Start Everywhere in the program.

[Hugidugi]

Hi, I'm actually working on a 6axis cnc milling support by Heidenhain (TNC 430) Correa and it's a 25 years old milling so my boss is looking for remplace it. One option I like from the tnc 430 by heidenhain is that I can start the program from everywhere I would... so for exemple if I have to make 3 holes with a drill and I would skip a line to skip the second hole I only have to put it in singleblock, call the line I would and press start.
My boss is looking for probably buy a Hurco milling and I wonder if someone know how this feature is call and if hurco make that option because I found this really helpful. I know Fanuc doesn't do it and you have to start only with a toolchange.
Thanks

- Hugo

 

[couch]

This is a pretty common feature on most machines. Haas and Brother both do this easily.

 

[beege]

I'm pretty sure FANUC does this, too, but it's a purchased $$$ option.

 

[sinha]

If the machine does not have this feature, GOTO statement can be inserted in the program for skipping a few blocks.

 

[CAMasochism]

If the machine does not have this feature, GOTO statement can be inserted in the program for skipping a few blocks.

Yea, that's what we have to do with our Mazaks. Mazak likes to tout all the features and fancy things that their machines can do, but the moment you mention that you will be running in EIA mode (because who the hell is going to be programming complex 5-6 axis parts on conversational control when you have a programming department) they turn sour faced because they know 70% of those features no longer apply.

 

[CNC Hacker]

Yea, that's what we have to do with our Mazaks. Mazak likes to tout all the features and fancy things that their machines can do, but the moment you mention that you will be running in EIA mode (because who the hell is going to be programming complex 5-6 axis parts on conversational control when you have a programming department) they turn sour faced because they know 70% of those features no longer apply.

How old are your machines? There are multiple ways to do this in EIA programs without resorting to GOTO statements. Both with modal and non-modal restarts.

 

[TeachMePlease]

Yea, that's what we have to do with our Mazaks. Mazak likes to tout all the features and fancy things that their machines can do, but the moment you mention that you will be running in EIA mode (because who the hell is going to be programming complex 5-6 axis parts on conversational control when you have a programming department) they turn sour faced because they know 70% of those features no longer apply.

Sounds like some of the guys that are super Mazak programmers that I've met

 

[gustafson]

I know my Brother will restart wherever I want,but it goes and grabs the previous tool and moves to the last location that tool was and pauses. Smart but annoying, the Heidenhain will just run from wherever you are, consequences be damned.

Heidenhain really, really, lets you play fast and loose, and it is difficult to get used to the rigidity of a G code control after years of being able to do whatever you please.

 

[sneebot]

I'm pretty sure FANUC does this, too, but it's a purchased $$$ option.

Fanuc Oi-MD will do this, don't believe it was an option. But it takes way to many steps that are somewhat convoluted,
and being Fanuc, completely non-intuitive.

 

[Turbowerks]

I’ve don it on my fanuc but i try not to been bit a couple times


When I find it I don’t need it
When I need it I can’t find it!

 

[SeymourDumore]

Haas will do this straight outta the gate.
It will read the entire program to make sure that all the correct modal codes are active, speeds, feeds, coolant or whatever else.
No need to go to a specific block number, and if the correct tool is in the spindle it won't even make a safety toolchange as long as you're starting on or after the G43 call.
Just cursor to the block you want to start in and hit the Green.
This feature, they got mostly correct on the f'in NextGen control even.


Fanuc based Makino Wire EDM does this as well, though you need to add an N number to the block you want to start in for it to search it.
Certainly not at all as easy as it is on a Haas, but doable.

On Fanuc mills .... I don't know ....

 

[DouglasJRizzo]

On Fanuc controls you can write the code so that it can easily pick up anywhere you want it, or use the GOTO command.
The best tho, would be Okuma OSP. You can specify a sequence or line number, hit "Sequence Restart" and the machine picks up where it left off without a hitch.

 

[Booze Daily]

On Fanuc controls you can write the code so that it can easily pick up anywhere you want it, or use the GOTO command.
The best tho, would be Okuma OSP. You can specify a sequence or line number, hit "Sequence Restart" and the machine picks up where it left off without a hitch.

Yep. I’ve done this in the middle of a canned cycle.

 

[sinha]

Please clarify.
Do you mean to say that if, for example, G71 is interrupted in the middle of execution, it can be restarted from the same point where it stopped earlier?

 

[Booze Daily]

Correct.
___

 

[gregormarwick]

Hurco are pretty smart about this, their behaviour is a lot like how Seymour describes the Haas above.

It's not 100% foolproof, and I don't think it can restart inside a canned cycle, but it works pretty well.

As usual, it's just Fanuc that are behind the curve.

 

[sinha]

I have no idea about other controls, but restating an unfinished canned cycle such as G71, from where it left, is not possible on Fanuc.

This means that, on a Fanuc machine, if a G71 requires, say, 30 roughing passes, and the execution gets interrupted after, say, 29 passes, then one can restart G71 only from the first pass, not from the 30th pass.

In other words, G71 can restart only from the beginning, even if it means air-cutting most of the time.
This is the only option if major modification in the program is not to be done. The other option is to scrap the workpiece, of course.

If a control is able to restart a partly completed canned cycle, from that point, then it is pretty advanced.

 

[Booze Daily]

The OSP control has a block counter. It counts every block processed, not to be confused with lines of code.

So if your G71 (G85 on OSP)makes 30 rough passes and you need to change an insert at pass 27, hit feed hold, look at the block number and after you change your insert, restart at that block number.
As with most controls, it will rapid to the previously executed XZ position then resume cutting.

 

[DouglasJRizzo]

Please clarify.
Do you mean to say that if, for example, G71 is interrupted in the middle of execution, it can be restarted from the same point where it stopped earlier?

On Okuma it would be a G85 bar turn cycle, but, yes, you could give it the line number and the control would pick up from there without missing a beat..

 

[sinha]

On Okuma it would be a G85 bar turn cycle, but, yes, you could give it the line number and the control would pick up from there without missing a beat..

That is great!

On a Fanuc, the maximum which you can do (which I have done once) is to bring down the start point of G71 for the second run, to approximately match the X-level of the last roughing pass of the previous cycle when the execution was interrupted. G71 starts roughing from the X-level of the cycle start point. Therefore, it will skip the previous roughing passes, above this level (Talking about external machining).

There is a caution, however:
After the roughing passes are complete, step-removal pass starts (taking about Type 1 cycle).
This will go up to the last point on the defined profile (in Q-block). Thereafter, it will come back to the new start point, showing dog-leg effect. This can gouge the workpiece.
Let us hope Fanuc modifies G71 to incorporate axial retraction, followed by radial retraction.