Lathe Crash!! bug? or not?

[Hymen]

My post developer and I have come across a situation where MCam will crash my machine but this does not show in verify or in backplot.

When running canned rough and finish turning. G71 and G70 codes respectively.

sample code:

code:

---

 (TOOL - 1 OFFSET - 1)

( FACE )

G0 T0101

G18

G97 S890 M03

G0 G54 X2.575 Z.03

G50 S2500

G96 S600

G99 G1 X-.0625 F.015

G0 Z.13

X2.575

Z0.

G1 X-.0625

G0 Z.1

( ROUGH )

X2.375

X2.475 Z.1535

X2.375 Z.1035<<<<<<<<<Canned rough start

G71 U.1 R.02

G71 P100 Q102 U.03 W.002 F.015

N100 G0 G42 X1.5286 S600

G1 Z.0035

X1.7285 Z0.

G3 X1.7485 Z-.01 R.01

G1 Z-.625

Z-.8716

G2 X1.9189 Z-.9901 R.125

G3 X1.9325 Z-.9996 R.01

G1 Z-1.1797

Z-1.2422

N102 G40 X2.375

G0 Z.1035<<<<Canned fin. start with below x value

( FINISH )

G18

X1.5286<<<<<<<<<<Heres the crash #

G70 P100 Q102

G28 U0. V0. W0. M05

T0100

M01

---

explained:

Knowing that canned cycles return to its original start position, the G71 start position is outside the stock boundry. This is OK and backplots/ verifies accordingly. But..

The G70 start position is inside that boundry in the X-axis. So on the return path, after completeing the N102 line it will rapid through the end of the part to the values specified before the G70 callout. This is not shown in the backplotter or in the verification tool. What is shown is the tool going to the N102 line them going home, which is not the case for the 15 Lathes we have here, which return to the values specifed previous to the call out of the G70.

 

I am posting this because I am curious to know if it is the way we have the machines configured here or, if not... well, I guess I'd like to say I'm suprised this has gotten so far without being caught. Maybe no one uses canned finish! Anyone? Anyone?

There is no simple solution on the post side to this issue! Take a shot if you have time I'd like to see it.

[High Sierra Plastics]

Hyman,

 

Either O.D. cutting or when it starts or when I'm at the end of a boring cycle when I edit my post, I have a situation were the machine could crash. I got so use to it that I just go through the program manually each time to avoid the crashes. It's been like this for as long as I can remember. (Early 90's, version 3 or so). I think you can set up a point to rapid to each time you begin or end the cycle.

 

Henri

[crazy^millman]

I am not sure how you are setting up your toolpaths but I have found making a manunal lead on and lead off for canned cycles does not cuase this problem for the lathe posting and finish canned cycles. I normally copy my toolpath to a seperate level then add my .05 to .1 move which is a line most times to make what I want work and give good clean code for the roughing and finishing cycle. To fully explain this I make a .1 Z direction line from the face then make a .05 X direction line to make sure I get prooper clearence and no problems with my canned cycle. I however like not using the canned cycles, but it seems alot of people running Fanuc and Fanuc style machines love them so adapt what you can to make it work within the parameters of what you got.

[?Mark]

quote:

---

I however like not using the canned

---

+1

In a dozen plus years here I've never seen a lathe guys use one...

[Tim Simmermon]

We just had a crash by us today because of something like this. The Fanuc control likes to have the same starting point for the rough and finish cycle. These need to be set using the approach points.

 

In a situation like this, canned cycles can be dangerous, but they allow for very simple modification on the shop floor.

[gcode]

I do my best to stay away from canned cycles

unless I am personally going to set up the machine.

 

Depending on how various parameters are set

the same gcode could run fine or lay the turret on the floor.

 

My day job doesn't use them cause we have a dozen different lathes with a dozen differnt controls

and canned cycles would be an unmanageable can of worms.

 

I will not deliver canned cycles when I contract program, because there are just too many variables. Backplot, verify and even gcode verification will not tell you the whole story where canned cycles are concerned.

[DavidB]

We run canned roughing cycles here always and I've never had a problem.We are using Okuma and Fanuc controllers.

 

There so easy for the guys to adjust depth of cut, feed rates and stock left in X and Z.

 

I find it interesting that you guys don't use them.

 

Each to there own

[chris m]

I use canned cycles all of the time, but never use the canned finish. There is a known bug in canned cycle posting for V9 that CNC Software fixed for me. The bug was affecting the posting [actually non-posting] of retract and reference point blocks. You should contact Roger Martin or somebody over at CNC, or Steve Biehl at Services 4 Automation [my reseller, who helped me sort out the problem] to see if that may be involved with your problem. The post fix was pretty simple, as I recall.

