VARIAXIS i600 G54.4

[navsENG]

Looks like he is trying to write the error to a shift.... Could it possibly be a sign value issue? (you could be probing .003" off, but it really needs to move -.003").

 

I'd double check that, tho really I dont see why you dont just write the actual coordinates to your P1 offset. 

[Jcncprogrammer]

7 minutes ago, C^Millman said:

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.

 

I have g55 set to COR, and the macro code below is updating the G54.4 P1, omit the S I accidently left it, but it was not in the program on the machine, i removed it at the control. but still off center .007 in x...My work offset error page is updating when i probe the part.

#5812 = #141 (write G54.4 Y error) (this code is updating the G54.4 P1

If im doing something wrong, let me know..

[Leon82]

After you write the shift, run the probe cycles again but don't write anything to see if it is correct

[Jcncprogrammer]

11 minutes ago, Leon82 said:

After you write the shift, run the probe cycles again but don't write anything to see if it is correct

So run it with the macro logic to write G54.4 P1 and then run it again with out the macro logic??? G54.4 p1 wont change unless its updated??

[Leon82]

9 minutes ago, Jcncprogrammer said:

So run it with the macro logic to write G54.4 P1 and then run it again with out the macro logic??? G54.4 p1 wont change unless its updated??

Yes. The second time is to verify it is writing and positioning correct

Check it again after you apply the g54.4 to see if it reads zero.

If the probe won't work with 54.4 active  you may have to use an indicator.

All of our matsuura came with the 54.4 but none of them worked. They would hang up and not alarm out if there was a value in there. Another parameter had to be changed. So you may be writing to it but it may not be applying it 

[crazy^millman]

I would need to see the macro and how you write out your offsets as S1 would update G54 and then S2 would do G55 from the Macros I have seen. Are you sure about the Macro and the process to get the probing to update the correct offsets and place?

[Leon82]

3 minutes ago, C^Millman said:

I would need to see the macro and how you write out your offsets as S1 would update G54 and then S2 would do G55 from the Macros I have seen. Are you sure about the Macro and the process to get the probing to update the correct offsets and place?

I think he said he removed the s2 at the machine

[Jcncprogrammer]

I removed S2 at the machine, and it is changing the G54.4 P1 offset. I switched parts in and out and let it run till it hit a G54.4 P1 and went and looked at the work pos error page. It is changing.

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 (Y YEB)
#5812 = #141 (write G54.4 Y error)
X0 Y0
G65 P9812 X1.75 Z-1.1 (X WEB)
#5811= #140 (write G54.4 X error)
G05 P0
G64
G20

G05 P0
G64
G54.4 P0
G20

[Jcncprogrammer]

Right now to make parts, im just having to go in and modify the X value from X0 to x.007 and its working, just wished i didnt have to do that... somethings got to be a miss right?

[crazy^millman]

19 minutes ago, Jcncprogrammer said:

Right now to make parts, im just having to go in and modify the X value from X0 to x.007 and its working, just wished i didnt have to do that... somethings got to be a miss right?

Yes something is a miss I agree why you need to get Mazak into you place.

[MIL-TFP-41]

Call up the “G0 A0. C0.” command BEFORE your G54.4 command, not after. 

Not sure if that will do the trick or not, but that is the format I use & know works. 

 

Also so add the A0.C0. to the line after your G53.1 call. Come to think of it it is necessary to be there. 

[Jcncprogrammer]

I have to cancel G54.4 before the rotary movement, and start it up right after. The machine gives me an illegal command in g54.4 if g54.4 p1 is activated while doing a rotary movement....

[MIL-TFP-41]

31 minutes ago, Jcncprogrammer said:

I have to cancel G54.4 before the rotary movement, and start it up right after. The machine gives me an illegal command in g54.4 if g54.4 p1 is activated while doing a rotary movement....

Yes, look at the sample I posted.

Cancel G54.4 & G68.2

Position Rotaries

Activate G54.4

Activate G68.2

Activate G53.1

Do your X & Y position move w/ your A & C

 

On second glance, it looks like your code should work. You say your hole is .007 off. Does that reflect the values written in the G54.4 register?

 

[Jcncprogrammer]

Were still having troubles getting things on center,  When G68.2 flips things around and x becomes y, does the machine know how to adjust comp error with g54.4 for updated axis, or does it shift the wrong axis. this is sorta what it looks like is happening??? Some have told me not to use both at same time, and some have said its okay, and some have told me that G68.2 should be all i need?

