Using G41.2

[Colin Gilchrist]

29 minutes ago, JB7280 said:

interesting, I don't think I've seen either of those first 2.  Where would something like an Okuma Multus fall?  Would that be Head/Table?

Yes, because one rotary is on the "Tool Side" (B-Axis Head), and the other rotary is used to "rotate the workpiece".

 

Here is an example of a Head/Head style machine:

https://www.cncpd.com/dms-5-axis-large-format-gantry-cnc-machine/

[Guest]

44 minutes ago, Colin Gilchrist said:

Yes, because one rotary is on the "Tool Side" (B-Axis Head), and the other rotary is used to "rotate the workpiece".

 

Here is an example of a Head/Head style machine:

https://www.cncpd.com/dms-5-axis-large-format-gantry-cnc-machine/

We have their 3 axis machines at work, they are okay, I wish they had a fanuc control

[crazy^millman]

Here is one I like that is a Head/Head.  https://www.fooke-portalfraesmaschinen.de/en/fraesmaschinen/langbett-portalfraesmaschine-endurar-pro-linear

 

or this one. https://www.fooke-portalfraesmaschinen.de/en/fraesmaschinen/kompakt-portalfraesmaschine-endurar-700linear

 

[motor-vater]

Our old post did stuff like that, but our New Postability post gives us this

N284
T284 M6
(T284 0.138 10-24 TREADMILL CARMEX MTS0250C42 24 UN)
(THREAD 1/4-20 HOLES)
(OPERATION NO - 20)
(OPERATION TYPE - THREADMILL)
G54
G08 P1
G90 G00 B0. C0.
S5536 M03
G43.4 H284 X-8.4788 Y.6615 Z9.0249
M8
Z7.1249
G01 G42.2 D284 Z7.0603 F16.61
Y.6695
X-8.4928 Y.6615
X-8.4941 Y.6646 Z7.0593
X-8.4948 Y.6679 Z7.0582
Y.6712 Z7.0572
X-8.4941 Y.6745 Z7.0561
X-8.4927 Y.6776 Z7.0551
X-8.4907 Y.6803 Z7.0541
X-8.4882 Y.6825 Z7.053

 

Which works fine in the Mori's, that being said I hate 5 axis thread milling because of the linearization of the code. It just starts to get bulky, So depending on the situation I would just asoon use a plane and then treadmill in 3+2. But to answer your original question our post with Mcam 2021 outputs a D value

[cncappsjames]

G08 P1?

That's the lowest level of Look-Ahead available on a FANUC. I think 8 blocks...

[huskermcdoogle]

6 minutes ago, cncappsjames said:

That's the lowest level of Look-Ahead available on a FANUC. I think 8 blocks...

Nothing like cheaping out on control options, or not using what you might have under the hood.  It's even worse when you have an option installed where the MTB spec'd it as standard, that should be implemented as it would save on maintenance, and they don't have anything configured nor know how to configure it......

 

[cncappsjames]

I kind of chuckle to myself when we are competing against other brands and they are whatever less... it's really irrelevant because at the end of the the day it's less. 

It's less technical expertise on the applications side to ADEQUATELY train your staff..

It's less machine capability...

It's it's less machine functionality...

It's just less everything. It's stepping over dollars to pick up pennies. 

[megaman]

On 2/24/2021 at 9:36 AM, Colin Gilchrist said:

You can set the Geometry Size to 0.0000, using a G10 line, or using Macro Variable Formulas in the NC  Code. Just wanted to point out that there is a method available to make sure the Operator doesn't miss making the change. In fact, you could 'save the current Geometry Size in a Common Variable, reset the Size to 0., and then restore the Size when the Operation is finished', all by using Macro Variable Formulas.

In fact, if you want to adopt Wear Comp as a standard, you could make your Post output G10 Lines in the header, to clear out all the Geometry Size values, to avoid the issue of an Operator forgetting to clear those values.

I have never been a fan of Full Control Compensation, and feel like any shop who still uses it as a standard, is basically still living in the dark ages. No offense intended...

Hi Colin,

I am looking through the manuals to try to figure out the G10 line I would need to writ into the code to be able to do this.  Right now we are using the Control comp and both Mazatrol and EIA read the Actual diameter to adjust the amount of compensation. Typically if we have a 1/2" endmill  and  the hole is  .003 small we will have the Actual diameter at .497 as an example.  Actual diameter compensation also can adjust this but can be missed easily by the operators since that is down near the bottom of the page of blanks.

