What's new
What's new

45° with radius does not work

Tornex

Plastic
Joined
Aug 20, 2021
Hello!

I have two fanuc machines. One with 18i-TB system

And one old O-TD

When I make this program on the 18i-TB systems it works with no errors. (Picture with color lcd screen)

But when I do exactly the same program to the old O-TD I’m getting an 055 alarm for the radius. Any clue why? The tool tip and tool radius is correct.
I have no one to ask here at work. I’m getting so tired of always doing things the wrong way. U know the feeling of being helpless 🥶

If someone is from Sweden it would be extremely helpful 👌🏻👍🏻
 

Attachments

  • IMG_0896.jpeg
    IMG_0896.jpeg
    2 MB · Views: 43
  • IMG_0898.jpeg
    IMG_0898.jpeg
    1 MB · Views: 43
  • IMG_0897.jpeg
    IMG_0897.jpeg
    1.1 MB · Views: 42
Hello!

I have two fanuc machines. One with 18i-TB system

And one old O-TD

When I make this program on the 18i-TB systems it works with no errors. (Picture with color lcd screen)

But when I do exactly the same program to the old O-TD I’m getting an 055 alarm for the radius. Any clue why? The tool tip and tool radius is correct.
I have no one to ask here at work. I’m getting so tired of always doing things the wrong way. U know the feeling of being helpless 🥶

If someone is from Sweden it would be extremely helpful 👌🏻👍🏻
Try adding a comma

N370 G1 X46 Z-10 , R3
I think that particular FANUC version needed the comma
 
Oh lots of answer this fast. Thanks 👍🏻
I will try it on Monday.

The R value, I have used it with I’m turning OD it’s works. But the. It’s not in an angle. Where the angle meets the start radius and ends with the radius.

I don’t have more exact coordinates. The drawing is “bad” I think I maybe need to know the exact coordinates for the start point?

The alarm 055 says something about to less space for radius
 
Oh lots of answer this fast. Thanks 👍🏻
I will try it on Monday.

The R value, I have used it with I’m turning OD it’s works. But the. It’s not in an angle. Where the angle meets the start radius and ends with the radius.

I don’t have more exact coordinates. The drawing is “bad” I think I maybe need to know the exact coordinates for the start point?

The alarm 055 says something about to less space for radius
If that is the alarm message then it sound like either your start point or end point is not correct.
 
The alarm 055 says something about to less space for radius

Your start and stop must be ok if it works on the other control. The alarms can be hard to sort. This may mean the control is not recognizing R3 correctly due to syntax. Somebody on here will probably know whats wrong.
 
id suspect your movement is less then the programmed radius.
I would be wondering how you get a radius when both lines are Z0, cant have that and make a radius, the Z value needs to be different if one is the start and the other is where it finishes. basically the tool needs to move in Z min amount = to the radius. X70 to X66 is a straight line
 
Hello!

I have two fanuc machines. One with 18i-TB system

And one old O-TD

When I make this program on the 18i-TB systems it works with no errors. (Picture with color lcd screen)

But when I do exactly the same program to the old O-TD I’m getting an 055 alarm for the radius. Any clue why? The tool tip and tool radius is correct.
I have no one to ask here at work. I’m getting so tired of always doing things the wrong way. U know the feeling of being helpless 🥶

If someone is from Sweden it would be extremely helpful 👌🏻👍🏻
Use I,J.K or a comma, older fanuc's don't like R in g2g3 lines, some will accept ,Rxx but some will not.
 
But when I do exactly the same program to the old O-TD I’m getting an 055 alarm for the radius. Any clue why? The tool tip and tool radius is correct.
I have no one to ask here at work. I’m getting so tired of always doing things the wrong way. U know the feeling of being helpless

BT Fabrication has the most logical answer thus far. Following is an extract from a Fanuc Manual on the subject.

Move amount of X or Z is less than chamfering value and
corner R value in the block where chamfering and corner
R are specified. (P/S alarm No. 055)


I'm more surprised that the program worked on the 18i control that it not working on the O-TD control

A Comma associated with C and R command is for the Direct Drawing feature, which is different to Chamfer and Corner Rounding with C and R.


Chamfering and filleting with G01 within a canned cycle does not work on all control versions.
I've never known that to be the case. Chamfering and Corner Rounding in a G01 Block is an option, but I've never encountered a machine with that option where the command can't be used in a G71 cycle, nor have I ever seen that restriction documented in any Fanuc manual or memo.
 
Last edited:

A Comma associated with C and R command is for the Direct Drawing feature, which is different to Chamfer and Corner Rounding with C and R.

I've never known that to be the case. Chamfering and Corner Rounding in a G01 Block is an option,

I don't know Bill.
I have an Oi-TD where the corner rounding is programmed just a straight G01 Xn Rn
I have an Oi-Mate-TD where the same must be programmed G01 Xn ,Rn, but they must be 90 degree angles
I have a MSX-850 where it's also G01 Xn ,Rn, but the angle does not need to be 90 gegrees
I have two older Haas lathes where G01 Xn Rn, but once again, only 90 degree angles supported.

But, I am utterly and totally confused by what is the difference in direct drawing programming or corner rounding/chamfering.
 
I don't know Bill.
I have an Oi-TD where the corner rounding is programmed just a straight G01 Xn Rn
I have an Oi-Mate-TD where the same must be programmed G01 Xn ,Rn, but they must be 90 degree angles
I have a MSX-850 where it's also G01 Xn ,Rn, but the angle does not need to be 90 gegrees
I have two older Haas lathes where G01 Xn Rn, but once again, only 90 degree angles supported.

But, I am utterly and totally confused by what is the difference in direct drawing programming or corner rounding/chamfering.
see now, this is exactly why I would post with IJK vs R, its annoying to edit as needed, but it works across all platforms, so if you have a repeat job, you just need to switch up a few M codes, and maybe modify a safety line. poof mostly proven program that will run on the majority of machines out there.

There are of course other opinions.

Also, and I think this gets closer to the OP problem, you can't start any canned cycle on a radius or champher move, has to be a linier motion
 
see now, this is exactly why I would post with IJK vs R,
Hmmm..... me thinks you've missed the boat at Post#1!
This thread is not about R vs. IJK, rather automatic corner rounding at the end of a linear move.
There is no G02 or G03, only G01 with an appropriate radius at the end of the move.
 
Hmmm..... me thinks you've missed the boat at Post#1!
This thread is not about R vs. IJK, rather automatic corner rounding at the end of a linear move.
There is no G02 or G03, only G01 with an appropriate radius at the end of the move.
no no, I'm on track. if you have a radius OF ANYKIND in the first line of a g71/g72 or g41/g42 then it will alarm out, regardless of whether or not its performed at the end of said g1 move, its still in the first line of the sub, and therefore no bueno same for last line of a sub, or turning off cutter comp. (some machines you can just cancel cutter comp, but again it leads to weird things if that program is used on some other machine)

It confuses the cornpooter, can't calculate every cut with some anomaly radi or chamfer at some random location. Especially on roughing canned cycles, cause every pass is determined based on the outline chosen, samsies for cutter comp, its got enough to calculate with plotting its way around a circle, toss in a user variable number, things would get weird in a hurry.

the ,C and ,R thing is super neato if all you do is hand write programs, saves a boat load of time with calculating radiuses, and chamfers (or worse radiuses with chamfers...) but it is a cheat, and doesn't work on every machine or in all circumstances.

I feel like I've had this very same argument in real life... oh wait I have... several times, for the very same reasons
 








 
Back
Top