VARIAXIS i600 G54.4

[Jcncprogrammer]

Hello all, I am new to 5 axis machining, and the company i am working for just bought a new variaxis i600 and got it up and going a few months back.  while i have had a few successful parts programmed on this machine. This one i can not figure out. We are having to machine on an extrusion that has most of the OD surfaces finished, and we have to machine pockets into the sides and various features on every side. 

We are holding the part in a 5th axis vise, on the center of the table.and probing x0y0 at the center of every part.

I am sure my part is on center in master cam 2017 and everything looks good as far as geometry and numbers go, but when i run the program everything is .01-.02" off center??

and inconsistent from part to part... We checked our setup, and the probe. my last conclusion was that it had to have something to do with the changing position relative to center of rotation?? Because Y and X are changing several thou when i look at the work offset page. Does this sound like something G54.4 would help resolve? As ive never had much issue with parts machined from a solid billet, its just when having to be on center of an existing part with finished surfaces. Does anyone knows anything that would shed some light on this??? It seems even Mazak and Mastercam are not able to help much with this issue...

Thanks

[Leon82]

it should

I use it along with the g68.2 twp on 1 part with a 20micron true position.  the datums are vary as the machine warms up so I have an moo to indicate them and put the off values in g54.4.

are you using the tilting work plane?

[jlw™]

You should not be probing these parts for G54.  You can probe them for G54.4 deviation from CoR, Mazak has a lovely little macro for the asking.  The G54 (or whatever) offset should be center of rotation for XY and Z.  If you do not know these numbers you can find them in the Machine Parameters page, Another (S Parameters) in #5 for each axis.

If you are probing a round feature it needs to be indicated to CoR on the table.  You are seeing a very small(ish) error and I bet a dollar it's coming from probing the parts and them not being perfectly on center.  Let's say you're off center .005 at A90.C90., roll that to A-90.C90. and it becomes .010 off across the part.  This is where G54.4 comes in, you "main" offset is G54 with CoR values, then the deviation from CoR goes in G54.4 and the machine will magically "track" the part with it's deviation.  There are two primary concerns here, 1. the farther you are from CoR the more the machine has to compensate and 2. watch out for odd rotary behavior.  In a trunnion machine that is minimal imo but in a head/table or head/head it can buck you in the futt in a hurry.  Do not ask how I know that.

[Jcncprogrammer]

This is great info,  I am using these lines to pickup the part, S1 would be the code to probe set G54, would i do S101 to set the part at G54.4 P1??

G65 P9812 Y15.6 Z-1.75 S1 (X YEB)
G65 P9812 X1.75 Z-1.1 S1 (Y WEB)

Also another question was on the Z for center of rotation you put in -42.889, but the parameter says 0, where did that number come from??

Thank you so much, excited to get back to the shop and try this out, will let you all know if it is magic!!

[Leon82]

If I remember correctly g10 L23 p1 will write to the g54.4 p1 offset. So you can incorporate that into a macro or enter it manually

 

S101 is usually g54.1 p1

 

[jlw™]

4 hours ago, Jcncprogrammer said:

This is great info,  I am using these lines to pickup the part, S1 would be the code to probe set G54, would i do S101 to set the part at G54.4 P1??

G65 P9812 Y15.6 Z-1.75 S1 (X YEB)
G65 P9812 X1.75 Z-1.1 S1 (Y WEB)

Also another question was on the Z for center of rotation you put in -42.889, but the parameter says 0, where did that number come from??

Thank you so much, excited to get back to the shop and try this out, will let you all know if it is magic!!

My machine is a table/head, my Z is the actual probed value of the part.  I do not have access to a Variaxis at the moment.  There is no Z offset in a table/head for CoR.  You will need to put your S5 parameter in your offset whether you use anything from G54 to G54.1P99.  You can just use the Renishaw 123 easy set to get the probed feature and then use a macro to take those variables to find the deviation from CoR and then those numbers go in G54.4 XYZAC.  If you do not have the probing macros for setting G54.4 you can call Mazak but I would suggest calling Renishaw.  They will be more helpful with the probing any way.  I would send you mine but all of my machines are table/head or head/head and they have minor difference in the probe routines.  I usually don't mess with any G10 lines, I always use the system variables to read and write the values I want.

