Fusion 360 Lathe Tutorial

[Music] hey everyone kevin from mechanicaladvantage.com today i thought we'd switch gears a little bit and instead of focusing on milling toolpaths we could take a look at what it takes to get started with lathe inside of fusion 360. to do this we're going to use a tutorial file that autodesk has supplied with fusion and to get to that tutorial file i'm currently in a project what i'm going to do is click on the home button and then i'm going to scroll all the way down until i find the samples directory and inside of samples there's a cam samples folder i'm going to double click on that folder and then i'm scroll down a little bit more until i find a file called 2x turning quick release and i can either double click on that file or right click on it and choose open and when i do that fusion's going to go ahead and open that file for me when i get the file open i can now close my data panel because i don't need to see the data panel anymore once i have the file open so we open this up we can see the part we can see it set it inside of a a chuck and we are ready to go ahead and add some tool paths now this part already has a setup and tool pass added to it we're not going to use these you guys can minimize these or i'm just going to right click on this setup and delete it all together and then now what you could also do is go up to the file and choose save as give this a name and choose what project you want it to go to so it saves to your directory i'm gonna hit cancel and you'll note that you can't hit the save button this is currently in read-only status so you can't change this file once you open it up all right once you have your files saved to your location we're ready to go ahead and make a setup so from the setup panel i'm going to choose the setup command and we're going to see our setup pop-up now if we look under the operation type we're set to milling and we're going to do a turning part here so i'm going to hit the drop down and i'm choose turning or mil turn and when i do the access is going to shift a little bit but fusion isn't quite sure where my center rotation is going to be so i'm just going to go ahead and it's looking for a z-axis i can click on any round face i'll just go ahead and click on that face right there it doesn't really matter which one you choose and now you can see my z-axis is lined up with the the axis of my part i also had to tell fusion which model it is that i want to machine in this case so where it says model nothing i'm just going to go ahead and click on the model itself and that gets me oriented that way so now i can see that i have uh the stock on my part and i'm gonna make a few more adjustments to it but for the most part we're we're making some progress here i don't like the way this x-axis is facing i want the x to to face away from me y to come up and z to run down the center line of the part so to fix the x-axis i'm going to expand up my models i'm going to expand out my design and then i'm going to expand out my steering quick release and i'm going to turn the origin on now what i can do is go click on the base of the x arrow and click on this plane and i have my x-axis now perpendicular to that plane facing the way i wanted to so i can go turn my origin back off so i don't have to see that and i can minimize this stuff one more time i'm pretty happy with my outcome there i'm gonna go set my stock diameters now i'm gonna do a fixed eye cylinder for this my stock diameter is going to be 2.75 and the length for this is going to be 3.5 inches so i'll type in 3.5 and when i look at this fusion put some of that stock in front and some of it in the back i really just want most of it to hang on to so what i could do is change my model position to offset from front and i'm going to do an opposite amount of 100 000 of an inch or 0.1 so we can come back and face that off and now you can see i've got more material behind it to be held onto and not as much to face off in the front and i should be good to go on my setup and i'm going to go ahead and choose okay so i've got my setup created we're ready to go and start adding some tool paths and we're going to start by facing this part off i should also note that this tutorial is meant to help you get started using tool pass inside of fusion 360 when when doing lathe parts this isn't going to be a complete comprehensive deep dive into every option of every tool path that i show in this so i might dive into a few options here and there but we're not gonna cover every single option in every tool path that we go through and look at so like i said we're gonna face this part so i'm gonna go to the turning menu and hit the drop down and choose face and i'm going to go select a tool now this this file this 2x turning file does have tools associated with it and we're going to use these tools to start out with so i'm going to start off by grabbing tool number one the ccmt 80 degree rougher let me go ahead and select that and then it may sound sort of funny but every tool path that i'm going to show you how to do inside of this once i select the tool that i want to cut with i'm just going to hit the ok button and see what i get so in this case i get a facing tool path and if i simulate this maybe we'll slow this down a touch what we'll see is fusion just goes and faces that front off of the part and it took a hundred thousandths of an inch cut off there and maybe