Can you give me an example how I can use a G10 line or macro to either include in the post or macro that i can somehow add either manually or thru Mastercam to output to get around not having to go through retraining all the operators to input the correct data. 

I find the information in the manual somewhat confusing on which parameters to change and if we would still be able to think in terms of diameter and not going back to a radial  offset mindset.

Any insight or clarification would be greatly appreciated!

[Colin Gilchrist]

48 minutes ago, megaman said:

Hi Colin,

I am looking through the manuals to try to figure out the G10 line I would need to writ into the code to be able to do this.  Right now we are using the Control comp and both Mazatrol and EIA read the Actual diameter to adjust the amount of compensation. Typically if we have a 1/2" endmill  and  the hole is  .003 small we will have the Actual diameter at .497 as an example.  Actual diameter compensation also can adjust this but can be missed easily by the operators since that is down near the bottom of the page of blanks.

Can you give me an example how I can use a G10 line or macro to either include in the post or macro that i can somehow add either manually or thru Mastercam to output to get around not having to go through retraining all the operators to input the correct data. 

I find the information in the manual somewhat confusing on which parameters to change and if we would still be able to think in terms of diameter and not going back to a radial  offset mindset.

Any insight or clarification would be greatly appreciated!

I would love to help you figure this issue out; however I don't have access to any of the Parameter Information I would need to get this working on a Mazak. The Control itself would need to be configured through Parameters, to make sure you're entering the data in the correct place.

I'm happy to provide some G10 sample code, but I can't guarantee that it would work correctly on your Mazak. This code is for a Fanuc 31i-B5 Control, so while it can serve as a good example of "how to do it on a Fanuc", you'll still need to consult with Mazak AE's to be sure the Parameters are set correctly.

(CLEAR TOOL RADIUS GEOMETRY OFFSET REGISTERS)
G10
L12P1R0.
L12P2R0.
L12P3R0.
L12P4R0.
L12P5R0.
L12P6R0.
L12P7R0.
L12P8R0.
L12P9R0.
L12P10R0.
G11

(SET TOOL RADIUS WEAR OFFSET REGISTERS HERE!)
G10
L13P1R0.0014
L13P2R0.
L13P3R-0.0004
L13P4R0.0001
L13P5R0.0008
L13P6R-0.0003
L13P7R0.
L13P8R0.0024
L13P9R0.
L13P10R0.0004
G11

L10= Geometry Length Register

L11= Wear Length Register

L12= Radius Geometry Register

L13= Radius Wear Register

P_ = The Offset Number you want to change. (Typically 1-200, but can be more, depending on your # of Offset Registers purchased.)

R_ = The "Register Value", either in terms of "Geometry (L12)" or in terms of "Wear (L13)" values. [Use 'R0.' to clear any of the offset values.]

Please keep this in mind:

• If you choose to control the offset value (load into the control), the Operator must make any "adjustments" in this G10 List, as it will always OVERWRITE the Registers, when the Program is restarted from the beginning.
• NOTE: You can certainly put a G10/G11 line, just prior to, or just after, a Tool Change (Operation). The advantage here, would be that you can "overwrite an offset value, with a new value for a given operation, on-the-fly". So you could use R0. for the initial wear offset, then use G10L13P1R-0.002 for OP1, and then use G10L13P1R0. for OP2, to clear out that wear offset value for the next cut. This can be done to adjust any cut within the program, but the Operator must be informed that G10 is in use, and they (or you) must edit the NC Code, so that the Wear Offset value is set properly, at the correct position within the NC Code.

 

 

 

[motor-vater]

On 2/25/2021 at 6:52 PM, cncappsjames said:

G08 P1?

That's the lowest level of Look-Ahead available on a FANUC. I think 8 blocks...

Just ripped out a quick path for the OP to show him an example of the D value. I never 5 axis threadmill so all of my defaults have not been set or saved for that path. The post lets me set look ahead to what ever I want/need in misc values

 

I honestly can not tell if you guys are bashing me over this or if I am truly missing something. If I am missing something Please help me out..

[huskermcdoogle]

12 hours ago, motor-vater said:

If I am missing something Please help me out..

I think that was just a comment based on seeing what we saw, and commenting around a generality in the MTB world where they don't train or setup their customers to their best potential right from the get go.

