Sign in to follow this  
Cavi Mike

Post outputting random M00's in my program...

Recommended Posts

Using "2D High Speed Area Mill Toolpath" I'm getting random M00's in my program. I found the line of code in the post that's doing it but I have absolutely no idea why this is being triggered.

 

This code...

pcan1           #Canned text - with move
      strcantext = sblank
      if cant_no$ > zero,
        [
        if cant_pos1$ = one | cant_pos1$ = four, pcant_1
        if cant_pos2$ = one | cant_pos2$ = four, pcant_2
        if cant_pos3$ = one | cant_pos3$ = four, pcant_3
        if cant_pos4$ = one | cant_pos4$ = four, pcant_4
        if cant_pos5$ = one | cant_pos5$ = four, pcant_5
        if cant_pos6$ = one | cant_pos6$ = four, pcant_6
        if cant_pos7$ = one | cant_pos7$ = four, pcant_7
        if cant_pos8$ = one | cant_pos8$ = four, pcant_8
        if cant_pos9$ = one | cant_pos9$ = four, pcant_9
        if cant_pos10$ = one | cant_pos10$ = four, pcant_10
        if cant_pos11$ = one | cant_pos11$ = four, pcant_11
        if cant_pos12$ = one | cant_pos12$ = four, pcant_12
        if cant_pos13$ = one | cant_pos13$ = four, pcant_13
        if cant_pos14$ = one | cant_pos14$ = four, pcant_14
        if cant_pos15$ = one | cant_pos15$ = four, pcant_15
        if cant_pos16$ = one | cant_pos16$ = four, pcant_16
        if cant_pos17$ = one | cant_pos17$ = four, pcant_17
        if cant_pos18$ = one | cant_pos18$ = four, pcant_18
        if cant_pos19$ = one | cant_pos19$ = four, pcant_19
        if cant_pos20$ = one | cant_pos20$ = four, pcant_20
        ]
      if cstop$, strcantext = strcantext + sm00 <-------------------THIS LINE
      if cgstop$, strcantext = strcantext + sm01

...is doing this.

X-.9094 Y-.781 R.02
X-.9227 Y-.786 R.02
G2 X-.9396 Y-.8003 R.4701
X-.9573 Y-.8139 R.4701 M00 <---- WTF?
G3 X-.9655 Y-.83 R.02
X-.9455 Y-.85 R.02
X-.9337 Y-.8462 R.02
X-.9255 Y-.83 R.02
X-.9455 Y-.81 R.02
X-.9573 Y-.8139 R.02
G2 X-.9755 Y-.8266 R.4701
X-1.0028 Y-.8433 R.4702 M00 <---- WTF x2?
G1 X-.9979 Y-.8653
G0 Z.25
X-.7544 Y.0671
Z-.0025
G1 Z-.0675 F50.
X-.7554 Y.048

For now I've changed that to a sm01 just to get me by, but I don't have a clue why it's doing this, and honestly not sure it's even something with the post, so this might be in the wrong sub-forum.

Share this post


Link to post
Share on other sites

Could it be Tool Inspection is turned on, in the Operation itself?

Something (in the path) is likely causing Mastercam to kick out "NCI 1020 Lines", in the middle of your path.

There are basically 2 mechanisms built into Mastercam which allow you to output "Canned Text", in the middle of a Toolpath. You might want to do this for "changing the insert", or "moving a clamp".

  1. With a "Chain-Based" path, you can right-click on a Chain (chain manager), and use "Change at Point", to add "events" at the endpoints of any entity in the chain. These changes are "tied" to the chain, which allows you to Regenerate the Operation, without losing those manual changes.
  2. Toolpath-Editor. This is the nuclear option, which allows you to physically edit the Operations "point-to-point" motion. These edits can be made to do "tool inspection", but more often they are used to remove a "bad plunge point" in the path. Also, when you use the Toolpath Editor, Mastercam will "lock" the operation. No changes can be made to the Op, without unlocking. But regenerating an unlocked path means you lose all your manual edits.

There is another mechanism, which has been built into modern Posts, but this exists at the "operation control" level. This is "Tool Inspection", which allows you to stop the machine and inspect your tool in the middle of cutting. The NCI File flags the motion as "rapid type #7", and this indicates to the Post that we have reached a Tool Inspection Point.

Inside 'prapidout', there is a condition 'if rpd_typ$ = 7', which allows you to "do something" when an inspection point is reached. Since we don't know "what you need", it is left up to the Post Developer, to add code to handle the inspection point. Typically, this would be a whole series of lines. First, we would capture the "current coolant on/off status(s)", which can be complex, depending on the type of coolant (V9 or X-Style) you are using. After that, we would shut off the spindle and park the machine (M00). Then, we need to add lines to 'restart the spindle' (at the prior RPM), Turn on the Coolant (same state as when we stopped), and we need to re-enable Tool Length Offset, so we need a G43 Hxx Zxx move to approach the part again.

Share this post


Link to post
Share on other sites

Nope, that's off. I've scoured the options in the toolpath parameters and can't seem to find anything. And it only gets triggered on those exact two places. It also only happened after I put a -.005 value in "Stock to leave on floors" which I just remembered, I just set it back to 0 and it went away. I'm almost certain now that it's a bug in the software.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us