VARIAXIS i600 G54.4

[crazy^millman]

Here is what posted code would look like for a Fanuc OKK Machine.

%
O0000 (68.2 PROGRAMMING EXAMPLE)
(T290 - 1/2 FLAT ENDMILL     - H290 - D290 - D0.5000")
(T62  -  1/8 DRILL           - H62  - D62  - D0.1250")
G00 G17 G20 G40 G80 G90
G80
G91 G28 Z0.
G28 X0. Y0.
M79
M11
G90 A0. C0.
(POSTABILITY 5-AXIS OKK VC-X350)
(EMASTERCAM FORUM HELP FROM 5TH AXIS CGI)
T290 (1/2 FLAT ENDMILL)
M06
G54 G17 G90
G94
G05 P10000
G00 A0. C0.
M78
M10
X-1.425 Y.7499 S1069 M03
G43 H290 Z.25 T62 /
Z.2
G01 Z0. F6.42
X1.175
G02 Y.4499 I0. J-.15
G01 X-1.175
G03 Y.15 I0. J-.1499
G01 X1.175
G02 Y-.15 I0. J-.15
G01 X-1.175
G03 Y-.4499 I0. J-.15
G01 X1.175
G02 Y-.7499 I0. J-.15
G01 X-1.425
G00 Z.25
G49
G05 P0
G80
G91 G28 Z0.
G54 G90
G05 P10000
M79
M11
A-90. C-180.
G68.2 X0. Y0. Z0. I0. J90. K0.
G53.1
M78
M10
X-1.425 Y-.1251
G43 H290 Z1.125
Z1.075
G01 Z.875
X1.175
G02 Y-.4251 I0. J-.15
G01 X-1.175
G03 Y-.725 I0. J-.1499
G01 X1.175
G02 Y-1.025 I0. J-.15
G01 X-1.175
G03 Y-1.3249 I0. J-.15
G01 X1.175
G02 Y-1.6249 I0. J-.15
G01 X-1.425
G00 Z1.125
G49
G05 P0
G69
G80
G91 G28 Z0.
G54 G90
G05 P10000
M11
A-90. C270.
G68.2 X0. Y0. Z0. I90. J90. K0.
G53.1
M10
X-1.425 Y-.1251
G43 H290 Z1.125
Z1.075
G01 Z.875
X1.175
G02 Y-.4251 I0. J-.15
G01 X-1.175
G03 Y-.725 I0. J-.1499
G01 X1.175
G02 Y-1.025 I0. J-.15
G01 X-1.175
G03 Y-1.3249 I0. J-.15
G01 X1.175
G02 Y-1.6249 I0. J-.15
G01 X-1.425
G00 Z1.125
G49
G05 P0
G69
G80
G91 G28 Z0.
G54 G90
G05 P10000
M11
A-90. C0.
G68.2 X0. Y0. Z0. I180. J90. K0.
G53.1
M10
X-1.425 Y-.1251
G43 H290 Z1.125
Z1.075
G01 Z.875
X1.175
G02 Y-.4251 I0. J-.15
G01 X-1.175
G03 Y-.725 I0. J-.1499
G01 X1.175
G02 Y-1.025 I0. J-.15
G01 X-1.175
G03 Y-1.3249 I0. J-.15
G01 X1.175
G02 Y-1.6249 I0. J-.15
G01 X-1.425
G00 Z1.125
G49
G05 P0
G69
G80
G91 G28 Z0.
G54 G90
G05 P10000
M11
A-90. C90.
G68.2 X0. Y0. Z0. I270. J90. K0.
G53.1
M10
X-1.425 Y-.1251
G43 H290 Z1.125
Z1.075
G01 Z.875
X1.175
G02 Y-.4251 I0. J-.15
G01 X-1.175
G03 Y-.725 I0. J-.1499
G01 X1.175
G02 Y-1.025 I0. J-.15
G01 X-1.175
G03 Y-1.3249 I0. J-.15
G01 X1.175
G02 Y-1.6249 I0. J-.15
G01 X-1.425
G00 Z1.125
G49
G05 P0
M05
G69
G80
G91 G28 Z0.
M79
M11
G28 A0. C0.
M01
T62 ( 1/8 DRILL)
M06
G54 G17 G90
G00 A-90. C90.
G68.2 X0. Y0. Z0. I270. J90. K0.
G53.1
M78
M10
X0. Y-.875 S2139 M03
G43 H62 Z2. T290 /
G94
G98 G81 Z.375 R.975 F4.11
G80
G49
G69
G80
G91 G28 Z0.
G54 G90
M11
A-90. C-0.
G68.2 X0. Y0. Z0. I180. J90. K0.
G53.1
M10
X0. Y-.875
G43 H62 Z2.
G98 G81 Z.375 R.975 F4.11
G80
G49
G69
G80
G91 G28 Z0.
G54 G90
M11
A-90. C-270.
G68.2 X0. Y0. Z0. I90. J90. K0.
G53.1
M10
X0. Y-.875
G43 H62 Z2.
G98 G81 Z.375 R.975 F4.11
G80
G49
G69
G80
G91 G28 Z0.
G54 G90
M11
A-90. C-180.
G68.2 X0. Y0. Z0. I0. J90. K0.
G53.1
M10
X0. Y-.875
G43 H62 Z2.
G98 G81 Z.375 R.975 F4.11
G80
G49
G69
G80
G91 G28 Z0.
G54 G90
M79
M11
A0. C0.
M78
M10
X0. Y0.
G43 H62 Z.25
G98 G81 Z-.5 R.1 F4.11
G80
G49
M05
G80
G91 G28 Z0.
M79
M11
G90 G0 A0.
C0.
M78
M10
G91 G28 Y0
G90
M30

