WCS Offsets

[Josh Kinney -Elite Engineering]

It seems this is new for X6.

 

If Op 1-10 use "TOP" WCS and Top is set to Offset -1 in the WCS Manager. Any and all ops will output "workofs$ 0.". If I change Op10 to use offset 3 and just output Op1 then Op1 will output with "workofs$ 3." also when it should still output "workofs$ 0.".

 

This is not how it behaved before X6. I set all my posts to use "if workofs$ < 1, workofs$ = 1" and it was handled properly.

 

This no longer works and is a real pita for the programmer. I've went round and round in the past with CNC Software about the WCS but honestly some thought needs to be put into how us end users are actually using it in our workflow.

 

Is there something I'm missing?

 

-Josh

[gcode]

Set Top WCS to "0" in the tool manager

then you can set OP10 to 3 if you want to, but I prefer to make a copy of TOP, change the workoffset to 3 and use it for OP10

[Colin Gilchrist]

Josh,

 

It may be new for X6, I'll do some investigation.

 

Work Offsets have always had a feature that was improperly documented in the past, and the help documentation has been corrected for X6. Here is the corrected entry from the help file for 'work offset numbers':

A setting of -1 is used to enable automatic work offset incrementing. Please note that -1 is an internal value, and is never output to the NCI file. This feature will automatically increment the work offset value by one, every time there is a toolplane rotation. This feature is typically used with a Milling machine that has a rotary axis. For example, if you use 3 axis VMC and you create four toolplanes that rotate around the X axis, all with a work offset of -1, you would get G54, G55, G56, and G57 respectively. You must set a work offset value in the toolpath parameters, or by assigning a work offset value to every toolplane.

 

 

Basically, a setting of '-1' tells the system "Increment the work offset number, whenever you see a change in the tool plane orientation".

 

Here is what I suspect is happening. When you are changing the Work Offset value for Op #10, to '3', I suspect that Mastercam is changing the Work Offset value for the Top plane. So any operation that uses 'Top' is now getting it's value from the Plane, as the '-1' isn't a real setting anyway, but a flag to tell Mastercam what value to calculate internally for the work offset value...

 

That said, I'll check and see if it behaves differently from X5 to X6...

 

A temporary solution might be: set '0' for Top, Then make a copy of the Top plane, and set the work offset value to '3' for the copy (maybe include "G57" in the plane name). That should give you the correct work offset for everything that uses '0', and output correctly when using that different work offset number.

 

Edit: beaten by Tom!!!

[Chris McIntosh]

Just for giggles I tested in previous versions to see if anything has changed, and no, it's consistent back through X3 at least.

 

As far as the -1 setting, I have always treated this as a "Mastercam automatically selects your work offset" setting. So as I see it, if you set the Top plane to 3, and the other operations use the same plane with a work offset of -1, Mastercam sees you have set the work offset to 3 later, and will link the two operations together since they are using the same plane.

[Josh Kinney -Elite Engineering]

I understand. Thanks for taking the time to explain. I really wish MasterCam would allow you to specify system defaults better and you could set "TOP" to start as "1". That's almost like having coolant always on until you turn it off. That horse is so beat it's turned into a fossil at this point. Really makes teaching new guys difficult.....

 

Just another step. Open file, set all WCS to "1"....

 

Thanks again guys.

 

-Josh

[Colin Gilchrist]

I'm making an Enhancement Request to redo the options for 'Tplane during automatic work offset number creation'. There is a setting in there for 'None', but it doesn't actually work. Even when you set it to 'None', a setting of '-1' for the Work Offset Number still forces Mastercam to automatically increment the work offset number when the toolplane orientation changes.

 

My thought is this: when set to "none", all '-1' Work Offsets should be reset to the Work Offset value of the selected Tool Plane, and no toolplanes are allowed to use '-1'.

 

In many of the posts I've written for customers (before joining CNC Software), I would usually rewrite the 'pwcs' post block to handle the numbers differently when entering work offset. I would setup my Fanuc-style posts to use 54-59 for G54 through G59, and 110-129 for G110 through G129. (Optionally, you could also set it up to use G154 P1-Pxxx). I always liked that better than entering '0' for G54, '1' for G55, ect.

 

I think in the future it would be really nice to have more options in the Control Definition file for setting up how the machine/control/post handle work offsets. Maybe the ability to define a style, format type, and value range, and have that tied into the post...

[Josh Kinney -Elite Engineering]

I agree and that is usually how I set mine up. Only thing is you have to cover all scenarios. If you have an old program that uses -1 your screwed. If the post respected workofs$ < 1 then you would be covered. In the past I guess I got by fine as long as you didn't assign another offset in a separate op using the same toolplane....

 

Unfortunately unless it's 100% foolproof it can't be implemented.

 

Were both on the same page, hopefully the enhancement request gets some traction

 

Thanks Colin,

 

-Josh

[crazy^millman]

In many of the posts I've written for customers (before joining CNC Software), I would usually rewrite the 'pwcs' post block to handle the numbers differently when entering work offset. I would setup my Fanuc-style posts to use 54-59 for G54 through G59, and 110-129 for G110 through G129. (Optionally, you could also set it up to use G154 P1-Pxxx). I always liked that better than entering '0' for G54, '1' for G55, ect.

 

Colin I and many others I know also support this logic for posting out work offsets and think this whole thing should really be given some thought.

[K2csq7]

Why not leave the options right there... keep it simple, 2 boxes for you to put numbers in, give the second field a checkbox that needs to be checked if you want to enable the P value. We really need only 2 input fields.

G54 (the 54, 55, or 56......)

P21( the 21, 22, 23.....)

And just have the numbers post out as input.

Then a chekbox for "lock this work offset and toolplane together", and a checkbox for "increment work offset from last work offset".

[Bryan Johnson]

A setting of -1 is used to enable automatic work offset incrementing

 

A feature that could vanish tomorrow, and I would never miss it.

I never leave this set at -1. The results are too unpredictable.

[Newbeeee™]

My feeling (fwiw) is that automatic work offsets are an accident waiting to happen. I would much rather mcam let me put the offset value in that I want, and then I change it when I want.

G54/55 etc are the easiest (and I bet most common) cause of machine crashes and having them autocreated is mad for the average (and below average!) user.

 

Colin - it would be great if mcam would allow a global setting/default so for me, I could leave the default as 54. Default -1 is bad bad bad !!!