Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Fanuc look ahead question

Thee Dragracer1951

By Thee Dragracer1951,
in Industrial Forum

 Share

Recommended Posts

Post dept Newbie

Post dept

Posted
Posted

All,

 

I have been working on adding some of this functionality to mpmaster for everyone to use. I'll be sure to document everything very well so it can be used as a reference. I'm having a problem though.....I don't have a machine.

 

If you've got some time to help, it will be beneficial to everyone.

 

Here are a couple of questions that I've got:

 

1. Anyone here using the new HPCC G05 P10000?

Looking for output format. Pg 78 of the 16/18i manual shows that it can be used along with G05.1.

 

2. I have seen several different formats for the G05.1 including the following:

 

Q1 - I have been told that this is for simple interpolation

Q2 - I have been told that this actually filters for arcs in the control and is an additional option.

P/R - Either the P or R address used to determine the acceleration/decceleration characteristics (range from 1-10)

 

Thanks for the feedback. I'll be adding the Mazak stuff as well.

 

Brett

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Well the G05.1 and G05 P10000 are not used at the same time when I have done it. You have either or from my experience.

 

The control I have for G05.1 QX sets Q1 turn on AI advanced Preview control/AI Contour Control mode and Q0 truns off AI advanced Preview control/AI Contour Control mode the G05.1 QX.

 

Where as with G08 PX the P1 turns on Advanced Preview Control On and P0 turn off Advanced Preview Control. Page 378 B-64124EN/01 for the Oi-Mc controls we have.

 

Now From what I am reading and going to try this wek is that you can use both on with no problem but you have to turn on the G08 1st then the G05.1 if you try ot do it the other way you will alarm out the control.

 

HTH

 

Email if I can be of more assistance, Also be glad to Beta this stuff for you as well on our Oi controls.

Link to comment
Share on other sites
Post dept Newbie

Post dept

Posted
Posted

Ron,

 

Looks good. For the G08 P1 and the G05.1 Q1....yes, turn on the G08 P1 then call G5.1 Q1. Also, both must be activated before G43.

 

With regards to the HPCC, I got this back from a local guy as well.

 

G05.1 Q2 is auto filter (for arcs as I had mentioned earlier) and can only run in G5P10000 HPCC mode.

 

So Q1 is not used with P10000 but if you've got the Q2 option you must call it inside the P10000.

 

I guess the only thing left before testing is to figure out the accel/decel option (the other optional parameter on that line). Perhaps this is a machine specific thing (it's not in the books that I've got).

 

Brett

Link to comment
Share on other sites
Guest CNC Apps Guy 1

Guest CNC Apps Guy 1

Posted
Posted

Brett,

 

If you need any of the Fanuc Control manuals in PDF I've got 15,16,18,21,31, (both T and M and iT and iM as well as 0i both M & T, just let me know what you want and I'll kick them to you.

 

I've got access to Fanuc Robodrill MATE with an OiMA that is there for me to play with "...if I have time..." and I've always got play time biggrin.giftongue.gif for that kind of thing. It has G8 P1 and G5.1Q1 AI-NANO I or whatever they are calling it this week.

 

quote:
...Perhaps this is a machine specific thing (it's not in the books that I've got)...

Yeah, those settings are machine builder specific.

 

I don;t believe you can run G8 and G5.1 simultaneously, it's either 1 or the other but not both. Each one has some restrictions too. To be safe anything opcode 3 I don't allow to run with the HSM options.

 

[ 01-30-2007, 11:01 PM: Message edited by: James Meyette ]

Link to comment
Share on other sites
Guest CNC Apps Guy 1

Guest CNC Apps Guy 1

Posted
Posted

Ok,

 

I ran the program below and all went well EXCEPT for the last G8P0 cancel. It alarmed out with a "5111 G08 CANNOT BE COMMANDED" Alarm on the LAST cancel.

 

You HAVE to call G8P1 BEFORE G5.1Q1 or you get the 5111 Alarm.

