Tolerance issue affecting lathe roughing

[gcode]

I posted this on the main forum and have received zero feed back.
I was hoping some of the developers would chime in but it's been crickets do far.
To me this seems like a mission critical defect

Post from main Mastercam forum

[Jeff]

That's crazy something that insignificant will cause crashes.

[gcode]

That's crazy something that insignificant will cause crashes.

to be clear, these differences did not cause real world crashes.

my programmer's file would not regen on my machine and the differences on our tolerance pages were the cause

[Jeff]

to be clear, these differences did not cause real world crashes.

my programmer's file would not regen on my machine and the differences on our tolerance pages were the cause

I meant to say crash Mastercam.

[TSmcam]

"Post from main Mastercam forum"

Does anyone go there anymore? I have, or had, a login. Can't remember it. It was a couple of years ago at least that I visited.

[Dylan Gondyke]

Just to note that there are a lot of non-default numbers in the lefthand tolerance screenshot. Curve Chordal Deviation, is used in many ways in toolpath calculation depending on the type. Toolpath tolerance in the left screenshot is 2.5x default value. It'll take a little investigation to understand what happened here but the initial takeaway is the settings that are causing an issue are loosened considerably in many aspects over installation defaults.

[Dylan Gondyke]

Just to update, Jeff (CNC Jeff) mentioned to me that he looked into this and called you, and it was the system tolerance that was causing the issue in this case.

[gcode]

Just to update, Jeff (CNC Jeff) mentioned to me that he looked into this and called you, and it was the system tolerance that was causing the issue in this case.

Yes.. I always though it didn't matter what the system tolerance was because it greyed out and wasn't in use,
Jeff said he thinks it's greyed out because they want people to leave it alone.
A white paper on the tolerance page with a brief description of each setting and it's functions would be useful
It would keep guys like me for getting in trouble blundering around in ignorance.

An example of this is the max arc length set to .0001.
To me this seems ridiculous because a machine tool can't do a .0001" long arc.
When my programmer set it this tight, arc endpoints, I's J's and K's changed a few tenths
and Vericut quit barking at him..
This is from the help section on min arc length..I guess they are talking about arc lengths inside the CAD system,
not arc's output by the post??

Minimum arc length

Defines the smallest arc Mastercam can create. An appropriate minimum arc length prevents creation of very small arcs, for example, when pocketing, creating fillets, etc.

[Dylan Gondyke]

The simplest way I can explain it is yes, these values are more CAD system values (think- things being drawn on the screen, not points being output), so you also have, for Min Arc Length, for example, a value in the Control Definition for the CAM side of life.

It'd be very difficult to drag together the places and things these values affect after 30 years of use in disparate ways. It's also a support nightmare when people change them- similar to the current scenario. It's essentially hidden away there in Config and is just not where most support people or users would immediately look. A user might change them while tinkering one day, see it didn't make a difference, shrug and move on....then be bit by failing solid features, toolpaths, or functions months later that are using their tweaked value. A reseller recreating the file from scratch on the same geometry might see no issue and might never discover the root cause.

Bottom line from my user-glasses-on perspective- unless you have very specific goals, venturing away from the default tolerances anywhere on that page is venturing into the unknown and away from the stable ground that all testing and 99% of real world work is performed on.

[Dylan Gondyke]

A good simple example. Try drawing the smallest circle you can with the default Config tolerances. It'll be one with a diameter of ~0.00006". How does this relate to the config tolerance? Well, the arc length of that circle is around 0.0002"- the default value of the minimum arc length in the config

[JParis]

The simplest way I can explain it is yes, these values are more CAD system values (think- things being drawn on the screen, not points being output), so you also have, for Min Arc Length, for example, a value in the Control Definition for the CAM side of life.

It'd be very difficult to drag together the places and things these values affect after 30 years of use in disparate ways. It's also a support nightmare when people change them- similar to the current scenario. It's essentially hidden away there in Config and is just not where most support people or users would immediately look. A user might change them while tinkering one day, see it didn't make a difference, shrug and move on....then be bit by failing solid features, toolpaths, or functions months later that are using their tweaked value. A reseller recreating the file from scratch on the same geometry might see no issue and might never discover the root cause.

Bottom line from my user-glasses-on perspective- unless you have very specific goals, venturing away from the default tolerances anywhere on that page is venturing into the unknown and away from the stable ground that all testing and 99% of real world work is performed on.

I 100% get what you're saying....so I'll ask....is there a reason that CNC doesn't just lock these values away?

I know from the support side of things that yes, it can be a nightmare tracking some of that stuff down....so if the preference is a user doesn't alter them, I am think maybe they shouldn't even have access to them..

JM2C

[Dylan Gondyke]

There ARE uses for adjusting them- like cranking down on system tolerance in micromachining scenarios. I can count on one hand the number of times I've gone in there to change the value with purpose.

I'd personally love to see an extensive warning message if a user goes to change some of these values. I think, like Gcode said, that's what the intention of the checkbox required to "Activate" the system tolerance was originally inserted for- to give pause to number punching in something different just to tinker. Locking them out entirely would be antithetical to the Swiss Army Knife approach Mastercam has always allowed, however.

[gcode]

There ARE uses for adjusting them- like cranking down on system tolerance in micromachining scenarios. I can count on one hand the number of times I've gone in there to change the value with purpose.

I sure hope the tolerance tables never get locked down.
That could cause some real problems

There are a couple of reasons I do it here
We had an old school programmer who worked here for twenty years
Back in the day extracting curves for toolpaths and solids was not nearly as trouble free as it is now.
You could spend hours cleaning up and trimming geometry to get a reliable chain.
This guy would just crank his chaining tolerance up to .008 or even .010. and carry on.
Five years later I open the file with my chaining tolerance set to .0002 and the file blows up

To open these files you have to adjust your chaining tolerance... then you forget to turn it back down
and the problems are passed on to new files.  That's probably why my chaining tolerance was up to .001 in
the screen shot.

Another setting we change here is "Curve Chordal Deviation"
We do a lot of large lathe parts that have profiles defined by point tables.
We use the points to create a spline which defines the desired profile.
If you chain the spline for a lathe toolpath the results are a heavily faceted surface.
We fix this by using the command "break many/arcs" with a tolerance of .0002"
The tolerance setting in "break many" is limited by the "Curve Chordal Deviation" setting
which I believe is set to .002" by default.
We learned to do this back in V9/X days. Current releases have a lathe toolpath filter that appears
to work pretty well on the these splines, but I've never tried it on a real part.
The profile tolerance for these features is .005" and I'm reluctant to deviate from a tried and true
process. These parts are too big and too expensive to risk on experiments.

[mkd]

Just installed 2023. Can't swing an arc on a mill. Cimco doesn't like it either. What the hexk changed?

[mega]

There was a story about creating basic small surfaces from 3 lines would fail below a certain size unless the system tolerance was set to some infinitesimal small amount