Plane offset question

[Greg_J]

Hello,

When I create a program using a 4th axis on a VMC and I'm using many different planes I need to make sure that the work offsets say 1 in the Plane Manager so that I don't get different work offsets for each plane; by default if I do nothing I will get G55, G56 etc. for as many planes as I use. 

 

Is there a way that I can force MC to always use G54 regardless of what plane I use with out changing the work offset in the Plane Manager every time I program a part?

 

 

Thanks for your input.

Greg

[crazy^millman]

Hello,

When I create a program using a 4th axis on a VMC and I'm using many different planes I need to make sure that the work offsets say 1 in the Plane Manager so that I don't get different work offsets for each plane; by default if I do nothing I will get G55, G56 etc. for as many planes as I use. 

 

Is there a way that I can force MC to always use G54 regardless of what plane I use with out changing the work offset in the Plane Manager every time I program a part?

 

 

Thanks for your input.

Greg

 

Mastercam file no, the post yes.

 

I forced myself to get in the habit of always updating them in the planes manager.

[Greg_J]

 

 

I forced myself to get in the habit of always updating them in the planes manager

 

I do too, if you miss one it can turn out real bad. (knock on wood nothing has happened yet) I always do a search after posting in Cimco for G55 -G59.

 

I have been finding that in the actual program in the Operations Manager not remembering in the Plane Manager is the issue, often under the Planes (WCS) tab the Work Offset is unchecked or it's grayed out then that's where I miss it.

 

Thanks for the help Ron.

[Reko]

I always do a search after posting in Cimco for G55 -G59.

+1

[SlaveCam]

Does anyone else dislike the "automatic" work offset numbering mechanism in plane manager? I don't want Mastercam to manage my work offsets by default so I always have to switch it to manual. This should be an option under settings.

[Newbeeee™]

Does anyone else dislike the "automatic" work offset numbering mechanism in plane manager? I don't want Mastercam to manage my work offsets by default so I always have to switch it to manual. This should be an option under settings.

Yup.

To repeat - this is a train crash waiting to happen.

You can change your post to disable it and enter 54 for G54 output, 55 for G55 output etc.

Do a search on here.

[JAMMAN]

Wow I have never had a problem with this, I just finished up a nasty 3 + 2 with 6 planes and never stepped out of G54. Perhaps my 2 5 axis posts are already hardwired for G54 only but I'm worried so now I'll check every time.

[jlw™]

I have been burnt by this several times.  It has also caused one crash in a 3ax VMC.  Coming from other softwares that only change it from G54 if I tell it to I had to really hammer in the habit to manage this in my plane manager.  I now have a habit of doing this every single creation.  It's like naming it, I just do it.

 

I know I can force it in the post but then I have to go undo it when I do want to use multiple offsets.  It would be so much better if the default was G54 then you had to tell it to increment.  Who ever thought that was a good idea any way?

[crazy^millman]

 It would be so much better if the default was G54 then you had to tell it to increment.  Who ever thought that was a good idea any way?

 

I have asked this question in my head and out loud on the forums many times. It has really made me wonder why this was put in also. 

[Sticky]

With MPmaster posts the first work offset is locked for the entire program unless you go into the misc values and turn it off.

 

In my case I have it permanently disabled because the last thing I want is one work offset for multiple planes.

[jlw™]

You use an offset for every plane?

[Sticky]

You use an offset for every plane?

 

Yes.

[jlw™]

4 and 5 axis?

[gcode]

Wow I have never had a problem with this, I just finished up a nasty 3 + 2 with 6 planes and never stepped out of G54. Perhaps my 2 5 axis posts are already hardwired for G54 only but I'm worried so now I'll check every time.

Mastercam mp based posted contain this line

 

use_frst_wcs : no$  #Use only the first WCS read and ignore all others in NCI

 

set it to no.. only one workoffest gets output

 

if you need more that one you have to set this switch to yes

[Sticky]

4 and 5 axis?

 

Exclusively.

[jlw™]

Hmm. Are you G10ing calculated offsets or setting up in the machine?

[Sticky]

Yep.

 

C'mon dude, we were just talking about this last week!

 

http://www.emastercam.com/board/topic/90001-older-mori-hori/

[jlw™]

Well, you said you use an offset for every single plane.  I do when I need it or for a tight feature but for every plane it's a bit redonkulous.  I can have hundreds of planes and I'm only going to do it when needed.

 

 

Also, my bad.  I don't remember every thread on here.

[Sticky]

I don't think it is redonkulous.

 

As a programmer, it is literally no extra work for me, the post does the work.

 

As a shop owner it saves time and money. It is a more flexible system that allows the operator, and even the programmer, a lot of liberties that are not available to one offset rotary work.

[jlw™]

Mostly agreed.  You must be working with a different caliber of operator.  I struggle with setup.  Heck, I can't even get people to read their setup sheets.

[Sticky]

Sometimes I am, sometimes I am not. In regards to this method though, it doesn't matter. If the operator has the ability to utilize the features, they can, and if they don't, the program just runs like "magic" like a single offset program.

[Tim Johnson]

"In the Plane Manager you have a choice between "Automatic" and "Manual". Click "Manual", grab the arrow and click your offset point (if needed) and type in the offset you want.

[Greg_J]

 

Mastercam mp based posted contain this line

 

use_frst_wcs : no$  #Use only the first WCS read and ignore all others in NCI

 

set it to no.. only one workoffest gets output

 

if you need more that one you have to set this switch to yes

 

I don't have "use_frst_wcs" in my post.

 

Its MPFAN.pst

 

Any ideas what to change in this one?

[crazy^millman]

I don't have "use_frst_wcs" in my post.

 

Its MPFAN.pst

 

Any ideas what to change in this one?

 

That is a not a Mastercam Generic Post option. That is a MPMASTER and other 3rd party post option. Either need to integrate that into the post you are using or change to MPMASTER to get that type of functionality.

[Brian Pallas]

I didn't do it on the mill posts, but on the post I use for the Mori NL's, I put a pop up alarm in if the work offset for if a plane isn't actually set to a number in the view manager.  The way I set the post up everything needs to be G54 for the main spindle and G55 for the sub, so I have the post toss an alarm if a plane isn't set to one of those two numbers.

 

A bit more to put in to cover the work offset numbers you would use on a mill, but you might be able to set up the same type of thing.