 

I am going to create a long program to test if there is a Cycle Time Differential running just G8P1, just G5.1Q1 and running both simultaneously. Also I'll test if incremental is faster than absolute and report the results.

 

 

code:
%

O0001(SAMPLE MAIN)

G0G17G90G80G49G40

 

G0G91G28Z0

G28X0Y0

G90

G90G52X0Y0Z0

 

G90G10L2P1X8.080550Y-6.11215Z-12.

G11

 

M1

N1T1M6

G17

/G8P1

G5.1Q1

G0G54X0Y0S2500M3

G0G43Z5.H1

M98P110

G5.1Q0

/G8P0

G91G28Z0M5

G90G28X0Y0

G49

M01

 

N2T2M6

G17

G49

/G8P1

G5.1Q1

G0G54X0Y0S2500M3

G0G43Z5.H2

M98P100

G5.1Q0

/G8P0

G91G28Z0M5

G90G28X0Y0

G49

M01

 

N3T3M6

G49

G8P1

G5.1Q1

G0G54X-4.5Y0S2500M3

G43Z5.H3

M98P101

G5.1Q0

/G8P0

G91G28Z0M5

G90G28X0Y0

G49

M01

 

N4T4M6

G49

/G8P1

G5.1Q1

G0G54X-4.5Y0.S2500M3

G0G43Z5.H4

M98P101

Q5.1Q0

/G8P0

G91G28Z0M5

G90G28Y0

G49

M30

%

Link to comment
Share on other sites
Guest CNC Apps Guy 1

Guest CNC Apps Guy 1

Posted
Posted

To say the difference in Performance of G8P1 and G5.1Q1 is stark is being FAR too kind. I'll let the numbers speak for themselves...

 

Fanuc Oi-MC Control

Programmed Feedrate of 250 IPM

 

1. NC Program - G5_1Q1ABS.NC

o Cycle Time – 1:27

o File Size - 52 KB

o HSM Algorithm - G5.1Q1

o Absolute Programming (G90)

o Arc Filtering

 

2. NC Program - G5_1Q1INC.NC

o Cycle Time – 1:27

o File Size – 50 KB

o HSM Algorithm - G5.1Q1

o Incremental Programming (G91)

o Arc Filtering

 

3. NC Program – G8P1ABS.NC

o Cycle Time – 3:07

o File Size – 52 KB

o HSM Algorithm - G8P1

o Absolute Programming (G90)

o Arc Filtering

 

4. NC Program – G8P1INC.NC

o Cycle Time – 3:07

o File Size – 50 KB

o HSM Algorithm - G8P1

o Incremental Programming (G91)

o Arc Filtering

 

5. NC Program - G5_1Q1ABS-NF.NC

o Cycle Time – 1:47

o File Size – 126 KB

o HSM Algorithm – G5.1Q1

o Absolute Programming (G90)

o No Arc Filtering

 

6. NC Program - G5_1Q1INC-NF.NC

o Cycle Time – 1:47

o File Size – 119 KB

o HSM Algorithm – G5.1Q1

o Incremental Programming (G91)

o No Arc Filtering

 

 

7. NC Program – G8P1ABS-NF.NC

o Cycle Time – 11:34

o File Size – 126 KB

o HSM Algorithm – G8P1

o Absolute Programming (G90)

o No Arc Filtering

 

8. NC Program – G8P1INC-NF.NC

o Cycle Time – 11:34

o File Size – 119 KB

o HSM Algorithm – G8PQ1

o Incremental Programming (G91)

o No Arc Filtering

 

9. NC Program – G8P1G5_1Q1ABS-NF.NC

o Cycle Time – 1:47

o File Size – 126 KB

o HSM Algorithm – G5.1Q1 & G8P1 Simultaneously

o Absolute Programming (G90)

o No Arc Filtering

 

10. NC Program – G8P1G5_1Q1INC-NF.NC

o Cycle Time – 1:47

o File Size – 119 KB

o HSM Algorithm – G5.1Q1 & G8P1 Simultaneously

o Incremental Programming (G91)

o No Arc Filtering

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...