[crazy^millman]

You need to go through a process of elimination and isolate what the exact problem is. Do certain things to prove out what you need figure our what does what you need and use that. Don't over complicate things if you don't need to. 

[crazy^millman]

Double Post

Edited January 30, 2018 by C^Millman
Double Post no reason to repeat myself.

[Leon82]

68.2 should be all you need for 3 + 2.

It sounds like you need to review the parameters as suggested.

From what I gather from This Thread is 54.4 was added apparently because 68.2 is not working as it should

[Jcncprogrammer]

If i was milling an existing 3" square block with 1/2 holes on each face the 5 axis machine could access, and each of these holes are on center of the block. and the block was clamped .05" off center in y and .1" off center in x on the table. and my mastercam program is all programmed true to the part and x0y0 is center and z0 is top of part. Will G68.2 place all the holes on center of part? Does it compensate automatically when i tilt the part up at A90.? How does it get the data it needs to shift axis to compensate for the part tilting and being off center?

[crazy^millman]

G68.2 will take the offset amount touched off from home on the machine to where you have established Zero on your part and adjust for the work offset amount put in the work Offset. If you are programmed for one things and the machine is not in that position that is the perfect time to use G68.2, but the workoffset must be from the home position and the 19700-19706 parameter must be input correctly ( For Fanuc) and then the machine will do all the work. If the part was 10" off in X and 10" off in Y and 3" higher than expect in Z and the program could run in the limits of the machine then the machine would run it you had programmed Zero at the Center of the part in X and Y and Top of the part. What I have seen people do in error is program the part from the center of rotation and have the part sitting up in space above the center of rotation and that is where they have programmed the Zero in Mastercam. They then go out and use the number from the center of rotation in the work offset and then try to make adjustments and wonder why it get messed up. That is the wrong way to go about it. A programmer need to think of G68.2 programming as no different than 3 Axis programming. You decide where you want you zero to be programmed from on the part. You make that your Zero for programming in Mastercam not caring where the COR is on the machine. You then go pick up your part from Home like you would any 3 Axis machine. Now you run your program and have a nice day. Again don't over think or over complicate the process. It is really as simple as programming a 3 Axis part the difference is instead of using more than one WCS for each face of the part or Index you will use the same WCS for all the operation, but the T-C Planes will now do the work for moving or indexing the part to do all the different faces and you are machining every feature like a 3 Axis machine, but not having to physically move the part the machine is doing all the heavy lifting and work for you.

There are post out there that will take the 1st WCS and use it for all 68.2 work even if the planes are not using the same base position for their values, but if you go from machine to machine where this is not a good way to program parts you get yourself in trouble in my opinion. I go with a known and controlled way of using the same WCS position for all the different Planes(WCS) needed to do the work. I create a point and then I will go pick that point for each new Place(WCS). Yes it is hard trying to explain to someone that even though the planes manager make not a distinction with color or anything that the different planes do different thing except for the Columns that show which one is the active WCS and which ones are the active T-C Planes they are different and do different things. Once you wrap your brain around that process and think like the software works and not what follows the way you think it should work then you will be able to see how it has to work.

Having the name of the WCS and T-C planes shown in the operation manager when dong 5 Axis work is also a good double check to make sure you are doing it correctly.

HTH (Hope that Helps)

[jlw™]

Jcncprogrammer, I use G68.2 on Mazaks daily.  Can you send me a simple part and let me put some paths on it and post you some code?  Seeing proper code may help you out a little.

[jlw™]

Then, if my code will not run in your machine it boils down to parameters as I am running it in 3 different 5ax machines and have tweaked parameters on all.

[Jcncprogrammer]

Cmillman, i am processing your info..lol jlw, let me draw up a simple part on solidworks and i will get it to you. Thanks to both you guys for being patient with me.

[jlw™]

No problem, if you have a file you can share it may help you more to see your part but I can make just a dummy part.  I was thinking if you had a part you are attempting and not having luck let me path it in your setup and send you code.  Then you will know in about 8 seconds if it's parameters or not.  All of my mills have post and go, I don't even have the editor opening for my mill code.  Any way, let me know if I can help.

[Jcncprogrammer]

Ok here is a simple part that has 1/2 holes drilled  in 5 sides machined from a 2x2" aluminum billet machined down to a 1.75"x1.75" block. Thank you jlw for being able to do this for me.

TESTPART.SLDPRT

[crazy^millman]

Here is how I would program the part for that machine. I programmed it in 2017 since I was not sure what version of Mastercam you were running. Sorry far back as I go on this system.

5TH AXIS CGI TESTPART.mcam