You can read your S5 parameters from here:

and if you want to probe in a Mazatrol program you can read Mazatrol WPC values here:

You can read/write G54, G55, etc here:

Extended offsets are here:

The values for "Dynamic Offsets" aka G54.2 are here:

and G54.4 WSEC are here:

[jlw™]

One little tidbit, I read the S5 parameters and write G54 every time... let's say my machines get "worked on" more than the manufacturer suggests so I don't trust G54 to just match the S5 values.  If you read it and write it into G54 every time you will eliminate any chance for human error.  Chalk that one up to experience.

[Zoffen]

^^^^^^^Great idea JLW!!!!

For the I-700 i programmed to match ops with 3+2 and full five i would program the part with it in the perfect center position in mastercam.  Then at the machine i would probe a feature that is "known" is mastercam and set an offsets i was not using and then calculate the difference from where the part was in mastercam to where the part sits in the machine. These are the values you should use in your g54.4 registers with your G54 still being the COR coordinates.

This would allow me very easily to probe an existing part and be able to track the existing datum around the rotaries with no problem.

[Jcncprogrammer]

If im understanding correctly Im going to set G54 to COS. and use my probe to set G54.4 P1, i could store it in say G55 (S2) and use macros to get it into G54.4 P1??

Here is the code i came up with to get the deviation put into G54.4 P1., Im using #100 as a place to store the values,

G65 P9812 Y15.6 Z-1.75 (?? set G54.4 P1) (X YEB)
G65 P9812 X1.75 Z-1.1 (?? Set g54.4 p1) (Y WEB)

#100 = [#5811-#5221] (SUBTRACTING THE PROBE READING FOR X FROM COS)
#101 = [#5812-#5222] (SUBTRACTING THE PROBE READING FOR Y FROM COS)
#5811 = [#100]    (sets the deviation in G54.4 P1 FOR X?)
#5812 = [#101]    (sets the deviation in G54.4 P1 FOR Y?)

Does this look reasonable??

[jlw™]

You are exactly correct Jcnc.  However, you must either do a little fancy Absolute Value work or you will subtract a negative from a negative but yes that is exactly what you do.  Remember, you're only looking for the total deviation and the direction.

You can see from this fabulous G54.2 illustration in the Mazak Manual:

All of that should be in your manual too.  If you don't have it or can't find it let me know.  I still have several Variaxis pdfs floating around some hard drives and thumb drives.

[MIL-TFP-41]

17 hours ago, Jcncprogrammer said:

If im understanding correctly Im going to set G54 to COS. and use my probe to set G54.4 P1, i could store it in say G55 (S2) and use macros to get it into G54.4 P1??

Here is the code i came up with to get the deviation put into G54.4 P1., Im using #100 as a place to store the values,

G65 P9812 Y15.6 Z-1.75 (?? set G54.4 P1) (X YEB)
G65 P9812 X1.75 Z-1.1 (?? Set g54.4 p1) (Y WEB)

#100 = [#5811-#5221] (SUBTRACTING THE PROBE READING FOR X FROM COS)
#101 = [#5812-#5222] (SUBTRACTING THE PROBE READING FOR Y FROM COS)
#5811 = [#100]    (sets the deviation in G54.4 P1 FOR X?)
#5812 = [#101]    (sets the deviation in G54.4 P1 FOR Y?)

Does this look reasonable??

 

I do something similar on Fanuc controllers, except you don't have to do the fancy math.

G65 P9812 Y15.6 Z-1.75  (X YEB)
#5811= #140 (write G54.4 X error)
G65 P9812 X1.75 Z-1.1 (?? Set g54.4 p1) (Y WEB)
#5812 = #141 (write G54.4 Y error)
	

variable outputs.pdf

[jlw™]

35 minutes ago, MIL-TFP-41 said:

 

I do something similar on Fanuc controllers, except you don't have to do the fancy math.

 

Dangit, that pisses me off that I forgot about the error output in the probing cycles.  Doh!

Thanks for the reminder!

[Jcncprogrammer]

49 minutes ago, MIL-TFP-41 said:

 

I do something similar on Fanuc controllers, except you don't have to do the fancy math.

G65 P9812 Y15.6 Z-1.75  (X YEB)
#5811= #140 (write G54.4 X error)
G65 P9812 X1.75 Z-1.1 (?? Set g54.4 p1) (Y WEB)
#5812 = #141 (write G54.4 Y error)
	

variable outputs.pdf

So after each probe cycle this will automatically load the correct deviation from COR into G54.4?  Do i still need the actual S value for G54.4 on the G65 line?  or will the following macro code do the work?

