Mastercam just bit me BIGTIME!

[Bob W.]

This is not the first time this has happened, but Mastercam randomly changed work offsets mid program on a program that had been previously run and proven. I had to make a few minor modifications to the program and I reposted with only slight changes (depths, etc...). It switched from a G54 to a G55 on a contour operation that was between a tapping operation and another contour operation. In NO OTHER LOCATION in this entire Mastercam file is there a work offset other than a G54 and this change was only on this particular operation, which was completely untouched. I nearly scrapped this mold because of it and I will have to modify multiple pieces to make it work.

 

After the first time (18 months ago?) I was shocked and this prompted me to start dry running every file at the machine before running. The problem in this instance was that the G54 and G55 offsets were very close so I missed it. It is also a 6 Meg file and I didn't stand there and watch every detail. I am so angry I can hardly see straight. Minor bugs are one thing, although very annoying. This just leaves me speechless... Anyone else run across this?

[BenK]

link

 

This was just talked about. My suggestion is to go through and check all of your work offsets just to make sure.

[gcode]

from the generic 5X post

 

I always set "use_frst_wcs " to "yes" unless I need to change work offset in a file.

 

#Work offsets

workofs$ : -1 #Initialize work offset

force_wcs : yes$ #Force WCS output at every toolchange?

use_frst_wcs : yes$ #Use only the first WCS read and ignore all others in NCI

[Bob W.]

gcode, that is exactly how I have my 5-axis post set up, but this was a 3 axis program. I frequently post out to multiple work offsets for patterned programs so limiting the work offset for 3-axis would be pretty inconvenient.

 

BenK, there aren'y any offsets to check. G54 was the only offset used in the entire file.

 

Here is some additional information:

 

This program was written entirely in X4 MU2 and the post is based on MP11.

 

Also, given the nature of this I would definitly call it a bug. I posted this program IN ITS ENTIRETY and it ran fine. Then I reposted again, full program, and G55 mysteriously appears. Any chance of getting a confirmation that this issues has or hasn't been fixed in the next release? Its not like people are crashing their machines over it (sarcasm).

[Joe788]

Anybody know how to make the post spit out a list of any/all work offsets used in a program?

[gcode]

quote:

---

mi9 - Lock on First WCS - Set in first operation

# 0 = No

# 1 = Yes

---

one of the reasons I use mpmaster for 3 and 4X

work..

 

to be safe you have to set this in every op

If you set it in OP1 and post the whole file

you'll be fine... but

if you post a couple of OPs in the middle of a

file, you may get burned if you haven't set mi9=1

in ALL ops

[Bob W.]

I think at this point I will alter my post to make this the default (mi9 = 1).

[gcode]

quote:

---

I think at this point I will alter my post to make this the default (mi9 = 1).

---

this is done in the control def on the Misc page

now

[Ron Branch @ Verisurf]

quote:

---

Anybody know how to make the post spit out a list of any/all work offsets used in a program?

---

Yes you will need to use buffers.

 

HTH

[Justin Beebe at Folsom Tool]

One way to check which can be kind of tedious is to post your program then before you send it to the machine search for G5. Then keep hitting search next and you will find every fixture offset in your program one at a time. Like I said kind of tedious but better than crashing a machine or scrapping a part. I have all my multi axis post set to universally lock onto G54 so I have to edit the post if I want to use another fixture offset. This is for the exact reason gcode is talking about. "If you post a couple of ops in the middle of a file you may get burnned". Not if your post is set to universally lock onto G54. My 3-axis posts are set up like yours because I frequently use multiple fixture offsets in a single program.

[Dave.L]

Justin, I have not had an issue but I do the same as you. I search my code for workoffsets and tap cycles. It only takes a few minutes and it just makes me feel comfortable.

[YoDoug®]

quote:

---

Anybody know how to make the post spit out a list of any/all work offsets used in a program?

---

The X+ set up sheet has an option to list work offsets for each operation.

[gcode]

There is a thrid way.. a bullet proof way..

but Mastercam will scream at you..

Put a "0" in EVERY toolplane you use in a toolpath. You will get yelled at about

duplicate workoffsets but all your output will be G54.

This is how I do it if I need multiple offsets

too. Every toolplane is correctly defined and I deal with the multiple offset yells.

