[Technical Ted]

3 year old Doosan v550 lathe. I've always been under the impression that offset changes only take effect at the next tool change. Something happened yesterday that now has me wondering if this is still true. Do I need to retake CNC 101?

[Technical Ted]

Lots of views but no replies! Maybe it'll help if I explain what happened. We're using T0101 to rough face & turn, we then flip the part so we're chucking on a good surface instead of a very rough out of round forging. So the tool comes down & I see it's going to take a fairly heavy face cut. I press feed hold, raise the Z wear offset .025 & restart the program. As the tool is facing the part I drop the Z wear offset back down .025 for the next part. The tool completes the facing, turns the od & the door opens ready to be flipped. As I'm getting ready to remove the part I see a .025 step above the radius. It appears the offset change took effect between the facing & turning (all in the same op) without a tool change in between.

[dcoupar]

Please post the section of your program where this occurred.

[gerc]

tool offset happens whenever it is called. so when you restarted if the control saw t0101 it will take the new offset.

[Technical Ted]

I can't get that until Monday night. but roughly here's the code that counts.

T0101
G0 X15.300 Z.070
G1 X12.000 F.010
Z.120
GO X14.900
G1 Z.070
G3 X15.100 Z-.030 R.100
GI Z-2.000
X15.300
G28 U0. W0.

That's the best I can do for now. Do you agree that I shouldn't get a step at the radius if I drop the Z offset .025 while the tool is facing the part?

[yardbird1969]

Hi Technical Ted,

I think we both need to retake CNC 101. Doosan PUMA 300 0iT-D less that a year old. Something happened to me but was embarrassed to ask. I am still pretty sure that applies to wear offsets. I had moved the wear offsets for the OD tools up +.03 and moved the ID tools down -.03 then moved the whole machine G54 out +.01 to take a cut then measure then adjust for the diameter finish size and tolerance then rerun. While the last tool of the program was still in process a OD tool facing down a shoulder i decided to go ahead and move the machine G54 back the -.01 so i didn't forget. When i did i witnessed the absolute Z position change while cutting. Now the tool didn't move but the numbers damn sure did. I should have depth mic the shoulder lengths but i didn't. I just reran the part and moved on. Maybe that has to do with the measure function and active tool offsets? Can you tell a little more about what you experienced?


Brent

Edit: we must have been typing at the same time.

[Technical Ted]

Hi Technical Ted,

I think we both need to retake CNC 101. Doosan PUMA 300 0iT-D less that a year old. Something happened to me but was embarrassed to ask. I am still pretty sure that applies to wear offsets. I had moved the wear offsets for the OD tools up +.03 and moved the ID tools down -.03 then moved the whole machine G54 out +.01 to take a cut then measure then adjust for the diameter finish size and tolerance then rerun. While the last tool of the program was still in process a OD tool facing down a shoulder i decided to go ahead and move the machine G54 back the -.01 so i didn't forget. When i did i witnessed the absolute Z position change while cutting. Now the tool didn't move but the numbers damn sure did. I should have depth mic the shoulder lengths but i didn't. I just reran the part and moved on. Maybe that has to do with the measure function and active tool offsets? Can you tell a little more about what you experienced?


Brent

Edit: we must have been typing at the same time.

Interesting, maybe I haven't lost my mind.

[gerc]

machines do what they are told, codes tell them what to do, once a machine is told an offset or a work cooridinate it will do just that. if you change midstream it should make no difference, but there may be a call that you are missing. ie: if at every tool change you call g54...etc it will read whatever change you made. same with tool offsets, if the tool you made the change to is coming up it will read the current tool offset. t0101 reads tool 1 offset 1 , any change that happens to offset 1 after this line will not happen til the next time it reads that line. same with g54,g55,g56... etc.

[Technical Ted]

machines do what they are told, codes tell them what to do, once a machine is told an offset or a work cooridinate it will do just that. if you change midstream it should make no difference, but there may be a call that you are missing. ie: if at every tool change you call g54...etc it will read whatever change you made. same with tool offsets, if the tool you made the change to is coming up it will read the current tool offset. t0101 reads tool 1 offset 1 , any change that happens to offset 1 after this line will not happen til the next time it reads that line. same with g54,g55,g56... etc.

I would have said the same thing three days ago. I may run over there tonight when 3rd shift starts & download a copy of the program. Check in the morning if you have time.

[Technical Ted]

Here's the program:
%
O2156
N010M53
M41
(T0101)(CNMG 433)
(ROUGH FACE & TURN)
M24
G40G54
G28W0
G28U0.
G97S0123M04
T0101
G00X15.700Z.070
M08
G50S0700
G96S0500
G01X12.000F.010
Z.120
G00X15.150
G1Z.070
G3X15.350Z-.030R.1
G1Z-2.500
X15.550
M09
M25
G28U0.W0.
M05
M52
M66(LOW CHUCK PRESSURE)
M00(FLIP PART)
N015M53

[gerc]

now that i think about, g54 is modal, so it very well might take affect right away. i never make a work offset adjustment during program execution. nor do i make a tool offset adjustment if that tool is currently running. now you have my curiousity up.

[yardbird1969]

"We're using T0101 to rough face & turn, we then flip the part" and then "As I'm getting ready to remove the part I see a .025"

Is it you personally at the machine and not second hand info? Is this something that only happened once?
If so and it wont scrap the part i'd try to make it happen again. If you can't get it to do it again then i'd just chalk it
up to just one of them things and move on. If it does it again then you have a problem IMHO. I see nothing wrong with your
program. Although I stand by my post #6... I think that gerc said it best in his post #8... That is the way they are supposed
to operate and i agree with him.

