Autodesk Inventor CAM: A Close Look at 4-Axis Machining

hello everyone uh as the presenter just said uh this is about four axis machining an inventor cam uh basically the same thing i'm going to show you today will pretty much work with the solidworks hsm i will also work with fusion 360. so the technology is basically the same throughout the products that our desk has i happen to be using inventor cam today so we worded it that way but it does work with pretty much any of the inventor cam products now the topic is 4-axis machining but you'll notice as i go through my presentation today i'm going to be talking quite a bit about part modeling uh most of the success you're going to have with machining in a four axis mode a lot of it really depends on what the model has in it and how the model is displayed so i'm going to be showing you both modeling techniques and machining tech techniques to get some of your weird four axis stuff roll it i just noticed a couple attendees dropped off hopefully they're not having web problems but anyway the first thing i'm going to show you is technically not four axis but i just want to talk about having your models actually match what you're machining or have your machining actually match what you expect in the model because sometimes what you draw as a model in what you machine is going to end up being different i feel it's important that you guys recognize the differences and go from there so again the first one not exactly four axis but we will get there so let me do this i'm going to bring this model up on the screen i do keep my model simple because it's all about concept but at the same time i want you to fully understand the step by steps that i do to create things i was gonna creole create all this live for you but i realized i wouldn't have time in one hour so a lot of what i'm going to show you today is pre-created but we're going to walk through step by step as to how it was created okay just an example this first part if i drag the end of heart up you'll notice it's basically just a cylindrical extrusion it is four inches diameter and it's one inch thick so those numbers may be important a little bit later but anyway it's a four inch diameter disc i put a few work planes in here we're going to be doing a little bit of slicing and dicing visually with those work planes but ultimately what i wanted to focus on is this slot i have a slot in here that has a sloped bottom on it uh this tends to be a little sticky issue for some people so let's take a look at this a little bit closer the first thing i did is created one sketch let me just show you a quick look at that sketch all it is is just one single line that runs from the center of the part out to the edge of the part and i've positioned it a half inch off the top all i'm doing with that line is basically establishing a half inch depth in addition to that sketch i've got another sketch which is 90 degrees from the first one same basic principle it's just a simple line but it establishes a quarter inch depth so i'm going to have a half inch deep on one side a quarter inch deep on the other side so those are two sketches i put in there just to start with now i do have another sketch here let me edit that real quick what this line represents is the slope that's going to occur from the half inch depth to the quarter inch depth now this number here this is basically a formula since i have a disk that's four inches wide that's got a two inch radius this is basically two times two times pi divided by four now just to kind of explain the math basically radius times radius radius squared so you've heard the pi r squared is the circumference of the circle that's exactly what i've done it's pi r squared but i divided it by four because i only want this to go one fourth of the way around that disk so it's going to go around that disk exactly 90 degrees so it's pi r squared to get the total circumference divided by four because i only want to go fourth of the way around now what i did with that sketch is actually created a 3d sketch out of it now this sketch let me just kind of make that sketch visible there that one we'll make it visible so you can see it the 3d sketch all that is edit sketch i use this tool right here to project a curve onto a surface so all i did is projected that line onto that circular face and you can see that line basically creates a new 3d sketch that goes one one-fourth of the way around that cylinder so that's how i established all my goods now what did i do with all that basically i made this surface so let me just hide some of these sketches here real quick well i'll leave that one visible i'll hide this one okay so what i did is i created this surface now what that surface is i took that bottom line it's a sweep my first profile curve is this bottom line right here so i'm sweeping that straight line up the path curve which is this outside 3d curve i was just showing you so i'm taking this line and i'm sending it up that slope now i drew the other line in there just for reference to show i'm actually not using it with my sweep so i basically have one line sweeping up another line i am using this guide orientation and i'm telling it to follow this circular surface that's the outside surface of the cylinder so basically as it goes around it's twisting as it goes up which creates the surface you see highlighted on the screen so with all that being said the last sketch i made is just a slot i have two things in here i have a line representing the center of the slot and i've got the slot drawn itself so all i did is said let's just make an extrusion of that slot that goes to that selected surface so what do you end up with you end up with a