Fanuc look ahead

[TheePres]

So, what bad things could happen if operator decides to delete all look ahead codes from a program?

[crazy^millman]

Nothing much just the possibility of scrapped parts is all. Not worried about making good parts then your good to go.

Upside programs run much faster. Downside faster you have the possibility of making scrap parts. Trying to program for mass and inertia can be done when using something like the NCSIMUL, CAMPLETE and Vericut tools, but with the correct look ahead settings no need you allow the machine to speed up and slow down where it needs. I do recommend tweaking these as needed per parts, but most people only run 5-10 parts and don't care. Running 1000 parts a year I will stand out there with a stop watch and dial programs down with the different settings. It has been a few blue moons since I needed to get that detailed on a project, but have done it. You can use different settings for different features on your parts. Semi for open areas, then 12st finish for smaller tight areas and then extreme settings for very tight tolerance very small areas. Why they offer the different settings to allow the programmer and the machinist the ability to dial them in as needed.

Give Jim a call and he can walk you them on your OKK machines.

[Leon82]

Is it formatted correctly? There needs to be a g49 before it.

You can also have it turn on automatically and then he can delete it all he wants.

 

 

[TheePres]

Thank You Ron,

I was looking for "back-up" on what i'm suspecting.

Part is scrap , all internal rad corners are oversize due to code being deleted and machine is overshooting all the arc movements.

But what I am also suspecting is that any parameters that pertain to the different "R" modes are not configured by OKK so regardless of what value i use it is defaulting to R0-R1.

[crazy^millman]

1 hour ago, TheePres said:

Thank You Ron,

I was looking for "back-up" on what i'm suspecting.

Part is scrap , all internal rad corners are oversize due to code being deleted and machine is overshooting all the arc movements.

But what I am also suspecting is that any parameters that pertain to the different "R" modes are not configured by OKK so regardless of what value i use it is defaulting to R0-R1.

That is easy to prove. Arc is an Arc and if you Vericut it and code is good then it is a accel/deccel issue not using the look ahead.

Need to make sure you are using the correct Nano codes. What options where purchased and what did the documentation say for using them list? Could be calling them wrong and not using them to their full potential.

[cncappsjames]

3 hours ago, TheePres said:

So, what bad things could happen if operator decides to delete all look ahead codes from a program?

ALL modern (mid-90's era and newer) CNC machines should be running some sort of look-ahead mode (G05, G05.1, G08, COMPCAD, etc...) on any sort of toolpath that is not a canned cycle. Period. End of story. There's always been varying opinions on this, however, the bottom line is of you want performance AND accuracy, you're running the correct High Speed Mode for the task at hand. If you're not, you're running slow, or you're running scrap.

There's only a few AE's that know anything about FANUC AICC tuning in SoCal. In all honesty, you're probably going to be talking to https://okkcorp.com/support/ in order to get any sort of high level support.

Just for curiosity's sake I was wondering how long we've been beating this high speed look-ahead horse, and it looks like since about 2004. That is a LONG time.

I know I've been training people to use the high speed modes installed on their machines since around 1997-ish. The fact we're STILL having this discussion does not show well for the Applications Engineers for their respective builders and dealers. When are we going to collectively get our customers adequately trained?

[crazy^millman]

1 hour ago, cncappsjames said:

ALL modern (mid-90's era and newer) CNC machines should be running some sort of look-ahead mode (G05, G05.1, G08, COMPCAD, etc...) on any sort of toolpath that is not a canned cycle. Period. End of story. There's always been varying opinions on this, however, the bottom line is of you want performance AND accuracy, you're running the correct High Speed Mode for the task at hand. If you're not, you're running slow, or you're running scrap.

There's only a few AE's that know anything about FANUC AICC tuning in SoCal. In all honesty, you're probably going to be talking to https://okkcorp.com/support/ in order to get any sort of high level support.

Just for curiosity's sake I was wondering how long we've been beating this high speed look-ahead horse, and it looks like since about 2004. That is a LONG time.

I know I've been training people to use the high speed modes installed on their machines since around 1997-ish. The fact we're STILL having this discussion does not show well for the Applications Engineers for their respective builders and dealers. When are we going to collectively get our customers adequately trained?

Right there with you why I have a job doing what I am doing.

[TheePres]

I'm curious though,  in your guy's opinion.  Should this fine tuning be performed by AE, or should it be done by machine builders??

 

[Leon82]

It depends on the controller and servo package. We have a feeler with an 18 control that will round corners unless you use exact stop along with aicc. The feelers with the 30 control run just fine. We even had a Makino that didn't have any sort of look ahead. We had to have the fanuc guy come down and add it.