Not sure if that helps you or not, but the above I could put anywhere on the table of the machine touch of the Zero like I have it set in the Mastercam program in the G54 work offset on the machine and expect it to run with no problem.

[crazy^millman]

These double posts are getting annoying.

 

 

Edited January 31, 2018 by C^Millman
Double Post no reason to repeat myself.

[Jcncprogrammer]

hmm, here is the way i did it, im guessing this wont work, see attached..

TESTPART.mcam

[crazy^millman]

5 minutes ago, Jcncprogrammer said:

hmm, here is the way i did it, im guessing this wont work, see attached..

TESTPART.mcam

It should work, but can I make a suggestion? What I will do it create my Top Plane and then I will use the create relative to create the correct planes for each of the faces in relational to that. Since you had the part moved to TOP you could just use the 4 planes already there and go about it that way. Front, Left, Right and Back.

Compare the front plane and your -90. Plane. Notice the difference between those 2. What you did posted through the post I have for a different control  and machine and I compared the drilling cycles and they are identical so it would work, but I like my planes a certain way and that is where the create relative has always served me well.

[Jcncprogrammer]

ok, cmillman. I will start doing that to make my life easier.Thanks!

 

[Barrier21]

Okay I ran Jcnc’s test program and here is what I got (sorry for the bad hand writing) but all numbers from from outer wall in hole to side of part are .729 and .719. Not sure what exactly is going on. I tried running JLW’s program and had to change some M codes for C clamp and unclamp and it started to run then when it goes to rotation it try’s going A90 (our machine can only do A-90) so tried making the numbers negative, after it rotates to A-90 when it hits the G68.2 line it still tries going back to A90. I tried changing some numbers and it just goes to odd positions. Maybe jlw post uses Euler angles and ours is Roll pitch yaw so the I j k numbers are different from ours?

[Barrier21]

Here is a snip of jcnc test program g68.2 at A-90 C180 and one from jlw test program g68.2 A90 C180. I am pretty confused lol

[MIL-TFP-41]

Hmmm

One program I see G54.4 P2 being used.

Are you writing your error to the P2 offset or the P1 offset?

[crazy^millman]

1 hour ago, Barrier21 said:

Okay I ran Jcnc’s test program and here is what I got (sorry for the bad hand writing) but all numbers from from outer wall in hole to side of part are .729 and .719. Not sure what exactly is going on. I tried running JLW’s program and had to change some M codes for C clamp and unclamp and it started to run then when it goes to rotation it try’s going A90 (our machine can only do A-90) so tried making the numbers negative, after it rotates to A-90 when it hits the G68.2 line it still tries going back to A90. I tried changing some numbers and it just goes to odd positions. Maybe jlw post uses Euler angles and ours is Roll pitch yaw so the I j k numbers are different from ours?

Leads me to believe that is a bad rotation point in the parameters for the COR on the machine. Has that been verified and checked by Mazak or someone who knows how to set them correctly?

[Barrier21]

The service guy who set up the machine supposedly got everything set up correctly. We’ve emailed mazak several times about getting our high pressure coolant set up and have been waiting for around a month or so now. But when he does come we will make sure he re calibrates and gets it done correctly. Just sent another email about doing mazacheck and ballbar and laser calibration. Will see how they respond! Thanks!

[Leon82]

You can indicate the bore in the table and compare it to the x Cor number it should be relatively close.

 

Our machine has the ez5 but we still ran a test part to dial in the numbers

[huskermcdoogle]

Drop the P1 word out of the G68.2 and you will be doing Euler angles,  

[jlw™]

Sounds like your parameters are not set correctly.  Until parameters are set the G53.1 line will basically index the machine A90 or A-90 and C will resolve to the wrong angle.  Sorry I was busy all day and didn't have time to look the parameters up.  I will go in a few minutes early to find my notes for you.  I can't believe Mazak hasn't called you back yet.  I'd be mad as a wet hen.