circular slot with a sloped bottom okay again not exactly four axis but we're getting there all this is kind of important you'll see a little bit later on so that is the way most people would model a typical slot and a part you establish where the bottom is you just draw your slot and you say extrude to the bottom boom done or maybe extrude and find some way to create the bottom either way it's got a sloped bottom now for machining on that how do you machine something like that well most people they would jump over to the machining side switch over to cam here real quick let me generate that tool path what they will do is they will use that centered line and do what's referred to as a trace operation the trace operation is basically go into the part follow the line and come out so here's my trace operation if i do a quick simulate on that you can pretty much see that it just goes into the stock makes the cut and comes out but here's a question for the group is that cut i'm creating going to actually match the model well if you're using a flat half inch end mill like i am the answer is no it's not going to match the model okay so let me give you an example here let me go back to the modeling side the way i modeled this anywhere i slice this model if i slice it at 30 degrees do a half section view here if i look right at that plane you'll notice my slot is perfectly squared which represents you know a perfectly square end mill that you're putting in there so if i slice it at 30 degrees again you'll notice it's perfectly square if i slice it at 45 degrees again perfectly square if i slice it at 60 degrees again perfectly square no matter where you slice it there's a perfect little square spot plot because i designed that surface to be flat no matter where it's sliced but if you machine that that's not what you're going to get so exactly what are you going to get uh well let me just go back to the cam here do a quick simulate uh we'll turn on the stock so you can actually see it i'll go ahead and run this it should run fairly quick we're just going to dive in we're going to walk right up that slope and we're going to come out now because i have a flat end mill you might notice a little oddity going on down here in the corner half of that tool did not cut all the way to the slope did it okay a lot of people think they you know they drew the slope that's exactly what the model showed how come it didn't machine that well it's real simple the bottom of your tool is flat it's not sloped so you're always going to get a little bit of a flat at the bottom and this one doesn't show it quite so much but you could have a little bit of flat up at the top actually since the tool was dragging up that slope the top of it is actually sloped but you'll notice you do have a little flat down here at the bottom so maybe it's important for you guys to make sure that the model matches what the machine's part is actually going to be uh now there's other ways to machine this part i can get a smaller ball cutter and go down there and whittle it to death and but most people are going to want to use the big tool and just cut it quick so if you're worried about interferences with maybe a pin that might go down into that slot or some other mechanism sometimes you may want to model the part the way it's actually going to look after its machine so let's take a quick look at that okay i have another part i'm going to open up so i'm going to show you a little bit different approach here now what i did on this particular part i've got the same extrusion i've got the same work planes actually i just copied the other part to make it easy i've got the same sketches there's the one line there's the other line there's the the flat slope line i've got the same 3d sketch in here everything is identical except this extrusion last time when i made that extrusion i selected the entire slot and just told it to cut that slot out this time i'm ignoring the slot i'm just grabbing a half inch diameter circle on the end see the quarter inch radius right there so i'm going to use that and this time the only thing i'm really doing different is i'm telling it to make a new solid rather than cut the existing solid so when you pull the trigger on this what you actually end up with is one solid body that represents the part another solid body that's going to represent let's say a half inch diameter tool i actually labeled it as tool so if you think about this i have that sketch which is basically the center line of that slot projected down onto that surface so you'll see the center line that slot right there is flat i projected it onto the bottom surface which has given me a center line that's sloped very easy to do guys very easy so what i'm going to do here is in your modeling side i can say i want to sweep using a solid the default here is using geometry hit this little button right here you can say i want to use a solid they call this a tool body like a half inch end mill so i can grab that tool body tell it to follow a given curve like the one i've got drawn in the bottom of that if i can find it there it is and as i'm doing that i can tell it to cut what am i cutting i'm cutting the other solid so i want to cut that solid there's a little preview of what i'm going to get now you'll notice you have the preview a little bit of flat here at the bottom you have the slope and you'll notice you also have a little bit of flat up here at the top because that's how the tool is going to basically you're emulating you're pretending that this red solid is going to be the tool making the cut so it's a different way of making the slot so if i come in here and take a look you can see the little flat on the bottom