VARIAXIS i600 G54.4

[Leon82]

Yea, you need to cancel it just like the twp

[Jcncprogrammer]

Thanks! It seems to be working now.

[jlw™]

I think that is actually a result of using the G68.2 and the G54.4 together.  G68.2 TWP will account for CoR deviation, why are you using both at the same time?

[Jcncprogrammer]

Can i just erase the g68.2 until i can get the post changed??

[crazy^millman]

9 minutes ago, Jcncprogrammer said:

Can i just erase the g68.2 until i can get the post changed??

Nope they serve 2 different things.

G68.2 is related to the direct output of the code from the CAM System and allows the machine to take what is posted and move it based of the adjustment on the machine from the workoffsets. G54.4 allow the machine to take what is posted and move it based of the adjustments on the machine in the workoffset only.

Removing G68.2 from posted code what was changed for that output is a disaster in the making. They serve 2 different purposes and you need to learn the difference in them both.

G68.2 is normally used for Canned cycles and other things to map the coordinate system to allow them to be used like in a Normal X,Y,Z plane where A0,B0,C0 are in place, but in all reality it might be X20,Y20,Z20 and A10,B20,C30 on the machine. G68.2 tell the machine to ignore that and understand it as everything is normal so run the code like a 3 Axis machine.

G54.4 allows you to take and use offsets on the machine to make up for any difference from where you expected the part to be and where it really is, but it cannot take code and map it to a 3 Axis direction from a 5 Axis direction that the G68.2 can.

[Jcncprogrammer]

My post kicks out the G68.2 on every tool?? Is there a box i can check to turn it off??

[Leon82]

Is the part entirely 3+2?

If you have the  twp in the post already you should be able to probe and go.

I was under the assumption that it had neither twp or tcp and you added the 54.4 option

[Leon82]

So if you have the 68.2 option you would use that on 3 plus 2 work and then you have to use the 54.4 for multi-axis work.

 

Is that what you're attempting to do?

[jlw™]

^^^ that's it right there.  There are a few parameters you have to change in the machine to get G68.2 to work correctly.  I haven't had to change it in several years, have you called Mazak?

[jlw™]

That is how all of my 5ax posts output.  If you want to send a simple part I'll program it and send you the code.  I can show you code/video of it running if you'd like.

[crazy^millman]

1 hour ago, Jcncprogrammer said:

My post kicks out the G68.2 on every tool?? Is there a box i can check to turn it off??

A box no, but their might be a switch in your post to turn it off. Depends on who you got your post from as to what you can and cannot turn on/off for output.

[crazy^millman]

34 minutes ago, jlw™ said:

^^^ that's it right there.  There are a few parameters you have to change in the machine to get G68.2 to work correctly.  I haven't had to change it in several years, have you called Mazak?

Not just Mazak many others if the parameters are not correct will give you a fit as well.

[Jcncprogrammer]

Im not finding much info for how to use g68.2..my post always kicks out g68.2 but it always has zeros for x and y..how do i get it to compensate for COR...

[Leon82]

I can't remember but I think they are always zero and the angles are in ijk.

But I can assure you when working properly it works.

Since you had previously centered the parts and this first one is not tracking the work offset properly you may need to double check the parameters as suggested. It can be as simple as 1 or 2 bits that needs to be toggled

[jlw™]

1 hour ago, Jcncprogrammer said:

Im not finding much info for how to use g68.2..my post always kicks out g68.2 but it always has zeros for x and y..how do i get it to compensate for COR...

If you are not using it to shift then XYZ will be ZERO and IJK will have your rotary angles in Euler format.  Send me a part, I'll put a few paths on it with working G68.2 post so you can see it.

