G05 vs G08 on Fanuc

[g huns]

Can anyone tell me what the difference is between these two? The books description is lacking and I don't see a big difference when the machine is running.

[?Mark]

From what I know G5 will turn on hpcc mode (high precision contour control) and you need a RISC processor for this ($$$ ).

 

G8 is a look ahead

 

hth

 

Mark

[g huns]

I have HPPC, worth every penny. Just wondering what it does that G08 doesn't. Other than drilling, I use it all the time. Just thinking of using G08 for some roughing, but the program looks like it's running about the same whether I use G08 or G05.

[Guest CNC Apps Guy 1]

You won't se a big difference unless you're running Complex 3D stuff. Then the diference is visible.

 

HPCC (Last time I checked) had a 2ms BPT (Block Processing Time)

 

Look ahead was around 8ms.

 

HTH

[?Mark]

quote:

---

Just wondering what it does that G08 doesn't

---

MUCH faster procesing speed=faster feed rates=more acurate toolpath

 

James, Psychomill and many others can give you much more detail about it

 

hth

 

Mark

[?Mark]

There he is

[DavidB]

G05 P10000 Turns on HPCC or on a Makino they call it SGI.

G05 P0 Turns this function off.

Use this function when doing 3D toolpaths.

 

The G05 P10000 must be called after The Tool length offset is registered.

G01 G43 H.. Z... F...

G05 P10000 (on)

And cancelled before sending the machine home in Z.

G05 P0 (off)

G91 G00 G28 Z0.

 

HTH

[Lars Christensen]

There are a list of parameters that controls G5, you migh have ajust those. Our Horizontal almost made cardwheels thru the shop, when I turned it on on some small detail stuff.

[Psychomill]

Coming in late on this one... ( had an operator do a major "oops" and have been wrenching on machines all week) ..... anyway....

 

James and David are right on. As well as Lars about parameters. I don't recall the exact difference in seek time and block read (or look ahead) but its something along the lines as described.

 

3D (as mentioned) will see a big difference. In normal 2D stuff, you won't see a big difference until you really start pushing feedrates. G8 on many machines will have certain limits set, from there G5 can take over. For example: In G8, a machine may not be able to process (or is limited to) feedrates under 900 or 1000 IPM. Beyond that you would need the G5 option. Now in most cases, G8 won't sustain accuracy to within preset limits beyond 600 or maybe 700 IPM if you're lucky. I roughing, this may not be a problem. You can however tweak the servos to increase this window. But I would only do this if you were ABSOLUTELY comfortable at this. You can easily "lose" your machine if you make a few wrong adjustments and your 'slower' feed stuff as well as accuracy in finishing will sacrifice.

 

Lars' comment is an example of poor parameter settings (unless the machine ain't bolted down). I've had machines in G8 that shook at the head so bad, like a jack hammer on steroids, that I thought it was gonna flip like a turtle. Obviously made adjustments to that one..

 

[jeff]

I run a fanuc 18i, and sometimes when I use G08P1 at slower feedrates,the machine gets a bit jerky when it switches directions,I don't run6-700 ipm, not even close, but sometimes when I run a program that switches feeds from <200ipm to around 40ipm or so it gets jerky.

Is this normal?

Do I not need G08 when going <200ipm?

[?Mark]

quote:

---

the machine gets a bit jerky when it switches directions

---

Jeff, it's normal.

We talked about it a couple years ago with Psychomill and others.

G8P1 makes machine "not cut corners" for lack of better description (at this hour... )

What might help is turning it on for feedrates and turning it off for rapid moves.

Other than that, "bolt the machine down"...

I think that was Psychomil's response to my similar concern at the time

 

hth

[Lars Christensen]

AND if you do use G5 make sure that you turn it of before any drill cycle!!!!

[g huns]

Started messing around with parameters a little today. Looks like parameter 8410 is the magic #.

 

"Allowable velocity difference in velocity determinination considering the velocity difference at corners"

 

I don't know what that means, but it makes her run like hell. I was also set for linear acceleration instead of bell-shaped. Finish isn't quite as good, but size stays the same, cut time is 2/3 faster and machine moves smooth a glass. Thanks for all the suggestions.

 

Hey John, wanna race?

[Psychomill]

quote:

---

I don't know what that means,

---

LOL!!!! Sounds like you're beginning to pick up a little "Janglish" or "Jenglish" (Japanese version of English). It only gets better.... Yeah right

 

Anyway, as I said, be real careful with the parameters. You can tighten up the bell too much (where its similar to linear) or loosen it too much where either way, undesirable results. Back up your parameters and make suttle changes until you're familar with the parameter controls. And with each change, back them up as a different file until you're through. Another tip is to run the machine for a while after a change before making another change. This way, in the "in between time", you can run normal part programs and make sure that what you've changed doesn't cause a mishap/problem with some other stuff during machining.

 

Once you're familar with it and have enough time behind you doing this, then you'll have a general idea for setting a "default" set to adjust other machines from. But never assume anything. Even if the models are the same. I've had them where the servos were tuned so differently (same machines, same model etc.) that a "default" didn't quite work the way I wanted.

 

good luck and let the chips fly!!

