Cutter comp errors with X5

[Bob W.]

With X5 I am getting errors at the machine that cutter comp is not being canceled after helical toolpaths. When the operation is posted individually it works fine but when the whole program is posted I get the error. It is repeatable and I was curious if anyone else is running into this. Of course the file is 50+ megs so sending it in is a real hassle.

[gcode]

Helix mill?

[Bob W.]

Right, the helix option under circle mill. After changing my toolpath to circle mill it worked fine.

[gcode]

I found this and reported it as a bug late in the beta cycle.

The response was that it was an enhancement to prevent gouges.

In the past you got a G41 (Comp on) and G40 (comp off) with each hole.

Now you get a G41 (comp on) for the first hole and a G40 comp off on the last hole with nothing in between.

I tried to explain that many (most ???) controls cannot rapid with cutter comp active and will not run this code.

 

Some will alarm out like yours did, some will rapid into the stock on entry to the 2nd hole. some will get lost

and mangle your part and some will run it properly.

 

If someone was getting gouges with helix mill/wear comp they weren't using the tool path properly.

In X thru X4 MU3 all you had to do was check "start at center" and set the lead-in/out arc to 90 degrees

and you'd get good code all day long.

 

Of couse if the tool was .05" smaller than the hole and you enter .100 comp at the control

bad things will happen, but that is not Mastercam's fault.

 

At my shop I have four machines that will run this code, 6 that will alarm out

and one that does a suicide dive into the stock.. Since I never know where a job will

wind up, I've lost a really nice tool path cause I can't safely use it.

 

In my view they have broken a really nice tool path.

At the moment the only workaround is to make a separate tool path for each hole, manually enter

G41 /G40 at the appropriate points in the posted code or don't use cutter comp.

 

There is no need to send in the whole 50 meg tool path.

Make a simple file with several holes, include it and the posted code in an email to [email protected]

 

 

Hopefully we can get this "enhancement" undone for MU1.

[Bob W.]

Thanks for the great explanation. It is a real bummer because I used the helix bore all the time. Now I have to go back and change everything from a helical bore to circle mill and I have already had to do it four times today. Unfortunately I always find out at the machine so it is even more tedious. I guess I will get good at spotting it in the future.

[gcode]

I've been putting the G41's and G40's in by hand.

Its very easy, especially if you've got Cimco Edit or NCplot to backplot the gcode as you do it.

Please send in a bug report. It make take some noise to get this "enhancement" reversed.

[Superman]

I was taught never to rapid between contours with comp ON.

 

If I was using "In Control" comp, my "rapid to point" can be anywhere in a radius that I have in the control for that tool ( depends on the "from where point", and if it didn't alarm out )

To me, this is dangerous code

 

a patch must/should be issued, NOT an MU release

[Bob W.]

UGH! They changed the way ramping toolpaths handle cutter comp as well, didn't they? In the past cutter comp was only enabled on the finishing pass. Now it looks as though cutter comp is active during the roughing pass too, and ramping doesn't usually lead out during the roughing pass. This is all going to cost a lot of wasted time as I am getting error messages at my machine on proven programs. Now I get to go back and change ramp toolpaths to 2D contour...

[gcode]

I was taught never to rapid between contours with comp ON.

 

 

EXACTLY!!

our newer machines with Fanuc 15i controls handle this without problems

the older machines do not ..

[Guest]

OK, so what am I missing.

 

Made a couple quick toolpaths, one of them is a helix bore with 2 locations, posted everything out, got no error and a G41/G40 at each position

 