Some of my programs have 10 to 15 work offsets.

When using this many I also label them and use mpmaster's ability to output workoffset labels.

 

quote:

---

if rot_on_x & stoolplname <> snull, pbld, n$, pspc, scomm_str, "TOOLPLANE NAME - ", stoolplname, scomm_end, e$

 

if rot_on_x & stoolplcomm <> snull, pbld, n$, pspc, scomm_str, "TOOLPLANE COMMENT - ", stoolplcomm, scomm_end, e$

---

That gives me and the operator a clue as to what to look for and a warning if I've made a mistake.

 

the system isn't foolproof by any means, but the tools are there to prevent this kind of thing.

 

I thumped a part a couple of weeks ago, but it wasn't Mastercam's fault.

I was in a hurry and didn't set up the work offsets properly.

It was a short program and I intended to edit

one G54 to G55. They didn't get around to needing the file for a couple of days and then wanted it for a differnt machine.

I forgot about the hand edit when I reposted.

Luckily it wasn't a crash but it sure jacked a

threaded hole up

That's the danger of relying on hand edits.

I try to do the work to get the output right,

but when we get in a hurry....

[Chris Rizzo]

You can stop the yelling in control def > Work System > Tplane during automatic work offset number creation and set that to NONE.

[gcode]

I'll try that..

I've never messed with this setting.

I wonder if it is what causes the toolplanes

to increment up by 1 if you run everything in default state??

[RandleXX]

OH Yeah!! The mysterious offset bug!! This has got me before also. Now I always do a quick printout using the X+ set-up sheet which lets me quickly scan every operation for the correct offsets.

 

All it takes is one bad offset and the part is SCRAP!!!

[Jayson Kramer]

Bullet bob is this a haas machine?

[Cad-Camr]

I side with Justin we have a protocol that we use that involves certain program checks on critical programs. We do searches in Mcam Editor to verify workoffsets, tool offsets. Also If a workoffset is not being used it is set to zero at the machine. Another safety protocol we use is no hand editing is allowed.

[Bob W.]

Jay, It is a Haas machine.

[Bob W.]

I guess I will have to implement those checks as well. This was also missed by Predator NC verification. I had a G54 offset typed in, but no G55. It didn't alarm or anything that the G55 was not set, it simply ran the simulation showing no issues. It is a PITA that I will need to double check every detail about these programs that Mastercam is posting out. It is really pathetic that it can't post the right offset 100% of the time. Of course, when this bug strikes it is never a cheap part I am working on...

[Cad-Camr]

Unfotunatly there is no forgivness in what we do. 99 things right and 1 thing wrong is often scrap. Mastercam is not perfect. That is why it still takes VERY highly skilled individuals to make everything come out right the first time.

[Jayson Kramer]

Bullet bob ,

This how my Haas posts out it tells me what offsets it uses and from the stock setup the size of stock.

 

Example:

%

O0100 ( SAMPLE REV: )

( SAMPLE )

(MACHINE TOOL : HAAS VMC )

(DATE - 19-04-10 )

(TIME - 11:33 )

(*)

(MATERIAL: )

(STOCK SIZE: X = 10.8062 Y = 7.6493 Z = 1.172 )

(HOME POSTION COORIDNATES ARE THE FOLLOWING)

(X= )

(Y= )

(Z= TOP OF PART)

(*)

( TOOL - 1 3" FACE MILL )

( TOOL - 2 3/8 DRILL )

(*)

(USING FIXTURE OFFSETS: G54 G55 G56 )

(*)

G20

G0 G17 G40 G49 G80 G90

T1 M6

G0 G90 G54 X-14.1062 Y-.7501 S2700 M3

G43 H1 Z2.25 M8

Z1.25

G1 Z1.2135 F30.

X1.8 F60.

Y-2.7998 F250.

X-12.6062 F60.

Y-4.8495 F250.

X1.8 F60.

 

Would this help you.

[Bob W.]

Jay, that looks great! How would I modify my post to get it to do that?

[Tim Johnson]

Another thing you can do is change every work offset Z in the machine so that if a bad offset code is called up it will overtravel in the opposite direction.

[Jayson Kramer]

Bullet bob does your haas have 4th on it?