G05 vs G08 on Fanuc

[SuperHoneyBadger]

Also, @cncappsjames, while I have your ear...

I'm seeing stuttering and jerky motion during code-dense dynamic paths with G131 on my 660 when the programs are in the data server, vs main memory. Is this expected behaviour? The programs are pushing 300kb, and it feels like it gets worse the bigger the files are. Any insight would be appreciated!

[crazy^millman]

56 minutes ago, SuperHoneyBadger said:

Also, @cncappsjames, while I have your ear...

I'm seeing stuttering and jerky motion during code-dense dynamic paths with G131 on my 660 when the programs are in the data server, vs main memory. Is this expected behaviour? The programs are pushing 300kb, and it feels like it gets worse the bigger the files are. Any insight would be appreciated!

No the tuning of the parameters needs to be done at the most common speeds and feeds to dial the machine in.

[TFarrell9]

This thread was revived at a pretty decent time for me, as I have a question pertaining to this function. 

We recently acquired a Mitsubishi MVR 35 with a Fanuc 18i-MB control. This is the first machine I've touched that's had the G05.1 AICC function. In order to control the speed/accuracy setting commands for this one, G510 Mx (x=0,1,2,3) must be commanded before the G05.1 Q1. If not, AICC will still activate, but it will default to M0 for the finishing/"slow" setting.

 

Anyways, I'm encountering a problem after indexing the RAH. G05.1 Q0 is commanded at tool end, before the RAH indexes. However, when it gets to G05.1 Q1 again (after RAH index, same tool), I get Alarm 5111 IMPROPER MODAL G-CODE (G05.1 Q1). I hit Reset, start the program from the G510 line and everything goes on as it should. 

I've tried adding another G05.1 Q0 before the G510 line, as well as a G80 for kicks, and no dice. I'm not seeing anything on the DRO for modal codes that would be causing this, so what could be holding it up? I know the mode is being cancelled because AICC no longer flashes after running G05.1 Q0.

[cncappsjames]

2 hours ago, SuperHoneyBadger said:

Also, @cncappsjames, while I have your ear...

I'm seeing stuttering and jerky motion during code-dense dynamic paths with G131 on my 660 when the programs are in the data server, vs main memory. Is this expected behaviour? The programs are pushing 300kb, and it feels like it gets worse the bigger the files are. Any insight would be appreciated!

You've run the same program, the same way on both CNC_MEM and DATA_SV?

300kb is nothing. I routinely run programs 3-4x that without the stuttering you are describing.

A note on DATA_SV management, I have seen a performance degradation when there are "a lot" of programs in the root DATA_SV. I always recommend customers to use folders and sub-folders. I don't have a definitive number of programs when the performance degredation starts unfortunately. It was just something I noticed accidentally. So I typically reccommend \\DATA_SV\CUSTOMER_NAME\PART_NUMBER\REV\ for a structure. This keeps things clean. organized and running smoothly... in my experience anyway.

[cncappsjames]

38 minutes ago, TFarrell9 said:

...I'm encountering a problem after indexing the RAH. G05.1 Q0 is commanded at tool end, before the RAH indexes. However, when it gets to G05.1 Q1 again (after RAH index, same tool), I get Alarm 5111 IMPROPER MODAL G-CODE (G05.1 Q1). I hit Reset, start the program from the G510 line and everything goes on as it should.

G05.1 is VERY picky about what is modal in activation/deactivation.

If I were a betting man, something is activated in your G510 MACRO that needs to be canceled. If you don't have access to the MACRO, cancel EVERYTHING between operations. 

G00G17G40G80G90G94G98
G49G53P1Z0.0S11460M03
N30001(Contour Back Edge for Inspection Surface - 3:00 Face)
G05.1Q1
G00G90G54...
G43Z4.0H#517
...
G40Y2.5625
G00Z4.0
G05.1Q0
G00G49G90G53P1Z0.0

 

I would try activating the G510 after the G54 or after the G43, the deactivating  either  before/after the G05.1Q0 or after the G49.  That's where I'd start.

Be careful with G49. If parameters are not set correctly, you will get a Z- move the equivalent to the length of your positive tool length offset.

 

HTH

[SuperHoneyBadger]

48 minutes ago, cncappsjames said:

You've run the same program, the same way on both CNC_MEM and DATA_SV?

300kb is nothing. I routinely run programs 3-4x that without the stuttering you are describing.

A note on DATA_SV management, I have seen a performance degradation when there are "a lot" of programs in the root DATA_SV. I always recommend customers to use folders and sub-folders. I don't have a definitive number of programs when the performance degredation starts unfortunately. It was just something I noticed accidentally. So I typically reccommend \\DATA_SV\CUSTOMER_NAME\PART_NUMBER\REV\ for a structure. This keeps things clean. organized and running smoothly... in my experience anyway.

I did not run the exact program, as it didn't fit in CNC_MEM. I think I have 350kb total there - the toolchange, renishaw and my macros are taking up some space of course.

We do save the programs to the root of DATA_SV, there are 10 programs there, taking up maybe 2Mb. I'll implement a folder structure moving forward. The machine with the server option is loaded up at the moment, but when I can I'll test some dynamic toolpaths at speed and see. I'm typically not operating the machines, so I don't get to see when EXACTLY this behaviour crops up.

[cncappsjames]

Between the MTB stuff in the \\CNC_MEM\SYSTEM\ , \\CNC_MEM\USER\, and the \\CNC_MEM\USER\LIBRARY folders.... MTB stuff, tool measurement, spindle probing, user MACRO programs, etc... should take up less than 500kb, leaving at least 7,500kb free space.

My personal opinion is ALL part programs should reside and run from the DATA_SV. This provides one with the possibility of network backups which on CNC_MEM isn't possible... at least not the same way.

 

HTH

[TFarrell9]

4 hours ago, cncappsjames said:

G05.1 is VERY picky about what is modal in activation/deactivation.

If I were a betting man, something is activated in your G510 MACRO that needs to be canceled. If you don't have access to the MACRO, cancel EVERYTHING between operations. 

G00G17G40G80G90G94G98
G49G53P1Z0.0S11460M03
N30001(Contour Back Edge for Inspection Surface - 3:00 Face)
G05.1Q1
G00G90G54...
G43Z4.0H#517
...
G40Y2.5625
G00Z4.0
G05.1Q0
G00G49G90G53P1Z0.0

 

I would try activating the G510 after the G54 or after the G43, the deactivating  either  before/after the G05.1Q0 or after the G49.  That's where I'd start.

Be careful with G49. If parameters are not set correctly, you will get a Z- move the equivalent to the length of your positive tool length offset.

 

HTH

Good call on the G49, that's what it was. Thanks James!

[Leon82]

You can speed up drilling with with peck clearance I think it's around 5200 or 5110 on fanuc. It usually defaults to .5mm.

 

I've used the g5.1on drilling before.  The only time it caused an issue is with the probe.

 

The danger lies in if you hit reset the program stops where it read ahead to. So if you page up you can potentially start in a spot where your not expecting.

[cncappsjames]

High Speed modes should NEVER be active during probing. EVER!