Sign in to follow this  
Followers 0
Brewster

G54.4 WSEC on Mazak VCU 400 5X

12 posts in this topic

We just got a new machine with the Matrix 2 controller. it has the G54.4 WSEC option. i am not familiar with this. we have a Variaxis 730 5x and use G54.2 on it. I was wondering how to set the data for G54.4 at the control and in a program. Do you set it similar to G54.2? does the center of rotation coordiniates need to be in G54? any information would be appreciated. thanks

Share this post


Link to post
Share on other sites

Jeremy,

Any insight you can give would be greatly appreciated. We have the Matrix 2 controller, and it is the first machine we have that has the G54.4 option. we have used G54.2 on our 730 variaxis. The G54.4 seems to be a little different as far as setting it up.

Share this post


Link to post
Share on other sites

G54.4 is slightly different than G54.2. Think of it as dynamic comp on steroids. It functions much like G54.2, however now you can use all of your go-fast options (G05P2, G61.1, etc..). The way I typically use it is to define your primary work offset as the center of rotation for rotary axes. Pivot point can be found by looking at the value of S5 (for x and y) and S12 (for z) in the machine parameters. Throw those numbers in G54. Next you need to find your part origin...doesn't matter how you do it but find the machine coordinate for the origin point in XYZ. Calculate the difference between this point and the pivot point (G54) and input this value into one of the G54.4 offsets. G54.4 is the deviation FROM the primary work offset so the sign of the values are critical.

 

That's it in a nutshell. I could go on to explain about correcting for A and C axis error by rotating axes but typically you will not need to do this. Very few people use G54.4 with values in any of the Theta fields. See programming example below:

 

O0001 ( PROGRAM - TEST )

( DATE - 10-08-13 TIME - 17:22 )

G20

G0 G17 G40 G80 G90 G94 G98

G91 G28 Z0.

G30 X0. Y0.

G28 A0.

( 1/4 DATAFLUTE SS W/ WIPER TOOL - 19 DIA. OFF. - 0 LEN. - 0 DIA. - .25 )

 

 

(FINISH TAB CONTOUR)

T19 M6 T3

G0 G54 G90 C0. A-90. S1400 M3

G54.4P1

X7.40058 Y1.16381

M8

G61.1 ,K0

G43 H#3020 C0. A-90. Z1.5375

G05 P2

Z.6375

G1 Z.12 F100.

G41 X7.53049 Y1.08881 F6.

G3 X7.5338 Y1.1013 I-.0217 J.0125

G2 X7.6114 Y1.2643 I.179 J.0148

G1 X7.88205 Y1.44684

X7.92381 Y1.46579

...

.....

 

Also notice that I am only moving A and C on the G54 line. After activating G54.4 move your X and Y to position.

 

Hope this helps,

 

 

 

p.s.- The EIA programming book gives a very good and elaborate description of the option.

1 person likes this

Share this post


Link to post
Share on other sites

G54.4 is slightly different than G54.2. Think of it as dynamic comp on steroids. It functions much like G54.2, however now you can use all of your go-fast options (G05P2, G61.1, etc..). The way I typically use it is to define your primary work offset as the center of rotation for rotary axes. Pivot point can be found by looking at the value of S5 (for x and y) and S12 (for z) in the machine parameters. Throw those numbers in G54. Next you need to find your part origin...doesn't matter how you do it but find the machine coordinate for the origin point in XYZ. Calculate the difference between this point and the pivot point (G54) and input this value into one of the G54.4 offsets. G54.4 is the deviation FROM the primary work offset so the sign of the values are critical.

 

That's it in a nutshell. I could go on to explain about correcting for A and C axis error by rotating axes but typically you will not need to do this. Very few people use G54.4 with values in any of the Theta fields. See programming example below:

 

O0001 ( PROGRAM - TEST )

( DATE - 10-08-13 TIME - 17:22 )

G20

G0 G17 G40 G80 G90 G94 G98

G91 G28 Z0.

G30 X0. Y0.

G28 A0.

( 1/4 DATAFLUTE SS W/ WIPER TOOL - 19 DIA. OFF. - 0 LEN. - 0 DIA. - .25 )

 

 

(FINISH TAB CONTOUR)

T19 M6 T3

G0 G54 G90 C0. A-90. S1400 M3

G54.4P1

X7.40058 Y1.16381

M8

G61.1 ,K0

G43 H#3020 C0. A-90. Z1.5375

G05 P2

Z.6375

G1 Z.12 F100.

G41 X7.53049 Y1.08881 F6.

G3 X7.5338 Y1.1013 I-.0217 J.0125

G2 X7.6114 Y1.2643 I.179 J.0148

G1 X7.88205 Y1.44684

X7.92381 Y1.46579

...

.....

 

Also notice that I am only moving A and C on the G54 line. After activating G54.4 move your X and Y to position.

 

Hope this helps,

 

 

 

p.s.- The EIA programming book gives a very good and elaborate description of the option.

 

 

Thanks for the run down! I did notice you didn't move A and C. I was under the impression that G54.4 could be used for simultaneous 5 axis. Is this correct?

Share this post


Link to post
Share on other sites

Yes. Full 5. G43.4 is also legal and you can use ipm instead of inverse time. :oldforumcheers:;

 

Great! thanks for the help. Setting it up in the control is the next challenge. It seems to be similar to the G54.2 as far as XYZ, but B and C seem different. I'm not sure what the "Common" data is for either.

Share this post


Link to post
Share on other sites

I don't us the common data. I set g54 where I want it and use it for top work, G54.1 p300 to C.O.R, and the difference goes into G54.4 p1. Do you use A and or C offsets?

Share this post


Link to post
Share on other sites

B and C as opposed to b and c are the angles at which the error is calculated from so say your error was calculated at B-90.0 and C270.0 those are the values which would go in B and C respectively.

Share this post


Link to post
Share on other sites

I don't us the common data. I set g54 where I want it and use it for top work, G54.1 p300 to C.O.R, and the difference goes into G54.4 p1. Do you use A and or C offsets?

 

I use C offsets on the 730 variaxis but not A because Im limited to only using G54.2 on it. The VCU has only been on the shop floor about 4 days, so I haven't had a chance to do a lot with it yet.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now
Sign in to follow this  
Followers 0

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us