Offset number in NCI file changes?

[Eduard Winckers]

I create a mill-program with changing work/coordinate offsets (i.e. G54, G55, G56, etc..), through Operations Manager, Tool Parameters, Parameters, (check) T/C plane and enter value (G54,G55,etc...) in Work Offset, Tool plane. The offset number is shown in the NCI-file (1016 record, *** # 9). I would expect that a chosen offset remains active UNTIL ANOTHER offset is entered. However, when I do not select T/C plane for a new operation, I get an unpredictable number in my NCI. (OK iw ould expect it to be soemthing like "-1", but not 54 when my last offset was 58!). Is anyone familiar with this behavior, is it possible to prevent this form happening?

Any advice is welcome!

Eduard

[Mark H]

Yes I have noticed this as well. As a rule I just set the offset for each operation regardless if it has changed from the previous offset.

[Eduard Winckers]

Are we looking at a BUG here? Or is this a Mastercam filosophy??

Hopefully we will also see a reply from a "Mastercam Official".

Eduard

[CycleTimeCharles]

I am not an "Mastercam Official".

but if you need to read the comments in MPFAN.PST

# 2) G54 calls are generated where the work offset entry of 0 = G54,

# 1 = G55, etc.

[Mark H]

What I think Eduard was trying to say was (Eduard correct me if I wrong)...

If the first operation's work offset is set to G58 (TC plane is checked, work offset is checked, value is 5, mi1 is 2). Then if the work offset is not specified (TC plane unchecked) in the next operation, G54 NOT G58 will be outputed.

So his question was... How do you keep the G58 without having to set the work offset for each operation?

Here is a thought, Eduard, did you try setting force_wcs : no in your post. The problem with this is that only the first wcs will be used and all others will be ignored.

[This message has been edited by Mark H (edited 05-08-2001).]

[gstephens]

If you are using any work offsets other than the default (G55-59 G54.1P1...)you need to make sure that you set them for EVERY toolpath. If you do 2 contours toolpaths, the 2nd one will have the same settings as the first, but if you do any other toolpath, it has its own set of defaults, so you need to check the work offset variable for each path. Also, if you leave the variable at -1, Mastercam automatically increments the variable (starting at 0 then 1,2,3,...) for each successive toolplane.

 

[Eduard Winckers]

Thank you all for your responses. Yes, Mark is right, the issue I am talking about has to do with multiple work offsets (s.a. G54 for op#1, G57 for op#2, G55 for op#3, G54 for op#4 etc...) where I tend to leave TC plane unchecked if there is NO CHANGE in offset! Since I need to use MULTIPLE OFFSETs it will not help to set "force_wcs:no". I write my own post and need to rely on the inforation in the NCI to be correct. I my post I NEED to check if the work offset changes, since this triggers a number of actions. As long as Mastercam outputs a "non standard" value in the NCI (i.e. someting like -1 or 0) I can issue a warning. I wanted to be able to 'see' if TC plane was checked...!

[Eduard Winckers]

Looking at the reactions, I have not seen ANY real solution to my little 'problem'. Does this mean that we use the work offset behavior AS IS???

Is the general conclusion that it is up to the Mastercam user to make sure he specifies the REQUIRED work offset for EVERY OPERATION? Thus saying that there is very little (or no) intelligence in either MCAM or the Post??

Eduard

[Guest CNC Apps Guy 1]

Well Eduard,

It's not really a problem. There are soooooo many possibilities that it just makes sense to leave it as is. Besides, what kind of "intelligence" are you looking for? The kind that reads your mind?

 

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

James Meyette

[Mike Freimann]

I don't think mind reading will be available for some time but, if I understand you correctly you want the last work coordinate if you don’t check the box. Why not make the default 10 then put a statement “if mi1= 10, mi1= prv_mi1” you may need to capture the prv_mi1 but I think something like that might solve your problem. Let me know if you need help. I realize that this may be leaving out a little but I like to figure out stuff like that.

Mike

 

[Eduard Winckers]

Thank for your suggestion, the problem however is: "what default??"

If the box is NOT checked is is hard (impossible?) to predict the work offset number that appears in the NCI (could be -1 of 54 or 0 or 58 or......). THIS is my problem!

[Luther_Heggs]

The offset # in the 1016 NCI line will be numbered whether you like it or not. If you specify a number under the the enabled "T/C plane..." the system will use that. If you don't, it assigned them for you starting at 0 and incrementing by 1.

It seems to match up your tool planes (NCI line 1014) and the tool plane origins (NCI line 1013). If you never define a tool plane for any operation, and have 3 operations, the first 2 that use TOP @ 0,0,0 and the third that uses TOP @ 1,0,0 the system will define the first 2 work offset no's as 0, the third as 1. If you set the work offset for the first 2 at 54, and nothing for the last operation, the system sets your work offset for the first 2 at 54, the last at 0 (in the 1016 line).

If you look at the actual binary nci you'll see that undefined work offset values in the 1016 line are set to -1. This leads me to believe that they are compared and numbered when the real (text file for posting) NCI is created.

Sounds like you should just set what you want to begin with.

[Webby]

Eduard - Either email your file to [email protected] or upload it to ftp.emastercam.com/incoming (and send an email notifying me that it's there).

Along with the file indicate us what you expect each WCS value to be per operation in your posted code. That way we can offer a programming change or a post change to suit your needs.