G68.2 with Renishaw probe on 31i model B5 Doosan VCF 850LSR

[Seedy steve]

 

Please check this code and let me know what is wrong, or how to fix it.

This is a bore measure path p9814, but I will need a boss measure code.

Here is the not working code that I tried...
O0000
(MASTERCAM    - 2023)
(POST         - DOOSAN_VCF_FANUC_AGG)
G00 G90 G17 G20 G40 G69 G80
G100
G00 G17 G90 G56
X0 Y0 (TOP MAPPED APPROACH POINT)
M11 M39 (B-AXIS UNLOCK, A-AXIS UNLOCK)
B49.741 A5.93
G68.2 X0. Y0. Z0. I275. J310. K243.109
G53.1
M10 M38 (B-AXIS LOCK, A-AXIS LOCK)
X0 Y0
G43 H35 Z1.
M165 P9832       at this point all looks well...
M165 P9810 Z-.25 F5.    Here the machine takes off 16." in X by the time it gets to Z-.25
M165 P9814 D2. S2   Then here it faults to (Path obstructed)
M165 P9810 Z1.
M165 P9833
G28 Z0.
G49
G69
M05
G200
M30
%

RMP400 probe.

 

Thanks in advance for any reply.

 

Steve.

[crazy^millman]

Is there something in the Probing macros that cancel G68.2? Would need to run them in single block and see if a G69 is called.

[cncappsjames]

Not knowing your machine's G/M codes, this is how I would format my programs.

 

O0000
(MASTERCAM    - 2023)
(POST         - DOOSAN_VCF_FANUC_AGG)
G00 G90 G17 G20 G40 G69 G80
G100

M11 M39 (B-AXIS UNLOCK, A-AXIS UNLOCK)
G00 G17 G90 G56B49.741 A5.93 <<<< Activate work offset with Tilt and Rotary positions only. Linear positions are after TWP is active.
G68.2 X0. Y0. Z0. I275. J310. K243.109
G53.1
M10 M38 (B-AXIS LOCK, A-AXIS LOCK)
X0 Y0 <<<<<< linear positions here
G43 H35
M165 P9832
M165 P9810 Z1.0 F100. <<<< NEVER move the machine around unless the Z is home with the probe UNLESS the probe is on AND positioning in protected mode.

M165 P9810 Z-.25 F5.
M165 P9814 D2. S2. <<<<<< Decimal points don't matter.... until they do. User them always to remove all doubt.  
M165 P9810 Z1.
M165 P9833
G28 Z0.
G49
G69
M05
G200
M30

 

If you still encounter problems it's one of two things; parameters not set correctly, or your probing software does not support probing while in TWP.

I'm pretty sure software F-4012-0519-AA or later is good to go. F-4012-0519-AW or later is best if you can get it.

 

[Seedy steve]

 

good to know.

Looks like we r ordering software... it did the same thing.

 

I did need linear movement pre positioning to get within the range of motion for the offset/ angle. before g68 . (top mapped approach point)

but thanks for clarifying things for me. We were not sure how to tell if the software was capable or not. looks like not.

 

s.

[Paul Anderson]

Good Morning,

I work for DN Solutions and have been away from here for a while. The embedded macros in the GUI, what you are calling with M165, don't support probing in TWP. The GUI macros only support the most common uses of probing. You will need Inspection Plus. The attached doc is from one of our dealers and explains how to generate macros for probing in TWP and required edits to the probing start and end macros. This has been tested on a DVF5000 but not on a VCF. Shouldn't be hard but the main thing is related to 2 parameters that MUST be on only during probing in TWP.

DN Solutions 5-axis Inspection Plus.pdf

[cncappsjames]

Interesting parameter differences.  

Why do you guys turn off LV3 off ever  @Paul Anderson? 

On 3/18/2024 at 6:05 AM, Seedy steve said:

I did need linear movement pre positioning to get within the range of motion for the offset/ angle. before g68 . (top mapped approach point)

I'm not familiar with top mapped approach point. 

I always have G54.4Pn in my code (Work Setting Error Compensation) which REQUIRES no linear position move until after G68.2

I missed you not having that function activated. My mistake.

There's different rules for different functions and different combinations of functions. 

[Seedy steve]

5 hours ago, cncappsjames said:

turn off LV3

IDK what that is... lol I am still learning g-code after 20 years!

this VCF has 3 meters of X , so if u r not close to position, it will often b out of range after g68.2 .

we r getting probing software Tuesday.

thanks again.

s

[Paul Anderson]

8 hours ago, cncappsjames said:

Why do you guys turn off LV3 off ever  

James, I haven't a clue why. The factory doesn't respond to questions of such magnitude. But it isn't just us. The Renishaw manual clearly states the need and use of these 2 parameters leading me to believe that having them on all the time is not universal.

[cncappsjames]

3 hours ago, Seedy steve said:

IDK what that is... lol I am still learning g-code after 20 years!

this VCF has 3 meters of X , so if u r not close to position, it will often b out of range after g68.2 .

we r getting probing software Tuesday.

thanks again.

#5400.5 = 1 (LV3) Rotates MACRO Variables to be read in active coordinate system - For Probing while TWP is active.

Interesting about being out of range. In a few machines I've encountered over the years,  for some unexplainable reason, I've had to set #1301.7 = 0 Stroke Pre-Check Off because for some reason the control thinks it is going to overtravel while TWP was active. It's only been on certain  FANUV CNC Series and Edition Softwares. But the machine never did overtravel.  High Level Math... one of the great mysteries for me.

[Seedy steve]

the problem probing at angle may not be the lack of software it seems...

If not, it may likely be connected to my post processor not agreeing with the machine!

I have been getting movement out of travel on the g68.2 line. the B axis on the head wants to08.nc turn upside down!

In case your curious...  

The V536 file is code that worked for another dept. found on this machine.

I have the team at inhouse solutions looking at it for me. I'm sure we will get it straight.

 

s.

V536LHB

[Paul Anderson]

1 hour ago, Seedy steve said:

the problem probing at angle may not be the lack of software it seems...

If not, it may likely be connected to my post processor not agreeing with the machine!

I have been getting movement out of travel on the g68.2 line. the B axis on the head wants to08.nc turn upside down!

In case your curious...  

The V536 file is code that worked for another dept. found on this machine.

I have the team at inhouse solutions looking at it for me. I'm sure we will get it straight.

 

s.

V536LHB 16.39 kB · 0 downloads

Something definitely looks wrong with your G68.2 lines. It looks as if they have the post setup for a C Axis machine, rotating around Z.

The order of rotations for Eulers Angles should be Z, X, Z again. The J's look good but the I's don't

[Seedy steve]

On 3/22/2024 at 11:49 AM, Paul Anderson said:

Something definitely looks wrong with your G68.2 lines. It looks as if they have the post setup for a C Axis machine, rotating around Z.

The order of rotations for Eulers Angles should be Z, X, Z again. The J's look good but the I's don't

Gotter figured out.

I J and K were ok

My A moves before g68.2 lines have been coming inverted +,-. When I fix this ,the code is seamless. the machine only uses B180. to correct pre positioning that is out by more than 90. deg. in A. That is why it took so long to find the trouble.