What's new
What's new

Fanuc Series O-M p/s 041 issues

ztwin13

Plastic
Joined
Jun 13, 2022
Having issues troubleshooting cutter comp on a new-to-the-shop used amera seiki with fanuc controller mentioned in the title. Pulled my tool path straight from my haas and made all appropriate changes to be fanuc friendly (I believe) and keep getting a p/s 041 alarm while trying to cut a profile.

T18 M6
S3000 M3
G00 G54 X0 Y.25
G43 H18 Z.5
G01 Z-.35 F60.
G01 G41 D38 X-.8125 Y0
G01 Y-.1875
GO1 X-.5625
G01 X-.0979 Y-.2907
G02 X0 Y-.4128 R.125
GO1 Y-1.5872
G02 X-.0979 Y-1.7093 R.125
G01 X-.5625 Y-1.8125
G01 X-.8125
G01 Y-2.1
G00 G40 X0 Y-2.5
G00 Z.5
G00 G53 Z0 M5
M30

I have geometry 38 set at .125 for a .25" endmill (my machine does not have a diameter column) and it refuses to go past the lead in line, though it leads in fine enough.

Any help troubleshooting this issue would be great! Also, long time user of the site but first time posting (I'm usually quite capable of troubleshooting but not today haha) so apologies if wrong thread or for any other reason I suppose haha.
 

latheman78

Cast Iron
Joined
May 28, 2022
Location
Southern Ca Mtns.
Typos I assure you. Also, quit being pedantic. It's quite literally not helpful.
Wow, I was trying to help, not busting balls. A typo when programming a CNC machine can cause severe consequences. If I were to need help programming I would have cut and pasted the exact code, that is what I assumed you did. Many of us do not use programming software, I pointed out a common mistake many people make including myself. Sometime typing a letter O instead of a ZERO can cause a complete mess. If you do it multiple times that can cause hours of troubleshooting to determine what you did. With your attitude I hope no one offers you assistance, you crash your machine and cause a lot of damage resulting in a large repair bill for yourself, or getting fired if working for others.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
Having issues troubleshooting cutter comp on a new-to-the-shop used amera seiki with fanuc controller mentioned in the title. Pulled my tool path straight from my haas and made all appropriate changes to be fanuc friendly (I believe) and keep getting a p/s 041 alarm while trying to cut a profile.

T18 M6
S3000 M3
G00 G54 X0 Y.25
G43 H18 Z.5
G01 Z-.35 F60.
G01 G41 D38 X-.8125 Y0
G01 Y-.1875
GO1 X-.5625
G01 X-.0979 Y-.2907
G02 X0 Y-.4128 R.125
GO1 Y-1.5872
G02 X-.0979 Y-1.7093 R.125
G01 X-.5625 Y-1.8125
G01 X-.8125
G01 Y-2.1
G00 G40 X0 Y-2.5
G00 Z.5
G00 G53 Z0 M5
M30

I have geometry 38 set at .125 for a .25" endmill (my machine does not have a diameter column) and it refuses to go past the lead in line, though it leads in fine enough.

Any help troubleshooting this issue would be great! Also, long time user of the site but first time posting (I'm usually quite capable of troubleshooting but not today haha) so apologies if wrong thread or for any other reason I suppose haha.
There's a parameter for the Fanuc Control that affects the way the TNR Comp Start Up is applied. The usual default is to start as shown in the following picture, along the line from X0.0 Y0.25, to be tangent with the line from X-0.8125 Y0.0 to X-0.8125 Y-0.1875. In this case your program will work fine.
PS041-1.JPG
The alternate parameter setting will have the TNR Comp applied as shown in the following picture, where the control will position the tool tangent to the Lead in Line and the next line feature. In this case the look ahead will detect interference with the line from X-0.8125 Y-0.1875 to X-0.5625 Y-0.1875,

PS041-2.JPG

I've only seen the above method implemented on one machine and therefore, I've only had to find the parameter once, so I don't know it off the top of my head. I'll see if I can find the parameter today, but alternatively, if your work-piece will permit it, change the target point for your TNR Comp start up line to be more positive in the "Y" axis as shown by the Light Blue line in the following picture:

