How to program CAM for ANGLED guitar necks in Fusion 360 | Complete Tutorial

hello everyone my name is austin shainer and welcome back to my channel in the last video we took on one of the most challenging parts of guitar machining flat guitar necks however in the world of guitar machining there's yet another final boss in order of magnitude more difficult next with angled headstocks angled necks are probably the number one thing that intimidates people about building guitars with cnc and for good reason it has a very complicated shape it requires precision in your glue ups and even more complicated tool paths and work holding not to mention that there's no single or even two-sided setup where all these features are accessible we're dealing with a three-sided machining monster so i spent the last few months thinking about the best ways the average person at home could take on such a project i came up with almost 100 different methods but each had serious limitations that essentially forced you to choose which part of the process you want to make difficult for yourself well frustrated with my options and about ready to give up i took to discord to get viewer opinions on the ideas that i was working with i was gently reminded by one of my viewers that i might be approaching this the wrong way but i shouldn't be thinking necessarily about how to work around the problem or finding the cheapest or fastest way to do this i should be developing a repeatable process for the guitar community regardless of complexity and then once i have a repeatable process finding ways to make it more streamlined and accessible to the public this changed my frame of mind as after all i am a process tech by trade processtechs develops safe and repeatable manufacturing processes that ensure quality by mitigating the chance of human error so if i put on my processtech cap how would this change my approach well that is precisely what i would like to show you i believe i have managed to develop a low-cost solution that should be achievable on nearly all desktop cncs even those with limited z clearance using nothing but a sheet of plywood 3d printer and some clever work holding to simplify and error proof my order of operations so let's not waste any more time and let me show you so jumping into fusion let's quickly talk about what makes a angled headstock neck unique compared to a flat headstock neck and why it's so much more difficult to machine and then we'll go into what the method looks like so if we take a look at this neck right here you can see that we have a perpendicular surface to my fixture right here which means we from this angle we have access to these holes this face and the outer contour but we don't have access to the rest of the neck right especially you might be able to if you have enough z clearance on your cnc but if you don't then basically you're stuck with just machining this little section in fact but here's an easier way to show you so if i hide my cnc and let's hide my fixture and just bring up my neck if we go into the manufacturing workspace there's a really cool tool in here that many of you you may not know about so if you go to inspect there's accessibility analysis and what this does is it lets you effectively see what part of your model is machinable with a flat cutter from any given direction so i selected my model and so if i'm looking at my model from this direction everything that's green here is machinable but if i even tilt it a little bit this way you can see that these side walls and these tuner holes aren't accessible and this back side is not accessible and so then i can flip the direction and i can see well if i'm machining it from this side all of this is accessible except if i turn it this way all of a sudden you can see that part of my headstock transition and my tuner holes aren't accessible either and so that means that really those two setups i can't hit all of the critical dimensions that i need to hit so there's actually a third setup that actually has access to just about everything but it presents a really big challenge for your cnc so let me see if i can rotate this real quick i think i have it on fixed let's go to free orbit there we go so if i mount my neck like this right then i have access to basically that entire top contour of the neck the challenge is is that raises my neck up at a very extreme angle and really high up on my cnc and i don't have the clearance for that so that effectively means that what we need to do is we need to both machine it from this side and then we need to machine it from this side and then we also need to machine it whatever we can from this angle to clean it up so that's a really tall order and that means that our work holding has to get pretty elaborate but there's also one additional thing that makes a angled neck much more difficult than a straight neck and that is a scarf joint so most of you watching this are probably familiar with a scarf joint but just in case you aren't essentially what you do is you take your blink and you slice it at an angle and separate it into two pieces and then what you do is you actually take this piece and you flip it 180 and then glue it together like this and what that does effectively is it allows the long grain in the neck to extend most of the way up the neck but then it switches the angle of the long grain of the neck to follow the actual neck break angle and the point of that is if you built this out of a single piece of wood what you'd end up with is short grain on this front face and that makes it particularly weak under string tension and it's very easy to snap your