[cncappsjames]

1 hour ago, TheePres said:

I'm curious though,  in your guy's opinion.  Should this fine tuning be performed by AE, or should it be done by machine builders??

That's not a simple X or Y answer because often, control options are installed in the field by either the Builder/Dealer and/or FANUC. Doesn't happen very often for us because we get them configured properly from the factory, then we change around 16 parameters that aid customer convenience and capability when we do training. I know how to do some servo tuning and have a basic working knowledge of FANUC Servo Guide though. I could get better at it and it's on my list of skills to be mastered. 

IMHO, an AE should know how to do it though because of your situation. It happens WAY too often IMHO. Builders could save themselves some grief if they handled it at the factory, but then again, I don't think builders should let improperly optioned machines out in the wild like they do on a regular basis. Some builders are worse than others. This totally unavoidable situation gives the control a bad name unfortunately when in all reality, it's 100% the builder.

We sell Matsuuras on the West Coast. Matsuura USA doesn't even import a machine without the correct option package installed. Why? Because it's just better that way. Is it more expensive? Perhaps. However, you factor in time wasted, perhaps some parts get scrapped, time and expense of field installing options, fine tuning options, time, energy, etc... you're way better off just doing it right from the get go. 

[cncappsjames]

3 hours ago, crazy^millman said:

Right there with you why I have a job doing what I am doing.

Same here.

[crazy^millman]

10 minutes ago, cncappsjames said:

That's not a simple X or Y answer because often, control options are installed in the field by either the Builder/Dealer and/or FANUC. Doesn't happen very often for us because we get them configured properly from the factory, then we change around 16 parameters that aid customer convenience and capability when we do training. I know how to do some servo tuning and have a basic working knowledge of FANUC Servo Guide though. I could get better at it and it's on my list of skills to be mastered. 

IMHO, an AE should know how to do it though because of your situation. It happens WAY too often IMHO. Builders could save themselves some grief if they handled it at the factory, but then again, I don't think builders should let improperly optioned machines out in the wild like they do on a regular basis. Some builders are worse than others. This totally unavoidable situation gives the control a bad name unfortunately when in all reality, it's 100% the builder.

We sell Matsuuras on the West Coast. Matsuura USA doesn't even import a machine without the correct option package installed. Why? Because it's just better that way. Is it more expensive? Perhaps. However, you factor in time wasted, perhaps some parts get scrapped, time and expense of field installing options, fine tuning options, time, energy, etc... you're way better off just doing it right from the get go. 

Pay me now or pay me later. Of the Builders Matsurra is one of the easiest machines to make a program for and get going from the start. We did have that one situation where the 5 axis Parameters needed adjustment, but put that one back on the customer. Cannot move the machine and not call your MTB to check it and then wonder why 5 axis surfaces are not lining up. Curtain AE (YOU!!!!) spotted that one tuned in the parameters and like Magic those bad programs I made were making good parts. Just crazy talk I tell you.

[cncappsjames]

I remember that situation. The programmer kept saying it was this, but really it was that. He was thinking 3-Axis realm, and I had to explain and prove that no, it's a 5-Axis realm thing and here's why...

Unfortunately, I don't think I was ever able to explain it to him in a way that made sense to him, but, the bottom line is it made good parts after the adjustment so... there is that.

Note to self; work on communication skills. 

[crazy^millman]

4 minutes ago, cncappsjames said:

I remember that situation. The programmer kept saying it was this, but really it was that. He was thinking 3-Axis realm, and I had to explain and prove that no, it's a 5-Axis realm thing and here's why...

Unfortunately, I don't think I was ever able to explain it to him in a way that made sense to him, but, the bottom line is it made good parts after the adjustment so... there is that.

Note to self; work on communication skills. 

The .003 mismatch they kept digging me on was the one issue i was referring to for that customer. I programmed it 5 different ways and kept getting that .003 mismatch. You had been explaining the other issues to them and this one came up. You took a look suspected something was a miss and then they fessed up moving the machine. You ran the Axis Check and then that .003 mismatch went away and they had a good part from the original program that was being called bad for weeks. You can never know how much I appreciate you finding that issue there were driving me crazy because CAMPlete and Mastercam didn't show it and I was running out of patience. Part of my new 5 Axis Test Part program is to Keller Half a Wall and then swarf the other half of the wall. If they don't line up with .0005" I tell a customer to reject the 5 Axis settings. This one test has saved me hours of issues. My AE friends love the test because now it shuts the customers up about the capabilities of the machine because it tests every thing you need to test on a 5 Axis machine. I also 5 Axis engrave the company name with a ball endmill dancing it on one of the faces. Several customers have made it part of their display pieces. 

