Opinions please

[gcode]

Machine -- 4 axis horizontal boring mill

Part  Ø50. hog out

I'm using a 5X swarf tool path to finish the Ø45. floor of a big radial pocket. Tolerance is  -0/+.050

The tool stays at X0. and the motion is in the Y Z and B axis. The tool path looks good.

The operator wants to cut it .010 heavy and he's shifting it with the G54 workoff Z setting

I'm saying he should leave the common alone and use the Wear in the TLO

He maintains it makes no difference, but I think because this is a rotary toolpath

rolling about Machine X0 Z0 we should be leaving the common alone and adjusting depth with the TLO's Wear setting

Who's right?

[crazy^millman]

1 minute ago, gcode said:

Machine -- 4 axis horizontal boring mill

Part  Ø50. hog out

I'm using a 5X swarf tool path to finish the Ø45. floor of a big radial pocket. Tolerance is  -0/+.050

The tool stays at X0. and the motion is in the Y Z and B axis. The tool path looks good.

The operator wants to cut it .010 heavy and he's shifting it with the G54 workoff Z setting

I'm saying he should leave the common alone and use the Wear in the TLO

He maintains it makes no difference, but I think because this is a rotary toolpath

rolling about Machine X0 Z0 we should be leaving the common alone and adjusting depth with the TLO's Wear setting

Who's right?

Adjust the tool offset using either wear or actual length and call it a day. Anything else might scrap the part.

NEVER AND I REPEAT EVER ADJUST THE COMMON.

The operator wants to pay for the original and the replacement plus the lost time then tell him go right ahead. If not then adjust the tool and shut his mouth!!!!!

[rgrin]

Currently doing something similar right now.  Adjusting the TLO is the right call assuming a couple things.

My findings are that the raw G-Code, if set to 0 stock will always cut the same Ø50. regardless of tool offset.  All the tool offset does is position where that diameter will be.

Now, if you were to run that toolpath all the way around the part then your TLO will affect your final size.

 

My opinion is that the probe/pickup sets the work offset and then it is my job to get the tools to cut correctly TO that offset.

[crazy^millman]

1 hour ago, rgrin said:

Currently doing something similar right now.  Adjusting the TLO is the right call assuming a couple things.

My findings are that the raw G-Code, if set to 0 stock will always cut the same Ø50. regardless of tool offset.  All the tool offset does is position where that diameter will be.

Now, if you were to run that toolpath all the way around the part then your TLO will affect your final size.

 

My opinion is that the probe/pickup sets the work offset and then it is my job to get the tools to cut correctly TO that offset.

Machine probably doesn't have a probe if it one of the ones I think it is at their shop. If it does still would be hard to get them to accept using the probe.

[Kyle F]

The operator is wild, I would love to see his train of thought that led him to this conclusion. 

Sadly I am lacking in understanding of exactly how a lot of machine control functions actually work LOL, but I get the gist of G68.2 (G54.4 I definitely need some reading material)

Now, tool length offsets, and how changing the offset will effect the part/program? that's about as F'ing basic as it gets. Apprentice level stuff. Should be an easy choice IMO, and to understand it you don't have to worry about euler angles and rotary toolpaths and center of rotations, etc.

With that being said,... more than a few operators at my shop have suggested much worse 

[ogu79]

THE OPERATOR IS SO RIGHT AND THE BIG MOUTH @crazy^millman YOU ARE THE BIG MOUTH AS USUAL

[crazy^millman]

3 minutes ago, ogu79 said:

THE OPERATOR IS SO RIGHT AND THE BIG MOUTH @crazy^millman YOU ARE THE BIG MOUTH AS USUAL

Thank you for stating the obvious,

[Leon82]

the work offset will either move the slot up or down or out position

[Greg Williams]

If the Machine has TCP then you are correct, without TCP which is probably the case on a Horizontal both options will work. I would use the TLO but shifting the common will also work

[Newbeeee™]

As it's the tool doing the cutting....and if you want it to cut either deeper or shallower....why would you adjust anything but the tool length (TLO or Wear)

Temp adjusting global Z has it's place (basic 3ax paths!) but changing this obviously affects ALL tools....where you only want to adjust the one....

[Matthew Hajicek - Singularity]

Yeah, if you have a 3 axis surfacing path interacting with that, adjusting the work offset would cause it to mismatch.

[gcode]

We ran the first part and it came out OK.

The operator did use Z axis WO Common to adjust tool length.

We are just roughing this part and have a ±.050 tolerance.

To me this just seems wrong, but it seems to be working, probably because we're just running G54

not G54.2.

The reason the guys do this is because the TLO can't be changed in the middle of a toolpath on this machine,

If you change the TLO you have to start the tool path over.

If you change the Z WO common it takes effect immediately.

This is significant when you have toolpaths that run for 1 to 3 hours between program stops.

[Kalibre]

Changing the WPC is terrible practice, even if it works on this particular part. Any workpiece correction goes out the window and all other features/tools are affected if the operator "forgets" to adjust it back.

Easier to just have the habit of defaulting to TLO for adjustments and pretending WPC is just going to scrap parts every time.

[Kalibre]

14 minutes ago, gcode said:

The operator did use Z axis WO Common to adjust tool length.

We are just roughing this part and have a ±.050 tolerance.

To me this just seems wrong, but it seems to be working, probably because we're just running G54

not G54.2.

The reason the guys do this is because the TLO can't be changed in the middle of a toolpath on this machine,

If you change the TLO you have to start the tool path over.

If you change the Z WO common it takes effect immediately.

This is significant when you have toolpaths that run for 1 to 3 hours between program stops.

