Error proofing gone bad.

[savagkd]

In an effort to insure the operator has loaded the correct length tool, I'm using the following in the header of the program.

 

/G10 L10 P9 R-24.716 (3/8 BULL ENDMILL 0.02 RAD)

 

/M6T9

/G65 P9862 B3. D9. H.03 I.375 J.012 R.375 T9.

 

The G10 line sets the desired tool length in the offset register. The H.03 in the tool measure line allows .03 error, anything over .03 errors out.

 

Block skips allow the operator to skip the tool measure for subsequent parts. Measuring 10 tools adds 2 min. to the 15 min. cycle time.

 

"Rant begins."

 

Today, the operator ran the first part with block delete off, and got a good part. On the second part he started the program, which read the G10, and when it moved to measure the tool, he stopped hit reset, turned block delete on and restarted the program. This overwrote the measured offset value with desired and scrapped 3 parts.

 

"Rant ends."

 

I should have seen that coming. My bonehead mistake.

 

Anyone have a better way to double check that the physical tool length is within a given value without the risk?

 

Thanks

 

Keith

[Joe788]

Just skip the G10 at the beginning. Input that theoretical length into a variable instead.

 

#850=-24.716

 

After your tool measure cycle, just compare the tool length to #850, instead of using the tolerance call in the tool setting macro.

 

Not sure what machine you're using, but on a Mazak, your length for T29 would be in #60029. T30 would be 60030, etc.

[savagkd]

Thanks Joe788,

 

But can I point the Renishaw macro to the variable for comparison? I want it to fault out if the operator to uses the wrong length tool.

[Joe788]

You'd need to add your own little macro after the Renishaw call in order to compare them. Are you familiar with macros? What brand machine and control is it?

[savagkd]

Unfortunatly, what I know about macros might fill a thimble.

 

This one is a Haas.

[Joe788]

Another option is to just set a flag that the G10 has been run, that isn't unflagged until the tool length measurement is complete. That way, if the operator tries to do the same thing he did earlier, it will stop him.

 

I think #750 should be available on a Haas. Maybe one of our Haas users can chime in? Just add these exact snippets of code to the first tool change/measuring sequence, and go test it out.

 

/#750=1.

/G10 L10 P9 R-24.716 (3/8 BULL ENDMILL 0.02 RAD)

/M6T9

/G65 P9862 B3. D9. H.03 I.375 J.012 R.375 T9.

/#750=0.

IF[#750=1.]GOTO555

GOTO556

N555M00(YOU G10ED THE TOOL WITHOUT RUNNING THE TOOL MEASUREMENT, DUMMY)

M30

N556

 

 

Here's a quick explanation of what's going on:

 

The #750=1 is basically a flag that's saying "we're cycling through with block skip off". It'll stay set at 1 until the tool measurement is complete. If he lets the machine finish the measuring cycle, the very next line is #750=0. So that turns your flag back off.

 

When it gets to IF[#750=1.]GOTO555, that's just checking whether or not the flag is still set. The GOTO is a line number "N555". On line N555, you have a program stop, with a note to explain why it stopped - and an M30 afterwards just in case the guy hits cycle start again anyways.

 

If everything ran correctly and #750 was set back to zero after the tool measuring call, the machine will simply read straight through the "IF[#750=1.]GOTO555" line, and hit the next line "GOTO556". N556 is just the block number for the line after your alarm lines - so the "GOTO556" just jumps you ahead 3 lines and the machine continues on its merry way.

[savagkd]

Thank you,

 

I'll give both options a try in my copious amounts of spare time.

 

I love this forum!

[Joe788]

The only thing that might not work, is the #750 may or may not be available. Worst case scenario is you just have to substitute "#750" in the above example, for some other #.