Cancel
Showing results for 
Search instead for 
Did you mean: 

G43.4, G43

Gears Phenom Gears Phenom
Gears Phenom

hello

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?

 

Thank you

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #
9 REPLIES

Re: G43.4, G43

Legend
Legend

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
G90
M11 M71 (BC Unclamp)
G00 B12.529 C90.
G90 G00 G53 X0.0 Y0.0 S12000 M03 M08
G10 L52
N19604 Q4 R0
G11
G43.4 H400
X.2244 Y-1.2878 Z6.0739 B12.529 C90.
M10 (B Clamp)
Y-1.8402 Z3.5881
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


Dennis Rathi
Creations Unlimited

Re: G43.4, G43

Gears Phenom Gears Phenom
Gears Phenom

thank you

I suppose in 3ax case G43 H can be also in separate line?

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: G43.4, G43

Legend
Legend

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. 

Glenn Balon
Production: NX 12.0.2 MP2 Primarily CAM

Re: G43.4, G43

Gears Phenom Gears Phenom
Gears Phenom

@TechniCsNC, @Dstryr, thank you for your answers

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: G43.4, G43

Phenom
Phenom
A few months ago I worked on a current Mazatrol. Here are some unorganized observations: I will say that each comp behaves a little different. The parameters can be set to configure the control to use offset tables, tool data, or a combination of both. There is G43, G43.1 and G43.4 for mill and G43 P1 for lathe type mazatrol tools. I started by making sure (flipping parameters) that none of them would cause a move when activating/deactivating. With the G43 ones - it still seemed to move unless at home position. G43.1 and G43.4 didn't move. I tried to make sure that G43.4 moves would be in "posture controlled" mode. I was never convinced it was. I ended up making a macro to activate each (by doing what was necessary.) Each worked like on a Fanuc once activated. My struggle was activating them wherever and whenever needed without motion. I set up the post to use lathe (G43 P1) for any lathe work with any head angle, (G43 G68) for mill prismatic, (G43.4) for mill 5 axis and allow (G43.1) prismatic unrotated to be used as well. Also - skip moves could not be made in any but G43 mode. A lot of my work was probing - I ended up using no comp to touch (had to turn off and make incremental move) so this meant I needed to turn off and on wherever. Also - G53 could not be issued in G43.1 mode. There were a lot of strange rules.
NX12.02
Windows 10 Pro

Re: G43.4, G43

Gears Phenom Gears Phenom
Gears Phenom

@Study@TechniCsNC@Dstryr

 

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
N37 G80
N38 G0 Z10.
N39 G69
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
N46 G49

or

G43.4 H1

C300

 

I want move only C on that line with tracking tool tip.

 

Thanks in advance

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: G43.4, G43

Phenom
Phenom
I would cancel G43 (maybe that is the G69 - should be G49?) then G43.4 on a line by itself (hoping not to move anything - just update the display) then move C. The value of F85.2 will decide if a C rotation will try to track XYZ to keep the tooltip in the same place (I think.) I set this to 0 I think - my goal is to program with coordinates locked to the table (mom_mcs_goto's.) Any axis position should try to stay at the displayed position if not specified on the block (which would cause linears to move when the rotary moves.) F85.3 has some significance as well. I just looked at the manual but the description didn't help me remember.
NX12.02
Windows 10 Pro

Re: G43.4, G43

Legend
Legend
I believe both should give you the result you want. Best to test though.

Keep in mind, line N45 the tip will also track the A axis.

Not confuse the issue, If you want the C only to rotate while doing linear cuts, try using axis locking on the X or Y axis. If you are just positioning in rapid only then you should be fine as is.

==============================
Best way I can describe is below.

Note: G43.4 and G68 codes are separate and cannot be used together.

G43.4 will keep the tooltip in the same position (relative to work offset) as the part rotates and tracks the part. Used for multiaxis toolpaths cutting in full 5 axis simultaneously.


G68.2 will update the coordinate system as you rotate, but works with the normal G43. The offset will be tracked as you rotate, but the tip will not remain stationary to work offset while rotating.
Glenn Balon
Production: NX 12.0.2 MP2 Primarily CAM

Re: G43.4, G43

Gears Phenom Gears Phenom
Gears Phenom

yes I want to track ofcourse line N45.

=======

I agree.

 

Thank you

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Learn online





Solution Information