[Barrier21]

Sorry for the late response but thanks Jlw! I talked to mazak apps and the guy said he doesn’t know anything about having to change parameters to get it to work.. But an apps guy and service guy are coming out tomorrow to re calibrate the machine. Turns out the first service man KNOWINGLY never calibrated the A axis and his actual excuse was he just couldn’t figure it out because he’s never done a Variaxis.. not to mention his numbers were off on the C axis as well and it took him 2 months to fess up to not doing it. Moral of the story is we’ve been trying to run parts on an uncalibrated machine and Mazak service here is really disappointing.. I can’t thank you guys enough for all the help though y’all are great people!

[crazy^millman]

19 minutes ago, Barrier21 said:

Sorry for the late response but thanks Jlw! I talked to mazak apps and the guy said he doesn’t know anything about having to change parameters to get it to work.. But an apps guy and service guy are coming out tomorrow to re calibrate the machine. Turns out the first service man KNOWINGLY never calibrated the A axis and his actual excuse was he just couldn’t figure it out because he’s never done a Variaxis.. not to mention his numbers were off on the C axis as well and it took him 2 months to fess up to not doing it. Moral of the story is we’ve been trying to run parts on an uncalibrated machine and Mazak service here is really disappointing.. I can’t thank you guys enough for all the help though y’all are great people!

Wow sorry, but I suspected something was wrong with the machine. I never would have imagined it was never done, but yes I have seen it and I chased a part for a customer a good month until the correct values were finally input into the machine. Like magic all the problems with mismatch and tolerance issue disappeared immediately with no programming changes needed.

Thanks for chiming back in.

[huskermcdoogle]

On 2/1/2018 at 6:14 PM, Barrier21 said:

Sorry for the late response but thanks Jlw! I talked to mazak apps and the guy said he doesn’t know anything about having to change parameters to get it to work.. But an apps guy and service guy are coming out tomorrow to re calibrate the machine. Turns out the first service man KNOWINGLY never calibrated the A axis and his actual excuse was he just couldn’t figure it out because he’s never done a Variaxis.. not to mention his numbers were off on the C axis as well and it took him 2 months to fess up to not doing it. Moral of the story is we’ve been trying to run parts on an uncalibrated machine and Mazak service here is really disappointing.. I can’t thank you guys enough for all the help though y’all are great people!

I don't know for sure, but I would imagine this is a problem for all builders.  There are going to be certain geographic areas where the dealers can't find competent people for doing these measurements, or lack the understanding of the functions to the point where they understand how tight they truly need to measure things too.  Probably best to keep this level of things in the hands of the apps guys, at least on a new install.  But I have had many cases in my past where our maintenance crew would work on a robot or machine tool and claim they didn't touch anything, but magically I have lost my home positions, or have a significant geometry error somewhere.  It always comes down to lack of mechanical or electrical understanding, they go digging into something without understanding the implications of their "repair".  It got to the point where I had to approve all procedures, in full, and anything outside of written procedures had to be approved by myself, verbal was ok, but usually these phone calls came very late in the evening.  Lots of time wasted becuase of the lack of application and or machine understanding.  The biggest thing though that I found to be a problem was they would use .001" plunger indicators for everything.  They would indicate to a couple thou at best and say, "but the needle isn't moving much any more, it's pretty good".  The reality was, that in most of those cases, they typically needed to be .0002" or better, worst case .0005".  After a few years or struggling, we finally landed a "machine tool specialist", he had lots of real world machine tool repair experience, and understood the measurements needed and how to take them, it was a huge relief to have him.  Only took me two times through to get him fully up to speed on a head alignment, physical alignment wasn't an issue, it was all in how to activate the head offsets and check if he got them right.  He had them on paper, all I had to do was get them into the control and help him verify.  Huge improvement.

It all comes down to the people and their training.  As machine tools become more advanced, the level of training that operators, engineers/programmers,  techs, applications folks,  receive needs to be much greater.  Ignorance is no longer an option.

[NOTW Programmer]

Has anyone else experienced having to send the machine home before G54.4 actually takes any effect? We have an AWEA FCV-620 that need this, otherwise, it gets lost and starts machining off the stock. Talk about dangerous !!!

[crazy^millman]

5 hours ago, NOTW Programmer said:

Has anyone else experienced having to send the machine home before G54.4 actually takes any effect? We have an AWEA FCV-620 that need this, otherwise, it gets lost and starts machining off the stock. Talk about dangerous !!!

No they have the parameters set wrong on the control to allow this to work. Fanuc should be brought in to help sort this out.