[TheePres]

James, we need to clone you.  I know of a place that could really use your expertise in getting some machines dialed in.

[cncappsjames]

Thanks for the kind words.

[PAnderson]

11 hours ago, crazy^millman said:

The .003 mismatch they kept digging me on was the one issue i was referring to for that customer. I programmed it 5 different ways and kept getting that .003 mismatch. You had been explaining the other issues to them and this one came up. You took a look suspected something was a miss and then they fessed up moving the machine. You ran the Axis Check and then that .003 mismatch went away and they had a good part from the original program that was being called bad for weeks. You can never know how much I appreciate you finding that issue there were driving me crazy because CAMPlete and Mastercam didn't show it and I was running out of patience. Part of my new 5 Axis Test Part program is to Keller Half a Wall and then swarf the other half of the wall. If they don't line up with .0005" I tell a customer to reject the 5 Axis settings. This one test has saved me hours of issues. My AE friends love the test because now it shuts the customers up about the capabilities of the machine because it tests every thing you need to test on a 5 Axis machine. I also 5 Axis engrave the company name with a ball endmill dancing it on one of the faces. Several customers have made it part of their display pieces. 

I do 5 axis apps for Doosan. I admit I don't know as much as you two guys. After a few years, still learning. 40+ years doing major CNC machining, started 5 axis after joining Doosan. We bring our machines fully optioned but still struggle with the AICC parameters sometimes. Seems the factory has a few sets of parameters floating around in engineers pockets.

If a machine is moved, shouldn't it be checked for level (obvious) and squareness?(not so obvious to a lot of customers) before running kinematics checks? Resetting the kinematics with the table or Z axis out of square makes matters worse, no? Also, doesn't AICC on a 5 axis working properly depend on tuning the machine to the parts your doing to a lesser degree?

I'm an in-house apps guy. I don't get to travel to customers much unfortunately. That is mostly left to dealer apps guys, who by the way, are just learning 5 axis too. Not a good look for us sometimes. I end up teaching over the phone or email. Definitely not the best way but I do what I can.

Ron, can you explain this test you came up with? I understand if you want to keep it under wraps but I sure could use a good, quick test. Any help is appreciated.

 

regards,

Paul

[Leon82]

We use a block with holes.

Face the 5 sides of theblock so you know the cutter height is dead on. Then machine two holes 180 degrees apart. Then check from the top face and one x face.

 

There are also the simultaneous ball and indicator tests

[cncappsjames]

@PAnderson, if we want to get down to the nitty gritty, you are correct. Servo tuning  should take place for each different part run. Very impractical in the real world. In my experience, the AICC parameters are set so that a max weight scenario will produce a good part, or won't give you servo overload conditions. In all honesty, this is the safest approach.

As far as machine geometry... yeah. CRITICAL to check squareness, parallelism, perpendicularity, etc... BEFORE making any changes to the kinematic parameters. 

Renishaw has a probing package available; Axi-Set. It comes with a sphere mounted to a mag-base. The thing about it is you MUST run it while the machine and axes are at operating temp. If they are not, there could be mis-match issues.

There's definitely more than meets the eye when it comes to this stuff without a doubt. Not all customers appreciate the time that goes into integrating and developing all the systems (mechanical, software, options, etc...) to help them do complicated things more easily. But like you, we just do the best we can with what's available. 

[PAnderson]

18 minutes ago, cncappsjames said:

@PAnderson, if we want to get down to the nitty gritty, you are correct. Servo tuning  should take place for each different part run. Very impractical in the real world. In my experience, the AICC parameters are set so that a max weight scenario will produce a good part, or won't give you servo overload conditions. In all honesty, this is the safest approach.

As far as machine geometry... yeah. CRITICAL to check squareness, parallelism, perpendicularity, etc... BEFORE making any changes to the kinematic parameters. 

Renishaw has a probing package available; Axi-Set. It comes with a sphere mounted to a mag-base. The thing about it is you MUST run it while the machine and axes are at operating temp. If they are not, there could be mis-match issues.

There's definitely more than meets the eye when it comes to this stuff without a doubt. Not all customers appreciate the time that goes into integrating and developing all the systems (mechanical, software, options, etc...) to help them do complicated things more easily. But like you, we just do the best we can with what's available. 

Thanks James. I am aware of Axiset and used it. We don't hype it a lot because Doosan has their own built into the machine. Not as robust as Axiset but does work. I do tell people privately about Axiset because of it's greater reach with more robust capabilities like tracking machines and getting trend info for each machine. As you know, as soon as more money is mentioned, people generally shut down at that point.