you can see the slope and if i start slicing it you think about this i go to work plane go to view let's do a half section view like i did before let me get to the decent amount default isometric view let's do a half section there there we go one thing you'll notice difference i'm slicing it at 30 degrees remember last time i had that perfectly flat bottom well if you take a round tool and you drag it up a slope the bottom is not going to be perfectly flat it's going to have a little bit of that curvature of the tool in it i think you can see that curvature right there so right there it shows curvature if i slice it at the 45 degree work plane you can see the same curvature if i slice it it's a 60 degree work plane you can see the same curvature now if i sliced it down on the very end which i don't have a plane there i wish i did uh again you would notice down here at the bottom when the tool initially plunges in it is flat down there so there is a way to model exactly the way it's going to look when it comes off the machine that's one of the things i wanted to show you today and this becomes kind of important when you start getting into rotary work because the way you design a slot versus the way the machine might actually cut it can look two entirely different ways that's the part that i wanted to show you i don't know if i have cam on this one yes i do so let me just go back over to cam generate the tool path again you're not going to see anything different this time other than when i simulate this and play it if i do an actual show part comparison you'll notice that the part and the cut are pretty much 100 identical now there's no mismatch between the part and what was actually cut before there was a little bit of mismatch so that's the first thing i wanted to show you is how can we make our parts match our machining or vice versa all right the next thing i want to show you uh let's go in here take a look at the next category pockets on the side of a part there's two things i wanted to pretty much show you here the first thing is what if you have a normal square pocket on the side of a round part now that's good you know i do have a flat pocket in here but the first thing you need to learn when it comes to machining in different orientations especially wrapping and things like that is how do you get your tool to align you'll notice my setup is set up for late i've got my setup here i've got z pointing down the center of the cylinder which is the way you would chuck this up on a lathe i think most of us would agree with that you put the z on the front of the part that's your turn cylinder now when you have a flat pocket on the top your tool has to come down vertically so you notice my z has changed here if i'm looking at my setup my z is pointing out the side if i go to this flat pocket my z is pointing up well obviously to machine the top of this i need to have the tool coming from up above okay so how do you do that well it's real simple if i edit this toolpath there's only one thing you really have to do you select your tool i've got a half inch flat end mill on the second page there is a tool orientation all i have to do is select the z-axis plane and an x-axis my z-axis plane is basically the surface you see they're highlighted my x-axis i just picked the edge of that pocket so that basically sets up your x and z in this orientation so now the tool is going to come down from the top without that your tool is going to be trying to come in from the side and it can't even see the pocket from from this z direction so you really need let me undo that you really need your tool to come down in a different orientation now i showed you the tool in here to make that happen what this does it's actually going to send out a rotation code to your machine to get from the front of this part to the top of that part since it's rotating on the x axis you should get a 90 degree x rotary or an a axis rotate a usually aligns with x b with y c with z so you would get a 90 degree a axis rotation assuming your tool your machine can rotate in that direction that's what you're going to get on an output so this is going to trigger your a b or c rotation code uh as far as that goes the rest of it's plain jane you know if i simulate that yeah it's just a pocket so i hit play turn that off so it'll run a little bit smoother and voila pocket okay now in addition to that i have another type of slot here i've got a wrapped slot now how do you draw a wrapped pocket uh one simple way to do it and there are some implications here is to start with a sketch now in my case i started with this sketch right here you look the numbers at it it's basically located four inches off the end of the cylinder it's a one inch wide slot and you might recognize that number basically what that number is since we've already discussed it that is the circumference of this cylinder which is pi r squared there's some circumference of this cylinder divided by 4 because i only wanted my slot to go across 90 degree spread so if i did some dimensioning on that wall there i don't know if i could do this on inspection or not let me see if i can touch that line and maybe that line see if it'll give me an angle uh yeah right there angle 90 degrees so basically to get a 90 degree slot i have to consider the circumference of the cylinder divided by whatever angle i want 90 out of 360 which is 1 4. okay so again you take that and all you have to do is do an emboss command now the emboss command if you've never done it before is actually pretty simple you click your profile which is my rectangle you can see it highlighted there you put in your depth that you want to go now you can do this as a raised embossment