neck at that point so that's also something that we have to take into consideration so we can either do this manually by ourselves in our home shop or we could actually find way creative ways to let our cnc do it for us and so now that we've kind of got this out of the way let me show you guys the method that i put together all right here's the game plan folks first thing we're going to do is we're going to rough trim our stock on the table saw and bring it down to the correct thickness either with a facing operation on our cnc or with a thickness planer if you happen to have one then we will place our fixture on the cnc and insert four dowel pins to align it with the machine then we're going to place our rough stock over the left side of the boundary with double sided tape this will allow us to bore out the tuner holes and dowel pin holes that will be used for alignment throughout the rest of the process then we will cut our outer contour so that we have a perfectly dimensioned blank to help us a lot when aligning the part for glue up now we can take the blank off of our cnc and split the part in two with either a pull saw or a bandsaw making sure to stay within a fairly generous safe zone now it's important to remember to stay as close to center as possible during this cut as any remaining stalk on either side of your saw kerf will effectively be our stock to leave in the next operation then we will place two dowel pins into the fixture and place the headstock side of our blank onto the fixture with double sided tape then we will be able to do a scallop operation with a ballnose end mill to true up the rough cut surface and leave us with a nice scarf joint at the appropriate angle then we will take that off and do the same thing for the heel side of the neck now we can take both parts off the cnc and clamp them together without glue and drill two dowel pin holes through both pieces so that we can realign them once we apply the glue now it's really important to take your time and get these as perfectly aligned as possible before you drill your holes because any mistake here can cause alignment issues later on then once the holes are drilled we will unclamp the parts apply our glue put them back together and then insert two dowel pins into our holes clamp them together and let the glue set once the glue is set we can now move our dowel pins on the fixture up one row and place the assembled blank on the fixture with the headstock hanging off the front of the machine this will allow us to mill out the truss rod slot and potentially face off the fretboard side in case there was any misalignment during the glue up the scarf joint and the fretboard side should now be complete now that we have the front side complete we will insert two dowel pins into the right side of the fixture and install the blank truss side down with double-sided tape then we will slide our 3d printed wedge up to the headstock and secure it down with two shoulder bolts these both serve as dowel pins and allow us to secure the part to the wedge at an angle then we will tighten down the wedge to the fixture the slots in our wedge allow us to accommodate any variation in the angle that may have happened during glue up then we will do our primary contour roughing and finishing strategies on the main portion of the neck and up to the headstock transition then we will take that blank off one last time flip it over and secure it headstock down to the same 3d printed wedge and fixture this will allow us to do our final contour roughing and finishing on the back side of the headstock making sure to clean up any remaining stock on the transition that we didn't have access to when it was flat this should leave us with a finished guitar neck ready to sand and apply finish okay so jumping into the manufacturing workspace let's go ahead and get this started so i created a folder structure here called angled next setup in my models and i created two components under that called stocks and operations and fixture so obviously in fixture i have my primary fixture here as well as my 3d print and any various hardware that i might need and then in the stocks and operations i created basically a folder structure for each individual orientation that we're going to need to machine this model in and the point of that is because unlike my previous videos where i had the model be the central piece and then i had a fixture that rotated to either side of the model depending on how we flipped our part we have enough unique orientations here that it was actually just simpler to create different stocks for each for each operation or orientation and then just copy our body over and so in here we'll go through these one by one and then we'll start programming the cam so i have my pre-split um operations so in here i have my raw stock which i will face off and drill the tuner holes etc and then i have my split stock as you can see here where i basically got my scarf joint now obviously we won't be machining the scarf here but this allowed me to generate my raw stock and create this gap here that we will need for machining it later so we actually had to split basically our model in two and separate it by a couple of inches so that way we could actually have room to saw our scarf joint without actually cutting into our model and then after that i have my scarf surfacing so if i bring this up in here let's go to bodies oh i'm in fixture that's why in here i have two models so i have my headstock side and then i have my heel side and pretty straightforward we're going to use those as our stocks to go ahead and machine and then i have operation