Brent

[Technical Ted]

"We're using T0101 to rough face & turn, we then flip the part" and then "As I'm getting ready to remove the part I see a .025"

Is it you personally at the machine and not second hand info? Is this something that only happened once?
If so and it wont scrap the part i'd try to make it happen again. If you can't get it to do it again then i'd just chalk it
up to just one of them things and move on. If it does it again then you have a problem IMHO. I see nothing wrong with your
program. Although I stand by my post #6... I think that gerc said it best in his post #8... That is the way they are supposed
to operate and i agree with him.

Brent

In the text you quoted, I was getting ready to remove the part to flip it over when the step was seen.

I am operating the machine & yes I can make it repeat. It doesn't affect the finished part so I can play around with it. When I went in last night to get the program, the 3rd shift operator & I raised the Z wear offset .025 & sure enough half the radius was missing. I don't know if this is a Doosan thing or just a problem with this machine. We actually have two of these machines that are mirror images, maybe left hand & right hand is a better way to phrase it. I'll try it in the other machine tonight.

[gerc]

Lots of views but no replies! Maybe it'll help if I explain what happened. We're using T0101 to rough face & turn, we then flip the part so we're chucking on a good surface instead of a very rough out of round forging. So the tool comes down & I see it's going to take a fairly heavy face cut. I press feed hold, raise the Z wear offset .025 & restart the program. As the tool is facing the part I drop the Z wear offset back down .025 for the next part. The tool completes the facing, turns the od & the door opens ready to be flipped. As I'm getting ready to remove the part I see a .025 step above the radius. It appears the offset change took effect between the facing & turning (all in the same op) without a tool change in between.

i'm very curious about this , if the new offset isn't called i'm not sure why that would happen?

[Technical Ted]

I played around a little bit last night & found out that both machines do the same thing & that it only happens with the wear offset.
Here's the program with the absolute & machine positions shown.

G00X15.700Z.070
M08
G50S0700
G96S0500
G01X12.000F.010 (Absolute Z .070 Machine Z 9.850)
Z.120 (Absolute .Z 120 Machine Z 9.900)
G00X15.150 (Absolute Z .120 Machine Z 9.900)
G1Z.070 (Absolute Z .070 Machine Z 9.825)
G3X15.350Z-.030R.1
G1Z-2.500

[gerc]

i'll try something like that on our lynx. i've never had that problem but i don't make offset or wear adjustments while that tool is running. something i was told many many many years ago. i guess maybe that is why.

[yardbird1969]

Ted,

well since both machines are the same you have me stumped!! Are these machines dedicated solely to this part? Have you had this issue on other parts? I have never in 26yrs of running NC machines even the old ones back in the day that i loaded programs with paper punch tapes that were set up to operate this way normally. Not one single MTB I've came across operates this way, that i know of. If it was me just for ****s and giggles leave the Z alone but try the exact thing but just on the X axis to see if it does the same thing. I suppose there ways around this (don't move while in operation) but I don't feel your doing anything out of the ordinary IMHO. You have me hanging and wondering what the hell is going on here. If you put your finger on it please post back with your solution.

thank you in advance
Brent

P.S.... I wish one of the Doosan factory guys would chime in on the matter.

[Technical Ted]

i'll try something like that on our lynx. i've never had that problem but i don't make offset or wear adjustments while that tool is running. something i was told many many many years ago. i guess maybe that is why.

Give it a try. You don't even need a part in the machine. Just run it in single block & see if the machine position changes when the machine feeds back down to the Z dimension that you faced at.

[Technical Ted]

Ted,

well since both machines are the same you have me stumped!! Are these machines dedicated solely to this part? Have you had this issue on other parts? I have never in 26yrs of running NC machines even the old ones back in the day that i loaded programs with paper punch tapes that were set up to operate this way normally. Not one single MTB I've came across operates this way, that i know of. If it was me just for ****s and giggles leave the Z alone but try the exact thing but just on the X axis to see if it does the same thing. I suppose there ways around this (don't move while in operation) but I don't feel your doing anything out of the ordinary IMHO. You have me hanging and wondering what the hell is going on here. If you put your finger on it please post back with your solution.

thank you in advance
Brent

P.S.... I wish one of the Doosan factory guys would chime in on the matter.

The machines were purchased for 2 similar parts from the same customer. We were suppose to run 100 -200 of these a month but presently just run a 100 pc order every couple months. We now run quite a few different jobs through the machines. I never noticed this happening on any other parts but usually the offsets are changed when the part is finished & the change is just .0002 - .002. It was a strange set of circumstances that led to this discovery.

I snickered a bit when you mentioned loading programs from tape, we're still using tape on an old Cinci lathe. I guess we're not the only ones, the tape is still available.

[gerc]

i did some testing today, and sure enough, it will pick up the wear comp adjustment in the next AXIS move. been doing this for 25 plus years and never ran into this issue. learn something new all the time. geometry changes didn't seem to affect it. work cooridinates do. i discussed this with a co-worker that has 25 plus years as well, and he was surprised. i think i'll continue my practice of never making an adjustment to the current tool, or work cooridinate while in execution. thanks for bringing this to light.