Adaptive or Contour paths on the CNC

[Jasonb]

I've answered this in a new thread as hopefully a few of the other CNC users may chip in to say what methods they tend to use when machining

In another thread John asked

What is your conclusion regarding adaptive tool paths v contour? I have only used the later. I  can see the logic in wearing out the cutter along the flutes rather  than the bottom. I would have to re learn what width of cut to go for  specially on steel.

Probably easiest to read my comments in the thread that I did the video for

https://www.model-engineer.co.uk/forums/postings.asp?th=181920#2798091

But basically I use the adaptive to remove the majority of the waste on all but thin sheet (upto 3mm), If there is a considerable amount of waste to be removed say an L shaped component then to reduce the work cutting from a rectangular block I'll saw a corner away first and set that rough L shape as my stock.

I typically use 6mm 3 flute cutters and on steel would be using a vertical depth of 6mm and a stepover of 0.6mm running at 5000rpm and feeding at 500mm/min

As an example these are the main tool paths to the current engine projects base.



Firstly an adaptive to remove metal above the solid body with a standard length cutter, done in two depths

Then a second adaptive with a long reach cutter to remove the remainder, you can see the levels as the tool paths stack up in 6mm increments and that stock has had the corner sawn out.

Lastly a ramp with a 1mm corner radius cutter to finish all the sloping surfaces as I wanted it to have draft angle like a casting


J

PS Enjoying following the bike engine build

[Jasonb]

Should add that in f360 there are two stepdown parameters that you enter on the 3D adaptive cuts. The first if the max depth you want to cut based on what your machine and tool can handle, I typically go with 1D so a 6mm cutter will be cutting 6mm vertically. The second is the fine stepdown which is what that 6mm will be divided up into as the cutter gets to any sloping surfaces, depending on what I'm doing the finish cut swith this will range from 1mm to 0.5mm

Attachment show the first 6mm has been removed and the finer steps cut as the tool moved up to -5, -4, -3 etch and the second 6mm layer started, second shows all the fine stepdowns but majority removed with as much of teh sid eof teh cutter as possible.

Photo safter all adaptive to that side



And finishing cuts done



Bead blasted

[steamer]

I use adaptive mostly   but I don't push too hard.   Certainly not 500 IPM!    50 is fast on my little Tormach.

Dave

[Jasonb]

Bit of a typo there now corrected it should have read 500mm/min not 500rpm which could have read as ipm

I have feed aluminium at upto 1000mm/min (39ipm) but feel happier at 600 as a general speed tweaking depending on tool and type of cut, 500mm/min (20ipm) for steel

Having a high feed rate does help if you are using the free version of F360 as rapids are derated to your feed speed. That's also another reason for using adaptive as if you set the stay down distance larger you have the option of a faster non engaged feedrate that compensates for the loss of a rapid return to the start of the next cut.

[dieselpilot]

The function of adaptive, if it's a good algorithm, is to maximize material removal while avoiding overloading the tool(mostly on inside corners). The "adaptive" part is adjusting chipload along the toolpath to keep the cutter at whatever max you've set in the parameters. Inside corners/radii are the trouble spots. The high feed portion is optional, but obviously, in industry it's key. Adaptive paths can waste a lot of time, if you aren't anywhere near the max load of the cutter. On light machines adaptive can keep chatter in check. It takes some testing to sort parameters

If cutting from a minimum stock blank like that you can do a few contour passes at full depth and not really be any slower and with that particular part not rick the cutter. That part has very little stock removal and no tight inside corners or radii. It's a poor example of the benefits of adaptive. For simple parts like this I don't bother with adaptive as it virtually always take longer, (mind you this is production where a few seconds ads up). If, like the OP in that thread, you're cutting from sheet, it's a different story.

Like all things, it takes time, trials, and experience to find what works "best".

[Jasonb]

Yes on those dog bone shaped links it is probably a toss up between the two, there was about 3mm ff waste at the ends so would need a few passes around the contour to avoid a heavy cut at the external corners, F360 tells me there is about 12 seconds in it between adaptive and contour.

[vtsteam]

Thanks for starting this thread, Jason. Even though I don't presently cnc mill, I'm interested in it as a topic, and these explanations of your experience and practice are really helpful. 

