High speed maching

[KMartin]

Hello could I please get some help with high speed maching .I am using a Kitamura and programing with mastercam . 

When I turn on high speed maching the code is G990 Q1   G05 P10000 .I was told that the P value determines the accuracy

of the tool path .   When I try to lower the value of the P  I get a fault . Should I have high speed maching turned on 

for a Parallel toolpath . Thanks for any help .

[Leon82]

Usually you would have a g49 above it, then activate the tool offset.

 

It's been a while but on the old shops 2xi we used g5.1q1 but I believe the option was g5.1 P10000

 

Is it fanuc or their new os

[cncappsjames]

G05P10000 is AI Contour Control (High Precision Contour Control compatible) P is not a function of accuracy. If machining condition is present, R would be. 

G05.1 is AI Contour Control/NANO Smoothing/Smooth Interpolation

Different options.

[cncappsjames]

On 10/26/2023 at 7:57 AM, KMartin said:

.....

Should I have high speed maching turned on for a Parallel toolpath .

Thanks for any help .

You should have the contour control functions active when machining period. The machine will perform better. Part quality will be better (provided the settings from the factory are good).

And contrary to popular belief myth, use them during canned cycles (maybe with one exception until testing your specific machine - rigid tapping).

Here's some DATA to back up my claim;

3:24 - W/ NO HIGH SPEED MODES
3:11 - W/ G05.1Q1, G05.1Q3, AND G131 D1
3:07 - W/ ONLY G05.1Q1
3:06 - W/ G05.1Q1 AND G131 D1
3:06 - W/ ONLY G131 D1

G131D1 is a Matsuura specific code that sets certain Acc/Dec parameters to favor positioning type moves (as opposed to profile type moves).

If your machine has R levels (on the G05P10000 line), G131D1 would be a rough equivalent to G05P10000R1 or G05P10000R0.

 

Hope that helps.

[neurosis]

On 10/26/2023 at 6:57 AM, KMartin said:

Hello could I please get some help with high speed maching .I am using a Kitamura and programing with mastercam . 

When I turn on high speed maching the code is G990 Q1   G05 P10000 .I was told that the P value determines the accuracy

of the tool path .   When I try to lower the value of the P  I get a fault . Should I have high speed maching turned on 

for a Parallel toolpath . Thanks for any help .

 

The  Kitamuras, I believe, use an F value for the high speed accuracy and there are 3 Q levels just to make it more confusing..  I wish that MTB's would just stick to a standard.   

On our particular machines, which were first generation Arumatik controls , I don't think that you can control the accuracy when using HPCC  (I'd have to look in to this to be sure) , but it looks like you're mixing code.

The code should looks like this if you're using AICC and trying to adjust the accuracy.

G990 Q1. F157.
G05.1 Q1

That would be equivalent to G05.1 Q1 R3 on our Fanuc controls

Those F values require the decimal point.   It's just like using R1 - R10 except the accuracy values, on our machines anyway, are as follows

R1= Q1 F12.

R2 = Q1 F59.

R3 = Q1 F157.

R4 = Q2 F12.

R5 = Q2 F59.

.

R7 = Q3 F12.

and so on.

I'd take a look at your manuals just to be sure. I'm also not the best at trying to explain things so. 

 

 

[cncappsjames]

20 hours ago, neurosis said:

...

I wish that MTB's would just stick to a standard.   

...

A lot of the differences are the option packages put on the individual machines. Some builders skimp on the options to keep their machines in a certain price range, others option the machines appropriately, and still others are somewhere in between. 

Then there is the expertise of the AE doing the training on the machine.  Some of those guys aren't fit to teach someone how to run a toaster let alone a complex CNC, then you have guys like @zoober, @YoDoug, and @CrazyMillMan just to name a few who are at the top echelon.

JM2CFWIW 

[neurosis]

1 hour ago, cncappsjames said:

A lot of the differences are the option packages put on the individual machines. Some builders skimp on the options to keep their machines in a certain price range, others option the machines appropriately, and still others are somewhere in between. 

That I can understand. 

What I'm talking about, is that we have 5 different machines built by 5 different companies, all using the same controls -  every single one of them uses different code to adjust the Acc/Dec parameters,  The Kitamuras are probably the most convoluted.   

[cncappsjames]

Well... if you knew which parameters to change to get the desired result, you could create your own G/M code... 

[KMartin]

Morning thanks for all the help .This is the code we needed to turn on the high feed  . The machine is a Kitamura but it has a Mitsubishi control .
(KITAMURA)
(MACHINE GROUP-1)
(PROGRAM   - test)
(DATE      - NOV-21-2023)
(TIME      - 11:54 AM)
(T9-1/4 ENDMILL.015RAD  -H9-D9-D0.2500"-R0.0150")
N100 G00 G17 G20 G40 G80 G90
N110 G53 X-29.0
N120 G91 G28 Y0.0
N130 G28 Z0.
N140 (COMPENSATION TYPE - COMPUTER)
N150 T9 M06 (1/4 ENDMILL.015RAD)
N160 (MAX - Z6.)
N170 (MIN - Z-.166)
N180 G00 G17 G90 G54 X8.1131 Y-1.4021 S3056 M03
N190 G43 H9 Z6.
N200 M08
N210 G94
N220 G990 Q1.
N230 G05 P1
N240 Z.1
N250 G01 Z-.156 F25.
N260 X8.1454 Y-1.338 F33.21
N270 X8.1611 Y-1.3068
N280 X8.1634 Y-1.3022 Z-.1576
N290 G03 X8.1694 Y-1.2769 Z-.166 I-.0502 J.0253
N6940 X8.0904 Y1.0142 F100.
N6950 G00 Z6.
N6960 G05 P0
N6970 G990 Q0
N6980 M09
N6990 M05
N7000 G91 G28 Z0.
N7010 G90
N7020 G53 X-18.0
N7030 G91 G28 Y0.
N7040 G90
N7050 M30
%
 

[JB7280]

On 10/29/2023 at 11:07 PM, cncappsjames said:

G05P10000 is AI Contour Control (High Precision Contour Control compatible) P is not a function of accuracy. If machining condition is present, R would be. 

G05.1 is AI Contour Control/NANO Smoothing/Smooth Interpolation

Different options.

James, do you know of any literature, or forum posts, where the differences between all of the different options is explained, including where/when they should be used?  Matsuura's options are great, and easy to understand,  But I've never totally understood the where/why/when of G08, G05P10000, G05.1, etc etc.  

[cncappsjames]

Explained? Not really. Reading through the FANUC manuals has helped me more than any single person or other resource.

Reading through a FANUC manual is a little different than reading through other sorts of technical information. FANUC manuals are best consumed from start to finish because more often than not, understanding one function is very helpful in understanding subsequent functions.

High speed functions can be somewhat of a tangled web and OFTEN require that functions be piggybacked in order to function properly (i.e. G05.1Q1 first, then G05.1Q3X0Y0Z0 after the G43) ... and sometimes require MTB support on top of that though not very often.

The FANUC Connection manual is also very helpful.

https://www.dropbox.com/scl/fi/nxoh585ycbki24p81z402/Connection-Function-v6.pdf?rlkey=1tyso6ga2wiw4va0dhewcoga3&dl=0

[cncappsjames]

Here's a few examples of what/where/when;

 

https://www.emastercam.com/forums/topic/107265-ai-high-speed-look-ahead-parameter-settings/?do=findComment&comment=1344976