number three which i'm calling trus trust slot overhang and in here i have my two stocks that overhang and i also have my model set up in this orientation so that way i can use that to select geometry for cutting out the truss rod slot and then in operation number four let's hide these real quick and in operation number four i have my two stocks here that i used to actually generate a third stock so i i was able to get my angle from that but then i i created a single piece body because sometimes what fusion does is if you have if you're selecting two bodies at the same time for your stock it can throw errors with z clearance later on and that became a big problem when i was developing this so i just used these two stocks to generate a single body for me and that's the body we'll be using for our stock and then we can go and hide this and then operation number five is we have it up at an angle and i kind of did the same thing where i generated a another third stock but i ended up not using that and i will actually explain why later but essentially what this let me do and i have the model here as well although it's kind of hard to tell that way we can select the geometry but effectively what this allowed me to do was have one fixture and then just orient my part in all the different various orientations and so that way i can make sure everything fits as we go through my order of operations so let's go ahead and close this out and we're going to go ahead and create our first setup for the pre-split so let's hide this and let's bring actually we need to bring that back and we'll bring up pre-split and let's hide these two and bring up our raw stock so let's create a new setup and in here let's go ahead and select our model as our stock um because we don't actually need the guitar in here because we've modeled in the dowel pin holes and the tuner holes into the stock itself so that's actually going to be both our model and our stock and then we'll say our work offset is selected point this front left corner of the fixture and if you're wondering why i do that go ahead and go back and watch my guitar bodies video where i go into that quite in great detail and then we will select our x and y axes here and here and then we will flip our x so that way we have our x going in this direction our y in this direction and our z going up and then our fixture we will go ahead and select this body right here and then in the stock selection we're going to say from solid we're going to choose the same model and then hit ok and now we've got our first setup so let's hide this for now and then let's go ahead and do the dowel pin holes so that's going to be the first things first we're going to go ahead and take care of the dowel pin holes so we'll go 2d boring operation and then we will select our end mill and for this we're going to use a quarter inch flat end mill hit ok i've already got my feeds and speed set up and then we will go to geometry we will select all of our dowel pin holes but not the tuner holes because the tuner holes are 10 millimeters and i'm using 3 8 dowel pin holes because that's more readily available for me here in the states and then i can go to heights and we want to make sure the bottom height selection goes down to the fixture and then we will go negative we'll just make sure it goes down below just a little bit so we'll go negative 0.03125 so it goes slightly below the surface so we're good there top heights looks like we can keep them the same let's just go ahead and make sure that yes top height is from whole top so we're good there passes we don't need any multiple passes we do want some stock to leave though because we want to get these dead on accurate so this is basically going to be a roughing pass so we'll go we'll leave 20 thousandths of an inch as stock to leave okay and while we're here let's go ahead and do the roughing for the tuner holes so let's go 2d boring operation in fact you know what let's right click this and then we'll say create derived operation 2d milling boring and what that's going to do is it's going to retain all of our previous selections and we're just going to change our holes so then we will come to the geometry tab unselect those and then select our tuner holes instead and let's just go ahead and make sure that our heights are set up correctly yes they are go to our passes yes we have stock to leave okay we are good now what we want to do is come back in and do a finishing pass on this that we will sneak up on the dimensions so that way our dowel pins fit perfectly they're not too tight and they're not too loose either they just kind of glide in so let's do a another boring operation so what we're going to do is we're going to right click this one create derived operation another boring operation and in this case we're gonna go to the passes and what you're gonna end up doing is you're gonna save this as a separate operation and then you will run it and you what you'll end up doing is you'll say okay instead of 20 thousands we're gonna leave ten thousands run it real quick test your fit and then if that's still too small maybe take five thousandths and then if you go all the way to zero and it still doesn't fit you can actually go negative point zero zero five and it will actually expand the hole for you a little bit so we're gonna go ahead and just leave this as point zero two zero for now and let's go and name these real quick so we've got dowel pin roughing tuner pull roughing and dowel pin sizing and then we're going to do the same thing we're going to go in fact we can just duplicate this instead of create derived operation