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?

[Laurens-3DTechDraw]

@martin.dunschen @LibertyMachine @al.whatmough

Indeed Martin!

Two seperate issue's.

Of which I'm pretty sure like @LibertyMachine says that the appearance of thin blades due to deflection had been tackled. Like being discussed in the thread you linked: Solved thin blades issue

In almost two years since that has been released, I've maybe seen the thing strips happen 10 times. And only with tools that have a chamfer and were being pushed to/over their limit. So deflection and wrong tool definition caused those.(We should allow for a chamfer on normal endmills. to help solve that)

The issue on which this thread was started and I think is a much harder one to tackle, but also very much needed ASAP, is a collision of the tool with a thin strip of stock 'head-on'.

[martin.dunschen]

So, do you think that being able to add a 'plug' (Al Whatmough's word for it) in the center of the area that is faced and that is machined away last would address the issues raised here? 

Position and size of the plug could be calculated in the software and/or user input. Maybe even the shape could be user input, from a sketch for example.

Let me know.

[LibertyMachine]

I'm not the most inventive sort when it comes to new software solutions.

However, I see two paths:

1) Rework the adaptive kernel so it arcs out of the cut at the end of the slivers. This would help reduce the part getting sucked into the tool. However, this would leave larger portions of material at the ends of the sliver, possibly causing new issues

2) Inside of the Adaptive operation(s), allow for some automatic shape generation, much like the "Tabs" option in 2D Contour. This would be called "Plug" or similar (hey, I said I'm not that creative) and we could choose from an oblong or round shape and choose where we want it. This would effectively automate what I currently do, and that is sketch an island that is smaller than the tool width. Adaptive to that island, and then face it off in multiple Z depths, using a "Both ways" toolpath

Apparently, I can't add an .f3d file to this thread. I suggest @al.whatmough perhaps migrates this thread over to the other forum we are discussing this idea

[Laurens-3DTechDraw]

@martin.dunschen

@LibertyMachine

To be honest this whole pug idea defeats the purpose of adaptive if you then face it.

Also it doesn't work for long thin parts. Because you would need a million pugs and a cutting time *10 to do the same area.

So if you ask me, this works great for facing work with adaptive. All other shapes that you machine with adaptive can have this issue, but won't be solved by the pugs. For those, we just need a way to not cut into the thin end.

[Laurens-3DTechDraw]

BTW.

Saunders video also shows why he is having the issue.

He defines the tool as a straight endmill. You can see that in the video. But you can clearly see it leaves a radius on the part. So it is a tool with radius but it isn't defined as that. So the adaptive can't help that.

One problem solved.

[LibertyMachine]

@Laurens-3DTechDraw I agree, the plug idea is not ideal. (I did say I'm not creative in these areas ) It's just what I've had to resort to to prevent tools from being destroyed or losing parts to gouges when the sliver takes the tool out. The "plug actually needn't be as big as I made it. 60% tool width, perhaps 2x tool width in plug length

If the Adaptive kernel can be worked to allow for reducing the sliver issue, that is great. However, at some point you (the software) will be forced to climb mill into a very thin and tall piece of material.

Unless......

that last sliver pass is done with a conventional cut approach. hmm....going to think on that one for a bit

If I have to choose between part, tool and machine safety and cycle time, cycle time will lose out every time. I don't value time that greatly. (relatively speaking, of course)

[kb9ydn]

As stated already there are two issues here.  The first is with leftover material like shown in the NYC-CNC video.  That one is due to things like tool/machine/work deflection, worn/dull tools, or having a radius/chamfer on the end of a tool that isn't defined in the CAM.  Even these issues could be mitigated by overcutting thin sections so that you aren't relying on the cutting tool to be exactly perfectly sized.  Even a 1-2% of tool diameter extra stepover would likely eliminate this issue.  But this one seems to be solved for the most part already.

The second issue is about how the ends of cuts are handled when the material left is fairly thin.  The problem comes when the tool path tries to cut around the end of a thin section.

Here (picture above) the cutter breaks through a thinner part of the material and there is a small bit leftover that can break off and get sucked into the cutter.  Also, with materials like aluminum that can be kind of stretchy, where the cutter breaks through you can end up with a sort of band or flap of material that detaches from the main block (instead of being cut off in small chips) and can also get sucked into the cutter.  This is essentially what happened in the NYC-CNC video.  You could minimize the formation of these flaps by not leaving long thin sections of material, although at some point you're going to have to cut through thin sections so I don't think these can be eliminated completely.  There may be a way to deal with these however by changing how the cutter approaches the material.

