Arc issue on Fanuc

[Guest]

JP whatever happened with this customer? was it the fanuc parameter? thanks Tim!! i will change those parameters in our 18i and 31i controls since this has happened

to me in the past. it always turns out that x,y,i, or j is off by .0001 but plots fine in cimco and runs fine on a fadal (go figure, those fadals)

 

Not exactly sure, supposedly they were having the machine guy, then someone "got sick", the job had to get out, so they moved the into a different orientation and I ran a path over the suspect area, that worked fine

 

 

So they got the part out but I still don't think they have dealt with the parameter issue, so it's likely at some point to come up again  

[Rick46]

Parameter #3410 - Tolerance of arc radius

 

Change it from 10 to 100, or simply increase the value present.

It shouldn't take much.

 

You can also take a look at #3403.

 

Tim is this info in the parameters assuming a 4 place decimal meaning the 10 actually equals .001 and 100 equaling .010

[Guest MTB Technical Services]

Tim is this info in the parameters assuming a 4 place decimal meaning the 10 actually equals .001 and 100 equaling .010

 

I was responding as f it was metric.

 

#3410 data is reflective of the unit of measure the machine is set for.

[Maclaw]

JP,

 

I made some tests today with my faulty program. When I worked with AIAPC/AICC (G5.1 Q1) on - the EXACTLY SAME NC prog that made the loop before - got executed properly (no loops)... I don't know what to think about this...

 

I took this test when prm #5008 bit QCR was "0" (look at my previos post, but Tim says it's obsolete on newer fanucs). Can you try this with your faulty program and give info if it worked for you aswell..? Tim - what do you think of all this...? I am still struggling that "my" workaround with the problem might be just plain luck - and you never know when it will hit you again... I don't know for 100% - just don't know...

[Rick46]

I was responding as f it was metric.

 

#3410 data is reflective of the unit of measure the machine is set for.

So this would be changing the machine parameter value from 10 mm to 100 mm ?? Im just trying to understand the logic here. because if it is default set to 10 mm that seems plenty enough of a arc tolerance to me. I too have experienced this enormous loop problem but on other machine controls not fanucs. and the key to the problem was switching to I,j,k output in the post. but have never seen this on a fanuc control. The 18i's I have used have had the control and machine being set up in inch mode not metric which I know is just a change of  paremeters to switch back and forth because they arrived in metric and I had them switched over to inch. also I know some areas in the 18i any ways, the 1000 would not be seen in metric, it assumes a four place decimal. In other words, 10000 equals 1.0", 1000 equals 0.1", 100 equals 0.01", etc.  jut trying to understand the logic here is all, thanks in advance.

[Guest MTB Technical Services]

So this would be changing the machine parameter value from 10 mm to 100 mm ?? Im just trying to understand the logic here. because if it is default set to 10 mm that seems plenty enough of a arc tolerance to me. I too have experienced this enormous loop problem but on other machine controls not fanucs. and the key to the problem was switching to I,j,k output in the post. but have never seen this on a fanuc control. The 18i's I have used have had the control and machine being set up in inch mode not metric which I know is just a change of  paremeters to switch back and forth because they arrived in metric and I had them switched over to inch. also I know some areas in the 18i any ways, the 1000 would not be seen in metric, it assumes a four place decimal. In other words, 10000 equals 1.0", 1000 equals 0.1", 100 equals 0.01", etc.  jut trying to understand the logic here is all, thanks in advance.

 

 

No.

 

It would be changing it from 0.01 mm to 0.1 mm.

That was just an example.

The point is to be larger than the resolution of the current unit selection.

This can effect either R-word radius or IJK.

 

As I previously described in the post about Glenn's output, there was an error of 0.0001 in the output of his code.

Simply changing the parameter value to a larger number eliminates the issue.

 

If your current value 0.0001 then it should be increased to at least 0.0002

 

FYI, every CNC on the market today uses Metric ballscrews.

While the controls can be switched between mm and inch for the purposes of programming, offsets and readout display, there are many parameters that must stay as metric values.

This is typical for thing like calibrating and establishing certain reference positions.

For example, I recently re-calibrated the Q-Setter on a Doosan MX Multitasking machine.

While the machine is set to inch, all the Q-setter reference positions for the B-Axis Head are stored in parameters as metric values.

[Rick46]

No.

 

It would be changing it from 0.01 mm to 0.1 mm.

That was just an example.

The point is to be larger than the resolution of the current unit selection.

This can effect either R-word radius or IJK.

 

As I previously described in the post about Glenn's output, there was an error of 0.0001 in the output of his code.

Simply changing the parameter value to a larger number eliminates the issue.

 

If your current value 0.0001 then it should be increased to at least 0.0002

 

FYI, every CNC on the market today uses Metric ballscrews.

While the controls can be switched between mm and inch for the purposes of programming, offsets and readout display, there are many parameters that must stay as metric values.

This is typical for thing like calibrating and establishing certain reference positions.

For example, I recently re-calibrated the Q-Setter on a Doosan MX Multitasking machine.

While the machine is set to inch, all the Q-setter reference positions for the B-Axis Head are stored in parameters as metric values.

thanks for the info and help on understanding how the parameters in the fanuc controls work, Im always scrolling through the pages trying to understand what they are and what they do or referencing back to my manuals as well..

[mike93]

what is the rounding point of pie for mastercam could this be an issue if the end points are not  on the arc. just grasping at  straws.

[Tyler Robertson]

Arc data is stored as double, at least when retrieving it from the API http://msdn.microsoft.com/en-us/library/643eft0t

[hopscotch]

Hi JP - control Fanuc Oi MC

I changed the parameter 5008 and the program ran well, thanks for the info.

This issue has cost me thousands on a mould insert that had to be scrapped

 Just wondering though if it will come back to bite me in another way down the track?

Has anyone encountered errors or crashes after changing Bit 5 (QCR) to one?

 

[Newbeeee™]

FWIW, on the later D control, it seems that the "standard" settings could be very different because the defaults are missing, and therefore different to the C.

This may help - a pdf of the differences between your C control, and the later D.

HTH

https://www.cnczone.com/forums/attachments/1/7/8/7/3/4/145265.attach

 

[JoshC]

I have seen this many times, Its normally caused by the Arc End point rounding, Go into the machine def, then the control definition, then the arc page and use No Rounding - Break arc on failure for the arc rounding settings in the bottom right of that page. I don't know why so many controls have problems with the 4th decimal place getting rounded but the Break on failure seems to always work nicely and should fix that problem that you are having. 

[PAnderson]

Hello All,

I had started this topic a while back.

This is not a Mastercam issue alone. It is a Fanuc issue but Mastercam can help eliminate it. It is an arc length issue as interpreted by Mastercam or any other CAM system. Read the last two posts in my thread for a possible answer. If the arc length is so small that the control assumes the end point is so close to the start point that it assumes it should be a full arc, then it will create a full arc, to a lot of peoples great surprise. And to a lot of cussing and throwing of objects. This mostly happens in High Speed tool paths that generate a lot of really small arcs. The remedy is to change the minimum arc length setting in Mastercam to something that the control will not assume is a full arc. Other CAM systems can have this happen also. I had it happen in Smartcam and Unigraphics back in the 90's. And I have had calls from customers as recently as a year ago.

Paul