Fanuc gurus? Look ahead and block speed on older controls?

[honeybunches]

Looking at an older machine for some aluminum work we need to do.  has a Fanuc 16 on it.  Rated max feed rate (for what thats worth) on the machine is 600ipm.  I would be just fine with that if the machine could actually drive a decent path at that speed.  

Can anyone elaborate with the certain control series and available options so I can at least have an idea of the real ability of the control?  I know Fanuc is about the worst at charging for every little detail so any other owner may be left in the dark with just what the control was setup to do.  

Now I realize machine mechanics would play into this as well, but trying to get an idea from the control side.  

 

Many controls today, we can actually look up the block speed processing rate and blocks of look ahead and typically have a good idea how fast the control can go.  Seems I was always in the dark with fanuc

[civiceg]

Are you using G5.1? Have you tried filtering the code in Mastercam? 

[huskermcdoogle]

series 16 or 16i?  That will make bit of difference.  Does it have hpcc?  If not, you won't be happy at high feed rates.  Box way or linear guide machine.

[honeybunches]

Sorry, the company was looking at buying it so I don't have every detail but I know it is a 16mb.  If it does not have certain options, are these things we can work the MTB to have turned on or is that a major upgrade situation?  Like new boards and such?  We don't want to get into major expenses on it right out of the blocks.  

 

Not looking to do crazy HSM paths that Brothers are doing.  Just be able to run say a 2" square path at 200ipm and be smart enough to hold a god path?  

[Leon82]

After parameter 1320 there are max feed rate values for handle rapid jog, etc. Scroll after and they will show up.

Parameter 1604 bit 0 set to one will set the g5.1 on automatically during feed. 

Otherwise use g5.1 q1 to turn on

G5.1q0 is off

Also g8p1 is a block look ahead also 

 

Fanuc can add the aicc 1 or 2 if you pay them if you don't have the option.

[Leon82]

You may need a software upgrade worst case.

 

We have a feeler with an 18i I think, and it is terrible at high speeds.

The next one was a lot better as far as blends and not rounding off corners and machining fast and was an 18 I also.

The guy tried to tweak the parameters but said a software upgrade was needed.

[huskermcdoogle]

I have never seen a 16mb have G05.1.  I have only ever had HPCC G05 P10000 and advance preview control G08 P1 on that control.  IMHO 16mb way pre dates the dawn of modern aicc. Chances are G08 might be good enough for what you are wanting.  HPCC is a 5 digit upgrade for added hardware as you would have to add a risc board and a data server, and that doesn't include any tuning, so you wouldn't get anything from it unless you know how to tune the parameters for good results, or have fanuc do the tuning (no experience on this front).  

[honeybunches]

hmm.  I will need to learn a bit more.  The machine is a makino, known for being able to turn corners at speed.  Or at least the modern ones.  This one has some age being a 16 control.  

 

From memory, I seem to remember one of our Haas machined had 250 block/sec and could not see its own nose, and seemed like anything more over 100ipm was out of the question really.  But the rated max feed was only 200ipm or so.  The makino is rated over 600ipm so I might have to hope they have some tricks there?  Or do they maybe do this with shear servo power back in the day to force that machine to take a crappy path?  

I might need some clarification of HPCC, AICC, etc.  

 

To try and narrow our issues, assume we want to run a 1/2" cutter around a 4x4" part at 200ipm, with square or mostly square corners.  Slowing for a finish pass is fine, but when roughing, we just don't want the machine to ruin the part.  With a modern machine with look ahead, they will anticipate the velocity and vector change and slow the feed momentarily to within the mechanical limits of the machine.  This is why Makinos are rated to insane feed rates.  Not that it will really do that in small parts, but it will at least get to the max possible feed rate.  

 

Was look ahead even a thing on the 16?  

 

 

[huskermcdoogle]

34 minutes ago, honeybunches said:

Was look ahead even a thing on the 16?

Older generation than what we know today, but yes, defintely a thing.

If its a makino you stand a chance that it might have some look-ahead control options of some sort and decent tuning.

[Tim Johnson]

600 IPM (15m?) seems slow for a Makino. I saw a Leblond Makino going faster than that at IMTS in either 1992 or 1994.

[Newbeeee™]

For the 16 series controls, there's 3x parameters for servo tuning. Redneck styleeee...

I would program a pocket and trial. G05.1 should work - you may need the R value after it (R1 to R10 for fine to coarse). This is dependant upon your MTB on whether they have this implemented in the ladder.

For the actual parameters, see here for the 0i, but I think they are the same - consult your yellow book of wisdom!

http://www.practicalmachinist.com/vb/cnc-machining/fanuc-hsm-g08-g05-1-settings-171099/

[honeybunches]

Well, made a few calls today and just cannot seem to find out the real ability of the 16mb control.  I talked to Fanuc trying to learn what the block processing speed might look like.  I realize that can be a moving target but some bearing would be helpful.  

