[SIG]

Oi MC control.
When I use entry exit arcs while side milling a round or square boss I get a
.001 bump on side of part. The program is right but for some reason the machine never get to the final endpoint before arcing out. Does anyone have an idea why?

[rgammage]

Hi SIG

I am probably the least qualified to answer this but have you tried:

Reducing feed rate? .... I have seen m/c take a new command before fininshing the first!

Overlapping the start and finish points?

Regards

Richard

[V1T1CO]

Sig:
what I do to avoid this issue is, include an overlap, .025" should be enough, the other approach is to take a zero pass around your boss w/out retracting,...
Hope I was able to help.
Regards:
V1T1CO

[Phyrexii]

Your machine could be over (or under) compensating for backlash - put an indicator on your part, and manually move it with your handwheel a tenth (.0001), then move it back. If it is overcompensating, there will be a jump on the indicator. Under compensating would result in no movement. Fixing that is just a simple parameter change (although I don't know which one).

Also, it may be possible that you are somehow in exact stop mode? If so, the machine will pause briefly between execution of each block, and it may leave a dwell mark. I don't know how to change that offhand on a FANUC machine, I know on my FADAL I turn it off with a G08.

And, lastly, if you don't want to overlap your start and end points, as suggested, you can start and end on a corner, where a bump will not show up.

[SIG]

Hi SIG

Reducing feed rate? Overlapping the start and finish points?
Richard

Yes.
Yes that works but I was thinking shouldn't a machine with the latest control follow its intented path. I have an 85 tiger 3 that would not do this.

Sig:
what I do to avoid this issue is, include an overlap, .025" should be enough, the other approach is to take a zero pass around your boss w/out retracting,...
Hope I was able to help.
Regards:
V1T1CO

Do you have this problem too?

Your machine could be over (or under) compensating for backlash - put an indicator on your part, and manually move it with your handwheel a tenth (.0001), then move it back. If it is overcompensating, there will be a jump on the indicator. Under compensating would result in no movement. Fixing that is just a simple parameter change (although I don't know which one).

Also, it may be possible that you are somehow in exact stop mode? If so, the machine will pause briefly between execution of each block, and it may leave a dwell mark. I don't know how to change that offhand on a FANUC machine, I know on my FADAL I turn it off with a G08.

And, lastly, if you don't want to overlap your start and end points, as suggested, you can start and end on a corner, where a bump will not show up.

I'll try moving hand wheel .0001 back and forth.
I don't think its dwell because this is leaving stock on.
On a square part starting in corner does work but its still a problem on parts I'am trying to make round.
This is a new machine for me and I did check backlashes and they seem fine.
Our old machine has and 85 tiger 3 on it and would all ways follow its path. It just ran slow, so we upgraded.

When I cut a round cavity it takes .0002/.0003 off at each quadrant.
It seems like a backlash problem but I've checked them and they seem OK.
I will check them again.

Thank you everyone for your repleys

[Phyrexii]

One other thing I just thought of -

Turning cutter comp on/off - make sure you are not turning it on or off during your entry arc move. I always include an extra move there to insure that the tool is in the correct position prior to entering the cut. Cutter comp can do some strange things as the control is positioning the cutter, and may be moving the cutter off the cut early to compensate (or something ;-).

[antoon]

hi... i would suggest comping on/off to an imaginary point of the componant (away from the componant)if possible as u will allways get a slight digin where the tool has on/off in the same spot.
hope this helps
antoon

[ChattaMan]

You could also try a larger roll on/roll off arc.

[Mitsui Seiki]

I don't know what the program looks like but try to pur two "blind blocks" before G40.

[hacksaw6150]

just travel past the point where you turned comp on-then roll off

[SIG]

One other thing I just thought of -

Turning cutter comp on/off - make sure you are not turning it on or off during your entry arc move. I always include an extra move there to insure that the tool is in the correct position prior to entering the cut. Cutter comp can do some strange things as the control is positioning the cutter, and may be moving the cutter off the cut early to compensate (or something ;-).

I'am not using cutter comp just G1,2 & 3 w/ I & J's.
I also just learned about exact stop and thats not it. It leaving stock on not stock off like a dwell might do. Good idea though and I did learn something I did not know about before.
Thanks

[sinha_nsit]

I think, the bump is the result of the next command starting before the end of the previous command. This does happen. Because of this reason, if you give two pependicular moves, you will observe some rounding-off of the corner. If you want a sharp corner, use "exact stop" feature (G09) instead of just G01. Another way is to insert a dwell command between the two moves.