that's too much so maybe what we could do is edit this we could go over to the passes tab and now i could turn on the multiple passes and i'm going to set my pass to be 50 000 or 0.05 per pass and then hit ok and let's see how that changed it now when i simulate it again we'll slow down just a little bit it's going to go through take its first pass it's going to come back and it's going to do a second pass and it cleans up to that green face i've got my simulation set to comparison so anything that's blue is remaining stock and anything that's green is finish stock and we'll go ahead and close that so that's our fin that's our facing tool path now let's go and work on profiling the outside of this we're going to do a roughing profile tool path for that so i'm again going to go up to the turning menu and choose turning profile roughing i'm going to go and select the tool in this case it's already going to use the one that i want it's already pre-selected and now i'm just going to choose ok and see what i get for tool path so we'll look at this from the top view here and we can see that we have some tool paths going across this part and we can kind of evaluate the tool path see what is that we like and what we don't like and i can see a few things that i don't like i'd like this tool path to cut farther past the back so when i part this off i don't have to go through as much material i also don't like how it's diving down here and maybe we'd want to change the amount of step down we do here things like that make it extend out farther so let's go look at some of those different options i'm going to edit this tool path and one of the first things i want to do is on the geometry is i want to extend it where it goes and cuts so from the front i'm going to give it a 100 thousandths of an inch tangential extension and on the model back i'm going to give it an offset here so i'm going to say minus 0.25 minus 0.25 and there you can see that that preview is showing me where it's going to cut to and i'll hit okay and see what i get and now when we look at this tool path so it starts cutting out farther and it's cutting farther past the back still away from my jaws and but you can see how it's diving in in both of these areas so maybe we could go and look at how we could make it stop diving in like that i'm going to edit this tool path and that's going to be controlled on the passes tab and it's going to be something called grooving so right now it's allowed to groove radio radially if you look at the the tool tab here i think it's pretty self-explanatory i'm going to hit the drop down and say don't allow grooving and now when i hit okay fusion's just gonna go and do straight tool paths across we're cutting past the back getting pretty much what i want right here so maybe one other change i might want to make is on the passes tab maybe i want this to do a deeper step down per pass so it's currently 50 thousandths of an inch let's make it 150 thousandths of an inch just so you can see the difference and we'll hit ok and now you can see that we have fewer roughing passes going across there so you can control the step down of your tool that way so i've got that taken care of now what i'd like to do is i would like to do a finishing tool path across here a finishing profile so i could go to the turning menu and say turning profile finishing but i've got a lot of the work done already so i'm going to right click on this tool path and say create a drive operation turning and now i'm going to choose that turning profile finishing go ahead and select that and then come in through here and change any options that i might want to change everything should be pretty identical with the exception that it's not going to do roughing passes anymore so i'll hit ok and what we're going to see is i get the tool path that i want however we do see that we get a little warning here and i've seen people work an awful long time to try to get rid of this warning symbol and this isn't anything that you have to fix so i'm going to go ahead and click on and see what it says and so it says a lead out has been modified to do to a gouge with the remaining stock so fusion's just letting us know hey you had something set wrong and it fixed it for you um i know what i need to change here so if i were to edit this i could go to my linking tab i could change my lead out exit i'm sorry make it different i don't want to be the same as the lead in and now when i hit ok now you see that i get a straight up a 45 out and i don't get the little uh soft warning symbol anymore for that so now i've got that uh taken care of what i'd like to do next is go through here and groove out between these two faces i want to get rid of this material in there so let's take a look at uh the tool path that we could use to to get rid of that particular area on our part and that tool path is going to be called groove so i'm going to go to the turning drop down and choose turning groove and i want to go select a tool i'm going to go select tool number 9 the grooving tool and like all the rest of the tools i'm just going to hit ok so once i get that tool selected i'll hit okay and see what i get for an option and a result and you can see that i get a tool path but it's not exactly what i want it's cutting way more material than what i wanted to do i only needed to go between these two faces right here so let's look at how we can confine this