VERICUT Users' Forum

dwiehr

Member

From: Hutchinson, MN

Registered: 2005-10-05

Posts: 17

Heidenhain iTNC530 - M94 problem

I'm having a problem getting Vericut (any version including 6.1) to work correctly with a line of code that has an M94 in it.  M94 is used to reduce the display of the rotary axis to less than 360.

Example:

1839 L C90.0 F3000.0 M94 C

It seems Vericut reads the M94, but ignores the rest of the line.  It should read the 'M94 C' portion of the code to reduce the C axis displayed degrees to less than 360 then move 'C90.0 F3000.0'.

I have defined M94 in the Word/Address dialog box trying both RotaryLinearRewind and RotaryAxisLinearRewind macros, but it doesn't work right with either of them.  If I move the 'M94 C' portion of the line up one line, all works well.

Example

1838 M94 C
1839 L C90.0 F3000.0

Any ideas?

Thanks,
Dave

danr

Member

From: Derby, UK

Registered: 2006-07-24

Posts: 19

Re: Heidenhain iTNC530 - M94 problem

I believe Vericut process the words on a line in the order in which it finds them in the classes in the Word/Address tree. Therefore words which are in higher classes (such as Registers - C and F) will be processed before words in the M Misc class (M94). This could be causing you problems and would explain why the correction you made solved the problem.

Try moving M94 to a higher class, or alternatively try creating a new class higher in the tree to contain M94. Whichever gives the most traceable change to allow you to find it next time!

Hope this helps.

Daniel

---

Current version: Vericut 7.0.3

dwiehr

Member

From: Hutchinson, MN

Registered: 2005-10-05

Posts: 17

Re: Heidenhain iTNC530 - M94 problem

Daniel, Thanks for the reply.

That got me closer to working but Vericut still has problems with it.  It almost works when I move the M94 to a higher class, but I also have to comment out, or delete the last 'C' in the line of G-code.

Works:

1839 L C90.0 F3000.0 M94

Doesn't work (how it's coded for the machine):

1839 L C90.0 F3000.0 M94 C

I'm thinking that Vericut is having a problem with 'C' in the line twice. It needs to evaluate the 'M94 C' before the 'C90.0 F3000.0'.

Any ideas on how to get Vericut to understand 'C' being defined twice in two different contexts within a single line of code?

Thanks,
Dave

jsmillett

Member

From: Chatsworth, CA

Registered: 2005-02-25

Posts: 42

Re: Heidenhain iTNC530 - M94 problem

Try this substitution:

'M94 C' -> 'M94'

This gets rid of that pesky trailing 'C'.  If M94 is always followed by the lone C then that should work.

---

Jerry Millett

dwiehr

Member

From: Hutchinson, MN

Registered: 2005-10-05

Posts: 17

Re: Heidenhain iTNC530 - M94 problem

Thanks Jerry!

Worked beautifully! It is always only the C axis that gets the M94 as the A axis is a trunnion which never rotates more than +/- 110 degrees.

Thanks to both Daniel and Jerry for helping me solve this problem!

Dave