PS041-3.JPG

Regards,

Bill
 

ztwin13

Plastic
Joined
Jun 13, 2022
Wow, I was trying to help, not busting balls. A typo when programming a CNC machine can cause severe consequences. If I were to need help programming I would have cut and pasted the exact code, that is what I assumed you did. Many of us do not use programming software, I pointed out a common mistake many people make including myself. Sometime typing a letter O instead of a ZERO can cause a complete mess. If you do it multiple times that can cause hours of troubleshooting to determine what you did. With your attitude I hope no one offers you assistance, you crash your machine and cause a lot of damage resulting in a large repair bill for yourself, or getting fired if working for others.
My brother. Go to your nearest contoller and type in an "O" after a "G" and see what happens. Come back after you face palm.
 

ztwin13

Plastic
Joined
Jun 13, 2022
There's a parameter for the Fanuc Control that affects the way the TNR Comp Start Up is applied. The usual default is to start as shown in the following picture, along the line from X0.0 Y0.25, to be tangent with the line from X-0.8125 Y0.0 to X-0.8125 Y-0.1875. In this case your program will work fine.
View attachment 366768
The alternate parameter setting will have the TNR Comp applied as shown in the following picture, where the control will position the tool tangent to the Lead in Line and the next line feature. In this case the look ahead will detect interference with the line from X-0.8125 Y-0.1875 to X-0.5625 Y-0.1875,

View attachment 366769

I've only seen the above method implemented on one machine and therefore, I've only had to find the parameter once, so I don't know it off the top of my head. I'll see if I can find the parameter today, but alternatively, if your work-piece will permit it, change the target point for your TNR Comp start up line to be more positive in the "Y" axis as shown by the Light Blue line in the following picture:

View attachment 366779

Regards,

Bill
I'll try this! The other thing I tried was using an "H" instead of a "D" as I was perusing leftover programs from the previous owners and saw they did that on a few threadmills, but ran out of time in clock to give it a go. I doubt it'll have any difference but you never know.
 

ztwin13

Plastic
Joined
Jun 13, 2022
Keep digging. Tell me what G and letter O together are supposed to mean. The letter O is a program call.
Quite exactly what I mean. There's literally no way I would have an O in such a manner in my program. It would be such a blatant and obvious mistake people with even an iota of program knowledge would point out.
 

latheman78

Cast Iron
Joined
May 28, 2022
Location
Southern Ca Mtns.
Quite exactly what I mean. There's literally no way I would have an O in such a manner in my program. It would be such a blatant and obvious mistake people with even an iota of program knowledge would point out.
You typed two letter O's. Believe it or not it happens to EVERYONE, novice and with decades of experience, some of the formats you use it is pretty difficult to see the difference, especially if you are far sighted or need reading glasses. My first post was not condescending and your response was 100% out of line. Whether you cut and pasted your mistake or miss typed copying your program, and you attack me for pointing out YOUR mistake. Good for you, once again I hope others see your attitude and don't help you. May your machines crash.
 

ztwin13

Plastic
Joined
Jun 13, 2022
You typed two letter O's. Believe it or not it happens to EVERYONE, novice and with decades of experience, some of the formats you use it is pretty difficult to see the difference, especially if you are far sighted or need reading glasses. My first post was not condescending and your response was 100% out of line. Whether you cut and pasted your mistake or miss typed copying your program, and you attack me for pointing out YOUR mistake. Good for you, once again I hope others see your attitude and don't help you. May your machines crash.
I agree. I did type those Os. You may think you're being helpful and I apologize for calling you a pedant. But, the majority of machine controllers will segregate words by letter. You type in one letter, get new word. Type in two (or multiple) letters back to back and some controllers will add an implicit O to the letters with no numerical value. Others, like the machine in question in today's thread, will assume you meant the GOTO function and fill in the rest of the "GOTO" (in this case the -TO) and apply the numeric to the assumed word/function. It was my understand (as it should have been yours) you were capable enough to be aware of this interaction with your controller. I was wrong. I apologize for expecting too much from you.
 

Vancbiker

Diamond
Joined
Jan 5, 2014
Location
Vancouver, WA. USA
Somebody’s Cheerios must have been pissed in this morning…..

If a reply to a post is not considered helpful, isn’t it easier to ignore it rather than flame the poor SOB that was suggesting something he felt helpful?
 

ztwin13

Plastic
Joined
Jun 13, 2022
Somebody’s Cheerios must have been pissed in this morning…..

If a reply to a post is not considered helpful, isn’t it easier to ignore it rather than flame the poor SOB that was suggesting something he felt helpful?
Oh probably. I really shouldn't have escalated it the way I did, but who am I to resist a good back and forth with strangers on the internet.

