Mycenter cutter comp problem

[Dualkit]

I have a Yasnac MX3 controller on a Kitamura Mycenter

I have a problem with it cutting too short of a path when using cutter comp G41 or G42 during a radius. I included the program which I am pretty sure is not an issue. I am just rounding the end of a 1" wide 1/2 thick piece if steel. Here is what happens. It is programed for a .520 radius with a compensation offset on D15 of .310, which should in fact create an actual machine position movement of 1.660 (.830 radius) along the Y axis, the machine moves a grand total of 1.5692. I did this cutting air so tool pressure is a non issue. I set the cutter comp on offset D15 to .000 and the thing moved 1.040 on Y (.520 radius) like it should. I also tried changing the cutter comp value from .310 to .320 expecting an extra .020 on the Y axis during the radius and I got an extra .0171. The X axis appears to behave
itself. I have had this machine for 3 months and still debugging it. Is there a parameter that may be wrong? Thanks in advance for any suggestions.

G91G28Z0
G20
G17G40G80G90
G53G0X-3.Y-3.
T5
M6
(1/2 EM)
G54G90G0X1.2Y-1.2S3000M03
G44
G41G17D15
G00X1.2Y-1.2
G1X.52Y-.52F20.0
G0Z1.0H5
Z.5M08
G1Z.1F50.0
G1Z-.6F20.0
G2X.52Y.52R.520F2.0
G1Z.1F20.0
G0Z1.0
G0Z2.0
G49
G40D0
M5
G91G28Z0
G53G0X-8.0Y-3.
M30

[Fred the thread]

Hi there,
when in G41 / G42, control looks ahead and considers next move (buffer).
If the next move is less than the radius value (comensation amount), then the control looks ahead again to consider the move after that.
It will always keep the cutter on the perceived work surface, which means that if the move after the radius move (G02) is not tangential to the G02 move for at least the amount of the the cutter comp. then the control has to stop short of that position, so it can make the next move after that and keep the cutter from violating what is thinks is the part surface. That is your N17.
(You part-program below is modified with line numbers in order to show you where the changes are.) Add F word (feedrate value ) to N9, or there wil be an alarm. Change the value in N17 to G1X1.0 and the problem will go away.



N1G91G28Z0
N2G20
N3G17G40G80G90
N4G53G0X-3.Y-3.
N5T5
N6M6
(1/2 EM)
N7G54G90G0X1.2Y-1.2S3000M03
N8G44
N9G41G17D15F10.0
N10G00X1.2Y-1.2
N11G1X.52Y-.52F20.0
N12G0Z1.0H5
N13Z.5M08
N14G1Z.1F50.0
N15G1Z-.6F20.0
N16G2X.52Y.52R.520F2.0
N17G1X1.0F20.0
N18G0Z1.0
N19G0Z2.0
N20G49
N21G40D0
N22M5
N23G91G28Z0
N24G53G0X-8.0Y-3.
N25M30

Good luck,
Fred the thread

[dcoupar]

I'm surprised it runs at all, given that you have 4 uncompensated blocks (Z moves) after the G41 command.

I've never had a problem with cutter comp as long as I turn it on with a linear move to the start of the profile, and turn it off with a linear move away from the end.

Also, just curious: why a 0.31 comp for a 0.25 radius tool?

Try this:

G91G28Z0
G20
G17G40G80G90
G53G0X-3.Y-3.
T5
M6
(1/2 EM)
G54G90G0X0.52Y-1.S3000M03
G44
G0Z1.0H5
Z0.5M08
G1G41Y-0.52D15F20.
Z-0.6
G2Y0.52R0.52F2.0
G0Z2.0
G40Y1.
G49M5
G91G28Z0
G53X-8.0Y-3.0
M30