5 Axis problem

[Christian Mora]

I have a problem in my OKK Vp400 machine which I try to adjust my center of rotation however I cannot move it, I use the parameters 19700 to adjust but by placing random numbers it reaches the same position, I checked the parameters however I still cannot make my machine work with 5 axis

[crazy^millman]

In MDI G43.4 and G68.2 don't show illegal G code do they?

[Christian Mora]

When I placed G68.2, it gave me the illegal G alarm. What I don't understand is that when the machine failed, it was out of nowhere. I'm starting to believe that some operator changed some configuration, but I checked my parameters and I didn't find anything strange.

[cncappsjames]

"IMPROPER G-CODE" alarms nearly always indicate the option/function isn't present in the machine. 

Command the following in MDI;

G68.2X0Y0Z0I0J0K0

G53.1

G4X5.0

G49G53Z0

G69

 

The ONLY way the #19700-#19705 parameters even matter is if you're using G43.x ("x" being different modes etc...), G68.x, or G54.4. 

If your code doesn't command those function, yiu could chance #19700-#19705 to all 0's  and it won't make a bit of difference.  

[crazy^millman]

Many times builder sell a 5 Axis machine without all the options. then people go to use the machine with those options only to find out they are not present. Then adding them can be a pain. for now will have to program from the Pivot point since it is a Head-Head machine. Need to get a hold of the dealer and see what options were purchased. Then if they were figured out why they are not working correctly. Also just heard of Okuma's with Faunc controls where the Mcodes in the book don't match the one the machine has. Took a seasoned veteran with a cheat cheat for one customer to get their Okuma VP machine running. Once the secret hidden codes were discovered and all the parameters dialed in the machine is running great.

[cncappsjames]

If FANUC options are installed in the field, the FANUC Engineer will not configure them. He or She will only turn them on. It is up to your builder/dealer to configure them.

Why is that you ask? Ask the guy at Haas that decided to call ANY single rotary axis "B" axis... he's got a part time gig at a few machine tool builders... I'm sure of it.

[crazy^millman]

14 hours ago, cncappsjames said:

If FANUC options are installed in the field, the FANUC Engineer will not configure them. He or She will only turn them on. It is up to your builder/dealer to configure them.

Yeah why I get work is this very reason. At least 20 different times I have had to go in and help dial in machines after this was done.

[Christian Mora]

Thank you for your comments, if I don't have this option enabled, what can I do to adjust it? I'm out by +0.025"

[#Rekd™]

Likely best to get your Applications Engineer in to help configure the machine correctly. 

[cncappsjames]

25 minutes ago, Christian Mora said:

Thank you for your comments, if I don't have this option enabled, what can I do to adjust it? I'm out by +0.025"

You'll need to adjust either your work offset or your tool length offset.... best I can recall anyway since i never program COR anymore.

[Aaron Eberhard]

Pragmatically, if you've programmed your part to what you believe the center of rotation was and then find out that it's not the real center of rotation, if you don't have TCPC/Work Correction, I would move the plane (or model) in your CAM system to the Real center of rotation and repost.    You can hack around trying to do individual work offset corrections, but if you're using simultaneous 5 axis motion, they'll all be wrong.   Moving the model in CAM will ensure that no matter what you do, it'll be correct without fiddling.

 

That's why TCPC is worth what they charge for it!  

[crazy^millman]

1 hour ago, Christian Mora said:

Thank you for your comments, if I don't have this option enabled, what can I do to adjust it? I'm out by +0.025"

Change the overall length of your tool in your program and re-post. Best way to check is to use a known gauge on the machine to check for these type of issues. Make a block with different angles and then do a shim check at each angle to ensure the changes you have made are exactly what you were thinking before cutting the part.