and then that way we can come back in and change the stock to leave and fine tune that fit and then the last thing we need to do is we need to create a 2d contour on the outside perimeter of the part and the purpose of that even though we've put a pretty decent sized stock on here is we want to trim it so that it's exactly the same on all sides because that's going to give you a really nice clean surface to reference off of when you're gluing this up for the scarf joint so let's go 2d contour and we still have our quarter inch flat we're good there in the geometry tab let's select this outer contour and then in the heights tab we're going to go down to selection this bottom face top height is stock top so we're good there everything else should be fine and then depending on what your cnc is capable of you can either take it in one pass or multiple passes i personally like to take pretty conservative cuts when i'm plunging through the material so i'm going to go .0625 inch step down and that should be good we don't need any tabs because we're going to be using double sided tape to hold this part down okay and let's simulate the whole thing and like always i'm going to be using comparison view although in this case it doesn't make a whole lot of sense because we actually are stock and everything is the same so we're going to that is going too fast it says tool collides with fixture but that's only because i'm going down below the surface that's okay so we're gonna do our dowel pin holes the rough sizing of them then we're gonna do our tuner holes and then we're going to come back in and resize all of those and then do our contour okay that looks good to me so now we can move on to the next setup and let's name this setup stock prep and so let's go ahead and create a new setup and before we select anything let's go ahead and make sure in our angled next setup folder that we turn off pre-split and we go to scarf surfacing so in between these two setups you will then have pulled off your blank and sliced it and then now we're going to put it back on the cnc and go ahead and surface our scarf joint so let's go ahead and pull this up and let's go ahead and do the headstock side first so let's say our model is this and our stock is this as well and then our work offset well let's do our fixture here and then our work offset is selected point same thing as before select x y axis here and here flip x everything looks good hit okay and now what we can do is we can come in and do a 3d scallop because we've already got stock to leave on here from cutting these apart so all we need to do is come in with a ball nose end mill and clean it up so let's do a scallop operation and the reason i'm chewing choosing scallop rather than a parallel or ramp or anything like that is we've got a very very thin edge down here at this front front side so we need to make sure that when we mill that it has as much material around it as possible so we avoid any kind of tear out or anything like that so what's nice about a scallop is that it kind of works from the outside in so when it cuts this edge it has as much material around it as possible at that point so it'll be as strong as it we can possibly make it so let's go to geometry and then we will say our tool machining boundary is selection and let's select this contour right here and we can say the tool can go outside the boundary actually no let's just go and do on center and then let's do contact point boundary so that way it can go slightly over the edge if it needs to and let's make sure we have a ball end mill selected so under tool select and then we'll go find a quarter inch ball end mill or whatever size ball end mill you're going to be using looks like i don't have my feeds and speed set up here so i'm going to do 16 000 rpm and we will do 75 inches per minute it's a pretty decent chip load we're also going to be taking really small little passes so we could probably be more aggressive with this but that's okay and then our bottom height is model bottom that'll work for us or we can do selection down to the fixture and then we can say passes we don't need any stock to leave we just need to make our make sure our step over is very fine so we'll go a thirty second of an inch you can make it smaller or larger depending on the size of bit you're using since i'm using a quarter inch bit 30 seconds seems to do leave a pretty nice surface finish so let's go ahead and hit okay i didn't turn off coolant so let's go back to the tool library or not to a library the tool tab and disable that and hit ok it's going to take a second to generate and let's simulate that real quick again it's not going to show the stock here because we selected the stock and our model as the same thing really what we just want to see here is the tool path and make sure it's doing what we want it to do so let's show our tool path here okay and yes it is coming up on that boundary there let's see what it does on this front edge speed this up just a little bit okay yep it's just touching that front edge but it's not having to roll over i put this little channel in here just in case i needed it to roll over but that's okay we don't need it so let's speed this up a little bit now and it works its way in surfacing that whole top face and now we have a very nicely dimensioned blank that we can just kind of sand very lightly to get any of those cusps off so that way we have a nice glue surface so what we're going to do now is we're just going to duplicate that and then change our setup to be the other model and let's name this real quick let's go and name this scarf headstock and then