If that was just a simple sample program that you generated and not what you actually use day to day, disregard.  But on a serious note set your misc int/real defaults to a value that gets you the output you normally use, IIRC that's done in the control def, I don't think kit can be done in the op defaults but I may be wrong.  I'm so guilty of not having these setup properly, like ALL THE TIME.  But then again, I am hardly ever on the same machine twice inside the same year...

[motor-vater]

11 hours ago, huskermcdoogle said:

I think that was just a comment based on seeing what we saw, and commenting around a generality in the MTB world where they don't train or setup their customers to their best potential right from the get go.

If that was just a simple sample program that you generated and not what you actually use day to day, disregard.  But on a serious note set your misc int/real defaults to a value that gets you the output you normally use, IIRC that's done in the control def, I don't think kit can be done in the op defaults but I may be wrong.  I'm so guilty of not having these setup properly, like ALL THE TIME.  But then again, I am hardly ever on the same machine twice inside the same year...

What Look ahead and values do you recommend? I have been using G05.1 R5 for most tests code thrown at the machine, Our original post was set up to output G05 P10000 and that is all it output, the new postability post gives me options, the Mori book is surprisingly vague on which look ahead work best  in any given situation. The big yellow book gives me the same kind of headache, I have only been using the new post on one machine so far, because we had to modify a few parameters related to G43.4... parameter 19754.5 mainly. Originally the machine had to return to B0, C0 in-between 5 axis moves, So I am playing with the new post with one machine designated as my test mule. I understand the precision differences in the look ahead and what they can do for me, but still trying to seek information regarding G05 vs. G08 vs. G05.1. Any help with that would be appreciated.

 

I do hate to thread Jack here, or break up a good Chuckle at my expense but in all honesty sometimes I feel like the Mori guys that are out here on the regular know less about these machines than I do and that scares the hell out of me. If this is a learning opportunity I'm all to happy to swallow my pride and ask for some help.

 

What is MTB world? I've been on here for a decade and I'm starting to see lingo I don't know. Do we have a secret language now like Wall Street Bets? LOL

[Colin Gilchrist]

3 minutes ago, motor-vater said:

What Look ahead and values do you recommend? Our original post was set up to output G05 P10000 and that is all it output, the new postability post gives me options, the Mori book is surprisingly vague on which look ahead work best  in any given situation. The big yellow book gives me the same kind of headache, I have only been using the new post on one machine so far, because we had to modify a few parameters related to G43.4... parameter 19754.5 mainly. Originally the machine had to return to B0, C0 in-between 5 axis moves, So I am playing with the new post with one machine designated as my test mule. I understand the precision differences in the look ahead and what they can do for me, but still trying to seek information regarding G05 vs. G08 vs. G05.1. Any help with that would be appreciated.

 

I do hate to thread Jack here, or break up a good Chuckle at my expense but in all honesty sometimes I feel like the Mori guys that are out here on the regular know less about these machines than I do and that scares the hell out of me. If this is a learning opportunity I'm all to happy to swallow my pride and ask for some help.

 

What is MTB world? I've been on here for a decade and I'm starting to see lingo I don't know. Do we have a secret language now like Wall Street Bets? LOL

Hi Pete,

MTB stands for Machine Tool Builder.

Several of us now work for MTBs, including James, Mark, and me.

[motor-vater]

1 minute ago, Colin Gilchrist said:

Hi Pete,

MTB stands for Machine Tool Builder.

Several of us now work for MTBs, including James, Mark, and me.

Oh that makes since, Then Yes I agree, Our MTB has done very little to set us up for success... The more I learn The more I despise Fanuc aswell, in General. I feel like the boss goes on the hook for these Million dollar machine centers, You get no help from the MTB, Very Little help from the sales People, and reduced functionality from the Fanuc People.

[cncappsjames]

1 hour ago, motor-vater said:

Oh that makes since, Then Yes I agree, Our MTB has done very little to set us up for success... The more I learn The more I despise Fanuc aswell, in General. I feel like the boss goes on the hook for these Million dollar machine centers, You get no help from the MTB, Very Little help from the sales People, and reduced functionality from the Fanuc People.

... and that is precisely why a machine tool purchase is a VERY important decision. It's sales, it's service, it's applications assistance, it's training, etc... 

Somebody could spend a billion dollars on a machine, but if they bought it from some guy that works out of the trunk of his car with no support behind him you are not going to get all you should. 

As a FANUC guy, I try to go out of my way to make sure our customers get the very most out of their machines. Sometimes I get pushback from the end users because "we've always done it that way", that's a hard situation. I just put the information out there, it's up to the end user to implement it.