or as a cut engraving i'm doing mine as a cut i'm telling it to go a quarter inch deep and you tell it wrap to face now when you turn on wrap to face you select the face that you'd like to wrap it around so by doing that i end up with this wrapped pocket now there's some good and bad to that i just wanted to show you how i actually created the wrap procket okay now when you get ready to machine something that's been wrapped go back over to the cam side generate these tool paths okay you've got the wrap pocket there now with this machining operation there's basically two things you need to do first of all we'll just do a quick edit on this the tool i'm using the exact same half inch end mill not a big deal but right here on the second tab notice it says wrap tool path when you wrap a tool path you basically pick your cylinder i'll clear that so you can see this you pick the outside of the part that's going to be the wrap cylinder now you notice it shows the wrap radius of two inches here the four inch disc has a two inch radius now if i tell it to wrap the cylinder based on the bottom of the pocket notice my wrap radius is a quarter inch difference so now it's looking at a one and three eighths or one and three quarter radius versus a two inch radius so you can use either one but there is a gotcha and i'm going to show you this in just a second so you can use the bottom of the pocket as your wrap radius or you can use the outer cylinder as your wrap radius i'm going to leave it on the outer cylinder that's really all i did is wrapping the toolpath by the way let me uncheck that notice the tool orientation is here just like i showed you a minute ago if you don't use tool orientation like i did on this first pocket you know keep in mind on the first pocket i wanted the tool to come straight down well this pocket your tool actually needs to be rotating so we are getting into rotary machining now so you don't really give a tool orientation because you can't have your tool coming straight down from the top it has to rotate with the cylinder so instead of using tool orientation i just tell it to wrap it so again just one click difference take your cylinder it shows you what radius you've selected there is an offset here we'll talk about that in a second so now the tool is actually going to be following the curvature of the cylinder i.e fourth axis machining now there are three commands that have this built into it what we call wrap tool path there's three commands that is the 2d adaptive the 2d pocket and the 2d contour a lot of these other milling operations do not have wrap options yet uh right now it's only in these three it's been in these three for a while there is a beta version out that actually has it in other places but i don't demo beta i don't show anything until it's done released in the product i don't like pointing people to futures this is what we have today is in adaptive pocketing and contouring well of course i'm doing a pocket right now so your end result tool path is the pocket mill that wraps to that cylinder okay if i do a quick simulation on this uh hit play here you can see it walk around and it cuts out a rotary pocket i'm going to make a slight change here let me rewind that i'm going to show the sock is transparent i'm going to hit play again again i've just got it plunging by the way you probably do this in multiple steps i'm doing everything today simple one tool path you can see it obviously in real life i'd probably take multiple passes going down just because i've got a lot of material there just pretend it's a really soft plastic but notice here as i watch this come around actually let me just get rid of the holder for a second so you can see the actual tool as this is coming around this is going to be the final pass there's something i want to show you here that's a little bit peculiar again a lot of demos to show you the gotchas about 4-axis machining as opposed to just throwing some part up there and say hey this is how you do it i do a lot of phone support and i deal with calls coming in all the time and people struggle with the same things over and over and over again so i chose to show some of those struggle points notice right here the tool is basically walking right down that edge zero clearance perfect cut now when i get down here to the end wall it's a perfect cut right along that edge if i go up the other side it's a perfect cut let it get finished here of course with that great big tool i'm going to have radiuses in the corners as to be expected i could use smaller tools i chose not to but if i get this done and i say show me the part comparison notice i've got an issue and by the way this is one of the sport calls i get hey i just did this slot and it's cutting the heck out of the end of my part here see those big orange patches it cut into that wall see that undercut we can't have that in real life you can't have undercuts so you gotta ask yourself why all of a sudden is there an undercut there something's not right okay let me show you what is actually going on in real life we'll close this simulation that wrapped pocket let me go back to the modeling i'm going to edit this sketch here i actually have a little tool drawn up in here that this is your half inch end mill i have a rectangle here it's exactly a half inch wide and i'm going to show you when you wrap a tool that tool is actually using the same center as your part is anytime you wrap a pocket or tell a tool to wrap around a cylinder guess what they're all using the exact same center point now what that happens with this tool we used a wrap radius equal to the outside diameter of the part so what's happening is is the tool let me move this tool