I have to say, I'm completely lost as to what the process is here. Like, they're changing their WPC mid-cut? To accomplish what?

[Leon82]

Make a path that leaves .05 and a finish with a. Force tool Change. Then you can repost after the feature is known to work

[Ben Wood]

If I understand what is happing either way will get the job done but adjusting the WO common is risky if he forgets to set it back.  I've made that mistake more then once.  I think a program stop before and after the toolpath and then using the TLO to make the adjustment would be the best way.

[cncappsjames]

I wish I could remove the common offset from the offset list. I had to drive 3 hours on a Saturday because "..we don't know what is wrong with the machine... no there isn't ANYTHING in the common offset...". Emphasis theirs. 

30 seconds after I arrive, problem fixed and I'm headed back home.

Uncool.

[Leon82]

6 hours ago, cncappsjames said:

I wish I could remove the common offset from the offset list. I had to drive 3 hours on a Saturday because "..we don't know what is wrong with the machine... no there isn't ANYTHING in the common offset...". Emphasis theirs. 

30 seconds after I arrive, problem fixed and I'm headed back home.

Uncool.

At my old place we had to call a service guy because the machine wouldn't come out of emergency stop 

There was a pile of boxes that had fallen over and pushed it in by the tool changer magazine behind the machine

[gcode]

8 hours ago, cncappsjames said:

I wish I could remove the common offset from the offset list. I had to drive 3 hours on a Saturday because "..we don't know what is wrong with the machine... no there isn't ANYTHING in the common offset...". Emphasis theirs. 

30 seconds after I arrive, problem fixed and I'm headed back home.

Uncool.

I hope you billed them driving time to and from your 30 second service call

[crazy^millman]

16 hours ago, cncappsjames said:

I wish I could remove the common offset from the offset list. I had to drive 3 hours on a Saturday because "..we don't know what is wrong with the machine... no there isn't ANYTHING in the common offset...". Emphasis theirs. 

30 seconds after I arrive, problem fixed and I'm headed back home.

Uncool.

My shocked face

[cncappsjames]

9 hours ago, gcode said:

I hope you billed them driving time to and from your 30 second service call

We did. We had no intention of collecting. We knew the bill would get to the CEO's Office though, and the bill created the desired effect. From then on when we asked them "...don't ask me stupid simple questions like that..." questions, they are FAR less flippant with their answers.  The embarrassment that situation created was pretty epic. I knew with absolute certainty the problem was that, but the setup guy vehemently denied putting any values in there but he was the ONLY person running that machine.

When I ask a question, it's not to waste time, even though it may feel like it. It is not to deflect anything. It is to get to the bottom of the issue as quickly as possible so the machine can get running again. More often that not, solutions are someone forgot something relatively simple. It's not a problem. I forget the simple stuff too from time to time. It's part of the gig.

[MIL-TFP-41]

25+ years ago in my 3 axis days I  would of sided with the operator, or at least sided with the people saying it does not make any difference. Now, with functions like TWP and TCPC being the norm rather than the outlier I would strongly insist people to adjust  wear offsets and leave the commons alone.

On our Toyoda bridge mill with a right angle head the macros write values to the common offsets depending on the orientation of the head. Not sure why Toyoda/Wele decided on that method, but it is effective. It did throw the operator for a loop, he came from a large 3 axis vertical and had the using common offsets method so long it was etched into muscle memory.

 

[crazy^millman]

15 hours ago, cncappsjames said:

We did. We had no intention of collecting. We knew the bill would get to the CEO's Office though, and the bill created the desired effect. From then on when we asked them "...don't ask me stupid simple questions like that..." questions, they are FAR less flippant with their answers.  The embarrassment that situation created was pretty epic. I knew with absolute certainty the problem was that, but the setup guy vehemently denied putting any values in there but he was the ONLY person running that machine.

When I ask a question, it's not to waste time, even though it may feel like it. It is not to deflect anything. It is to get to the bottom of the issue as quickly as possible so the machine can get running again. More often that not, solutions are someone forgot something relatively simple. It's not a problem. I forget the simple stuff too from time to time. It's part of the gig.

 

14 hours ago, MIL-TFP-41 said:

25+ years ago in my 3 axis days I  would of sided with the operator, or at least sided with the people saying it does not make any difference. Now, with functions like TWP and TCPC being the norm rather than the outlier I would strongly insist people to adjust  wear offsets and leave the commons alone.

On our Toyoda bridge mill with a right angle head the macros write values to the common offsets depending on the orientation of the head. Not sure why Toyoda/Wele decided on that method, but it is effective. It did throw the operator for a loop, he came from a large 3 axis vertical and had the using common offsets method so long it was etched into muscle memory.

 

 

Both of you support this statement that this loud mouth will repeat.

On 5/10/2024 at 10:05 AM, crazy^millman said:

NEVER AND I REPEAT EVER ADJUST THE COMMON.

 

[Newbeeee™]

Viewing this on the PeaSea, it shows "NEVER AND I REPEAT EVER"

I have no need to click "expand".

Wise words Ronaldo

 

[ogu79]

10 minutes ago, crazy^millman said:

 

 

Both of you support this statement that this loud mouth will repeat.

 

The all-mighty big programmers Go xxxxing read what the original question was! The all-mighty big xxxxing programmers, you all are so ignorant and do not even realize that you all do not have any understanding that even close to the operator and still mucking him! Shame on all of you! The common offset is handy in many cases, and all the machine builders keep that option. Yes, it has consequences, and you have to be careful, but every single touch on the CNC machines has that potential too.