What is Smoothing Fusion 360 CAM? FF128

hi folks let's dive a little deeper into what exactly this smoothing setting is in fusion 360 cam what does it do when should we use it and when should we not use it welcome to other fusion Friday [Music] a great way to show what smoothing does is to compare these two shapes the shape on the left has a normal circle the shape on the right though is a bit different I've taken that same circle that's shown with a construction line and instead I've added this as a spline let's delete that and recreate it just to show you what I did we're using the spline tool we'll start it in the bottom left will intersect it through the top of the circle and we'll double click here to end the spline so it's definitely not the same shape but it's about the same area but we're going to see massive differences in how fusion 360 handles the shape and how the cam and tool paths are formed around it we're back in the cam environment 2d contour hold down the Alt key lets me pick just that single contour for the arc click OK click on simulate and I've got show points check what's cool about this so we can see two black dots one at the beginning and one at the end we post this code out you can see we've got quite a few lines of code but to better digest what's going on let's pull this into NC viewer so let's head to NC viewer comm I'm going to take that file and just drag it over here and we've got the lead in with our arc what I like about this is if we click on that point right there that takes us to the line before so that's the end of the Z plunge and if I click on the next line its line 142 move the tool to the end of that arc so that tells me that this line here and 140 handles that code right there and what does that line start with it starts with the g2 if we Google G code G to take a look at this tormach article and we can see that G 2s and G 3s are arcs happens to be the g2 our clockwise so if we look at this tool path the tools moving around it like it would a clock and G threes are counter clockwise and this is a great time to tie back into what G code does and it's actually pretty simple it's G ones for straight lines then g2 and g3 s4 arcs and that's a great segue into the shape to the right which is relatively similar in overall size but this spline really wreaks havoc because CNC machines generally speaking can't handle splines so what happens is it takes that spline and it breaks it down into sections of lines and arcs so we've got the same 2d contour set up here no smoothing on yet when we click simulation look at all those points this is how many lines or segments it has to break down our code to get some approximation of that shape and this is kind of one of those aha moments when you realize that there are so many steps along the way that where changes happen between what you have in the CAD side or the engineering or design side and the part that you actually end up taking out of the machine and those changes relate to things like surface finish of the part as well as accuracy and tolerance so in this case we're telling Fusion and the fusion cam side hey I know you don't have a way of converting splines into g-code so break that spline down into various segments to give me code that can run and how we break that down relates directly back to really two things the tolerance and the smoothing tolerance is simple and it comes first in this process your tolerance setting is you telling fusion 360 how accurate and how detailed you want it to make that model that it's gonna drive the g-code off of yes that's right it's not actually using the cad model here to dry this tool path but rather it's making an STL file in the background or tessellating it subject to your tolerance of how closely that should match this shape so what's important there's two things one is it's okay to have a really low or tight tolerance sometimes that's important because you want your final product or your final tool paths to match the cad side of things it's worth noting though that having a really tight tolerance can really increase your computation time and as a general rule on especially on things like adaptive roughing strategies which on large parts can sometimes take a bit of time to compute you're also already leaving stock to leave so there's no need to drive a super accurate tolerance when it's just a roughing up as a general rule we leave it somewhere between half a thousand and one thousandth of an inch we can actually see what's happening with that tolerance setting with the $1 ins of setting simulate that tool path wrap it to the end of it notice I've got stock check here so we can see our stock that lets us then right-click stock save the stock I'm gonna say this one has one 1000 two 1000 tolerance click OK now notice this looks the same simulate go to the end of tool path right click stock save stock and this time I'll type two zero zero one zero tolerance what we can now do is upload these STL files to fusion I've oriented each model in the same location by clicking the corner of the viewcube and then double click on my mouse wheel that zooms out so that they should be in the identical position and that lets us compare especially around the areas where there's more curvature since at the top of the hill as well as at the bottom of this quarter here we can see the different levels of resolution between the 1000 Sand the 10th out tolerance we zoom in on the 1000 the tenth value you can see how many fewer stl services there are on the 10th ow or higher tolerance diversion so the other way of thinking about is tolerance is really affecting the baseline solid model smoothing happens after that what smoothing