Adaptive machining improvement?

[LibertyMachine]

This idea is prompted by THIS THREAD and my own personal experiences.

When Adaptive clearing a large area of material where there is nothing left at the Z plane (almost as if you had faced it) the last few cuts can get quite hairy, especially if you have enough depth of cut or it's a troublesome material. Currently, pretty much the only way to prevent part or tool destruction would be to Adaptive clear to an "island" and then have a facing operation remove that last little bit.

I'd like to think there could be a way to better automate it. I'm thinking a small dialog much like there is for 2D Contour and "Tabs". Select "Island Safety" or some such name and define shape and location. Or, it could be parameter driven, such that it would be 60% of tool width or similar.

Thoughts, comments, criticisms?

[LibertyMachine]

Checkbox, imo. This issue isn't really noticeable when dealing with shallow depths of cut. Not certain what it should be called...

[Steinwerks]

I vote checkbox with default on, and setting controlled in Compare and Edit dialogue. Also in Show Advanced in HSMWorks. 😉

[Laurens-3DTechDraw]

@al.whatmough

I vote always on. 

We praise ourselves on delivering toolpaths and settings that are right 99% of the times. I mean we don't want 1000 settings, we just want to do it right for the user. And personally, I think it's always the safe/good choice.

Productivity loss should be minimal. I mean the only loss you have is the extra repositioning move. Which can, of course, add up in the end but it's not like you are adding 20%.

On the other hand, you also get productivity gain in easy programming where you now have to work around this problem. And quite often go slower(Programmed or with the feed-override at the machine) when you get to this problem part of the cut.

I would like to know what @Rob.Lockwood thinks about this.

[Laurens-3DTechDraw]

@martin.dunschen

Have you seen if this method doesn't cause unwanted extra moves on a piece with 90 degree corners?

Because I think you get a pretty small radius on the first couple of cuts on the outside as well.

[Rob.Lockwood]

@Laurens-3DTechDraw 

I see a behavior that is probably good the majority of the time (and should be default-on) but that is highly likely that a user will want to alter it; so the question is whether to expose the option in the UI or not, rather than whether to give the user the option. This seems like one that belongs buried (in compare/edit) like the 'stay down linking distance' parameter, hopefully to be driven in the future by a work-piece material definition, or something.. but it would probably require some real world testing to see where it excels, how much impact is had on overall effeciency, etc. If the tradeoff is such that users want to change the behavior more than something like 1-2%, a checkbox is probably warranted. I doubt very much that this needs more exposure within the UI than a checkbox, and a checkbox with in concert with a compare/edit dialog exposed parameter (to control radius size) seems the maximum a user would need.

Probably, the easiest way to evaluate is to toss the feature out as a kernel update with a defeat option buried in compare/edit, and see how many people use it/complain..

[kb9ydn]

I would say definitely default to enabled.  The efficiency impact I would expect to be minimal and less important that tool safety.  Premature wear/breakage of tools is a hit to efficiency as well.

For those who want to override it though; I expect they would want to control the minimum radius value so having a check box really gets you nothing.  You might as well just have a numerical value that always defaults to some safe value, like a percentage of the tool radius (200%??) or maybe relate it to the maximum depth of cut or something like that.  If you want to change the value, fine.  Otherwise leave it alone.  The difference in UI real estate of a check box and a number entry box I think is insignificant (in this case).

As for where to put it; I generally don't like hidden parameters but this one is probably ok not being exposed in the main UI.  If people complain about efficiency it could be exposed later.

C|

[angelo.juras]

I like all these suggestions. If that last sliver of material was the optimal load amount, it could eliminate some of the issues. What if that last cut where the endmill changes direction doesn't roll around the edge of the material and engages material. Instead comes off like tangential extension. Yes, it looses its constant engagement for a moment but that could help. I will provide an image of what I'm talking about.

[Rob.Lockwood]

@kb9ydn I think the difference is less real-estate, more 'what does this DO'/'paradox of choice' logic.

A check box is fairly straightforward in that regard; un-check the box, get the old behavior. A percentage leaves someone screwing with the percentage box to figure out the optimal thing.

Al brought up the stay-down percentage option, and I think it's a great parallel. What is the correct setting for that option? I bet the percentage of users that can even tell you a single relevant detail of 'how it works' is fairly slim, and communicating it clearly through UI is seemingly a difficult task, let alone the number who could genuinely answer my question. Hell, i'm not sure I could answer it with a straight face.

