Cancel
Showing results for 
Search instead for 
Did you mean: 

Mazak Variaxis 5axis - G43 Question

Gears Phenom Gears Phenom
Gears Phenom

Hello,

I would like to ask if you use in nc code G43 H.. or only G43 , or even none.

And what about turning mode ?

 

example:

One customer use G43 only and for turning - none.

Other customer use G43 H..

 

Is there some rules? Or how does it work?

I just want to make it clear.

 

Thank you for answers Smiley Happy

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #
7 REPLIES 7

Re: Mazak Variaxis - G43 Question

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Is this a 5 axis mill?

What are you talking about when you say "turning" - is this their orbit-turn module?

 

We use "G43 H".  If we have the 5 axis option, "G43.4 H" for variable axis paths (only).

 

It may depend on 

- options / setup of machine

- what kind of tool data you use (EIA or Mazatrol)

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: Mazak Variaxis - G43 Question

Gears Phenom Gears Phenom
Gears Phenom

Yes 5axis.

By turning I meant lathe mode, nothing special

In example from manual there is no G43 or H:

aa.JPG

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

Re: Mazak Variaxis - G43 Question

Experimenter
Experimenter

Hi,

 

I have just checked the post processor manual for a variaxis and the recomendation is to use G43 with a H command.

We use this and we do not have any issues moving from a matrix II to a Smooth control.

 

Regards

Re: Mazak Variaxis - G43 Question

Valued Contributor
Valued Contributor


Hello Juraj.
On the Mazak, you can also use variable #3020 (tool in the spindle).

Mazak Turn
-----------------
G54.1 P1
G0 G90
G0 G43 P1 X28. Y0.0 Z4. H#3020
G97 S50 M204
X24.27 Z0.0


Mazak Mill
-----------------
G54.1 P1
C0.0
G68 X0 Y0 Z0 I0 J1 K0 R45.
G43 X6.1179 Y0.0 Z10.0179 H#3020
Z10.0179


Kal.

 

NX 9.0.3.4 MP12 | PB 9.0.3.2 | NX11.0.2.7 MP13 | PB 11.0.2 | VERICUT 7.3.4

Re: Mazak Variaxis - G43 Question

Legend
Legend

We ran our Variaxis without G43 or H

 

We do set the parameters to use the Mazatrol tool data. So we could use tools in G-code and Mazatrol seemlessly.

 

In this mode. If you do use them in your code it does not make a difference.

 

If you want have a tool go to a Z position in MDI You will need to call G43 when you move to the Z position.

{Paul Schneider}, {CNC Programmer}, {DRT-Rochester}


Production: {NX11.0.2,MP5, NX12.0.2, MP4}

Re: Mazak Variaxis - G43 Question

Phenom
Phenom
A smooth I worked with had some options. There is a tool system where tools have dimensions in the tool data. There is also an offset table - this machine has 999 offsets. You can configure the machine to use either of these by themselves or both (added together.) H relates to the offset table as I recall. For lathe tools - you need to configure to use the tool system to get head comp for current B angles. This happens by G43 P1 - the current B angle is used to throw the tool offset. The effect is similar to G43.1 (non-dynamic.) G43.1 and G43.4 are available (as options I think) for mill tools.
NX12.02
Windows 10 Pro

Re: Mazak Variaxis 5axis - G43 Question

Gears Phenom Gears Phenom
Gears Phenom

Thank you all for reactions

I will keep in mind all your tips

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

Learn online





Solution Information