N152 T3 M6
N154 G0 G90 G54 X-.9111 Y.5343 A0. S1069 M3
N156 G43 H3 Z.25
N158 Z.1
N160 G1 Z0. F15.
N162 G41 D3 Y.7843 F25.  <<<<<<------on
N164 X-.8464 Y1.0258
N166 G3 X-.9111 Y1.0343 I-.0647 J-.2415
N168 X-1.4111 Y.5343 Z-.0313 I0. J-.5
N170 X-.9111 Y.0343 Z-.0625 I.5 J0.
N172 X-.4111 Y.5343 Z-.0938 I0. J.5
N174 X-.9111 Y1.0343 Z-.125 I-.5 J0.
N176 X-1.4111 Y.5343 Z-.1563 I0. J-.5
N178 X-.9111 Y.0343 Z-.1875 I.5 J0.
N180 X-.4111 Y.5343 Z-.2188 I0. J.5
N182 X-.9111 Y1.0343 Z-.25 I-.5 J0.
N184 X-1.4111 Y.5343 Z-.2813 I0. J-.5
N186 X-.9111 Y.0343 Z-.3125 I.5 J0.
N188 X-.4111 Y.5343 Z-.3438 I0. J.5
N190 X-.9111 Y1.0343 Z-.375 I-.5 J0.
N192 X-1.4111 Y.5343 Z-.4063 I0. J-.5
N194 X-.9111 Y.0343 Z-.4375 I.5 J0.
N196 X-.4111 Y.5343 Z-.4688 I0. J.5
N198 X-.9111 Y1.0343 Z-.5 I-.5 J0.
N200 X-1.4111 Y.5343 I0. J-.5 F7.5
N202 X-.9111 Y.0343 I.5 J0.
N204 X-.4111 Y.5343 I0. J.5
N206 X-.9111 Y1.0343 I-.5 J0.
N208 X-.9758 Y1.0258 I0. J-.25
N210 G1 G40 X-.9111 Y.5343   <<<<-----Off
N212 G0 Z.25
N214 X2.0294 Y2.7897
N216 Z.1
N218 G1 Z0. F15.
N220 G41 D3 Y3.0397 F25.   <<<--- on
N222 X2.0941 Y3.2812
N224 G3 X2.0294 Y3.2897 I-.0647 J-.2415
N226 X1.5294 Y2.7897 Z-.0313 I0. J-.5
N228 X2.0294 Y2.2897 Z-.0625 I.5 J0.
N230 X2.5294 Y2.7897 Z-.0938 I0. J.5
N232 X2.0294 Y3.2897 Z-.125 I-.5 J0.
N234 X1.5294 Y2.7897 Z-.1563 I0. J-.5
N236 X2.0294 Y2.2897 Z-.1875 I.5 J0.
N238 X2.5294 Y2.7897 Z-.2188 I0. J.5
N240 X2.0294 Y3.2897 Z-.25 I-.5 J0.
N242 X1.5294 Y2.7897 Z-.2813 I0. J-.5
N244 X2.0294 Y2.2897 Z-.3125 I.5 J0.
N246 X2.5294 Y2.7897 Z-.3438 I0. J.5
N248 X2.0294 Y3.2897 Z-.375 I-.5 J0.
N250 X1.5294 Y2.7897 Z-.4063 I0. J-.5
N252 X2.0294 Y2.2897 Z-.4375 I.5 J0.
N254 X2.5294 Y2.7897 Z-.4688 I0. J.5
N256 X2.0294 Y3.2897 Z-.5 I-.5 J0.
N258 X1.5294 Y2.7897 I0. J-.5 F7.5
N260 X2.0294 Y2.2897 I.5 J0.
N262 X2.5294 Y2.7897 I0. J.5
N264 X2.0294 Y3.2897 I-.5 J0.
N266 X1.9647 Y3.2812 I0. J-.25
N268 G1 G40 X2.0294 Y2.7897  <----Off
N270 G0 Z.25
N272 M5
N274 G91 G28 Z0.
N276 A0.
N278 M01

 

I used the standard MPFAN that installs with X5

[Guest SAIPEM]

I found this and reported it as a bug late in the beta cycle.

The response was that it was an enhancement to prevent gouges.

In the past you got a G41 (Comp on) and G40 (comp off) with each hole.

Now you get a G41 (comp on) for the first hole and a G40 comp off on the last hole with nothing in between.

I tried to explain that many (most ???) controls cannot rapid with cutter comp active and will not run this code.

 

Some will alarm out like yours did, some will rapid into the stock on entry to the 2nd hole. some will get lost

and mangle your part and some will run it properly.

 

If someone was getting gouges with helix mill/wear comp they weren't using the tool path properly.

In X thru X4 MU3 all you had to do was check "start at center" and set the lead-in/out arc to 90 degrees

and you'd get good code all day long.

 

Of couse if the tool was .05" smaller than the hole and you enter .100 comp at the control

bad things will happen, but that is not Mastercam's fault.

 

At my shop I have four machines that will run this code, 6 that will alarm out

and one that does a suicide dive into the stock.. Since I never know where a job will

wind up, I've lost a really nice tool path cause I can't safely use it.

 

In my view they have broken a really nice tool path.

At the moment the only workaround is to make a separate tool path for each hole, manually enter

G41 /G40 at the appropriate points in the posted code or don't use cutter comp.

 

There is no need to send in the whole 50 meg tool path.

Make a simple file with several holes, include it and the posted code in an email to [email protected]

 

 

Hopefully we can get this "enhancement" undone for MU1.

