New Mazak i700 Variaxis

[DC Gorn]

I have a new i700 and a new inhouse post. I am trying to do basic 5 axis positioning. In my DMU's I could just have a single G54 and I could machine from any direction the machine knows where they coordinate system move to so I could position anywhere with a single coordinate system. On the Mazak using G54 it seems to keep the coordinate fixed so the 5 axis position is way off once you start rotating. Do I really need a new coordinate system for every 5 axis position? I notice in the book they talk about dynamic shifts with G54.2 and G54.4 does that have something to do with it? Any clues how I setup the planes in Mastercam to get this to work?

 

[Joe788]

If you want to just do it quick and dirty, you need to put your Mastercam/WCS origin at the the machine's A and C axis center of rotation.  Then you can use one offset for all of your different orientations, and won't need G54.4 or G54.2.

 

If you want to do it right (which you should), you're going to need a little training in how to use G54.4. The post should support it.

 

Call this guy and have him come out for a day: http://www.dbssolutionsllc.com/services

[DC Gorn]

With what I paid for a fully supported post I am going to have a tuff time getting approve to fly someone out to show me how to use it. I have a application engineer from Mazak in house today. He can explain how they work but not how to set it up in Mastercam.

[Joe788]

With what I paid for a fully supported post I am going to have a tuff time getting approve to fly someone out to show me how to use it. I have a application engineer from Mazak in house today. He can explain how they work but not how to set it up in Mastercam.

 

I haven't seen the post, so I'm not sure how it works - but I'm assuming there's a Misc Integer that you'll turn on to activate G54.4, G54.2, G43.4, etc.  

 

If you're just doing 3+2 work, focus on getting G54.4 working for you. Don't worry about G43.4 unless you're doing rotary work, and G54.2 is just previous generation (less capable) G54.4, so don't worry about it either.

[DC Gorn]

I have the Inhouse post. I just talked to my reseller. He had me turn on "datum tracking" in the post I noticed it still calls G54 and G54.2 P1.  I was told the G54.2 P1 page should reflect the distance from the trunion point to the coordinate.

 

P1 is (I think) :

X 1.05

Y 2.26

Z- 3.512

 

Any idea what I would put in G54? The distance from machine home to the Trunion point? Or the distance from machine home to the WPC system?

 

Sample program:

 

(T3     - 1/4 FLAT ENDMILL     - H3     - D3     - DIA .25")
(G10 G90 L21 P1 X0. Y0. Z0. A0. C0.) *** New With post edit***
G00 G90 G17 G20 G40 G80
G91 G28 Z0.
G28 X0. Y0.
N1
(T3     - 1/4 FLAT ENDMILL     - H3     - D3     - DIA .25")
T3 M06
G00 G90 G54
S2139 M03
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
A-45. C90.
G54.2 P1 ***New with post edit***
A-45. C90.
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
X-4.21 Y1.6147
G43 H3 Z2.6688
Z.8688
G94 G01 Z.5981 F6.42
X-3.96
X0.
X.25
Z.7981
G00 Z2.6688
X.23 Y-1.268
Z.8688
G01 Z-2.2889
G41 D3 X-.02
X-3.98
G40 X-4.23
Z-2.0889
G00 Z2.6688
G49
M05
G54.2 P0 ***New with post edit***
G91 G28 Z0.
G28 X0. Y0.
M46 M43 (A-AXIS UNLOCK, C-AXIS UNLOCK)
G28 A0. C0.
M47 M44 (A-AXIS LOCK, C-AXIS LOCK)
M30
%

 

What I changed in the inhouse post (I changed both these to 1):

 

wt_dtrack         : 1     #Setting for the datum tracking function for 3+2, and either datum tracking
                           #with length compensation or TCP for simultaneous 4/5-Axis
swt_dtrack_vec     : 1     #0 = Do not output datum track vector (user must set on controller),

 

Thanks for your help so far Joe788 I can look at upgrading to G54.4 after I get the post working as intended.

[Joe788]

Basically on the "dynamic offset" page, the G54.2P1 values need to represent the incremental distance from the A/C center of rotation, to your actual part origin.  The Mazak applications guy should be able to help explain this to you. If he can't, ask him to put you in touch with one of the others who can.

 

We do it like this:

 

Set G54 to the machine's center of rotation.

Set G54.1P1 to your part's origin.

 

Add this macro call at the top of your program:

 

G10 L21 P1 X#70001-#5221 Y#70002-#5222 Z#70003-#5223

 

This will automatically fill in your G54.2P1 register with the difference between center of rotation and your part origin.

 

The code in your post should work fine after that. Although I'd recommend removing the A and C clamp/unclamp calls everywhere. The machine knows to clamp and unclamp on its own. You only need to command it to unclamp if you're going to be doing a rotary cut.