cutter comp

[s0l0seven]

Hello,

I am having a problem with generating the right code for our boss 9.

If I do a contour with multiple passes while the compensation is set to the control it will give me code like this. I believe a lot of this is not needed and my machine dose not like the cuter comp going on/off and why the G0 is in there I don’t know. Can someone point me in the right direction in changing the post or do I have something wrong in the parameters.

N136 G0 Z.1 |

N138 G1 Z-.0689 F6.4 |

N140 G2 X0. Y-.9754 I0. J0. F.5 |

N142 G41 G2 X-.9754 Y0. I0. J0. | CC is on

N144 G2 X0. Y.9754 I0. J0. | .5 of ark swung why

N146 G40 G2 X.9754 Y0. I0. J0. |cc is off

N148 G0 | why is this in there

N150 G1 X.9004 |its repeated all over again

N152 G2 X0. Y-.9004 I0. J0. |

N154 G41 G2 X-.9004 Y0. I0. J0. |

N156 G2 X0. Y.9004 I0. J0. |

N158 G40 G2 X.9004 Y0. I0. J0. |

N160 G0

[bryan.davis]

This looks more like a problem with the operation than with the post, though the fragment of code youve given dosnt tell me enough about what you are trying to cut.

a few basic questions

1 what controller has your machine?

2 in the geometry section of your toolpath definition is there a single geometry element (ie a single chain) or multiple elements?

3 in the in/out definition have you tried set roll on to first pass only and roll off to last pass only?

4 what EXACTLY is the problem, does the machine stop due to incorrect geometry/parameters, doe it cut the part incorrectly, or is there a quality problem?

[s0l0seven]

1) Its a Bridgeport Boss 9

2) 1 chain one element

3) I am assuming you ment under lead in and lead out enter/exit on first/last depth cut only. Yes this dose help get rid of the G0. However my cuter comp still goes on and off and which seems to brake up the circle in to halves, half on half off.

4) The problem is that the Mastercam swings half the ark with the cuter comp on then shuts it off for the rest.

At the machine it would swing half the ark and then stop, and give you an error saying unspecified feed rate (or some thing like it).

I don’t know way but I think it was because it would have a line with G2 then a line with G0 then a line with a G1 with no Feed on that line.

Maybe???

I could e mail you the file if you wanted, its not completely dun though

Thank you

[bryan.davis]

your going to have to forgive my ignorance, but all bridgeports Ive used have either Fanuc or Heidenhein controllers, so Im assuming this is the case.

the code you show isnt Heidenhein language so Im going to assume that its fanuc/ISO

what post are you using?, have you tried the MPFAN post?

Generally speaking the unmolested MPFAN post is pretty bombproof, and should generate working NC code for 80% of ISO machines as it stands and 100% with a little tinkering.

Try using the MPFAN post and see what the code looks like, if it looks similarly faulty then the problem is definately in the operation.

You could send me a file but I would not be able to look at it untill next week

[s0l0seven]

Bridgeport now uses only Fanuc and Heidenhein.

But up to a few years ago they offered their own control too, for many years.

Like Boss 4 through Boss 10, SX 7, DX 32, BPMC, are just what I know of.

[bryan.davis]

Still the code is close enough to Fanuc that by testing the operation on the MPFAN post should provide valid information.

if the code looks correct then you have a choice of either adapting the MPFAN post to suit your needs of modify your BOSS post allong the lines of the MPFAN

[gstephens]

Problem 1: Mastercam v8 will NOT output a full circle. Period. Your post can be customized (A LOT) to make it happen, but it's most likely not worth it.

Problem 2: You ALWAYS, ALWAYS, ALWAYS have to use lead in/out LINES if you are using cutter comp (unless you happen to be using a Fadal machine) because the control will not pick up cutter comp on an arc.

[s0l0seven]

Well I fingered out the problem.

There was no G17 in the code.

Here I am thinking it should be model on startup, but the control wants to see the G17

------------

Hay G-man whets the theory on why Mastercam brakes up circles; that seams kind of stupid. Dose it do it in nine.

Hay G-man who said you were ever on??????????????

[ 01-02-2002: Message edited by: s0l0seven ]

[Phil Orenstein]

As one who used a DX-32 (the next generation after BOSS series) years back and had a lot of aggravation posting to Bridgeport's proprietary controls, I remember a particular idiosyncracy in the way their control interpolated circles. It may be a controller issue, not Mastercam as to why it breaks up your arcs and circles. Check your default G Codes for multi-quadrant circle input, whether it is On or Off and absolutely TURN IT OFF!

Hope this helps.

Phil

[gstephens]

quote:

---

Hay G-man whets the theory on why Mastercam brakes up circles; that seams kind of stupid. Dose it do it in nine.

---

Answer 1: No clue. Maybe PDG has some insight, although I'm not sure how long he's been around.

Answer 2: No comment.

[Allan Brown]

Not all machines can handle full arcs, and I think the Mastercam philosophy has always been to boil things down to the essentials, and at times to the lowest common denominator as far as code is concerned. For instance, a Circle Mill toolpath may be covered by custom cycles on certain machines (e.g. a G13 on a Haas), but the arcs and lines output long hand will run on all machines - it's way more flexible that way. We're all doing alright machining lines and half circle arcs.

--

If and when full arcs are implemented, we would certainly need some sort of switch in the post so that we could continue to post out 1/2 circle arcs for machines that can't handle full arcs. Something like this would be my suggestion:

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

[Guest CNC Apps Guy 1]

LOL @ Dave.

quote:

---

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

---

Hey PDG, why don't you guys put it in just like Dave says. Maybe it'll just work.