So this is my idea for how to figure out (hopefully) when the cutter is approaching a bad situation:

If you look at the angle of the leftover material in front of the cutter this can give you an indication of whether you are approaching a dangerous situation.  In the above picture you have a fairly small angle (less than 90 deg) which is ok.  It's ok because it means there is probably sufficient material ahead so as to not deflect and get sucked into the cutter.

But when the angle of material ahead of the cutter gets larger you may be running into trouble and should exit the cut now, or maybe even just before you get to this point.

If you keep going though you may get to where the material angle is extreme.  This is potential disaster.  At this point the feed direction would normally start going up and then back around to the right, trying to round off the end of the thin section.  If that thin section deflects it will be pulled back into the cutter, which could easily lead to tool breakage.

And then as the tool goes around the end of the thin section the material starts being pulled back into the cutter.  This is when cutters break.

Eventually as the cutter comes back around the thin section, it will be pushed away again and things go back to ok.  This is still not wonderful though since there is a lot of overcutting, meaning that there is a large stepover compared to the thickness of material left over.  It would be better if the tool was shifted up, maybe 1/8 of a diameter.

So anyway that's my idea.  I think if you could limit the material angle ahead of the cutter to less than maybe 120deg(?) that would keep you out of trouble.  If the angle gets too big, exit the cut and try approaching again from a better direction, where the angle is smaller.

I would attach the file with the tool path example I used but it won't let me.  It's nothing special though, just a simple 2DAdaptive with the most recent HSMXpress.

C|

[Laurens-3DTechDraw]

@kb9ydn

Great explanation of what I believe is happening & I think a great suggestion on how to avoid it.

[LibertyMachine]

Ooooooh. This looks promising. Curious what it does for an open face where it's not working up against a shoulder

[martin.dunschen]

Hi LibertyMachine
I am limiting the smallest turning radius of the tool so it is not able to turn around and keep contact with the stock with a small turn, so it will also make a difference for open faces. I will try and post an image here later.

[Steinwerks]

I very much like the latest version!

I'd have been involved more if I weren't so slammed at work right now, but I appreciate the discussion! 

[Laurens-3DTechDraw]

@martin.dunschen

René is the only one with Legend status but you have just earned yourself hero status!

Those screenshots look 100 times better.!

I think we would need to do some tests to find out the best minimum radius to set but man that looks good.

@Steinwerks@LibertyMachine @kb9ydn

Thanks guys for the input. Because I'm already seeing a great improvement coming from this user debate/discussion and without us all chiming in we can't make a general improvement.

[LibertyMachine]

@Laurens-3DTechDraw I agree. I wish a lot more of these interim solutions were floated by a particular group of users before becoming set in stone..almost like there should be a forum for this sort of thing ......  

[al.whatmough]

@LibertyMachine  I agree - @martin.dunschen stands out as a developer keen for feedback throughout the development process.

We actually have an internal process for recognizing employees when they do great work.  based on your comment, I am sure you all agree Martin is well deserving of such a rewards.

[kb9ydn]

@martin.dunschen, @al.whatmough

Interesting!  So you're putting a limit on the minimum outside cutting radius, similar to how there is a limit for minimum inside cutting radius.  I think that should accomplish the same thing as what I was suggesting, and probably be easier implement since there is already a check for inside radius.  If this minimum outside radius were set to say 1.5-2x to the tool radius, anything thinner than 1-2x the tool radius would have to be taken in multiple swipes.  Of course at the end there will always be that last little sliver to deal with, but that's less of an issue.  It's those long flappy pieces that are more trouble.

This looks like it has real potential.  I'm hoping it ends up as a settable parameter that we can play with.  

C|

[al.whatmough]

@kb9ydn @LibertyMachine @Laurens-3DTechDraw

This is the next question

"I'm hoping it ends up as a settable parameter that we can play with." 

How would you expect to control a setting like this?  the stay down % was an example of a control that turned out to be confusing.  Let's try to get this one right.

We are open to feedback.  The goal is:

It should be intuitive & easy to set a default that works across the board.  Modification should only be needed by power users.

[angelo.juras]

Very good work @martin.dunschen. Looking forward to trying this on a machine.

[LibertyMachine]

@al.whatmough Personally? I don't want to mess with it. It's part of the kernel calculation, I just want it to do exactly what it's intended to do. That being said, I can see how many power users would want to play with it to push it's limits. I'd suggest just making it a "hidden" setting that's only accessible in the Compare and Edit dialog. Remove it from the view of the average user

[al.whatmough]

So is this an option that should always be on, or controlled by a checkbox?

It does have an impact on efficiency.

[LibertyMachine]

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