can somebody please explain me on some examples of using these functions?
Could you show me some working nc prog. examples on 3+2 and tcpm machining you have?
I have some questions:
(mazak vrx i700)
It is neccesery to use G43.4 in one block with XYZ BC H ? Or it is possible to just put G43 H on separate line just before move? (for example like traori)
G43 H.. - can it be on separate line just before move as well?
I'm not sure about mazak but here is a Fanuc 31i output for G43.4
( operation: CONTOUR_PROFILE )
( stock: 0.00 )
( depth of cut: N/A )
G91 G28 Z0
M11 M71 (BC Unclamp)
G00 B12.529 C90.
G90 G00 G53 X0.0 Y0.0 S12000 M03 M08
N19604 Q4 R0
X.2244 Y-1.2878 Z6.0739 B12.529 C90.
M10 (B Clamp)
G01 X.2241 Y-1.8306 Z3.586 D400 F50.
X.223 Y-1.8211 Z3.5839
X.2211 Y-1.8117 Z3.5818
X.2185 Y-1.8024 Z3.5797
X.2152 Y-1.7934 Z3.5777
X.2111 Y-1.7847 Z3.5758
You can have on a separate line, but.....
1. Verify that the machine does not actually do a movement on the G43.4 line without a coordinate, it could be dangerous.
2. My code has the G43.4 H# on its own line, but I have seen some machines alarm out if there is no move commanded on the G43.4. I was always able to to work around this with a parameter change though. Ask your machine tool builder if you run into errors, or dig through the manual.
3. G49 cancels the G43.4, make sure you test the behavior of the machine when G49 is called. I have seen machines move down in -Z by the tool offset distance when G49 is commanded. Moving home (G91 G28 Z0) before the cancel usually eliminates this issue.
thanks I have already found some parameters in manuals too, it will be fun
I am wonder what machine will do in such case:
(G43 is active)
N36 X14.641 Y54.641
N38 G0 Z10.
N43 G43.4 C300. H1 I want to track tool tip with C rotating - Could it work like this?
N45 X81.603 Y58.66 Z-45. A-90
I want move only C on that line with tracking tool tip.
Thanks in advance