[cncappsjames]

On 3/16/2021 at 5:28 AM, motor-vater said:

I honestly can not tell if you guys are bashing me over this or if I am truly missing something. If I am missing something Please help me out..

Not bashing you at all... just lamenting the option you were given for your machine.

[crazy^millman]

8 hours ago, Colin Gilchrist said:

Hi Pete,

MTB stands for Machine Tool Builder.

Several of us now work for MTBs, including James, Mark, and me.

Paul does also.

I work with many MTB's not just one.

[huskermcdoogle]

9 hours ago, motor-vater said:

I feel like the Mori guys that are out here on the regular know less about these machines than I do and that scares the hell out of me.

Well unfortunately, they only know what they knew when they hired in, or what some guy they had working for them decided to educate them on. I'm not aware of much for formal training out there that isn't just bare bones basics of the machines.  When it comes to advanced features, the only way the AE's learn about them is if they get a project that they need to use those features on.  Which in lay the problem, who knew to spec that option in the first place unless it was standard on the machine in the first place.......

As for what mode to run your machine in.  You will either have to do some testing, or see if you can get a hold of a Mori Apps engineer and see if they can get you some Mori specific documentation on the option.  I would guess you would want to use G05.1 Q1 R#, but you might also have other options like nano-smoothing which would add another wrinkle into things but would be well worth using in many cases.  James would be the pro around here with those options.  However Matsuura has custom codes to turn all that on and off such that it is done properly and in the right order, fully utilizing the capability of the control and machine.  IIRC/IMHO, Matsuura is the only builder using Fanuc controls that does this particularly well and consistently across their product line.  I'm guessing if it isn't happening already the other builders are starting to catch up on this, but I haven't been on a new machine in a while so I wouldn't know firsthand.

[crazy^millman]

15 hours ago, huskermcdoogle said:

Well unfortunately, they only know what they knew when they hired in, or what some guy they had working for them decided to educate them on. I'm not aware of much for formal training out there that isn't just bare bones basics of the machines.  When it comes to advanced features, the only way the AE's learn about them is if they get a project that they need to use those features on.  Which in lay the problem, who knew to spec that option in the first place unless it was standard on the machine in the first place.......

As for what mode to run your machine in.  You will either have to do some testing, or see if you can get a hold of a Mori Apps engineer and see if they can get you some Mori specific documentation on the option.  I would guess you would want to use G05.1 Q1 R#, but you might also have other options like nano-smoothing which would add another wrinkle into things but would be well worth using in many cases.  James would be the pro around here with those options.  However Matsuura has custom codes to turn all that on and off such that it is done properly and in the right order, fully utilizing the capability of the control and machine.  IIRC/IMHO, Matsuura is the only builder using Fanuc controls that does this particularly well and consistently across their product line.  I'm guessing if it isn't happening already the other builders are starting to catch up on this, but I haven't been on a new machine in a while so I wouldn't know firsthand.

Cough, Cough, Cough, ,

,

,

,

,

,

,

NO some are not doing it well!!!!

[huskermcdoogle]

14 hours ago, crazy^millman said:

Cough, Cough, Cough, ,

,

,

,

,

,

,

NO!!!!

Well, out with it!  Don't let my perceptions muddy the waters if it isn't actually what is happening out there. 

[crazy^millman]

23 minutes ago, huskermcdoogle said:

Well, out with it!  Don't let my perceptions muddy the waters if it isn't actually what is happening out there. 

That better?

[cncappsjames]

Some MTB's/Dealers do a good job on the options.  Others, not so much. There are two "basic" problems in play 1a) Price point  and 1b) Knowledge/Experience of the factors in play.

[Leon82]

We bought a Makino ps95. It didn't even have aicc. Fanuc came down after we bought it afterwards and we bought the option. The professional p control seems nice but it's basically an oi control. Terrible blends even with large lead in radii and overlap. 

 

Z axis creeps up as it warms. Machining blades you're dropping z while it's creeping up. Every time you drop zee an extra .0001 it bites you. 

 

It ruined Makino for our company and we'll probably never buy another one.

[cncappsjames]

On 3/18/2021 at 3:42 PM, Leon82 said:

We bought a Makino ps95. It didn't even have aicc.

Ooooooof. 

Wow. At that point it's not even a matter of just buying the option. It's gotta be tuned. Usually Makino doesn't do that stuff. I'm REALLY surprised.