 

The person from CNC who said this was an enhancement has never machined anything in their life.

They shouldn't be allowed anywhere near the Cycle Start button.

 

It is truly SAD when a CAM company doesn't have ANYONE in development who understands the proper application of Cutter Radius Compensation.

It should be obvious to anyone who has actually cut metal on a machine that you should turn comp on and then off for each hole.

 

Whoever approved this "enhancement" should be fired!

[gcode]

3 holes 3 diffent sizes selected as enities

toolpath is circle mill/helix with wear comp turned on

slightly modified X4 mpmaster post upgraded to X5

stock mpfan posts yeild the same results

 

(T239 - 1/2 FLAT ENDMILL )

 

 

G00 G17 G20 G40 G80 G90

G91 G28 Z0.

N1 T239 M06 ( 1/2 FLAT ENDMILL)

G00 G17 G90 G54 X-1.1521 Y.6618 S1069 M03

G43 H239 Z1.

Z.1

G94 G01 Z0. F6.42

G41 D239 X-.9021 Y.4118 <------ comp on

G03 X-.6521 Y.6618 I0. J.25

X-.6521 Y.6618 Z-.25 I-.5 J0.

X-.6521 Y.6618 Z-.5 I-.5 J0.

X-.6521 Y.6618 I-.5 J0. F1.93

X-.9021 Y.9118 I-.25 J0.

G01 X-1.1521 Y.6618 <----- no comp off

G00 Z1.

X1.7316 Y.0549

Z.1

G01 Z0. F6.42

X1.8566 Y-.0701 <--- no comp on

G03 X1.9815 Y.0549 I0. J.125

X1.9815 Y.0549 Z-.25 I-.25 J0.

X1.9815 Y.0549 Z-.5 I-.25 J0.

X1.9815 Y.0549 I-.25 J0. F1.93

X1.8565 Y.1799 I-.125 J0.

G01 X1.7316 Y.0549 <---- no comp off

G00 Z1.

X-.576 Y-1.3578

Z.1

G01 Z0. F6.42

X-.187 Y-1.7468 <--- no comp on

G03 X.202 Y-1.3578 I0. J.389

X.202 Y-1.3578 Z-.25 I-.778 J0.

X.202 Y-1.3578 Z-.5 I-.778 J0.

X.202 Y-1.3578 I-.778 J0. F1.93

X-.187 Y-.9688 I-.389 J0.

G01 X-.576 Y-1.3578

G00 Z1.

G40 M05 <------ comp offf

G91 G28 Z0.

G28 Y0.

G90

M30

%

 

The new Ikegias HBM's with Fanuc 15I's I program have no trouble with this

some of our older machines do very bad things with this code.

[Guest]

OK, working with Tom, I got it.

 

If you use acrs the output is bad. if you use points, the output is good.

 

So the current work around would be to use points as geometry for Helix Bore.

 

I agree, THAT HAS to be fixed.

 

THat does not function the same as it did in X4.

 

If it was supposed to be that way, then both methods should output the same if you ask me.

[gcode]

weird

I get the same (bad) results whether I use points. points at center of arc or arcs.

I'm using a stock 3X VMC mpfan post for the tests.

[Dave Ball]

This came up today during an X5 Rollout so I tried to reproduce it and I also get the same (BAD) results using arcs center points or just points.

[Guest]

This came up today during an X5 Rollout so I tried to reproduce it and I also get the same (BAD) results using arcs center points or just points.

 

Did you try turning on Perpendicular entry?

[gcode]

If you check

"Start at Center"

and

"Perpendicular Entry"

it will post properly..

but this still needs to be fixed..

It worked fine for years..

IMO this was a "fix" for a non existent problem

 

 

[Dave Ball]

Ok so it seems "Perpendicular Entry" is the key, with it set, I get good code regardless of "Start at Center" setting or type of geometry selected. Thanks for the tips. IMO this now needs a "fix"

[Chris Bell CNC Software]

Hi guys,

 

This has been logged as bug number cnc00086684. Thanks for the help.

[gcode]

Thanks Chris

 

 

[Glenn Bouman]

I tried a couple samples and sometimes it would put the G41/G42 on an arc move. This should never be allowed.

 

There is a setting in the Control Def for this but it is only read by the post not when generating the toolpath.

 

Take this into account when you make the fix to the software

[gcode]

The In House mpmaster will yell at you and post an M0 if you have a G41/G42 on an arc move.

A very useful feature IMO