Ultimately, our industry has a plethora of different brands and their differentiating systems. Along with a barrier to entry in the form of expensive equipment, machinery, and software it's not hard to imagine many users of this forum are struggling with older machines that have a distinct lack of technical support otherwise. I shouldn't just assume there aren't a few out there where my above mentioned interaction on the controller applies.

On the same hand, however, I mention quite explicitly the brand and model of my controller. And, generally, common courtesy is to only reply if you possess distinct and particular knowledge, especially with such a niche issue. Replying instead with what was arguably a pedantic statement, was not helpful.

TLDR; I'm sorry to latheman78 for carrying it out so far, but, as far as I'm concerned, try to only reply if what you have to offer carries at least minimally significant value.
 

Vancbiker

Diamond
Joined
Jan 5, 2014
Location
Vancouver, WA. USA
And, generally, common courtesy is to only reply if you possess distinct and particular knowledge, especially with such a niche issue……

Yep, in a perfect internet forum world. Unfortunately……it’s not so perfect.

Honestly about half the replies to posts like yours end up with worthless advice/suggestions. A good BS filter is good to have handy.
 

angelw

Diamond
Joined
Sep 10, 2010
Location
Victoria Australia
I'll try this! The other thing I tried was using an "H" instead of a "D" as I was perusing leftover programs from the previous owners and saw they did that on a few threadmills, but ran out of time in clock to give it a go. I doubt it'll have any difference but you never know.
Was "D" also used in the previous owner's programs? There are parameters to specify the Offset System being used as well as whether "D" or "H" is used in Cutter Radius Compensation.

Regards,

Bill
 
Last edited:

ztwin13

Plastic
Joined
Jun 13, 2022
Was "D" also used in the previous owner's programs? There are parameters to specify the Offset System being used as well as whether "D" or "H" is used in Cutter Radius Compensation.

Regards,

Bill
I didn't have the chance, time, or patience to filter through all the old programs but I didn't see any D values, only H, so I figured I'd give it a go today
 

memoryman

Aluminum
Joined
May 24, 2013
Location
Kitchener ,Ontario, Canada
I didn't have the chance, time, or patience to filter through all the old programs but I didn't see any D values, only H, so I figured I'd give it a go today
I'll answer with trepidation...
Cutter comp.B and Care options; depending on the control's software version, either one may not be available or enabled. What is your control's software version? e.g. MC-0469
 

ztwin13

Plastic
Joined
Jun 13, 2022
There's a parameter for the Fanuc Control that affects the way the TNR Comp Start Up is applied. The usual default is to start as shown in the following picture, along the line from X0.0 Y0.25, to be tangent with the line from X-0.8125 Y0.0 to X-0.8125 Y-0.1875. In this case your program will work fine.
View attachment 366768
The alternate parameter setting will have the TNR Comp applied as shown in the following picture, where the control will position the tool tangent to the Lead in Line and the next line feature. In this case the look ahead will detect interference with the line from X-0.8125 Y-0.1875 to X-0.5625 Y-0.1875,

View attachment 366769

I've only seen the above method implemented on one machine and therefore, I've only had to find the parameter once, so I don't know it off the top of my head. I'll see if I can find the parameter today, but alternatively, if your work-piece will permit it, change the target point for your TNR Comp start up line to be more positive in the "Y" axis as shown by the Light Blue line in the following picture:

View attachment 366779

Regards,

Bill
This worked. It was exactly as you described so thank you very much. I never occurred to me the controller would attempt to comp the lead in line as well haha I'll know better in the future.
 

ztwin13

Plastic
Joined
Jun 13, 2022
I'll answer with trepidation...
Cutter comp.B and Care options; depending on the control's software version, either one may not be available or enabled. What is your control's software version? e.g. MC-0469
You know, I looked at that once, but that was forever ago. I looked pretty in depth through the book we received with the machine, but that lead no where. Also, the previous owners were thread milling with it so I was quite confident the software had the capabilities I needed. All moot points, as angelw pinpointed the exact cause of the issue so all is good now!
 

memoryman

Aluminum
Joined
May 24, 2013
Location
Kitchener ,Ontario, Canada
You know, I looked at that once, but that was forever ago. I looked pretty in depth through the book we received with the machine, but that lead no where. Also, the previous owners were thread milling with it so I was quite confident the software had the capabilities I needed. All moot points, as angelw pinpointed the exact cause of the issue so all is good now!
The options are not public knowledge; glad that your issue has been fixed.
 








 
Top