tool path a little bit i'm going to edit this and the first thing i'm going to do is go to the geometry tab and i'm going to turn on the rest machining option rest machining means machine the rest of the stock that's left over after the previous operations so after the profile finishing operation what's left if i hit ok now you'll see that fusion does a much better job of limiting the tool path but it's still cutting a little bit more than i'd like it to cut so we can further refine this tool path by editing the groove and on the geometry i'm going to choose a different front and back so for the front i'm going to choose a selection i'm going to select that face and for the back i'm going to choose another selection and i'm going to choose that face right there so now we're going to limit between those two and when i hit ok you'll see that the tool path now does a much better job of staying between those faces so let's look at a couple other little things that we can change with the grooving tool path so i'm going to edit this and i'm going to go to the passes tab and what i want to do is instead of doing a full step down i'm going to choose a partial step down and so i'm going to set my step over amount here to be a hundred thousandths of an inch or 0.1 and i'm going to set my maximum grooving step down to be point three or three hundred thousands and now i can hit okay and what we should see is fewer tool paths and it doesn't step down quite as far so let's see what that looks like in the simulation i'll simulate that starting with the grooving tool path and let's slow this down just a little bit and so it's going to come down here it's going to do that 300 000 step down and go across and clean this up this tool path is going to do a clearing tool path before it gets done finishing before it cleans itself up now one other change i might want to make is on the passes i'm leaving 40 i'm sorry i'm leaving 40 thousandths of an inch to clean up on the walls i'm going to i'm going to change that to a much smaller amount so i'm gonna say .005 to clean up so i'll go ahead and say .005 that gives me less material to clean up now let me simulate this one more time without the stock on and i'll slow this down a little bit and i want to jump forward just a little bit more so some of the collisions that we're going to see let me slow that down one more time some of the collisions that we're going to see on this aren't really going to be there so i'm going to jump back here and hit play now what you're going to see is we're doing the final cleanup pass here i think uh in a second it's going to come over here it's doing the clearing pass it's pushing down and coming across and now it's going to come and get ready to do the cleanup pass on here the finishing pass now notice it pushes the tool down it slides across and it's going to pull the insert back up the wall which often isn't desirable so let's look at how we can maybe fix that if i were to edit this tool path i'm going to go to the passes tab and now this tool is allowed to go up and down i'm going to change the option so it goes only down so we make that change let's simulate that one more time try to jump a little bit farther ahead slow it down one more time and hit play again we're going to see that clearing pass first and then we're going to see the the finishing tool path come up so now this time what will happen is the tool is going to be pushed down it's going to go roughly halfway across so it's pushing the tool down it's going to go into its finishing tool path and then it's going to go to the other side and repeat the process but instead of to pulling the insert up it's going to push the tool down and then meet where it left off so there it's pushing the tool down the wall it's going to slide across this is the finishing tool path go across that little fillet meet where the last tool path was and now we're done with the finishing tool path on the groove so we've got the outside groove taken care of and now we just have to worry about taking care of the inside bore and parting this part off so let's go look at how we can do that before i do my inside profiling i want to drill that hole up first so on the drilling panel we're going to grab the drill and if i go to the geometry tab i can hover my mouse over that diameter and see that that diameter is roughly an inch and so now i can go back to my tool tab and let's go select a tool again in this file is a drill it's a 6160 force drill so almost an inch so that'll work so we'll select that guy and then for the geometry i'm going to click on that whole face now right now what it would do is it would wrap it through the front of the part and start drilling the hole right there so we want to make a couple changes to it i'm going to turn on auto merge whole segments which is going to recognize that that other part of the bore is also part of the hole so that works out and then i'm going to go to the heights tab and say that i want to drill the tip through the bottom which is going to bring the shoulder down and i want to go plenty past the bottom of this part so i'm going to say 0.3 300 000 past to get drilled through there so that when i come back i don't have to worry about my tool um bottoming out or anything with when i do my inside profiling and then on the cycle tab i think i'll choose to do chip breaking partial retract and i'll do an accumulated pecking depth of 