[John Roberts]

All interesting stuff . I guess you guys use G wizard to check step over, step down and feed and speeds before cutting the part.
I know nothing of Fusion360. I use Visualmill for my CAM

[blighty]

how are you getting on with the "free" version of Fusion 360? as in tool changes, speeds and feeds.
plus, as the free one only lets you have 10 drawings in the bit the left (sorry forgot the name of it) how does it work when your doing assembles with more than ten parts.

when fusiongeddon  happened a few years back, i got the 3 year lic' yes i can have tool changes and don't have to archive anything.
but you lost quite a few function. so seemed a bit silly that now you have paid for it you get less on some points.

swings roundabouts.

[steamer]

All interesting stuff . I guess you guys use G wizard to check step over, step down and feed and speeds before cutting the part.
I know nothing of Fusion360. I use Visualmill for my CAM

Fusion 360 has a full simulation package as well, which has saved my bacon more than once.

Dave

[Jasonb]

All interesting stuff . I guess you guys use G wizard to check step over, step down and feed and speeds before cutting the part.
I know nothing of Fusion360. I use Visualmill for my CAM

F360 has a fairly good tool library and each tool has a list of speeds and feeds for various materials that you can just click on and use, I have entered data for the tools I commonly use such as the earlier mentioned 3-flute cutter which I have set as no coolant, 5000rpm, 500mm/min feed and will adjust that if needed depending on the job. If it is a tool I don't often use then I'll pick it from F360's list and also pic the material and then make any adjustments to suit my machine which is often a reduction in spindle speed to my max of 5000rpm and a pro rata reduction in feed to keep chiploads to what the KX-3 can handle. F360 will give you surface speed and chipload based on spindle speed, feed and number of flutes entered or you can do it the other way by entering chipload it will give you the feed rate for that cutter and speed.

As Dave says F360 also has a simulation so you can see your stock being cut away to leave the final part, it will flash up red if it detects a clash such as plunging deep into the work rather than a leading outside of it, or if you don't have enough tool stickout it will show the effects of thr collet holder ploughing through the work not only as a clash but negative material removal. If you look at my screen shots of the green and dark blue images these colours show the model surface in green and any stock left in the blue so you can see if you need to go back into an internal corner to remove material left by one that is too large for example. It can also show toolpaths though I often find they clutter things up on a complex part. You can also model fixtures and vices etc if you want which will allow you to see if the tool runs into something it should not.

Typical simulation here , (don't know why I had the cuts start with a helical ramp)

<a href="https://www.youtube.com/watch?v=_WLXVA2JzBM" target="_blank">http://www.youtube.com/watch?v=_WLXVA2JzBM</a>

Stepover and stepdown again F360 fills it in but I find it is usually more than my machine can manage so reduce to what I have found works which taking that 6mm cutter in steel would be 1D or 6mm Ae (vertical stepdown) and 0.1D Ap (sideways stepover)

[Jasonb]

how are you getting on with the "free" version of Fusion 360? as in tool changes, speeds and feeds.
plus, as the free one only lets you have 10 drawings in the bit the left (sorry forgot the name of it) how does it work when your doing assembles with more than ten parts.

It's not been too much of a problem

I don't have auto or even quick change tooling so need to stop and replace a tool and set it's height so provided I group operations done with the same tool together its been no real loss to me. I can still run a part with say three paths without stopping if it is the same tool so could flatten the top, use adaptive to remove the bulk and then do a finish contour without having to run each separately. Only if I want to say then drill a hole do I need to close the previous program and load the next which is a few seconds rather than just clicking on start once tool has been manually changed. Simulation gives me a good idea of how long until a tool change is needed so I can go off and do something else in that time if it's a long one.

Speeds and feeds are not affected so no problem there.

Rapid's are affected and default to cutter feed rate, I do get an increased run time due to this but by tweaking things it can be reduced. Firstly the rapids on my Machine are a lot less than on an industrial one so difference between feed rate and rapid is a lot less. As said I tend to remove most of the waste with adaptive feeds and F360 has the options to set a" fast non engaged" feed rate so if cutting feed is 500mm/min I'll set the non engaged to 1000mm/min which is not far below my rapid rate. I can also get more non engaged time by setting the staydown distance and percentage high. There is also the option to cut "both ways" with a lot of the paths which can save time but I find the machine sounds a lot happier climb cutting so do just about everything climbing. This is where the simulation is good a sit gives you a time for each operation and you can play about to get the run time down.