i've got this set up to where i can swing it back and forth to show you like the motion of the tool if this tool is going back and forth sorry for my jumpy graphics okay if my tool is going grab back and forth like this okay when it comes over to the top if you told it to use the wrap radius on the outside of the cylinder that tool is going to stop right right there where you're at the outside of the cylinder okay that's as close as i can get it by hand notice what's happening to the bottom of the tool it's actually gouging that wall why because the slot is a perfectly 90 degree slot based on that center point your tool is using the same center point but you've got this difference now if i pulled the center line of the tool on over to the edge of that slot you notice you'd have a perfect alignment but guess what we don't cut with the center of the tool we actually cut with the sides of the tool right so if you're cutting based on the outside diameter there you're going to be undercutting by that much on that sidewall okay so that's why now if you tell it to cut based on the lower inside diameter like right there you would be under cutting here and not gouging at the bottom so you need to decide are we going to use the outer cylinder as the limit control are we going to be using the inner cylinder as the limit control okay and that is the one option you have in that wrap toolpath command let me go back to machining here real quick okay now last time i showed you uh let me just do the setup generate the toolpaths okay that wrap pocket last time i was showing you that we were using the full two inch wrap radius so i chose the outside of the cylinder this time i'm going to clear that i'm going to choose the bottom of the pocket as my wrapping cylinder so i'm showing a wrap radius of 1.75 this time when i say ok there's my new tool path if i simulate that just fire this off real quick i'll try to slow it down when it gets to the last lap come on get down here okay when it comes into this last lap again it's never a problem on the side walls because that one inch never changes but when i come down here because i'm using the bottom of the pocket now it's not going to gouge that sidewall but notice it's leaving a little bit of distance here at the top of the tool now the bottom is actually on the corner i don't know if i can rotate the screen careful enough to show that the bottom is truly getting into the bottom but notice at the top you've got some uncut area here so no matter how you approach this as long as the tool and the part are sharing the same centerline axis you're gonna get one variation or the other now i will tell you guys i i feel like when i thought about this i was like i feel like i'm pointing out all the bad parts of the software my point is i want you guys to be educated and i want you guys to understand why things are working the way they're working and by the way me personally i've worked with edgecam smartcam chemx command sdrc i have been through nine or ten different machining softwares i have a pretty broad knowledge of what the other guys are capable of doing and by the way they all use the same math algorithms for this type of procedure so it doesn't matter whether you use an r product or someone else's product you're going to be fighting the same battles because they're all using the same map okay just to point that out it's not a flaw in the software i'm just showing you how we can get around that flaw okay so you can see there's a little bit of a mismatch there again all that depends on whether you tell that wrap pocket to use the engine three quarter radius or the two inch radius or by the way if you grab one of these you can offset that let's say i offset it by an eighth of an inch i can actually split the difference that's why they give you an offset value here so i can actually tell it to go halfway between the bottom of the pocket and the top of the pocket so if you don't want to completely over cut or you don't want to completely undercut you can split the difference and it'll actually split the difference and do half and half uh but again because i'm showing you all this of course i have a possible workaround i've actually provided this to a few people on phone support as a workaround for this type of machining how about if we start lying to the software there's a concept for you how do you lie to the software okay of course we all do it right what i did is i made a sketch let me slice the graphics come in here i said what yes what if i compensate for that half inch tool so i took this wall and i offset it a quarter inch i took this wall and i offset it a quarter inch that is where the center line of the tool resides i think we all agree on that simple map now if i extend those two center lines down they actually meet at this point right here so i extended them down created a point and then i drew a circle on that point now why did i do that real simple because inventor can do multi-body solids i made an extrusion based on that center point that extrusion is using that sketch i basically made a solid i think it goes all the way through the part it didn't have to or maybe it just goes an inch deep i don't remember but i made an extrusion there but i made it as a second solid okay that's food for thought so let's go back to the cam side my first setup is using the center of the part and you saw the two tool pads that i created that one and that one right i made a second setup but on my second setup i didn't mean to double click that on my second setup come on show it to me i actually use the center of that little cylinder so i'm making a setup based on that is my pivot point everybody's scratching your head saying oh