does is says hey if I can get from this point to that point and say get rid of a couple of points in between so long as that tool path doesn't violate the smoothing tolerance I'll go ahead and get rid of those extra points the cuz there's no way for g-code to directly handle splines it has to convert it into lines and segments we see that with the show points and you'll really see that when we post out the code and we look at how long that code is 119 lines to run that toolpath versus 23 lines total to run the similar shape and similar length to a path when it's just 1g code to handle this arc the reason we want to take advantage of smoothing especially on shapes like these splines is that just like driving a car when you change lanes or you make a turn you do so in a fluid manner both because it's more comfortable to drive that way but also because it's what your car wants to do you're you don't stop turn the wheels step on the gas move again stop turn the wheel it would be very jerky and a lot of times when we're at the CNC machine we wanted to either go fast or we want to make beautiful parts and smoothing coincidentally can help us with both so let's duplicate this tool path and we're gonna remake this one way that I called 1,000 right click Edit passes check smoothing and we'll leave it at the default tolerance right now which is one thousandth of an inch click ok so let's compare these two tool paths simulate look at the number of black dots 1 2 3 4 5 6 7 8 9 10 11 but if we zoom in it's actually 4 than that because a lot of these are two points each point is a line of G code that your machine has to process and it represents a change it represents um acceleration or deceleration and and we it's not what we're looking for when we think about very smooth fluid motion look at the one with one pausing we get rid of almost all of those control points what's awesome is that I know we were able to reduce all of those lines of code without changing the final result by more than one thousandth of an inch so that's really important because there are instances where tolerances and precision really matter but as we've started to learn more about the high-end machine tool world it's funny there's this little diagram you kind of get three different things speed accuracy and surface finish and for me you would think that accuracy and surface finish are the same thing but they're not because accuracy or tolerance would really relate to hitting every single little microscopic point along this unnatural spline shape whereas surface finish a lot of times says hey I'm going to ignore some of those subject to a very small smoothing deviation but I'm gonna let that machine move in a much more fluid manner and that's a good thing the other area where we see smoothing really come into play is the shorter G code and what that means is less code for your machine to process which has two major benefits first off you don't have a modern vertical machining center with things like high speed machining or look-ahead or a really good processor it's just not going to be able to handle the code that you may have even seen this if you're just running a traditional adaptive tool path and your machine just can't keep up the other reason is simply memory size some of these old machines hexam that aren't even that old really don't have much memory so smoothing by reducing the length of code can help reduce the file size which is really important and finally I'll end with a pretty big can of worms which is that on some machines the machine takes care of all of this so this is going to get into more controller specific things often seeing on high-end machines but in short your machine isn't even running the g-code it's using the g-code that we post out and it's processing that it's rida stealing that into its own version of motion control so if you've used the hause there's a code like 187 fanuc has these herm lay has these Siemens has these which are their own versions of smoothing or machine profile tweaks that help it change its own parameters of the tool path and you can set similar things like tolerancing and smoothing as well in those machine parameters and on a lot of those controllers they're better suited to handle it so ironically in those situations you may actually be better off leaving smoothing unchecked here in fusion and letting the controller handle it but for most of us especially those that are running machines like the tormach and the hodge generally smoothing is a really good thing to have turned on and finally we'll end with just a quick demo which is take a look at this the same tool path with smoothing on you can see it's moving around this arc in a nice fluid manner great here's what happens when it's turned off it's just really jerky and just so you see it's not just a tormach thing here's that same bit of code on our hosnian three and here on the Hoss the first tool Pat doesn't have smoothing on as we walk around a circular type shape you can see that the machine accelerates and decelerates running that same tool path but with smoothing turned on you can see now it moves around this circle and a very smooth very fluid manner that just goes to show you where smoothy really can't help troubleshoot or improve your machine performance and help you make better parts I hope you learned something hope you enjoyed take care folks see you soon [Music] you [Music]

Channel: NYC CNC

Views: 33,793

Keywords: tormach, fusion 360, how to, cnc, machine shop, nyc cnc, DIY, machining, milling, CAD, cnc machining, cnc milling, smoothing toolpath, smoothing, surface finish

Id: kSI8FaNpO8k

Length: 12min 35sec (755 seconds)

Published: Thu Apr 19 2018