Parameter toggling while machining

[kevbo]

I am using A Fanuc 18i-T controller and was wondering if it is possible to adjust parameters during maching. My current issue is that I have an automated process so that when a tool breaks, I have no detection method which results in alot of scrap, quick. I have researched options through Fanuc with no results. I have looked at aftermarket add on options that are just too expensive. My idea is to try and use parameter #1828 (position deviation limit), during each cutting cycle to basically monitor the load amount. If the insert breaks, the position deviation should increase, resulting in a servo alarm. Currently, the limit is set a little above the rapid traverse state which is normal. What I would like to do is be able to set it lower during a cutting cycle, then return it to the oringinal setting when going back to a rapid motion through the program. Is this possible? Any examples or ideas would be appreciated.

[ou812]

Originally Posted by kevbo I am using A Fanuc 18i-T controller and was wondering if it is possible to adjust parameters during maching. My current issue is that I have an automated process so that when a tool breaks, I have no detection method which results in alot of scrap, quick. I have researched options through Fanuc with no results. I have looked at aftermarket add on options that are just too expensive. My idea is to try and use parameter #1828 (position deviation limit), during each cutting cycle to basically monitor the load amount. If the insert breaks, the position deviation should increase, resulting in a servo alarm. Currently, the limit is set a little above the rapid traverse state which is normal. What I would like to do is be able to set it lower during a cutting cycle, then return it to the oringinal setting when going back to a rapid motion through the program. Is this possible? Any examples or ideas would be appreciated.

Kevbo,

You can toggle parameters with a G10. This is explained in the fanuc programming manual.

OU812

G10L50; Parameter entry mode setting
N_R_; For parameters other than the axis type
N_P_R_; For axis type parameters
G11; Parameter entry mode cancel
N_: Parameter No. (4digits) or compensation position No.(0 to
1023) for
pitch errors compensation +10,000 (5digit)
R_: Parameter setting value (Leading zeros can be omitted.)
P_: Axis No. 1 to 8 (Used for entering axis type parameters)
Meaning of command

[MysticMonkey]

Hi Kevbo,

Unfortunately Parameter #1829 will not help control the size of the finished dimension nor is it related to the spindle/axis load when a tool breaks.

You only options are

1. Tool Load Monitoring - (Option, not sure if it's on the 18i)
2. Tool measurement and comparison with a tool setter (options + hardware)
3. Employing someone to measure the finished product during operation

[kevbo]

1. Mystic thanks for your response, but I think you misunderstood me. The parameter I was refering to was 1828 (position deviation error). It is not the dimension on the product that I am trying to control with this, I am trying to figure out a way to get the servos to recognize that there is an insert broken when the tool bar is beating the part to death.

2. ou812, thanks for your help also. I have never seen or used G10 before on any application, ( I'm no expert), but I had heard of it in the past and thought this was what I was looking for. I spent most of the day looking through the Fanuc operators manual, but did not find any information on it. Any addtional info would be appreciated. Thanks.

[MysticMonkey]

Hi Kevbo ,

I did understand you and I know what your trying to do

Parameter 1829 relates to the difference between the programmed position and the position indicated by the motor encoder

in the stopped state.

for example if the servo's were off and there was nothing holding the x-axis up on a slant bed it would drop.

this would cause a difference between the commaned value and the "actual" position. When this error is greater that P1829 the NC will give an emergency stop and a positional error causing you to have to re-enable the drives.

If you adjust this to detect any position change on the x-axis servo when a tip breaks the value is going to be so small that you will get a lot of false positives. If you get any positional deviation at all.

[Fanucguy]

Hi Kevbo,
ou812 response is correct and could be something worth exploring but difficult to find the "sweet spot" in the settings to really solve the issue...GE Fanuc has several options to consider...ask them about miAdapt...it does a nice job sensing spindle load and can be used in various ways.
It really comes down to how much load is being generated during the cycle and how much variance in load there is to act upon...If your breaking an 1/8-inch drill in aluminum on a machine with 20 hp there’s really no additional load generated when the tool breaks…
I have a lot of experience with Tool Monitoring systems with mixed results..ATAM Systems has a pretty good one.
I’ve seen this same problem time and time again over my 30 years in the industry and I’ve seen it addressed in a multitude of different ways. The best way to fix it is, don’t break the tool. Not trying to be a smart … but I worked on projects where companies were eating tools like candy.Slight changes to the process; changes in the tooling package and re-programming the machine to match can make a huge difference. I’ve seen it go from only 2 parts to 2000 parts without breaking tooling…and then they set it auto select a new tool based on usage…. Hope this helps….