 

C

[chris m]

Hymen; you have mail

[Guest]

Hymen broken???

 

[Hymen]

This has been submitted to QC and we've also added a request to put in an additional leadin line (add line) so Mcam leaves a safe distance in Z for rapid positioning when starting the canned cycle using a style described below.

Everything we do here is canned. Simple to read edit and change for the various materials and sizes we run here. Inconels monels steels HY-80... With the canned rough and finish you edit one block of code and it adjusts your rough and finish...Easy!!! Short runs 1-10 pcs. Large parts no smaller than 3". 15 machines all with Fanuc controls.

Here's the example:

When starting a part from the face on a radius you cannot have a tapered lead in to roll any burrs off the face or to have a nice blend that has efficiant/safe code. I will typically use .100 at 2 deg lead in and off for OD and ID work. On the face that works out to a Z start position of Z.0035, which is just too close to be rapiding at. The only current fix for this is to add geometry to your part to simulate the lead in then use (add a line .0965 @ 0 deg). Which gives you a Z start position of .1 The "extend start of contour" is useless when starting on a radius. Previously I have only roughed in canned, not chaining the radius and used extend start point, then finished longhand because of this. Canned rough and finish very simple and user friendly.

Sure I could start at centerline, or at the ID, and cut up through the radius but at low SFM, Feed and large diameters this adds a lot of time to the cycle, not to mention cutting air.

 

Ehh?

Broken?

Maybe popped?

I think it time to change my name.

[Hymen]

Really all CNC Software has to do is have the Canned finish pick the same line the rougher draws its start point info from in the NCI. But is it that easy? I don't know? Buffering these Numbers doesn't really work either if you are using multiple canned roughh cycles as I do.

So for the time being its create additional geometry or hand edit.

[Hymen]

Is there a master list for bugs in X2?

 

Heres a lead in bug.

I get a 10" value in X when I use a .0965 @ 0 deg. add a line to a 2 deg .1 long geometry leadin.

[Bruce Gibson]

What size is the tool nose rad? I think if it is the same as or larger than the lead in/out you run into this problem. Try changing the length of the lead in to .15 and see if this happens. One way to fix it is to draw both lead in lines and turn off the add a line...

Can you upload the file?

[Hymen]

CNMG 432 is being used.

Thanks Bruce.

I just want to point out that there are problems with this.

At .1 it runs fine.

At .0963 it's ok

.0964 bad

.0965 bad

.0966 OK

.0965 just happens to be the lead I want to use as it gives me a Z canned start position of .1. The geometry lead in I use is .1 long at 88 deg.

.1 gives me a lead of .1035.

If I change my lead by a deg to 3 deg and use .0948 I have have no problems and still get the .1 Z start position I want.

I know this is nothing! But in reallity it is something and so I just wanted to point this out. Trying to draw as much attention as possible to the Lathe aspect of MCX2

[Hymen]

Can someone from CNC Software come forth and at least tease me in to thinking canned cycles are being addressed sometime in the near future.

I've sent items to QC and have not gotten a confirmation of receipt....

 

There is a silly cycle going on here.

Canned cycles don't work 100% out of the box therefore no one uses them, so no one complains about them so no fixes them.

 

A problem since V9 these will never go away until more of us that actually use canned cycles complain.

I found more problems when splitting canned cycles and the output start position these hit the floor today and I sure am glad a knowledgeable guy was the one to run it!

[DavidB]

Hymen can you email me your file?

[Hymen]

You ever get that file?

[Hymen]

bump

[gcode]

Hymen,

have you sent this stuff to [email protected]

That is the best course if you want Mastercam

to look at it.

[Hymen]

Yes I have.

This is one where I don't get a confirmation email.

Seems nobody wants to tackle these issues there.

[Thee Dragracer1951]

I also have never used canned turning cycles as I have different controls on my machines. I personally never saw the need for them except to be able to write code at the machine. Every time I have sent an email to QC, I have gotten a response. Just curious, because I am sure that you have, but,have you also sent this to your reseller. I usually do that first. Splain to them that you are trying to get QC's attention in the matter.

[Hymen]

The guy who writes post for my reseller sent it in and he did not get a response. He works for my reseller. And for most of the other issues I've sent in got responses and repair control #'s attached to them, just not any of the 3 I sent in about canned cycles. Not complaining here just making a statement.