Renumber tools problem in version 8 - Help!

[kathy]

Hello Everyone,

When I use the 'Renumber Tools' command in the Operations Manager, the tool numbers change successfully, however the length & diameter offsets numbers remain unchanged. Example: when TOOL 1 changes from TOOL 8, the tool number changes to 1, but the diameter offset number is still 48 and the length offset number is 8. Unfortunately, the value '8' will process out in the code as 'H8' for 'Tool 1'. Big time crash.

…

N4 M1

N5 M6 T1 ( .129 DIA , DRILL/BORE )

N6 M3 S1000

N7 E1 G0 X24.501 Y18.5

N8 Z3.0 H8

N9 G83 G98 R0.16 Z-.0567 Q.04 F4.

N10 X15.001

…

We don't need auxiliary diameter or length offset numbers, so I've been playing around with the post to assign the tool number value 'T_' to the 'pltoffno' 'H_' value without much luck.

I'm not really happy about going in and changing all those numbers by hand.

My settings are as follows: Job Setup, Tool Offset Registers, From Tool.

Mastercam Version 8, Level 3

Kathy Richardson

Mfg. Engineer, CNC Programming

Applied Aerospace Structures Corp. (AASC), Stockton, CA

phone: 209-983-3203

fax: 209-983-3375

website: www.aascworld.com

 

[CycleTimeCharles]

Since you renumbering the tools anyway, go to Job Setup and set "Tool Length Registers" to "Add" "Length 0" and "Diameter 0"

Select regen and your tool renumbering will be fine.

Only use Tool offset Registars" from Tool if your tool library has D and H values that are not the same or have no relationship to the T value.

[Keith Graydon]

Hi Kathy,

We program our Monarch VMC's to call tool offsets thru a parameter function.

in this case P13.P13 on this controller is TOOL IN SPINDLE. this controller uses a single offset register for both length and dia. Described as "D".

so the code looks like:

N8 T12 M6

N9 G90 G0 X0. Y0. D(P13) E1

N10 Z 2.0

very cool. tool in spindle is always the active offset. hasn't crashed yet!

hth

-Keith G.

[Keith Graydon]

oops TYPO alert!

please disregard the "b in brackets preceeding D=(P13)

shoud read as......

N8 T12 M6

N9 G90 G0 X0. Y0. D(P13)E1

N10 Z 2.0

-Keith G.

[kathy]

Thank you for your help!

I changed my settings in the Tool offset Registers from 'From Tool' to 'Add' and it worked like a charm!

It's a little disconcerting to see the length / diameter numbers in the tool parameter different from the tool number. However, if it works right in the Operations Manager and I get good code, I'm happy.

I was also thinking the setting 'From Tool' was my default, so I went back and checked my Version 7.2 Job Setup up and saw that it wasn't.

In my Smartcam code generators (pre Mastercam years), I assigned the tool number variable to both the T & H values and never had a problem!

- Kathy

 

[kathy]

I’m still having trouble with tool renumbering – recently I brought in an older .MC7 file and could not get the tool length register to reflect the tool number.

On every new program I make, I go through each tool and double click the tool number field to set the Dia. and Length Offset Register fields to reflect the correct number. This way I know the code will be right.

Several months ago, I programmed a panel where I didn’t make sure the tools were all reset, and depended on the regen to produce the correct H number. Guess what, there was one bad tool (T3, H5). And yes, the wrong tool punched through the panel.

All of this is a pain in the neck – why can’t the software just renumber tools correctly? I am also going to work on the post – that is the failsafe way to get code I need.

- Kathy

------------------

Kathy Richardson

Applied Aerospace Structures Corp. (AASC), Stockton, CA

phone: 209-983-3203

fax: 209-983-3375

website: www.aascworld.com

[tooling]

view the reply post for screen configure problem. remove the check in the assign tool numbers sequentially

[Allan Brown]

You can always override the tloffno ('D') and tlngno ('H') variables in the post before they are output to be extra sure.

e.g.

tloffno = t

tlngno = t

pbld, n, "G43", *tlngno, pfzout, scoolant, next_tool, e

[kathy]

Dave,

That is what I ended up doing! No more problems

...

ptllncomp # Tool length compensation

tlngno=t

*zr, *tlngno, ptloffno

...

Thanks, Kathy