let's duplicate and then in here we need to edit our setup and we need to hide our headstock scarf and show our heel scarf so now we just need to change our model to here and then go to our stock and change our stock to that as well our work coordinate system is already set up for us and our fixtures already set up so that should be good to go now we just need to update the tool path because right now it still thinks that tool path is on the other one so let's right click that and go edit and then we're just going to change our machining boundary and hit ok and now we have the exact same tool path but set up on the other side and real quick before we move on let's rename that as well to scarf heal okay and now let's go ahead and create a new setup and inside that setup we need to hide scarf surfacing because we're no longer using that and now we're moving on to truss slot overhang so let's show that real quick and let's hide our stocks for a second and this time we're actually going to be using our actual guitar neck as our model so we'll go ahead and select that because now we have geometry on the neck that we need to select like the truss rod slot and then let's go ahead and set our work coordinate system so same thing as before selected point select x y axis here and here and then flip our x and then on fixture we'll go ahead and select our body there and then in stock we're going to go from solid and in this case what i'm going to do is i'm going to use both of these models as my stock like that in this case that works what doesn't work is when you flip the part the body over because then your stock it has to basically create a boundary box that's higher than the parts you want to machine since it's in this orientation the boundary box extends below the machine so it doesn't really matter to fusion that you have two bodies selected but it just does matter when let's say when you're in this orientation and now all of a sudden it thinks the top of the model is over here whereas in this case it knows the top of the models where we want a machine anyway so doing it this way is not a problem in this instance but we will get more into that later so let's go ahead and hit ok and let's hide our stocks so we only are dealing with the model and let's go a 2d pocket 2d pocket and we're going to do this one by itself first because we're going to end up doing a stock to leave on it and then we will come back in and do the others and then one to clean that up so that's going to be our selected geometry as that bottom face in this case we need to switch to an eighth inch end mill because the distance here between these two is point two one eight eight so it's smaller than my quarter inch so this is the only time i'm going to be using an eighth inch end mill so let's close that out tool library and we'll go to eighth inch end mill 16 000 rpm and i'll be a little bit more conservative here let's go ahead and say 50 inches per minute and then geometry we're already good there heights let's say we it's already set to selected contours but i like to forcibly let's say select it down so i know that i'm going down to the right height top heights from stock top so we are good there and then passes we're going to do multiple depths and i'm going to go down a 16th of an inch at a time and we want to leave a little bit of stock to leave but we only want to leave it on the side walls we don't want to leave it on the floor so we're going to take axial off to zero and just leave 20 thou of radial stock to leave and we will say we'll allow the cutter to cut in both directions and then our maximum step over is going to be less than half the bit so we're going to go .06 that should be good so let's go ahead and see i need to turn off coolant again so disabled and hit okay so that should be good and now we can move on to the pockets for the other ones so let's go 2d pocket and then we will go same quarter inch flat it's already got our settings so we're good there and we will just go ahead and select both of these because it will be able to accommodate for the depth and then we're going to leave it as selected contours in this case because that way i'm not only going to one depth i'm going to whatever depths that i had selected and then in passes we're not going to leave any stock to leave at all but we will do multiple depths of 0.065 and our maximum step over will be 0.06 so a little bit less than half the bit and we will allow it to go both ways and let's turn in lead or turn off lead-ins and lead outs we just kind of want it to plunge going in and we will set our entry positions as right here that way where our bits not going to try to plunge in outside the model or into the model we're going to try to make it plunge right here hit okay that's looking pretty good and then let's go ahead and do a clean up pass on this and then we'll simulate this as well so let's go create derived operation 2d milling 2d contour and we've already got our settings so we're good there and we've already got our chain selected so because we did the derived opti a derived operation so we're good there heights it's already going down to that selection in this case we want to take off multiple depths and we don't want any stock to leave and that looks good so let's go ahead and let's simulate this now just like we did with the dowel pins and the tuner holes we're going to sneak up on that with this operation so make sure to save that as a separate operation on your computer so that way you can take a little bit more off and a little bit more off etc so let's go ahead and simulate that whole thing now we can actually see