TOOL NUMBER DRIVE H&T NUMBER PLEASE!!

[Bo Price]

My day job has me stuck in X5, I have a copy of 2017 I use when I'm moonlighting.  No issues with the 2017, but I can't get the X5 tool numbers to sync with the H&T values.  It's like the programmer before me locked parameters somehow.  I've change to my own machine definition and that's solved most of my issues but I still have to manually input T H and D values for each tool.  Any advice would be great,

Cheers,

Bo Price

[gcode]

sounds like the post is hard coded  ( or just broken)

 

[Bo Price]

Sorry I didn't specify it will post fine but when I'm programing my tools in the page where my tool spindle speed etc are listed the tool length and diameter numbers will not snyc with my tool number listed.  Even when I use the right click-edit operations and re-number tools I still have to go in every operation and manually put in the proper tool values.

[Leon82]

Is there an add# value in the control definition for h and d?

 

[Colin Gilchrist]

X5 was buggy with the Tool Numbers matching H and D numbers.

You can fix this in 60 seconds and never worry about it again.

Open your Post Processor File, in a Text Editor.

Find the Variables at the top of the Post, and add these two Global Formulas, starting in the 1st column:

tllngno$ = t$

tloffno$ = t$

Now, every time you Post, MP will ignore the settings in your Tool Page of the Operation, and will Force all H and D numbers to match the tool number.

You can ignore whatever is inside the dialog box in Mastercam. Only the T# will matter, since the global formulas will do the work for you.

[gms1]

1 hour ago, Colin Gilchrist said:

X5 was buggy with the Tool Numbers matching H and D numbers.

You can fix this in 60 seconds and never worry about it again.

Open your Post Processor File, in a Text Editor.

Find the Variables at the top of the Post, and add these two Global Formulas, starting in the 1st column:

tllngno$ = t$

tloffno$ = t$

Now, every time you Post, MP will ignore the settings in your Tool Page of the Operation, and will Force all H and D numbers to match the tool number.

You can ignore whatever is inside the dialog box in Mastercam. Only the T# will matter, since the global formulas will do the work for you.

I have to deal with this every day here because I switch from 4 different machine control styles all the time. Not being able to match what I see in mastercam and the posted code scares the bajesus out of me because of all the lovely gotchas Ive had with this software over the years. Do people use this type of global parameter stuff all the time?

[Ocean Lacky™]

In your Control Definition/ Tool, What are the settings?

Try "Add To Tool" radio button and Length and Diameter settings should be "0"

[Colin Gilchrist]

3 hours ago, gms1 said:

I have to deal with this every day here because I switch from 4 different machine control styles all the time. Not being able to match what I see in mastercam and the posted code scares the bajesus out of me because of all the lovely gotchas Ive had with this software over the years. Do people use this type of global parameter stuff all the time?

Once you make your Post do the work, it is 100% rock solid. 100% of the time. You NEVER have to worry about setting anything incorrectly again. No messing with MD, CD, or Toolpath settings.

In other Posts, where you might have an offset, that is handled like this:

tllngno$ = t$

tloffno$ = t$ + 40

So you post with the first Post Processor, and everything matches (T/H/D). Now, you post with the 2nd post, and H = T, but D = T + 40.

 

Wouldn't you rather do this one time, and never have to worry about anything besides the T#?

This is what these two Global Formulas give you; peace of mind.

[Colin Gilchrist]

1 hour ago, Ocean Lacky™ said:

In your Control Definition/ Tool, What are the settings?

Try "Add To Tool" radio button and Length and Diameter settings should be "0"

While this normally works; in X5, the settings are BUGGY. Which means that even with that setting "correctly" set in the CD, you can grab T11, and have "H13" stuck in the Operation Dialog. It is a bug.

I know because I scrapped a $4k piece of material over this very bug in X6. Since that was on a contract job, I never got paid for my programming time. To say I have some experience with this annoyance would be an understatement. So now, every single Post I write gets those 2 Global Formulas right at the top of the Post.

[Newbeeee™]

2 hours ago, Colin Gilchrist said:

While this normally works; in X5, the settings are BUGGY. Which means that even with that setting "correctly" set in the CD, you can grab T11, and have "H13" stuck in the Operation Dialog. It is a bug.

I know because I scrapped a $4k piece of material over this very bug in X6. Since that was on a contract job, I never got paid for my programming time. To say I have some experience with this annoyance would be an understatement. So now, every single Post I write gets those 2 Global Formulas right at the top of the Post.

x5 is the reason why we implemented x+ set sheet and configured it so we got planes and t/h/d and coolant output. 1x click and a great (fast) double check.

and ouch Colin...

[Bo Price]

Thanks Colin!!

Cheers,

Bo

[Colin Gilchrist]

57 minutes ago, newbeeee said:

x5 is the reason why we implemented x+ set sheet and configured it so we got planes and t/h/d and coolant output. 1x click and a great (fast) double check.

and ouch Colin...