As I design and Draw in Alibre and just import a STEP file from that into F360 for the CAM I don't have a problem with the 10 active items. ten is more than enough for me to have as instantly editable and I can still have a lot more there which with a bit of shuffling about can be changed from read to editable quite easily. I do think it is possible to have more than one part in a single F360 file as you can treat each as a sepertate body but as I don't use it much have only gone down that route for cutting from irregular stock where I model that as a body.

[Hugh Currin]

Jason:

Very useful and interesting thread. I haven't been depending on the F360 feed/speed numbers but since you've found them usable I'll give them a second look. Yes, the feed/speed numbers should be solid, but depth of cut and step over are very machine dependent. I'm moving back and forth between a Bridgeport sized knee mill and a small bench top mill (PM728). My sense of capacity gained through the knee mill isn't useful on the bench mill, it required noticeably lighter cuts. You're rule of thumb should prove useful, they sound like they are in the ball park.

Thanks.

Stepover and stepdown again F360 fills it in but I find it is usually more than my machine can manage so reduce to what I have found works which taking that 6mm cutter in steel would be 1D or 6mm Ae (vertical stepdown) and 0.1D Ap (sideways stepover)

[blighty]

Jason

so not as bad as first thought.

but as using 360 for all drawings, cam stuff and multi part assembly's. plus having  a cnc lathe with tool changer and a mill with jobs with 12plus tool changes.
the free version that i was  using would of rendered most of it useless. or do separate tool paths and load them up as and when a tool change was needed.
could see a lot of scrap being made if i did that.

do you find yourself cheating with tools as in... ill make it a 3mm rad cos' im using a 6mm cutter. if its a 2mm i will have to do another tool path and change the cutter......
also like....use bull nose cutters, you can use the same tool for roughing and finishing on a "3d" surface. saves on a tool change.

[Jasonb]

Well if you had all that lot it would be worth paying so you could get the best out of the equipment.

If I was not happy with Alibre or did not have so many engines drawn up with it then it would be worth thinking of no longer paying for Alibre and put the money into Fusion but as I like Alibre and only do a few hours son the CNC a month don't see much point at the moment.

With the amount I do it is no big deal to change a tool so I won't let that dictate what I do. However I do find now when I'm drawing up an engine that if a part is likely to have some or all of it done on the CNC then I'll draw it up a bit differently. For example where I would have chosen a nice easy round number for an internal fillet, lets say 3mm which would have allowed me to either drill out the corner points or wind a 6mm cutter into the corner I'm more likely to now draw the radius at 3.2 or 3.3mm just so the 6mm cutter on the CNC can run around the internal corner rather than into it which gives a high percentage engagement and if chatter is to be avoided the speed needs reducing.

I don't tend to use a ball nose for roughing and then finishing as the slow surface speed in the centre means you can't feed so fast so I will tend to use a flat cutter to do the adaptive leaving about 0.3mm and then go back and run a finish path with the ball on a fine stepover. I have bought 4 flute ball nose cutters for this rather than the usual 2 flute as the finishing cuts are small I can feed twice as fast with the 4-flute than a 2-flute with same chip load and get the job done in half the time

Also depending on the part I quite often use a corner radius cutter rather than a ball nose for finishing because the surface speed is greater with a 6mm cutter that has a 1mm radius corner than it is with a 2mm ball nose so closer to optimum cutting speed and less chance of clogging the cutter particularly if working on aluminium. They are also stiffer and have better reach than small ball nose cutters. I have these in standard and long shank which are good for 2 or 3 degree draft angles where a small dia ball nose would see the holder or shank hitting the work and the long neck ones are fragile.

That base "casting I showed earlier is a good example, screen shot from the simulation showing how the 1mm internal fillet could be reached with a reasonably rigid tool rather than needing a fragile long neck 2mm ball cutter cutter. Part is 34mm high and tool needs to run 1mm below the bottom to complete ramp cut so I had 37mm stickout but as stepover was only 0.2mm very little load on it and good enough to go straight to paint.