I guess I may be missing a complete manual explaining how the look ahead features work, if any can be simply turned on, or what hardware might be needed for an upgrade.  

It think it is just a large hassle to move a machine in only to find out it won't do what we need.  

 

Fanuc did say the 16 was the hotter of the control series in the 16/18/21.  Guess that is good news, but realize there is a big difference in back then and now.  

[Newbeeee™]

16 was very capable. If you power the thing up and enter G05.1Q1 in MDI, and it doesn't alarm, you have simple contour control. This will be at least 40 block lookahead and will do what you want providing you're prismatic style machining - ie contours with G2/G3. If you output G1's for arcs, you'll potentially choke it.

This is the prog format you need

• N0101 T1 M6
• M1
• ( 14MM DIA KNUCKLE ROUGHER - 56MM RELIEVED - 60MM OUT )
• ( FACE TOP + )
• G10G90L12P1R7.
• G05.1 Q1 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<THIS ACTIVATES AICC. YOU MAY NEED G05.1Q1R# (R1, TO R10)???
•  
• G54 G0 G17 G40 G49 G69 G80 G90 X77.798 Y64.3 S10000 M3
• T3 M8
• G43 Z10. H1
• Z1.
• G1 Z.1 F500.
• Y-50.3 F3500.
• G2 X65.829 R5.984
• G1 Y50.3
• G3 X53.86 R5.984
• 　
• 　
• 　
• G1 Y-50.3
• G2 X-53.86 R5.985
• G1 Y50.3
• G3 X-65.829 R5.985
• G1 Y-50.3
• G2 X-77.798 R5.985
• G1 Y64.3
• G0 Z10. M9
• G28 Z10. M19
• G05.1 Q0 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< THIS CANCELS
• G49 <<<<<<<<THIS IS NEEDED BUT MAYBE IN YOUR TOOLCHANGE MACRO. TOOL LENGTH CANCEL AND IS EITHER NEEDED HERE, OR IN YOUR TOOLCHANGE AS YOU CANNOT RECALL G05.1 UNLESS THIS HAS BEEN ACTIVATED AFTER CANCELLING (G05.1Q0)

[Leon82]

6 hours ago, newbeeee said:

16 was very capable. If you power the thing up and enter G05.1Q1 in MDI, and it doesn't alarm, you have simple contour control. This will be at least 40 block lookahead and will do what you want providing you're prismatic style machining - ie contours with G2/G3. If you output G1's for arcs, you'll potentially choke it.

This is the prog format you need

• N0101 T1 M6
• M1
• ( 14MM DIA KNUCKLE ROUGHER - 56MM RELIEVED - 60MM OUT )
• ( FACE TOP + )
• G10G90L12P1R7.
• G05.1 Q1 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<THIS ACTIVATES AICC. YOU MAY NEED G05.1Q1R# (R1, TO R10)???
•  
• G54 G0 G17 G40 G49 G69 G80 G90 X77.798 Y64.3 S10000 M3
• T3 M8
• G43 Z10. H1
• Z1.
• G1 Z.1 F500.
• Y-50.3 F3500.
• G2 X65.829 R5.984
• G1 Y50.3
• G3 X53.86 R5.984
• 　
• 　
• 　
• G1 Y-50.3
• G2 X-53.86 R5.985
• G1 Y50.3
• G3 X-65.829 R5.985
• G1 Y-50.3
• G2 X-77.798 R5.985
• G1 Y64.3
• G0 Z10. M9
• G28 Z10. M19
• G05.1 Q0 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< THIS CANCELS
• G49 <<<<<<<<THIS IS NEEDED BUT MAYBE IN YOUR TOOLCHANGE MACRO. TOOL LENGTH CANCEL AND IS EITHER NEEDED HERE, OR IN YOUR TOOLCHANGE AS YOU CANNOT RECALL G05.1 UNLESS THIS HAS BEEN ACTIVATED AFTER CANCELLING (G05.1Q0)

G49 above the g5.1q1

[honeybunches]

Thanks.  Don't have access to machine right now, but I do have the programming manual and there is nothing in it at all about G5 or G8.  Not as a standard or option.  I would think if there was any ability there at all, it would have made it in the book?  

Or is there any possibility there are some preset parameters that the MTB might have edited to make this more of an automatic function?  Sort of like the Haas HSM, you don't need to do anything to the code, the control  just looks at it and knows what to do.  

[Leon82]

2 hours ago, honeybunches said:

Thanks.  Don't have access to machine right now, but I do have the programming manual and there is nothing in it at all about G5 or G8.  Not as a standard or option.  I would think if there was any ability there at all, it would have made it in the book?  