[crazy^millman]

1 hour ago, PAnderson said:

I do 5 axis apps for Doosan. I admit I don't know as much as you two guys. After a few years, still learning. 40+ years doing major CNC machining, started 5 axis after joining Doosan. We bring our machines fully optioned but still struggle with the AICC parameters sometimes. Seems the factory has a few sets of parameters floating around in engineers pockets.

If a machine is moved, shouldn't it be checked for level (obvious) and squareness?(not so obvious to a lot of customers) before running kinematics checks? Resetting the kinematics with the table or Z axis out of square makes matters worse, no? Also, doesn't AICC on a 5 axis working properly depend on tuning the machine to the parts your doing to a lesser degree?

I'm an in-house apps guy. I don't get to travel to customers much unfortunately. That is mostly left to dealer apps guys, who by the way, are just learning 5 axis too. Not a good look for us sometimes. I end up teaching over the phone or email. Definitely not the best way but I do what I can.

Ron, can you explain this test you came up with? I understand if you want to keep it under wraps but I sure could use a good, quick test. Any help is appreciated.

 

regards,

Paul

Paul, On a limited Head-Head Vertical machine make a Pyramid and then 3 Axis Keller part of the Pyramid with a bull endmill. Then kick the head over to then bottom cut the other half of the surface. With a perfectly set machine there should be no difference between those 2 surfaces using the correct speeds and feed. Then to start working on parameters for speeds and feeds going fast and then faster and use that same part dropping the Z -.05 between each iteration of the cuts. Now people start to understand how mass and kinematics come into play. I will then drill, tap and thread mill cross intersecting holes this help to test G68.2 or G43.4 posting and codes. I also have a Circle, Diamond and Square shape for 3 Axis, then at 3+2 and then have a full 5 Axis CDS shape I cut. Full Travel 5 Axis machines Vertical or Horizontal the part I shared on CamInstructor has some of those features with others I didn't share. On full 5 Axis machines I cut the same surface 3 times. I keller(surface machine) with the bull endmill the top 1/3. I bottom cut the middle 1/3 and then swarf cut the last 1/3. This then teaches most places how to program part and think about them differently. Rinse repeat the step down and go faster then faster to help them again understand how all the different things needed to do correct 5 Axis motion come into play.

In some situations I am the last resort person called in so I have learned over the years what the role means. People are not happy and project is not where it should be. I need to come up pick up the pieces and repair the relationships as best I can. Not always able to and not fun when no matter how hard you worked to get working it still doesn't happen. They sting and not something I like to have happen, but I realized long ago I can only do so much.

22 minutes ago, PAnderson said:

 As you know, as soon as more money is mentioned, people generally shut down at that point.

People always tripping over $1000 bills to save that penny. Yes I know all about it.

[PAnderson]

34 minutes ago, crazy^millman said:

Paul, On a limited Head-Head Vertical machine make a Pyramid and then 3 Axis Keller part of the Pyramid with a bull endmill. Then kick the head over to then bottom cut the other half of the surface. With a perfectly set machine there should be no difference between those 2 surfaces using the correct speeds and feed. Then to start working on parameters for speeds and feeds going fast and then faster and use that same part dropping the Z -.05 between each iteration of the cuts. Now people start to understand how mass and kinematics come into play. I will then drill, tap and thread mill cross intersecting holes this help to test G68.2 or G43.4 posting and codes. I also have a Circle, Diamond and Square shape for 3 Axis, then at 3+2 and then have a full 5 Axis CDS shape I cut. Full Travel 5 Axis machines Vertical or Horizontal the part I shared on CamInstructor has some of those features with others I didn't share. On full 5 Axis machines I cut the same surface 3 times. I keller(surface machine) with the bull endmill the top 1/3. I bottom cut the middle 1/3 and then swarf cut the last 1/3. This then teaches most places how to program part and think about them differently. Rinse repeat the step down and go faster then faster to help them again understand how all the different things needed to do correct 5 Axis motion come into play.

In some situations I am the last resort person called in so I have learned over the years what the role means. People are not happy and project is not where it should be. I need to come up pick up the pieces and repair the relationships as best I can. Not always able to and not fun when no matter how hard you worked to get working it still doesn't happen. They sting and not something I like to have happen, but I realized long ago I can only do so much.

People always tripping over $1000 bills to save that penny. Yes I know all about it.

Thanks, just as I suspected. Wasn't sure what you meant by kellering. Haven't heard that term in 20 years or so.

Once in a while, we get a customer that is not happy with the speed (mostly) when AICC is turned on. There seem to be a million parameters that control Accell/Decel and the values to be used with R1 through R10. Can you tell me what the main ones are that influence G05.1?