Same thing applies regardless of the Mastercam Version. Your solution was to implement another method of manually checking for issues inside the Mastercam Operation. I'm sure it was effective for catching the errors, but it requires extra time to spot the issue, then more time to go and fix the issue inside Mastercam, and repost the code. With the Globals, it just eliminates any possibility of messing up. And it's one less setting the programmer has to concern themselves with. The only thing I worry about is setting the correct tool number, and the Post takes care of the H/D settings.

 

[Newbeeee™]

Fully agree Colin and i also implemented your post mods 😆

But x+ is also great to catch coolant and planes too. Planes especially because that can be an expensive bang... 

[jlw™]

Speaking of X+ in regards to this, does any one know of a way to get X+ setup sheet to output a misc int/real?

[gms1]

21 hours ago, Colin Gilchrist said:

Once you make your Post do the work, it is 100% rock solid. 100% of the time. You NEVER have to worry about setting anything incorrectly again. No messing with MD, CD, or Toolpath settings.

In other Posts, where you might have an offset, that is handled like this:

tllngno$ = t$

tloffno$ = t$ + 40

So you post with the first Post Processor, and everything matches (T/H/D). Now, you post with the 2nd post, and H = T, but D = T + 40.

 

Wouldn't you rather do this one time, and never have to worry about anything besides the T#?

This is what these two Global Formulas give you; peace of mind.

I too got burned a few times on very expensive parts due this crap. I think I just went the opposite away than you did and now I just double/triple/quadruple check these things. Your fix looks like something i should have done a loooooong time ago lol. That is going to be a hard thing to break for me not seeing the stuff in mastercam match my posted code

[Colin Gilchrist]

12 minutes ago, gms1 said:

I too got burned a few times on very expensive parts due this crap. I think I just went the opposite away than you did and now I just double/triple/quadruple check these things. Your fix looks like something i should have done a loooooong time ago lol. That is going to be a hard thing to break for me not seeing the stuff in mastercam match my posted code

While hard to break, once you do, and your Post takes care of making everything work, all you have to worry about is the proper Tool #. That's it!

The only people whom this fix doesn't "work" for, are programmers that want to use "multiple D values" with the same tool number. In that case, I typically use a Miscellaneous Integer, and have that control the "D value" for a particular operation. I add some logic that "detects" if that MI is active, and if it is, I use the 'update global' function in MP to have 'tloffno$ = mi_value', instead of 'tloffno$ = t$'.

The nice thing about using the Global Formulas to control the H/D values is that you don't even have to look in the H/D parameter fields in the Tool path. Just ignore them, no matter what they are, because the Post takes care of it for you, every time.

If you are one of the programmers who always has T = D = H, then the fix takes 30 seconds, in each Post that you have. It takes longer to open and save the Post, than it does to paste these formulas into the Post itself. (Just make sure the formula starts in the 1st column!!!!)

Quote

now I just double/triple/quadruple check these things.

How much extra time and anxiety could be saved if you just never, ever, had to worry about this particular bug?

 

[kens1]

I have a machine with a 24-tool magazine where we have standard tools set up with preset lengths (using D & H registers of 25+). When I renumber the tools in my program, I input the starting tool number, increment by one and turn off the "length and diameter offset value to be added to tool". I would get the proper tool number with the saved offset number (from my tool library), so I would get T15 H30, for example. If it was a non-standard tool and I wanted D & H to match the tool, I would check the boxes to add 0 to the tool number (T16 H16). A few months ago, I started getting D=0 & H=0 on all tools that I renumber, whether the boxes are checked or not. I didn't do anything to change the post or the control definition. Any thoughts?

[Bo Price]

On 1/9/2018 at 6:55 AM, Colin Gilchrist said:

X5 was buggy with the Tool Numbers matching H and D numbers.

You can fix this in 60 seconds and never worry about it again.

Open your Post Processor File, in a Text Editor.

Find the Variables at the top of the Post, and add these two Global Formulas, starting in the 1st column:

tllngno$ = t$

tloffno$ = t$

Now, every time you Post, MP will ignore the settings in your Tool Page of the Operation, and will Force all H and D numbers to match the tool number.

You can ignore whatever is inside the dialog box in Mastercam. Only the T# will matter, since the global formulas will do the work for you.

I've entered these values at the top of my post and the D value is following the tool but the H value is not, any ideas?

[Bo Price]

This is the first time I've ever edited a post so bear with me:)

[Colin Gilchrist]

Sorry, I think I gave you a spelling error.

Try this:

tlngno$ = t$

[Colin Gilchrist]

If you start typing 'tl' into the Mastercam Code Expert Editor, there should be a "code help" that drops down, and is filtered based on what you type into the Post. You can hover over the variables that are displayed, and a help tip will pop-up, telling you what the variable is used for...

[Bo Price]

Most excellent!!!  I'm really excited to have this fix.  I"m going to put this in my post for my shop version which is 2017 and doesn't have this issue, but you can never be too safe!!!

I'm just usig the Mastercam X Editor to edit the post, how would I get Code Expert Editor?  

 

Thanks again!!  I owe you a beer or 6 if you ever make to the Left Coast!!

[Leon82]

In the start menu under mastercam folder usually.