Whip Arm or Touch Probe

[Rob_Bish]

Im looking for a few opptions/opinions on which way to go about setting the post for our Brother TC32B broken tool probing. When the tool length is below 3.2 inches i neeed to use the touch probe not the whip arm. G65P*** for touch probe. M200 for whip arm.

Thanks Rob

[Guest]

I believe this is achievable with the post

 

Do you already have you tool lengths defined?

 

If you do you can set a check for them to check the defined length of the tool and then output the proper tool check routine.

 

If you are going to check before the tool runs the ptlchg_com section is likely where it would have to be, if at the end of the tool then in the pretract section.

[Rob_Bish]

Yes the tools are defined.

[Rob_Bish]

Dont think i have defined them correctly as I only output 0.

Am I on the right lines tl_oal$ etc.

Rob

[Guest]

What post are you using?

 

I use these varables to get the info out for tools

 

code:

---

fmt     2 pilot_dia               # 20007 Parameter line

fmt H 2 flute_len

fmt 2 oa_len

fmt 2 shldr_len

fmt 2 arbor_dia

fmt 2 hldr_dia

fmt 2 hldr_len

---

[Rob_Bish]

I am using a Generic Fanuc 5X Mill tweaked for our Brother machine.

Rob

[tryon]

Can you get into your G65P**** program? i would add a check in the beginning of that program to check the length of the tool in the spindle and have the Macro decide. This way you could standardize the broken tool detect.

 

IF[#[#4120+10000]]GT3.2]GOTO200

(TOUCH PROBE SECTION)

;

;

;

M99

 

N200(WHIP ARM CHECK LONG TOOL)

M200

M99

[Guest CNC Apps Guy 1]

Another option, you could format oa_len$, create a postblock where you want to do the Tool Breakage Check. In that postblock check oa_len$ and if it exceeds whatever value you set, then do the other type of Tool Breakege Check.

 

ptlbrk #Broken Tool Detection

if oa_len$<2.3, pbld$, n$, "G65P***", e$, else, n$, "G65P***R****", e$

 

Just a thought. Handling within the Macro Call would work as well. Handling it within the Post Requires an accurate tool definition. Handling it within the Macro does not. It can read the active tool if set up properly.

 

On most machines I get hold of that have custom MACRO B, I create a tool cchange MACRO that does several things, it sends the machine to tool change position automatically at the execution of an M6, it detetects the new tool number in the spindle puts that number in a Macro Variable -usually #506 because it will keep track of it even if the power gets turned off-, then I have that tool's height ofset value written to another Variable - usually #516- so then I can do chcks on that value if I ever need to. CUSTOM MACRO B is very powerful. It's main limitation is the guy creating the MACRO.

 

HTH