We had a customer recently complaining about cycle time and they were comparing our DNM5700 (570MM Y Axis) against a Robodrill, for petes sake. Sometimes these still need adjusting because I know they don't always come from the factory set the best way. Any insight you can provide.?

Much obliged for this info Ron.

[cncappsjames]

1 hour ago, PAnderson said:

...As you know, as soon as more money is mentioned, people generally shut down at that point.

Especially in your market. On the high-end side of the business it's not quite as bad, but it's still there to a certain extent. Annnnnnnnnd no matter how good the probing packages are, they still won;t get you down to the single digit micron level. Probing is "almost" a static endeavor. I mean, sure the axes are moving under servo load, but all the dynamic things that go on during the metal removal process are not present (i.e. high velocity motion, dynamic cutting forces, spindle deflection, etc...) so it'll only get you so close. You've got to cut a part to get the rest of the way there. IMHO of course.

[cncappsjames]

@PAnderson we had a customer that wanted some reporting capability but didn't feel the need to get the Renishaw package as the Matsuura package was meeting his needs so we added this to the bottom of the check so he could so some tracking.

@Leon82, if you're running Matsuura's eZ-5, drop this in before your M30 after the cycle runs and you can get this report.

This would be for an A/C Kinematic VMC.

Make sure you have a device in your active I/O (i.e. USB, CF, etc...)

#900=[#870-#880]
#901=[#871-#881]
#902=[#872-#882]
#903=[#873-#883]
#905=[#875-#885]
POPEN
N700DPRNT[NOTE*ALL*UNITS*IN*MM*BELOW]
N800DPRNT[PARAMETER*19700*X*ERROR*IS*#900[13]]
N801DPRNT[PARAMETER*19701*Y*ERROR*IS*#901[13]]
N802DPRNT[PARAMETER*19702*Z*ERROR*IS*#902[13]]
N804DPRNT[PARAMETER*19704*1/2*OFFSET*Y*ERROR*IS*#904[13]]
N805DPRNT[PARAMETER*19705*1/2*OFFSET*Z*ERROR*IS*#905[13]]
N807DPRNT[*]
N9000DPRNT[CORRECTIONS*TO*MAKE*NOTED*BELOW]
N9002DPRNT[IF**A**ARGUMENT*IS*A1*THE*FOLLOWING*CHANGES*WILL*BE*MADE]
N19700DPRNT[PARAMETER*19700*WILL*BE*CHANGED*FROM*#880[33]]
DPRNT[*TO*#870[33]]
N19701DPRNT[PARAMETER*19701*WILL*BE*CHANGED*FROM*#881[33]]
DPRNT[*TO*#871[33]]
N19702DPRNT[PARAMETER*19702*WILL*BE*CHANGED*FROM*#882[33]]
DPRNT[*TO*#872[33]]
N19703DPRNT[PARAMETER*19703*NOT*APPLICABLE*TO*A/C*KINEMATIC*MACHINES]
N19704DPRNT[PARAMETER*19704*WILL*BE*CHANGED*FROM*#884[13]]
DPRNT[*TO*#874[33]]
N19705DPRNT[PARAMETER*19705*WILL*BE*CHANGED*FROM*#885[23]]
DPRNT[*TO*#875[33]]
PCLOS

M30

%

 

HTH

[crazy^millman]

2 hours ago, PAnderson said:

Thanks, just as I suspected. Wasn't sure what you meant by kellering. Haven't heard that term in 20 years or so.

Once in a while, we get a customer that is not happy with the speed (mostly) when AICC is turned on. There seem to be a million parameters that control Accell/Decel and the values to be used with R1 through R10. Can you tell me what the main ones are that influence G05.1?

We had a customer recently complaining about cycle time and they were comparing our DNM5700 (570MM Y Axis) against a Robodrill, for petes sake. Sometimes these still need adjusting because I know they don't always come from the factory set the best way. Any insight you can provide.?

Much obliged for this info Ron.

Some customers are never happy. Can be the best program in the world and still complaining. Heard compliant after complaint about a project as it was running. Not efficient I didn't take the age of the machine and how slow it is into account and other things. Then we get the finishing stage and over almost 50" part is within .002" top to bottom. Other places no worse that .0016. Similar easier and smaller part they were seeing as much as .03" deviation. I have to break out the book on what specific parameters effect what. Do you have the Fanuc 5 Axis Help PDF from Europe? There is also a Power Point I found that has good information on this.

Here is a link to both and I offer them freely and make no claim about the authenticity or accuracy of information. In other words use at your own risk.

Fanuc 5 Axis Machining PP

Fanuc 5 Axis Help