Why do T, H and D values keep changing? 2020

[Jobnt]

Tried the search, it just hangs for several minutes and doesn't do anything, sorry if this has been covered.

Not sure what's causing this. There's literally no pattern. 

T1 H1 D1

T2 H3 D3

T3 H15 D15

T4 H5 D5

T5 H22 D22

T6 H5 D5

Are there any bugs associated with this or is anyone else having this issue?

[#Rekd™]

I got tired of this.... @Colin Gilchrist showed me how to modify my post so that it forces the T and D to match. 

[crazy^millman]

MCD issue. Change the MCD to fix this issue.

[Colin Gilchrist]

Global Formulas to the rescue!

tlngno$ = t$

tloffno$ = t$

 

Add these formulas, near the top of the Post, starting in the First Column, and you'll never have a H/D number that doesn't match the Tool Number. 

[Aaron Eberhard]

As Ron Said, it's probably this:

I have that set up on my Robodrill for example, where it's old enough that it doesn't understand a diameter offset for tool #5.  I have to use offset #5 for the length, so I have the Diameter offset set to 100 so it will give me 105. 

Also, make sure that nothing changed about using head numbers.

[Jobnt]

1 hour ago, Colin Gilchrist said:

Global Formulas to the rescue!

tlngno$ = t$

tloffno$ = t$

 

Add these formulas, near the top of the Post, starting in the First Column, and you'll never have a H/D number that doesn't match the Tool Number. 

Nice, easy, clean fix. 

28 minutes ago, Aaron Eberhard said:

As Ron Said, it's probably this:

I have that set up on my Robodrill for example, where it's old enough that it doesn't understand a diameter offset for tool #5.  I have to use offset #5 for the length, so I have the Diameter offset set to 100 so it will give me 105. 

Also, make sure that nothing changed about using head numbers.

I have my CD set up to use From Tool. This does make it easier to fix them using the tool manager instead of doing each operation but doesn't keep them the same. If I change it to Add to Tool and set both to zero will that force them to align in the tool manager?

 

Is there a way to do this with a script? Iterate through the tools and align H and D?

[Tim Johnson]

 

 

2 hours ago, Jobnt said:

Tried the search, it just hangs for several minutes and doesn't do anything, sorry if this has been covered.

Not sure what's causing this. There's literally no pattern. 

T1 H1 D1

T2 H3 D3

T3 H15 D15

T4 H5 D5

T5 H22 D22

T6 H5 D5

Are there any bugs associated with this or is anyone else having this issue?

I'm trying a process to make it easier on the operators to hold dimensions on an extrusion that has crazy tolerances.

It's somewhat similar what's above but I'm doing it on purpose.

KITAMURA HX800iLTGA 709-801-604.docx

[Jobnt]

4 minutes ago, Tim Johnson said:

 

 

I'm trying a process to make it easier on the operators to hold dimensions on an extrusion that has crazy tolerances.

It's somewhat similar what's above but I'm doing it on purpose.

KITAMURA HX800iLTGA 709-801-604.docx 45.72 kB · 0 downloads

Back in the day we used different H and D values to do very much the same thing. It's much easier to let the operator make the change via an offset than to re-program or edit the program.

[Tim Johnson]

1 minute ago, Jobnt said:

Back in the day we used different H and D values to do very much the same thing. It's much easier to let the operator make the change via an offset than to re-program or edit the program.

I'm hoping it will help them. They're currently running a similar prototype part and are having a bad time with it and the programmer has been sick for the last couple days.

[JParis]

16 hours ago, Jobnt said:

Nice, easy, clean fix. 

In my opinion, it's not a fix....the fix is to get your control def squared away

I appreciate what Colin is offering but at the end of the day it simply covers for the programmers bad habits and is a crutch. I prefer to teach my 'grammers to work in a properly thought out and constructed work process flow.

JM2C YMMV

 

 

[Newbeeee™]

59 minutes ago, JParis said:

In my opinion, it's not a fix....the fix is to get your control def squared away

I appreciate what Colin is offering but at the end of the day it simply covers for the programmers bad habits and is a crutch. I prefer to teach my 'grammers to work in a properly thought out and constructed work process flow.

JM2C YMMV

 

 

Butttt....back in the day (X6/7ish?) wasn't there a bug where the occasional THD error was thrown even when the Mach/Control Defs were correct?

Which is when Colin suggested this?