[angelo.juras]

[kb9ydn]

@Rob.Lockwood

Yeah fair point.  A check box is easier.  I was just thinking that anyone who really wants to mess with it would not be satisfied with an on or off setting.  I guess it really depends on how much of an impact it has on efficiency.  If the impact is minimal then it probably doesn't matter.  What it does do though is relieve some of the burden on the developers to pick a "perfect" value up front.  Since it's still sort of an unknown I think it's better to have more flexibility from the user's end instead of less; at least for right now.  Later on once there's more data on it, a better decision can be made for the long term.

As for the stay down percentage, the biggest problem there is that there is no explanation anywhere (help files or tool tips) of what the percentage actually is.  Percentage of what?  And why is it a percentage instead of just a simple distance?  To me it would make FAR more sense to have two values that control stay down, a minimum distance and a maximum distance.  Below the minimum distance it will always stay down down.  Above the maximum distance it will always retract.  Between those two it can do whatever it wants.  This allows for maximum flexibility, minimal UI space, and is easy to understand and explain.

Or if you want even simpler, just have a single threshold distance where any move shorter than that will stay down and any move longer will retract.  The existing "maximum stay-down distance" already kind of looks like it should do just that, but it doesn't.  In fact this specific setting has honestly baffled me from the very beginning.  

C|

[Laurens-3DTechDraw]

@angelo.juras

Pretty sure I would hate that more than the current move.(Both aren't good for the tool but the current then at least doesn't cost any time.)

You just don't want to come in on the thin end unless you have to. So for an (adaptive) facing operation, you have to and it's fine. But if you have the possibility to start from the thick end I would say do it.

[AmishSolanki]

Just making my way thru this thread, funny enough this has always bothered me. I recently came across this issue again with some 4140PH last week.

The sliver left here became extremely hard, would get pushed when the endmill moves to the backside, and well the noise it made when the endmill broke it off was... not nice. Endmill didn't break but by the end it had some nicks on it.

Lots of good options you've all left here, I like being able to leave the way it works as it is (for easier material) but then for some harder stuff as in below, it would be nice to have some options to deal with this. Cheers!

[Rob.Lockwood]

@AmishSolanki in the instance shown, I think using Slot clearing option would help tremendously, and potentially be a better option even than this proposed change..

[scottmoyse]

Here's another interesting option. And a bit of a discussion on it. @Rob.Lockwood you have access to this in your box of tricks don't you? What do you think?

https://www.instagram.com/p/BoxAqVqAWoy/

To me it still looks like it has the potential to leave a slither, but maybe adjusting the diameter of the bore will disrupt the toolpath enough to control the width of the final slither?

[Laurens-3DTechDraw]

@scottmoyse

And a lot of the high feed sidemilling tools cannot do the helix down.

So for me, that's not really the solution either.

I must say that with more and more practice I can get it to behave the way I want with the curve-in radius. ()

Made a short video for @Gujustud to show the differences in curve-in radius. Not sure it applies to the case he showed in this thread but other cases could work great.

[scottmoyse]

Maybe there isn't one answer Laurens. Maybe it needs a few options, so dismissing this along with other options because it isn't perfect might not be the right approach. And it shouldn't have taken you the length of time it has to solve it in your environment/application, lesser humans will never get it.

[Laurens-3DTechDraw]

@scottmoyse

We do strive for perfection right?

I'm all for a solution to the problem, but less so for 10 "hacks" that might work for a different case each.

I don't think that makes it any easier on the user either.

And I would have gotten to all this with the curve-in radius much quicker if it had just been shown in all three softwares instead of being buried in the compare and edit or show advanced.

[scottmoyse]

10 hacks? Let's not exaggerate.

[Rob.Lockwood]

@scottmoyse yeah, but until pretty recently, they weren't even doing microsteps or any sort of 'bottom up' functionality, so the whole toolpath was just utterly worthless.. It may be a bit better now, but i'd still put my money on that toolpath being more competitive with adaptive clearing circa 2010, with 'pillar cutting' being the possible singular exception.

Officially, we're a few versions back, so I have a hard time playing with NX's 'new toys' in general.. and if i'm being honest, the applications for this don't exactly fit the work we're doing.

[Anonymous]

Hi All, 

Was this issue ever definitively solved?

I know this is an older thread, but we just had a nice 1/4" tool snap when it sucked a thin wall into itself during adaptive clearing.  (6005-T5 aluminum extrusion with 1/8 inch walls.)

When it clears a pocket and goes through the wall it make a super thin unsupported wall that vibrates and finally broke a tool.

We of course have the latest version of F360 cam.  Is there an option or a knob we can turn to avoid this phenomenon?

Thanks!