yeah that will probably work duh why didn't i think of that okay so i made a second cylinder i set up the setup based on that of course it throws your stock off a little bit honestly i don't care how big the sock looks as long as it cuts what i want it to cut okay so i made a second set up and i did another wrap on that same pocket let me generate that real quick so there it is it pretty much looks identical to what we had before but again look at the center that i based everything on so now if i simulate that one and do a quick play on this it goes in does it's cutting of course again more stock showing but i don't care about that as it cuts all this oh that was the last path one okay see if i can zoom in on this run it forward you'll notice as it comes down to that side wall right there it's actually doing a perfect cut on that side wall top and bottom kind of hard to see that the top and bottom are following that maybe i can get to it at the 45 degree angle so there it is you can see that i'm basically hugging that wall with the top and the bottom of the cutter so it's now a perfect cut on that sidewall if i could get your guys applause that'd be great but no we have another problem that just showed up if i go ahead and simulate this on out yes we got perfect cuts on the side walls but what happens when you offset your rotational center up like i did you might notice the side wall back here let me do a show part comparison if you look at that because i've got an elevated center i have an elevated crown in my part back there yeah come on try and rotate the screen and show you this but see how it's elevated in the center you can see the arch right there and you can see the arch on the other side right there yeah we got the perfect cut on this end wall but we did not get a perfect cut on that side why because we have an elevated center which elevates your wrapping radius which basically gives your crown and your whole pocket toolpath so even though i gave you a workaround to get perfect sidewalls now we've got a secondary issue to deal with but believe it or not i do have a total solution for you if you do the wrap pocket on the original surface and if you do a wrap pocket on the fake center then you actually took both of them and ran them you would end up with the first one being cut which is going to machine the bottom of the pocket then you're going to end up with the side walls being cut and what you end up with there is a perfect cut on all four sides no gouging no overcuts no undercuts everything is cut clean so hopefully that makes sense to you guys if i run on both and by the way the second run didn't even have to be a pocket mill it could have just been a one pass contour but since i had the pocket mills already growing up i figured i'd show it that way so that is some cute little tricks on plain radial four axis pocketing i am going to get a little bit deeper every step goes a little bit deeper so that being said let's take a look at the next example uh let me open this up open up side slot b actually side slot a so some people have to do cams and slot work on the size of cylinders i see this as a common failure when i see people do slots again this sketch is fairly simple it's a half inch wide so half inch tool you recognize that number that's basically telling it from center to center i want to go 90 degrees around the cylinder we're going an inch and a half up we're going to go three inches and we should have an inch and a half on the back side so it's basically just a typical slot now the number one thing that i see people do with a slot like this is they will go to their modeling and they'll do an emboss okay so if i go to emboss you basically pick the profile that already saw it you could join or cut i do want to wrap to face i'm going to wrap it to that face you can kind of see the little red preview there looks like exactly what i want so when i say okay voila perfect little slot and it's exactly 90 degrees it's got the dimensions on it i want so it's going to go in one inch it's going to transition and go out one inch so again perfect little slot fairly easy to come up with but guess what it's not right again i'm trying to show you what what you're going to encounter in real life this slot is not what you think it is if i take that embossment and go a little deeper with it let's say a quarter inch can anybody see anything wrong with it actually if you look carefully you'll notice there's a little bit of taper going on with it the embossing when it wraps around the cylinder i've got that perfect half inch at the outside of the cylinder but the closer it gets to the center that size is actually reducing check this out if i edit that feature and go an inch deep you can tell that that embossment is reducing all the way through that slot you see the v-notch in the front you see the b-notch in the back and you can actually see it here if you compare the width of that to the width of the top so that's something that people run into and actually if you go all the way down and i can prove the math here 1.999 i can't go all the way to 2 inches because it'll fail but if i bring it all the way to the center everything in that slot basically points to the center line of the part so it's at the center line apart here all the way through that it's at the center eye of the part so if you follow the bottom of that groove you basically have a straight center line that's what the emboss command does i just want you guys to be aware of that okay now how do you get around that well this obviously is not working so we'll throw that away i'm going to open up plot b and show you a different approach this is the same approach that i did just a minute ago