0.75 inches so once the tool gets in three quarters of an inch it'll pull all the way back out to get rid of the chips and go back in and start pecking one more time i'll hit okay and now we have the drilling tool path that removes the majority of the material out of this bore so what i want to do first is rough out the material that's left right there and to do that i'm going to choose turning and choose uh turning profile roughing and i'm going to go grab a tool out of this part and we're going to see that there is an id boring tool number six is what we're gonna run with now when i choose tool number six it's set up to default me to be inside profiling when you're working on the inside of a part like this you need to make sure your turning mode is inside profiling instead of outside profiling on the geometry i'm going to choose to cut from model front and i'm going to cut to a selection i want to go down to this depth right there i'm also going to do a hundred thousandths of an inch uh tangential extension on the front of this again as well so we're going to add that value in there and then now we're going to go look at the radii this is sort of the first time where this matters a lot what we're doing and this is where the tool is going to lead in is on the clearance it's going to start cutting from the inner radius and it's going to cut out to the outer radius so i'm going to change this to be a selection and i'm going to choose on that face right there and i'm just going to give it a value of say minus 0.1 that should be enough for what we want to do i want to start cutting from this selection right here and i want to cut out to this selection right there so those are my three things that i want to click on and i'm going to choose ok and now i should get a tool path that goes and roughs out that material on that part i want to make sure i left a little material on the wall so i'm going to go to the passes and it did it left a little bit of material to come back and clean up so i'm good on my roughing tool path for this what i want to do is one more tool path so i'm going to say turning profile finishing it's going to be the same tool for my geometry this time i'm going to go to model front to model back on my front i'm going to do my 100 000 of an inch tangential extension sorry i'm going to change that to be hundred thousandths of an inch there now on my radii i'm gonna do this one more time i'm gonna say from a selection i'm gonna click on that face i'm gonna do an offset of minus point one hundred thousandths of an inch i want to cut the same way from this selection right here and this time because i want that to be included i'm going to say minus .05 and then i'm going to cut out to this selection right there so those are my three values that i'm going to choose and we'll hit okay and there we get a a profiling tool path that goes and cleans up the material that was left that the drill didn't do and came across to make one small change to this i'm going to edit this and on the passes tab i'm going to change the direction to be instead of front to back i'm going to say back to front and then hit ok and now if i were to simulate just this tool path without the stock on what'll happen is the tool is going to go inside the board it's going to drag across from back to front and clean up the inside of this so i've got that bore taken care of now so the majority of the work on this part is done i only have one last thing to do and that's going to be to part this part off so from the turning menu i'm going to choose turning part fusion is going to grab a grooving tool path if you've used one i think there's a better uh parting tool in here so we're gonna go grab tool number five for this i'm gonna go ahead and select that and then just hit okay and what we'll see is fusion goes and parts this uh part off but it's cutting way more material than it needs to it's starting outside of the stock and it's finishing at the center line and we don't need it to go that far so i'm going to go edit this and on my geometry everything is okay there but on the radii we can say the outer radius is going to be the model od and then the inner radius is going to be the model id maybe we can give it a little bit of an offset so minus 0.05 or minus zero two should be enough we'll just go ahead and do that and hit okay and now we're not cutting nearly as far when we when we come down with this part so it's not going towards the center line nearly as much so if i come back to my setup i'm going to go ahead and simulate this i'm going to turn my stock on i have tail set as my option so we're going to face this part off now we do our roughing profiling it comes and does a finish profile it grooves out the area between those two flanges it does our drill it roughs our bore it cleans it up and it parts it off and there we have a finished part that's ready to post out so hopefully you guys like this one i know it's a little different i usually focus on milling things but i thought i would do a little tutorial on how to get started with lathe if you have any questions please leave them in the comments below and as always thanks for watching

Channel: Mechanical Advantage

Views: 16,393

Keywords: Autodesk, Autodesk CAM, Inventor HSM, Inventor, SolidWorks, HSMWorks, lathe, cam, tutorial, quickstart, getting started

Id: rHCf6GLyrx0

Length: 21min 31sec (1291 seconds)

Published: Thu Oct 22 2020