[Leon82]

I think you will have to omit the s because you don't want to write the wcoff.

Just the error to 54.4

[MIL-TFP-41]

1 hour ago, Jcncprogrammer said:

So after each probe cycle this will automatically load the correct deviation from COR into G54.4?  Do i still need the actual S value for G54.4 on the G65 line?  or will the following macro code do the work?

The only thing I would verify would be if the Renishaw variable outputs are the same for Mazak as they are for Fanuc. They *should* be.

[Jcncprogrammer]

Just checked the Mazak probe documentation and #140 and #141 are error for x and y! Thanks for all the help! It is greatly appreciated!  I will be able to verify it at the machine on Wednesday. Hopefully this thread has made a resource for others to help understand it as well. Or it may just be that I am the only g54.4 dummy...:)

[jlw™]

11 minutes ago, Jcncprogrammer said:

Or it may just be that I am the only g54.4 dummy...:)

Nope, we all had to learn it some how.

[Jcncprogrammer]

When i select the g54.4 on the misc value page and post my code it does not post a G54.4 P1. Can I simply go through and find and replace G54 with G54.4 P1?? Or is there more to it than just replacing G54 in the code??

[MIL-TFP-41]

10 hours ago, Jcncprogrammer said:

When i select the g54.4 on the misc value page and post my code it does not post a G54.4 P1. Can I simply go through and find and replace G54 with G54.4 P1?? Or is there more to it than just replacing G54 in the code??

There is alot more to it than that. G54.4 does not replace your regular work offsets, it corrects the part deviation.

Your code would look something like this: (table/table machine)

>
	M132
G00 G90 G54 A-46.5 C-180.0
G54.4 P1
G68.2 X0.0 Y0.0 Z0.0 I-180.0 J-46.5 K0.0
G53.1
X1.9505 Y-6.0538 A-46.5 C-180.0
G43 Z6.0 H1
	

[Leon82]

On the fanuc if the 54.4 value are all set at zero it doesn't activate .

 

If your control is the same you can have it post out all the time and when you do need to use it you just have to put your error in the 54.4 p1 offset.

Then you won't have to manually add it each program

[navsENG]

On 1/21/2018 at 5:41 AM, jlw™ said:

You should not be probing these parts for G54.  You can probe them for G54.4 deviation from CoR, Mazak has a lovely little macro for the asking.  The G54 (or whatever) offset should be center of rotation for XY and Z.  If you do not know these numbers you can find them in the Machine Parameters page, Another (S Parameters) in #5 for each axis.

If you are probing a round feature it needs to be indicated to CoR on the table.  You are seeing a very small(ish) error and I bet a dollar it's coming from probing the parts and them not being perfectly on center.  Let's say you're off center .005 at A90.C90., roll that to A-90.C90. and it becomes .010 off across the part.  This is where G54.4 comes in, you "main" offset is G54 with CoR values, then the deviation from CoR goes in G54.4 and the machine will magically "track" the part with it's deviation.  There are two primary concerns here, 1. the farther you are from CoR the more the machine has to compensate and 2. watch out for odd rotary behavior.  In a trunnion machine that is minimal imo but in a head/table or head/head it can buck you in the futt in a hurry.  Do not ask how I know that.

IS that an e-1550? I recognize those COR numbers..... Y is a little off from mine but X is within a thou or two ..

[jlw™]

8 hours ago, navsENG said:

IS that an e-1550? I recognize those COR numbers..... Y is a little off from mine but X is within a thou or two ..

It is an e1600.

[Jcncprogrammer]

The program ran for a while and then this happen? Illegal Command in G54.Is this something to do with the C180?

[Jcncprogrammer]

I went in and modified the code by hand and put in G54.4 P0 before the rotary move and then G54.4 P1 after it and it didnt alarm

out, only unit it reached another rotary move where A was at -90?? Do i need to cancel the code before any rotary movements?

[crazy^millman]

Just now, Jcncprogrammer said:

I went in and modified the code by hand and put in G54.4 P0 before the rotary move and then G54.4 P1 after it and it didnt alarm

out, only unit it reached another rotary move where A was at -90?? Do i need to cancel the code before any rotary movements?

Yes that information and process needs to be sent back to your post builder. Most post builders already do this so odd yours is not doing it.