on that other part if i go to create a sweep using solids i can use this as my half inch tool i want to align that with the outside cylinder basically it's going to use that center line i want to select this solid is the one that i'm cutting i do want to do a cut and the curve i want to follow is this curve now rather than wrapping the entire slot all i did is i wrapped the center line that is a 3d sketch tool i'll back up show it to you in a second but notice the end result it's going to use that tool body to actually cut that slot out and you're going to end up with a slot that looks exactly like it would if it came off the cnc machine you'll see some radiuses in here as it's going down that slope that is basically exactly what you'd have coming off the machine so again it's one of those things do you want to have the model look exactly like the machine part this method will do it now i told you i'd go back and show you that 3d sketch there's the 3d sketch basically all i did was i used this projector surface i grabbed that black line and told it to project it to the cylinder and that's where that purple sketch came from so it's not a not a complicated thing to do so that is one approach now you'll notice to machine something like this on the machining side let me just actually open up another part on the machining side what happens is you create a tool path now ideally let me zoom in on this ideally what you would want to do on the machining is you'd want to take that blue line which pretty much follows the center line of that slot i think you can see it go through there come on so you would want that as a path and then you just want to trace it right well actually when i was prepping for this demo i tried doing the trace on it guess what if you try a trace there is no wrap option i told you earlier the wrap option is only in adaptive machining pocket milling and contouring unfortunately the trace it's not in there yet uh so i was like okay if i can't trace the center line how am i gonna machine this silly thing well real simple what i did and again you guys do the same thing is i just did a regular 2d contour and with that contour let me show you what i actually selected going to edit that same half inch tool i've been using all day right here i am wrapping the tool path my wrap cylinder is the two inch radius it's the outside of the cylinder for a contour all i did is all i had to do is select one side of that pocket since that pocket is perfectly drawn and it's a half inch all the way through i don't really need to know where the center is i can use the edge of the pocket so i basically said i want to contour that line i've got it highlighted in red right now you can see that is my contour selection shown in blue so basically i'm just saying okay follow that contour now if you follow the contour and you're telling it to wrap your toolpath is going to show up up here at the top of the part okay to compensate for that you know if you think about contour most your compensation is stepping sideways i want to step down so what i did to compensate for that as i basically just went to my depths page my heights page i said take that selected contour and just go down another half inch so basically i'm just telling it to push that tool path down a half inch from where it is and that's how the tool path ends up at the bottom center of that slot so with that being said again just a quick simulation on it uh just hit play you can see it just walks right through there so long story short guys this tool is basically doing the exact same thing as my tool body is doing when i created the slot in the first place so it's a hundred percent perfect match so that looks exactly like the model if i actually show a part comparison this should come up and really show no differences whatsoever yeah it's hard to rotate the screen without messing that up so okay one last thing to show you i've got about eight minutes left uh there is a simple stuff what i call simple uh these slots and stuff i'm showing you is probably the most difficult thing you could do in in four axis but just an example to do a slot like this maybe you've got a thread or a screw or something that just needs to keep going you know the last one i showed you a side approach slope and then going out this one's you know what if you have this well the way i created this is real simple i started with one sketch extruded the cylinder i made another sketch now the purpose of this sketch because i wanted my cut to go out of the park on both ends i drew a line from center to center and then i just added a one inch extension on each end all that one inch is for is just to make sure i go one inch beyond the solid itself okay so that's all i did there i went in the 3d sketch by the way if you go into 3d sketch they do have a helical curve option under my 3d sketch is my helical curve all i did on that is i told it the diameter of my cylinder which we knew was four inches i wanted a two inch pitch wanted to make four revolutions now my part is six inches long but since i extended it one inch on each end i actually have eight inches of total length so four inch diameter two inch pitch four revolutions adds up to eight inches and then i basically just anchored this top point on that point right there just to tell it to start at the perfect 90 degree point so that's how i created that uh once i had that path in there let me just make it visible i told it i wanted a work plane at the end of that path normal to the path now if you notice it is slightly tipped you want your plane to be normal to that path uh you don't want it flat because if it's half inch wide you're going through as a spiral your groove is going to