Or is there any possibility there are some preset parameters that the MTB might have edited to make this more of an automatic function?  Sort of like the Haas HSM, you don't need to do anything to the code, the control  just looks at it and knows what to do.  

If the machine has it parameter 1604 bit 0 set to 1 will turn it on automatically.

On some machines you may need to shut it off for digit tapping.

[Newbeeee™]

6 hours ago, Leon82 said:

G49 above the g5.1q1

Not on a Robodrill with a 31iA5.

By memory it wouldn't toolchange without the G49 and it had to go where it is.

I then modded the post to standardise and this runs purfik on a 0iMC, 0iMD and 0iMF control

[Leon82]

1 hour ago, newbeeee said:

Not on a Robodrill with a 31iA5.

By memory it wouldn't toolchange without the G49 and it had to go where it is.

I then modded the post to standardise and this runs purfik on a 0iMC, 0iMD and 0iMF control

Yes on the robodrill you would need it above and then before you zero return g49 g53 z0 is what we use

[Newbeeee™]

1 hour ago, Leon82 said:

Yes on the robodrill you would need it above and then before you zero return g49 g53 z0 is what we use

Have you tried it above?

This program snippet would run in both our Robos by just removing the preselect toolcall adjacent to the M8. This program will run on the controls I listed above (the 0i range).

I'm sure it wouldn't run in the Robos with the G49 before the G05.1Q0 and had to be exactly where it is. This was trial and error etc and back about 6 years now, and the Robos were parted out 3 years ago but I'm sure I'm right in saying the format is this way because it had to be this way.

[Leon82]

26 minutes ago, newbeeee said:

Have you tried it above?

This program snippet would run in both our Robos by just removing the preselect toolcall adjacent to the M8. This program will run on the controls I listed above (the 0i range).

I'm sure it wouldn't run in the Robos with the G49 before the G05.1Q0 and had to be exactly where it is. This was trial and error etc and back about 6 years now, and the Robos were parted out 3 years ago but I'm sure I'm right in saying the format is this way because it had to be this way.

At my old place we stuck the 49 above the g28zo and it worked fine. Yes prestage would alarm out.

The 5.1q0 was always out after the last retract z before the g49.

I have also gotten alarms not using g49 before the g5.1 q1

 

Because your using g49 to home z in the robodrill is probably why you don't need it before turning it on

 

[Leon82]

We had the master cam guy write it into the post so it will come on on any path that is not a drilling cycle.

The matsuuras, we have the parameter set to come on automatically. Their IPC doesn't work unless the fanuc  one is on

[Colin Gilchrist]

For anyone looking into High Speed support for a 3X or 4X machine: MPMaster  (Mill 4X) has support for 4 different High Speed modes already built into the Misc Reals. You enable the different modes by setting MR2 to '1-4'. 'MR3' supports the R1-R10 values to change the precision.

All the logic to automatically turn the modes off for Drilling, and detect changes in the settings is already built in. So if you have 2 operations in a row, with the same Tool, Plane, and HSM settings, the Post will just keep the same mode active. However, if you change values, it will cancel the active mode, and output a the new settings. If the post detects a Plane change, it will cancel theactive mode  (before or after G49), cancel Tool Length Offset (G49), change the plane (rotate), re-activate G43 length comp, and turn onthe new HSM mode.

It is fairly sophisticated logic. You can modify the output formatting, but the architecture is all there for you.

[So not a Guru]

8 minutes ago, Colin Gilchrist said:

MPMaster  (Mill 4X) has support for 4 different High Speed modes already built into the Misc Reals.

+1

I have used this for many posts, sometimes it takes a little editing to get exactly what you need for a specific machine.

[honeybunches]

Dang it, sorry to drag up this old thread but we are reviewing this machine.  We did buy it and have in the shop and been too busy to mess with it much until now.  We are running tests on it and seems we really need some look ahead.  You can hear it get cranky.  Again, a 16MB control, and verified in the 9000 params HSM is not turned on, and neither of the two look ahead options.  Still a bit unclear on them but I am certain we do not have the RISC processor so if that totally terminates the use of G5, we will have to excuse that see if there are other options available?  Not sure if any parameter testing is going to require wiping out the memory or not?  

We have not tried a G5 or G8 in MDI but if it is not enabled in the parameters, it would not work, correct?  

We also have linear accel, not bell, and seemed that was preferred for HSM work?  Not really wishing to tune servos right now but since we don't have work on it yet, it seems to best time to figure out if we can get more from the machine.  

[honeybunches]

I was in error on this for some reason and should have checked the programming manual first.  The manual indicates G8 is standard for the machine.  No indication of what all it does but I am sure it will help.