m30

which produced a pecking cycle like this:
feeds to z-1mm at f60 from 50mm up
As I keep clicking it rapids back up to 50mm
Back down to 3mm
Feeds to z-2.
Rapids to 50mm
Rapids to 2mm
Feeds to z-3mm
Rapids up to 50 and is finished.

This dosn't seem quite right, as there is a seemingly random move to Z2 in there. It's also odd to rapid back up to Z+50mm each time as well.

So, to fix the rapid back to Z+50, change the G98 to G99 which tells the software to return to the programmed R level (Z+3) and not the Initial level (Z+50):

Code: Select all

g21
[billet x50 y50 z20
G00x0y0m03s2000
G90G1Z50.h01F2000
G83g99r3.z-3.q1.f600x0y0
G80g00z50.
m30

There is a configuration file in C:\Program Files\Denford\VRMilling5 called cycles.ini
This can be edited in Notepad.
Under the section for G83 [83], the command Peck Z = 4 means that after a return to initial or return to R level, there will be a rapid back down to 4mm above the last peck depth.
To make the cycle work as explained in the help file: “Rapid traverse out to R point. Rapid traverse back to within 1mm of depth of Q cut”
Then set this value to Peck Z = 1

Now, the peck sequence should be like this:
Rapid Z+50
Rapid Z+3
Feed Z-1
Rapid Z+3 (Return R level)
Rapid Z0.0 (Rapid back to 1mm above last peck)
Feed Z-2
Rapid Z+3
Rapid Z-1 (Rapid back to 1mm above last peck)
Feed Z-3
Rapid Z+3
Finished

Hope this makes sense...I believe it behaves like the Fanuc high-speed peck drilling cycle in that it will rapid back very close to the last cut depth.
It would seem we have set the default to 4mm above last cut, to make it less likely to crash or stall the machine.

[Denford Admin]

After looking at the cycle closely we've found that it was not behaving correctly and certain presumptions had been made.
The cycle has been corrected in v5.33 VR Milling which will be available shortly.

The following document explains how the G83 peck drilling cycle should work:

[Denford Admin]

v5.33 is now available:
viewtopic.php?f=2&t=2860