be less than a half inch so make sure your your tool is lined up with that path now all i did there is i created the sketch there's my helical sketch here's my other sketch that sketch is basically my one half inch wide tool one inch because i wanted to go a half inch deep and i've got it sticking out a half inch i usually just center it and tell it how wide and how long so there's the tool path and then i just did a sweep and i told it to do a cut so that's how my slot ended up in there i think that's self-explanatory enough from there i did come in here to machining let me just generate the tool paths here the first time i attempted to cut that i basically told it that i wanted to do a pocket mill because i knew pocket mill would clear out the whole pocket i was going to use an undersized cutter 3 8 of an inch but when i pocket milled it i realized it would not run out the end of the the part i needed my tool to actually go beyond the edge of that surface if you just say pocket that your tool center stays inside that outline so my tool center was about where my cursor is and i had corners here that weren't being cut i thought okay well i can solve that so i just did a contour on one side of the slot that's the contour for the left side of the slot as i'm going to call it okay then i did another contour for the right side of it so basically i've got two conjurers one walking through right to left the other walking through left to right now there's nothing special in these that i haven't already showed you i'm just going to go to edit tool i used a 3 8 tool instead of a half inch i am wrapping the tool path based on my 2 inch diameter 2 inch radius uh no special depth considerations i did have to turn off all my lead-ins and lead outs i did not want all those arcsan and arcs out and i just basically wanted to do a plunge but i did put a two-inch extension on my lead end now where does that show up right here if you see that green arc right there my wall ended right there where my cursor is but i wanted the tool to keep going so i basically just told it to do a two inch extension it does follow that same contour so now you can see the blue is where the tool pad actually is this green is basically just to lead i did the same thing on the lead and i really didn't have to have it on the lead end but i did it anyway just to show you that two inch extension does follow the contour so with that being said i can grab this setup say simulate for the bird's eye view here we'll just run this you can see it kind of goes through it's cutting looks like the side that's closest to me again if you have a really deep pocket you want to do this in multiple levels i'm just doing a single level i found when i do multiple levels you get so much geometry going on in there it's really hard to explain things and let people see what they need to see then i come back in and i basically climb cut the other way to machine the other side wall so completely exiting the part on both ends i'm getting a nice clean cut in and out let's go ahead and finish that out again you can rotate the part and look at it and see that everything's pretty much nice clean cuts perfect match so uh i guess the only thing i haven't shown you is post processing uh in my case i'm going to my posts i do have like a mill turn set up this can actually be four axis milling or mill turn uh i'm just going to post it as a mill turn i've got a haas machine if i post it hit save yeah it's already there it comes up and you can obviously see got everything turning the machine on and getting it oriented and you see a series of z with the c-axis move there's your rotation so it's moving the z which is the length of the part putting your c-axis rotation moves in and between the two you get the perfect spiral cut so again an hour's not a lot of time to show you everything that's possible with four axis uh my main purpose today was showing you that four axis machining may or may not actually match the four axis parts that somebody gives you because when you're dealing with flat ended tools you do get some interesting results and mismatches uh hopefully i've shown you enough to be able to handle situations like that when you run into it again in my opinion machining is one half of the process how you build the model is the other half they do need to coincide with each other but there's usually a way to get a perfect four axis toolpath even if you have limitations in the software uh again i hate pointing out our limitations but by the way it's a limitation in all the software's out there that i've seen maybe someday the math will get better but this is what we're dealing with now hopefully you learned something today if not i'm hoping to open up your eyes to potential problems other than that i think i'm done if you guys have any questions you can post them in the question panel i'll try to answer them if not uh have a good afternoon this pretty much ends our presentation again i hope you learned something throughout the day uh i hope if you get into four axis machining you don't make some of the common mistakes um you know doing these webinars in my opinion saves me a lot of support calls uh again we can answer this stuff over support but nine times out of ten just getting you guys aware of the way software's think will make you better programmers all right i don't see any questions coming in if you have questions in the future just send them to your sales rep and they'll get them to one of the tech guys we'll get answers for you anyway have a good afternoon

Channel: Hagerman & Company, Inc.

Views: 44

Keywords: CAM, Autodesk, Inventor

Id: i0KndXI8gVI

Length: 59min 55sec (3595 seconds)

Published: Mon Dec 20 2021