In your case, instead of reducing the feed (which will waste time), introduce a dwell (G04) of, say one second, between all moves where you are getting a bump. If it still does not work, try a higher dwell time. This will, of course, leave a "water mark" on the surface, but the surface will be smooth.

[Dan Fritz]

When any Fanuc control finishes interpolating a feed move (G01 or G02/G03), it begins the next move as soon as the servos "catch up" with the theoretical positon calculated by the CNC. Since there is always a bit of following error between the CNCs theoretical postion and the servo's ACTUAL position, the CNC has to wait for the servos to catch up before making the next move.

Fanuc contols have a set of parameters for the "In Position" zone. (INPx, INPy,and INPz). These parameters determine how big the in-position zone is. If the control makes a G02 move and DIGITALLY gets to its destination, it has to wait until both the X and the Z axes servos get within this in-position zone before it can make the next move. If the in-position zone is set too small, you'll have "dwell" marks at each intersection. If the in-position zone is too big, the control will take off too soon and will leave stock.

I'm "on the road" right now, and I don't have the 0M-i manuals handy. Look in the parameter manual for the INPx, y, and z parameters and make them smaller. See if that helps.

[SIG]

I think, the bump is the result of the next command starting before the end of the previous command. This does happen. Because of this reason, if you give two pependicular moves, you will observe some rounding-off of the corner. If you want a sharp corner, use "exact stop" feature (G09) instead of just G01. Another way is to insert a dwell command between the two moves.

In your case, instead of reducing the feed (which will waste time), introduce a dwell (G04) of, say one second, between all moves where you are getting a bump. If it still does not work, try a higher dwell time. This will, of course, leave a "water mark" on the surface, but the surface will be smooth.

I think your right about the next command starting before the previous finishes. Can I assume this is happening in all three axis. If so how do you cut a surface with any accuracy?
How can I Finishing a tight tolerance arc( say .5000 shut/off radius on the corner of a block)?
Is there a way to tighten up the tolerance in the control or the drives or servos to minimize this?
Thanks

[barryhc]

Hello SIG.

I think what you are seeing here is the result of Following Error ( Axis Lag ). This is common, and in fact normal for all of the "Closed Loop" machines that I have been involved with. It is the result of acceleration at the beginning of each move that the control executes. The machine is always "behind" the control because of this. The control is always initiating the next command before this "lag" has been closed out.

Fanuc G09 Exact Stop mode will cause this "lag" to be closed out before the next command is executed, however, that "stop" is effectively a dwell, and will cause some overcutting at that point.

The solution is still to overlap that point. When you are on the outside of a circle, using a straight line to the start of your circle eliminates the first half of the problem, and leaving in a straight line eliminates the second half.

It is a bit more interesting to get this overlap when you are inside of a circle, as it requires short partial arcs before and after the beginning and end of your main circle command.

Hope this helps ! > Barry

[Mitsui Seiki]

I think your right about the next command starting before the previous finishes.

Try to put two "blind blocks" between the commands.

[SIG]

Sig:
what I do to avoid this issue is, include an overlap, .025" should be enough, the other approach is to take a zero pass around your boss w/out retracting,...
Hope I was able to help.
Regards:
V1T1CO

That will help.
Thank you

[SIG]

When any Fanuc control finishes interpolating a feed move (G01 or G02/G03), it begins the next move as soon as the servos "catch up" with the theoretical positon calculated by the CNC. Since there is always a bit of following error between the CNCs theoretical postion and the servo's ACTUAL position, the CNC has to wait for the servos to catch up before making the next move.

. Look in the parameter manual for the INPx, y, and z parameters and make them smaller. See if that helps.

I'll try it first thing tomorrow morning.
I did flip through the operation manual and found something about this but I didn't understand it. Thanks, your explanation makes it clear.

[Rick Linnabary]

Hello,
I agree with the things that have been posted. I would use an entry line and arc (about 50% of cutter diameter) along with turning cutter comp on the entry line and off on the exit line. Also you need to overlap the start and end point where you enter the part. CNC machines are like a car, you can't turn 90 degree's left at 40 MPH without slowing down first. A CNC has acceleration and deceleration in the machine parameters that tell it to slow down when it gets ready to take a turn and then speed back up after it makes the turn. As a result it never "perfectly" reaches the programmed point, there may be .0005 - .002 or more error depending on the machine condition, how the parameters are set, how backlash compensation is set as so on.
You do not want to use exact positioning control, it will slow you down and also tend to leave dwell marks on the part and possible gouges in the corners.
Hope this is of some help.

[SIG]

Try to put two "blind blocks" between the commands.

I 'am going to try it tomorrow morning.

Thanks for your suggestion.