Undesired repeat of G28 in transform/rotate functionality.

[Carbonwerkes]

Hey guys-

 

Hopefully a quick question-

 

Im doing a simple 4^th axis op (basically, just cutting bar into a hexagon, for custom preload nuts).

 

Im leveraging the ‘transform/rotate about origin’ functionality, so that I can just do a contour/face path and then repeat per 60 deg rotation in A.

 

Problem is, my post (MPMASTER 2017) is setup to export a G28 on completion of an operation. It seems the Transform/Rotate is literally just a ‘Copy selected ops X times’ function, along with the translation/rotation commands it inserts. So, I end up with a G28 in 6 cycles here.

 

Yea, I can hack the post to prevent that, or manually edit the code, or even just setup a G53 type thing to limit travel, but it seems like this should be a native option (to prevent retracts until the end of a program, not just end of op, when you have a Transform/Rotate op). And, it may, so perhaps it is in the Misc Integers, or some manual entry I can add between ops in the Toolpath tree. But, I have not found a reference to best practices here, and I would be grateful for any guidance.

 

Kind regards

Rob

[Colin Gilchrist]

4 hours ago, Carbonwerkes said:

Hey guys-

 

 

 

Hopefully a quick question-

 

 

 

Im doing a simple 4^th axis op (basically, just cutting bar into a hexagon, for custom preload nuts).

 

 

 

Im leveraging the ‘transform/rotate about origin’ functionality, so that I can just do a contour/face path and then repeat per 60 deg rotation in A.

 

 

 

Problem is, my post (MPMASTER 2017) is setup to export a G28 on completion of an operation. It seems the Transform/Rotate is literally just a ‘Copy selected ops X times’ function, along with the translation/rotation commands it inserts. So, I end up with a G28 in 6 cycles here.

 

 

 

Yea, I can hack the post to prevent that, or manually edit the code, or even just setup a G53 type thing to limit travel, but it seems like this should be a native option (to prevent retracts until the end of a program, not just end of op, when you have a Transform/Rotate op). And, it may, so perhaps it is in the Misc Integers, or some manual entry I can add between ops in the Toolpath tree. But, I have not found a reference to best practices here, and I would be grateful for any guidance.

 

 

 

Kind regards

 

Rob

 

The MPMaster Post might have an option to suppress the retract, but I don't think it does this for Transform. I know the Generic Posts do not have that option.

Just do yourself a favor and edit the 'pretract' Post Block to use G00 G90 G53 Z0.

G53 is non-modal, and will not cancel your active Work Offset or Tool Length Offset. Also, there is no danger of the machine cancelling an offset "immediately", and crashing the machine.

This is an edit I make to almost every Post I ever work on. I despise 'G91 G28' moves with a passion. Many of the crashes I've seen over the years have been attributable to G28 home moves cancelling something, or unexpectedly moving the spindle to XY zero.

[Orvie]

This can also be accomplished by unchecking "force tool change" in the parent operation, and make sure you check "remove comments" in the transform operation.

 

[Carbonwerkes]

Hi Orvie-

I didn’t have the ‘force tool change’ enabled here, and removing comments uncheck didn’t alter the output from the Post at all. But perhaps this would help for some circumstance- so I thank you for the ideas-

 

 

Colin-

Thank you for the guidance. Im an aero engineer learning Mastercam/Post coding as time and migraines permit, so Im not all that clear on which instances in the Post to alter (there are two Pretract subsections (Pretract and Pretract0), and within them, some conditional logic with their own SG28 references.

 

I did modify them to a condition  I felt was reasonable. Following is the output for the first couple of passes. Can you let me know if this is more or less what you would want to see?

N120 T186 M06 (5/8 INDEXABLE FLAT ENDMILL)
N130 (MAX - Z1.)
N140 (MIN - Z.5)
N150 G00 G17 G90 G55 A0. X.54 Y.9047 S3101 M03
N160 G43 H186 Z1.
…cut commands
N230 Z1. F50.
N240 G00 G90 G53 Z0

N250 G00 A-60. X.54 Y.9047
… cut commands
N330 Z1. F50.
N340 G00 G90 G53 Z0

At present, the machine still homes Z between rotations of the table, but it doesn’t home the table- which is a big win.  Is that just a function of where my machine controller defines G53 to be?

 

Thanks again for the help in this-

 

Regards

[ajmer]

double check if this is set to 0 in the mpmaster posts

ret_on_indx : 1     #Machine home retract on rotary index moves, (0 = no, 1 = yes)