[JParis]

6 minutes ago, Newbeeee™ said:

Butttt....back in the day (X6/7ish?) wasn't there a bug where the occasional THD error was thrown even when the Mach/Control Defs were correct?

Which is when Colin suggested this?

Honestly, I couldn't even guess at this point...I cannot say there was, I cannot say there wasn't...all I can say is I don't remember one of that type causing me any problems.

[Jobnt]

1 hour ago, JParis said:

the fix is to get your control def squared away

Unless there's something besides what was mentioned above (i.e. the CD being wrong, mine is not) then it seems there isn't a "fix".

Hence why I asked this: 

17 hours ago, Jobnt said:

Is there a way to do this with a script? Iterate through the tools and align H and D?

The thing is, these T, H and D values match when I start the program. Somewhere down the road they lose their xxxx and I have no idea why or what's causing it.

[Jake L]

1 hour ago, Jobnt said:

The thing is, these T, H and D values match when I start the program. Somewhere down the road they lose their xxxx and I have no idea why or what's causing it.

Not quite what you're looking for, but this is what I added into my post a while back.

pofsnumchk   #Check if T# equal H# / D#	
	  if t$ <> tlngno$, result = mprint(shofsnumwarn + " - T" + no2str(t$))
	  if t$ <> tloffno$, result = mprint(sdofsnumwarn + " - T" + no2str(t$))

 

If there are H / D numbers that don't match the T number the post throws a warning.

If you do need offset numbers to be different than the tool number, you can ignore the warning and still get good code.

[Jobnt]

11 minutes ago, Jake L said:

Not quite what you're looking for

Ideally I'd like the H and D values inside Mastercam to stay the same and quit randomly changing.

The post fix is a fix, but it does not solve the problem because my setup sheets are based on the NCI file not the posted file and will post the errant code.

A script to iterate through all the tools and change the H and D values to match the T would be the second best solution. 

[#Rekd™]

21 minutes ago, Jobnt said:

Ideally I'd like the H and D values inside Mastercam to stay the same and quit randomly changing.

This is what I experienced.......randomly changing although my control definition was set correctly. This was happening back in X7 and I have experienced it in MC2019, MC2020. 

 

 

[Aaron Eberhard]

Ah, okay, that's a different problem and changing the CD wouldn't be it.

I've never had a tool change T/H/D on me unexpectedly..    I know that you can change the H or D offset # in toolpaths > Tool page without it throwing up a warning and it's only saved with that toolpath:

I've accidentally filled out the wrong field due to fat fingering when using tab to move between fields?

If you can catch in the act, I'd send a file over to QC to see if there's anything logged against it.

[cncappsjames]

I always have "Add to tool" selected and it's set to 0 since the advent of the MD/CD. That said, I've also forced my H/D to be T in the post from time to time just in case. I can't recall ever having that problem where random H's and D's pop up. It's probably a work flow issue that creates that problem. 

 

On another note, I've had Tool Offset C (4 column; H/HW, D/R/DW/RW) on just about every machine I've spent time on since the mid-1990's. 

[#Rekd™]

3 hours ago, Aaron Eberhard said:

I've accidentally filled out the wrong field due to fat fingering when using tab to move between fields?

I have had it with the tools set to be numbered sequentially (for a Haas umbrella tool changer) and the tool number goes to say T1 and the H and D go to 0. Once I go into edit tool and type 1 into the T number it changes the D and H accordingly. But without doing this manually it sometimes puts in other numbers.

Not sure of the culprit.

[Newbeeee™]

4 hours ago, #Rekd™ said:

This is what I experienced.......randomly changing although my control definition was set correctly. This was happening back in X7 and I have experienced it in MC2019, MC2020. 

 

 

Yayyyyy....I haven't yet lost my mind.....

[Newbeeee™]

6 hours ago, Jobnt said:

The thing is, these T, H and D values match when I start the program. Somewhere down the road they lose their xxxx and I have no idea why or what's causing it.

Honestly, X+ every day and twice on Sundays!

1x click to check THD, G54/55etc status, Coolant, etc - it's a fantastic double check. Because it's the hot job when someone is on your back that always bite, and we all know whose fault the bang will be....

[Jobnt]

Is there a Chook / Nethook / VBS that I can run to iterate through the tool library and align H's & D's with T's? 

[JParis]

Select all toolpaths, right click >> Renumber tools

[Jobnt]

I don't want to renumber the tools. I want to align the H and D values with the current tools. 

In fact, I'd wager a guess that renumbering tools is one of the things that throws them off.