Rant: work offsets in X4

[Bucky Cornstarch]

Can anyone tell me if there is a way to set a default in Mastercam X4 so a new operation uses the same work offset as the previous operation?

 

Here's the situation: I opened up a program I was working on yesterday so I could add an operation. (chamfer the outside) The previous operations were using work offset #5 (G59). On the added operation, Mastercam defaulted to work offset #0. Of course, I didn't notice, and since my work offset #0 is about 3 inches below work offset #5, I now have a wasted toolholder and a nice gouge in one of my Kurt doublethrows. I'm hoping there is no spindle damage.

 

Yes, I know I should have double-checked the code before I ran it, but this shouldn't have happened. And, (flame suit on) I never had this issue with V9.

 

I've checked through the System configuration settings and can't seem to find anything. Maybe something I can set in the machine or control definitions? While I know it is late on a Good Friday, any help would be appreciated.

 

Thanks,

Jim

[Dave.L]

New operations are created based on the current WCS you have active in view manager and that's where the workoffset is located.

 

It's just something you need to be aware of and watch for.

 

I have my operations manager show the workoffset and I have setup my post so the workoffset numbers match (instead of trying to remember 0 = 54

[Bucky Cornstarch]

Makes sense Dave, thanks. I'll need to start paying more attention to the WCS.

 

(I could never have my post like yours; too many years of 0=54, 1=55, etc. Besides, how do you handle G54.1 P21?)

[Dave.L]

quote:

---

(I could never have my post like yours; too many years of 0=54, 1=55, etc. Besides, how do you handle G54.1 P21?)

---

Jim,

 

It's a piece of cake and you would like it much better, trust me.

 

I am sure the pro post mods could figure a way to handle G54 thru G59 and G54.1 P1 thru P48 but what I did is simple.

 

We don't use G54 thru G59 anymore. We only use G54.1 P1 thru P48 (48 offsets are enough for us).

 

So, 1 = G54.1 P1, 2 = G54.1 P2, 48 = G54.1 P48

 

This also works well since OP1 is G54.1 P1, OP 2 is G54.1 P2, and so on.

 

It works well for us. If you want to try it, email me and I will send you the post block code to edit.

[gcode]

This is one of the reason I use mpmaster.

Set mi9 = 1 and forget about it

 

# mi9 - Lock on First WCS - Set in first operation

# 0 = No

# 1 = Yes

 

You can set this in the control def so its on by default.

[Bucky Cornstarch]

gcode, thanks, will look into it Monday morning. (I use a modified version of mpmaster.)

 

Dave, I'll send you an email. BTW, that makes perfect sense. I use G54.1 P# for everything (and leave the offsets in the machine for specific jobs) and G54-G59 for "oddball" jobs. Unfortunately, this crash (I hate that word ) happened on an older VMC that I use for prototyping and tooling and the control only has G54-G59.

 

I think my biggest problem is that I am really pissed at myself for allowing this to happen. I haven't crashed a machine in years, and, as the boss, I'm always telling my operators to watch each tool as it goes to each work offset. Of course, I didn't do that this time.

 

(I did show my second shift operator my booboo. He laughed at me )

 

After a nice dinner and a glass of Zinfandel, I am over it. I do find myself wondering why I am checking the Mastercam forum at 9:00 on a Friday night, however.

 

Thanks again,

Jim

[Chris Rizzo]

I prefer the direct offset entry as well. 54=54, 55=55.

 

For the 54.xx i just add a zero. So for g54.34, I enter 340 in my part file.

[Dave.L]

quote:

---

I use G54.1 P# for everything (and leave the offsets in the machine for specific jobs) and G54-G59 for "oddball" jobs.

---

Jim, another option instead of leaving the offsets in the machine would be to add them to your program since it sounds like your workholding is in a predictable location.

 

We use pallatized systems that are very accurate and we make models for our setups. So, we don't touch off any offsets, they are all loaded via G10 commands.

 

You could add G10 commands to you programs to do the same thing, it works very well.

 

quote:

---

I do find myself wondering why I am checking the Mastercam forum at 9:00 on a Friday night, however.

---

That's what us technical junkies do

[Newbeeee™]

+1 to the G10.

We also use it for diameter offset as well.

It's a lot neater storing datums and offsets in the program, and less chance of slykdexic fingers entering the info into the control...