[cncappsjames]

On 1/24/2006 at 11:35 PM, Lars Christensen said:

AND if you do use G5 make sure that you turn it of before any drill cycle!!!!

Updated for 30i Series Controls on a Matsuura 5-Axis Machine w/ FANUC 31i-B5 Control (date of test 12/1/2023)
Test - mix of  G81, G83, and G84 cycles

(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 specific to Matsuura machines and assigns acc/dec values to the appropriate parameters. The D is used for positioning type cutting as opposed to contouring type cutting. So we can definitively say that it IS indeed faster to run your canned cycles with at least FANUC's G05.1Q1 mode active.

Hopefully we can finally put that myth to bed.

 

[SuperHoneyBadger]

On 2/23/2024 at 6:42 PM, cncappsjames said:

The D is used for positioning type cutting as opposed to contouring type cutting.

So drilling and reaming can leverage hi-speed? I have all my posts (31i - VX660's) configured to not output G131's on canned drill cycles, I thought it was a no-no?

[cncappsjames]

On 2/26/2024 at 7:11 AM, SuperHoneyBadger said:

So drilling and reaming can leverage hi-speed? I have all my posts (31i - VX660's) configured to not output G131's on canned drill cycles, I thought it was a no-no?

Yes you can. It is kind of an Urban Legend that you can't or shouldn't. I have been doing it for years. On a Matsuura we don't have any trouble rigid tapping with the mode(s) active. For other manufacturers I would consult their Applications Engineers for guidance.

[cncappsjames]

The opinion probably came from the early days (pre- [b]i[/b] Series Controls) when because the function was called "look ahead" and there were not any levels attached to it. It was either on or off. So, it was thought there was no benefit to a "look ahead" for positioning type tool-paths because it was just going from A to B and it wasn't performing any contouring type motion. But with modes and levels, you gain some functions.

[SuperHoneyBadger]

Thanks for the info! Added the D to my hi speed post block and we'll try it out.

Saved ~30 sec on a high volume job with M203's recently, we'll see if there are savings for us with the D1 positioning (decent # of holes across 4 offsets). Maybe we can get another cycle for the shift since the run time is only 10 minutes or so. Always another trick to learn! Thanks again!

[cncappsjames]

What's the manufacture date of your machine @SuperHoneyBadger?

[SuperHoneyBadger]

35 minutes ago, cncappsjames said:

manufacture date of your machine

One is 2018/09

The other 2019/02

[cncappsjames]

Ok, you're probably up to date on code formatting. Touch panel machines built after 12/21 can do multiple non overlapping m-codes on the same line, and have a few other pretty awesome functions. Depending on a number of programming paths, plane changes and canned cycles, I've seen 20% reduction in cycle time old vs. new. Sometimes more.

Matsuura does have a software update available for the 5-Axis machines built prior to that date. It's not free - I have absolutely no idea of the cost so don;t ask. I don;t even know the ballpark number unfortunately. I do know FANUC and the Matsuura factory needs to get involved which is why it costs. Me, I'm trained to do the Matsuura side software update (I believe I'm the only non-factory guy in the US that can do it) but FANUC needs to come out and update the CNC System Series and Edition software. See below for the machine's requirements top be eligible for an update.

In order for any 5-Axis Matsuura to receive this update it must have the following;

1. FANUC-31i-B5 Control

2. Panel-i or iHMI interface

3. FANUC System Software Series G423 or greater

4. FANUC System Software Edition 49.0 or greater

5. Software from Matsuura

6. Software installation from Matsuura (or a factory trained engineer).

 

              If items 1 or 2 are not true, then the machine cannot get the update period.

              If items 3 and 4 are not true, the machine dealer must issue a request to Matsuura USA, Matsuura USA must issue the request to FANUC to update the System Software to the minimum required for the update and Matsuura USA must issue the software request to Matsuura Japan. There would be a charge for the FANUC trip, how much depends on location; the 3 tiers for travel are less Than 4 hours, 4-8 hours, and 8-12 hours. Not sure what Matsuura is charging for the updates. Probably depends on proximity to Minneapolis, Minnesota.

[crazy^millman]

13 hours ago, cncappsjames said:

Ok, you're probably up to date on code formatting. Touch panel machines built after 12/21 can do multiple non overlapping m-codes on the same line, and have a few other pretty awesome functions. Depending on a number of programming paths, plane changes and canned cycles, I've seen 20% reduction in cycle time old vs. new. Sometimes more.

 

This one statement here is enough to drive me crazy with some customers. Customer has 7 Makino T1 machines and they range in age and I can tell the difference in the control, but they cannot and I tell them a statement like this and get the deer in the head light looks.

[SuperHoneyBadger]

15 hours ago, cncappsjames said:

multiple non overlapping m-codes on the same line,

So, start coolant, start spindle, unlock rotary could all activate on a single line and would happen simultaneously?

I'll have to try it and get out the stopwatch

[cncappsjames]

5 minutes ago, SuperHoneyBadger said:

So, start coolant, start spindle, unlock rotary could all activate on a single line and would happen simultaneously?

I'll have to try it and get out the stopwatch

M203 M08 M132 can all be in the same line.

This would ONLY apply to 5-Axis Matsuura machines WITH touch panels AND built after 12/2021.