[MIL-TFP-41]

Pretty sure you want/need G68.2 on every orientation change

Example

G49 G53 Z0.0
G69 (Cancel 68.2)
G54.4P0 (Cancel G54.4)
M132(unclamp both rotaries)
G00 G90 G54 A-60.0 C0.0
G54.4P1
G68.2 X0.0 Y0.0 Z0.0 I-0.0 J-60.0 K0.0
G53.1
X1.0248 Y-6.2961 A-60.0 C0.0 (The A-60. and C0 are redundant & not totally necessary)
M131 (Clamp rotaries)
G43Z4.5H#518

 

 

[Leon82]

42 minutes ago, MIL-TFP-41 said:

Pretty sure you want/need G68.2 on every orientation change

Example

G49 G53 Z0.0
G69 (Cancel 68.2)
G54.4P0 (Cancel G54.4)
M132(unclamp both rotaries)
G00 G90 G54 A-60.0 C0.0
G54.4P1
G68.2 X0.0 Y0.0 Z0.0 I-0.0 J-60.0 K0.0
G53.1
X1.0248 Y-6.2961 A-60.0 C0.0 (The A-60. and C0 are redundant & not totally necessary)
M131 (Clamp rotaries)
G43Z4.5H#518

 

 

Looks like our matsuura code 

[MIL-TFP-41]

Just now, Leon82 said:

Looks like our matsuura code 

Its not a coincidence....

We have 2 MX 330's and 2 MAM72-63V's running that same code.....and three 5 axis robodrills running very similar code (difference being those are B/C machines)

 

[navsENG]

On 1/24/2018 at 5:32 AM, jlw™ said:

It is an e1600.

Very good. The updated 1550... They fixed all the stuff that's wrong with ours LOL.

[jlw™]

18 minutes ago, navsENG said:

Very good. The updated 1550... They fixed all the stuff that's wrong with ours LOL.

LMAO, they broke everything else then!

[navsENG]

1 hour ago, jlw™ said:

LMAO, they broke everything else then!

Is G68 and G68.2 one in the same? My machine just uses G68 for coordinate rotation... We use this whenever we rotate the B axis. 

We mainly do 3+2, Ive never done any full 5 work on this machine. Is that where you would use G54.4? That's something I would like to get figured out.... 

[crazy^millman]

2 hours ago, navsENG said:

Is G68 and G68.2 one in the same? My machine just uses G68 for coordinate rotation... We use this whenever we rotate the B axis. 

We mainly do 3+2, Ive never done any full 5 work on this machine. Is that where you would use G54.4? That's something I would like to get figured out.... 

Older Mazaks it was just G68. It might have changed and G68 is for 4 Axis and G68.2 is for full 5 Axis. Really comes down to the control and builder.

[Jcncprogrammer]

I have some code that i would like you guys to look at.. here im probing X and Y on an existing part that i have to put a few holes in 
on center in x. but the holes are .007 off..whats going on??

G0 G17 G40 G80 G90 G20 
G28 G91 Z0
G28 G91 X0 Y0 C0 A0
T01 T24 M06
G00 G90 G55 X0 Y0 A0 C0
G43 G90 H1 Z3.

G65 P9810 Z2.5
G01 X-.5 F25.
G65 P9812 Y15.6 Z-1.75 S2 (Y YEB)
#5812 = #141 (write G54.4 Y error)
X0 Y0
G65 P9812 X1.75 Z-1.1 S2 (X WEB)
#5811= #140 (write G54.4 X error)
G05 P0
G64
G20

G05 P0
G64
G54.4 P0
G20

 

then later i do this drill cycle and its way off .007 off center off the part?? Im not liking this at all..probe is calibrated, part is indicated....never have this problem with the haas...

N4 (OPERATION  4)
G0 G17 G40 G80 G90 G94 G98
(P STANDARD DRILL - 0.322)
T37 T33 M6
G55
G54.4 P1
G0 A0. C0.
G68.2 P1 X0. Y0. Z0. I0. J0. K0.
G53.1 P2
G0 X0. Y4.8014
S1500 M03
G43 H37 Z3.
M08
Z.05
G83 G98 Z-.6 R.05 Q.05 F15.
Y6.3014
G80
G0 Z.05
G94
Z3.
M09
M05
G69
G54.4 P0
G49
G0 G28 G91 Z0.
G90
G90
M01

Any Ideas???

 

[Jcncprogrammer]

Sorry OMIT the S2 in the probe cycle...i forgot to edit them out on my post

[crazy^millman]

I am confused you are adjusting the G55 or P1? I see the S@ on your probing to adjust the G55, but I don't see the logic to update the P1. What are you doing to make the adjustment? Are you adjusting the workoffset or are you adjusting the compensation for error offset? To me you are not going about the process correctly.