Idea for descriptions comments?

[[email protected]]

Hi All, I recently programmed an Inconel part with 6 deep pockets. The operator would often have the tool break before finishing all 6 pockets. Then they would just start from beginning or have trouble finding a good place to restart from. So I copied that operation 5 times and labeled each pocket. I used the operations description/comment whatever you call it when you label your operation and it posts with paranthesis around it. 

That made me think it would be nice if there was a way to get a line number or some way of finding the individual pockets inside one pocket operation. I figured if anyone would know it would be here. If not maybe someone that works for CNC software thinks it's a neat idea and will implement something like it idk figured it was worth a shot

[JParis]

IN a case such as that, I would program each pocket in its own operation and use "Force Tool change" , then I could place a manual entry between them and give them a clear place to restart a particular pocket.

JM2C

KISS theory applied

[cruzila]

My post uses the Tool for the N number so I would put something in the note to add additional N numbers for each tool change.

[[email protected]]

Thanks, I did program each pocket into its own operation and labeled them so now the post puts the "comment" at the start of each operation. I do appreciate the force tool change and M00 suggestion. Because I didn't know what force tool change did for like 5 years programming and used to add all the necessary code in by hand lol. These guys are pretty good and they are using program restart and checking the z depth to get the program as close to where the previous tool failed. As far as what cruzila said I am a bit lost on what you meant by "I would put something in the note to add additional N numbers for each tool change" Anyway thanks for the responses because the guys on the floor just told me my threadmill is wearing out and they were adding n numbers between the holes to know which ones to re run. With 16 holes I really didn't want to crowd my toolpath manager with 16 operations instead of just 1. We are changing to a .25 cut length multi profile threadmill once they come in, so hopefully that takes care of the tool wearing out so fast.

[cruzila]

(pocket 1)

N1 T1 M6

"NORMAL GCODE"

(POCKET2)

(N1200 )  ---------------------"this is reminder for the programmer"

N1 T1 M6 

N1200  --------------add here

"GCODE BLAH BLAH BLAH...

 

There is also a feature to retract for tool inspection based on tool time. Never used it. Someone here may chime in?

[AHarrison1]

59 minutes ago, cruzila said:

There is also a feature to retract for tool inspection based on tool time. Never used it. Someone here may chime in?

This will need a post modification.

Similar threads related to inspection

 

Edited Thursday at 08:15 PM by AHarrison1
more info

[Aaron Eberhard]

Is this a common enough thing that it would be worth throwing in a tool break check between pockets? 

[Newbeeee™]

Although I didn't do it much, I always used what JP suggests - force tool change.

Becuase this gave 100% correct retract/spindle stop, and more importantly, correct re-start procedure with H+D calls and G43 (talking Fanuc).

"Usual code", nice and easy where everyone in the shop has seen it a million times before so no worries.

Where stopping mid prog for tool wear check with the M00 and then press the go button again can lead to all kinds of crasheroos depending what the operator did, and how the machine parameters are configured (from different machine to different machine).

 

[Colin Gilchrist]

6 hours ago, Newbeeee™ said:

Although I didn't do it much, I always used what JP suggests - force tool change.

Becuase this gave 100% correct retract/spindle stop, and more importantly, correct re-start procedure with H+D calls and G43 (talking Fanuc).

"Usual code", nice and easy where everyone in the shop has seen it a million times before so no worries.

Where stopping mid prog for tool wear check with the M00 and then press the go button again can lead to all kinds of crasheroos depending what the operator did, and how the machine parameters are configured (from different machine to different machine).

 

This is where your Post Processor can be edited to properly track what is active, cancel it, retract safely, allow you to inspect/change inserts, and then output a proper restart block, with speeds/feeds, spindle on, and Tool Length Comp reinstated. I would hesitate to use Tool Inspection feature combined with Lead In/Out, because Tool Inspection feature only forces a retract move, it does not "also output lead in/out".

[Leon82]

on fanuc controls i usually single block the tool the the g43 line then switch to edit and search for the comment or the z depth i was at of the operation i want to resume, then start it back up if i don't have a force tool change in there . it works during twp also but tcp i never do because it can move unpredictably.

[Kyle F]

On 1/9/2025 at 11:23 AM, [email protected] said:

Anyway thanks for the responses because the guys on the floor just told me my threadmill is wearing out and they were adding n numbers between the holes to know which ones to re run. With 16 holes I really didn't want to crowd my toolpath manager with 16 operations instead of just 1. We are changing to a .25 cut length multi profile threadmill once they come in, so hopefully that takes care of the tool wearing out so fast.

If I'm ever threadmilling a tough material, or a high quantity of even stainless steel, I'll usually program a rougher threadmill and a finisher threadmill. and by finisher it's basically just for a spring pass or two. Really helps with the woes of dealing with adjusting cutter comp. I'll use the same process for tight tolerance bores/whatever (rougher/finisher/finisher-finisher LOL). Especially helpful when running a pallet pool. 

3 hours ago, Leon82 said:

on fanuc controls i usually single block the tool the the g43 line then switch to edit and search for the comment or the z depth i was at of the operation i want to resume, then start it back up if i don't have a force tool change in there . it works during twp also but tcp i never do because it can move unpredictably.

That's a smart way to go about it. I'm such a puss I don't ever start from anything other than an N block haha.

[Newbeeee™]

6 hours ago, Colin Gilchrist said:

This is where your Post Processor can be edited to properly track what is active, cancel it, retract safely, allow you to inspect/change inserts, and then output a proper restart block, with speeds/feeds, spindle on, and Tool Length Comp reinstated. I would hesitate to use Tool Inspection feature combined with Lead In/Out, because Tool Inspection feature only forces a retract move, it does not "also output lead in/out".

Absolutely - had my post dialled for inspection tool check too and it worked a treat, except the calculation for the distance was "reasonably inaccurate".

But it did stop, retract properly, and get going again properly, so it worked well for visual or changing inserts on a facemill.

If swapping out a solid because the edge has gone, obviously reset tool length. was needed, which meant handwheel and "reset" gets hit and....

[mc since v3]

As far as N#'s, i have mine tied to the op # so the setup sheet and program use the same. if there is a problem it is easier to track down.