the blue and green because we actually have a stock that's larger than our model so it's milling out this side or not this side the truss rod let's look at it down a little bit there we go make sure it goes green to the bottom but not green to the sides yes so we have a little bit of stock to leave on the sidewall and we want it to go green all the way around on these inner contours here now you will notice that i have a little bit of blue left over and that's only because i didn't model in the radius into this part of the neck it's just left square in my model so it's leaving a little rounded corner that's totally okay i'm not worried about that so we went green down to that surface and we go green on this one as well yes and now okay so we have a lead in here that plunged into our model so we're going to have to fix that but right now it is cleaning up that side wall so yes it went green right here so let's hit play real quick that looks good let's take off the lead in on that last cleanup operation okay and right click that final contour edit go to our linking tab uncheck lead in and uncheck lead out hit okay let's just simulate that one portion real quick just make sure we don't run into that again yes we are good we didn't plunge into our model this time okay we are burning through this pretty quick so that is already done on the truss rod side now there's one other thing you could do so after you've glued up your material so this actually is a section where the model itself has already been cut and glued and now we're cutting the truss rod slot but if you did notice that maybe your scarf joint overhung the face a little bit and you needed to flush those up you could do a small facing operation to just clean up that entire face along that scarf joint if that's what it ended up happening for you then go ahead and add a facing operation in here but for now we're going to go ahead and move on let's name this truss slot overhang and that one is now complete okay so it's hide trot trust slot overhang that's a hard word to say sometimes and let's do neck roughing show that and let's go create new setup this is where we're going to get into some really challenging tool paths so this is going to be probably the meat of the video right here okay now that we're in our new setup let's open up that folder and let's go model is right here and then we will do work orientation is selected point right here select our x y axis here and here flip our x just like always looks good our fixture is right here and then our stock is from solid and what we're going to do is we're going to bring in this camstock one now remember when i was showing you guys this i created a separate completely solid body stock that didn't have two bodies and there's going to be a very important reason for that and i'll show you guys that in a moment so we'll select that in fact actually you can kind of see it's trying to create a boundary box here from the bottom up to the top and then it actually it's hard to see in this light but it actually extends all the way out and so it thinks the stock is significantly thicker in this area than it actually is so we'll go into that in a second hit okay and let's go ahead and create a contouring operation and the main purpose of doing a contouring first here is only to give our 3d adaptive and scalloping tool paths or not scalloping parallel tool paths a lot more room to work with so that we can somewhat preemptively avoid some of those rapid collision to stock errors fusion 360 really likes to actually model from or not model machine from the outside in as if like you're holding the part in a vice and it's not really intended to cut a contour first and then machine but the way we typically do things with guitars to not or not guitars in general but in woodworking and cnc routers is to kind of do it that way and so we kind of have to work around the rules a little bit and that's one way to do it so let's go ahead and do 2d contour and we need to find the sketch in here so i've got this sketch that we can set up as our contour so let's hold the alt key let's hide our stock real quick so we can see this a little better hold the alt key and we're going to select each individual piece and the only reason i need to do that is because i have this as a closed selection and i don't want to select a contour coming across here because that's going to cut into our model so i only want to select these pieces here if you don't have this then you just need to create a sketch and project in the faces of your model so that way you can get access to the whole thing and we need to make sure that our arrows are flipped over so they have to be on this side of the line not on the inside so let's make sure everything's flipped to the outside go one here okay that looks good and then we can come into our well let's switch our tool back real quick because right now we still have the eighth inch tool so we need to go back to our quarter inch tool so we'll go quarter inch flat end mill coolant is disabled good avoid that error message and then we will go to selection the bottom of our fixture or the top of our fixture and this is going to get really tricky right here and i will show you guys why i have to do this in a moment so i'm going to not change my clearance height and let's see what happens in a moment and we'll go passes multiple depths and we're going to go 0.0625 inches we don't need any stock to leave and we don't yes we do want some finishing passes so we're going to go two finishing passes of 0.125 inches and that's to give ourselves a lot of little extra room so let's go and hit okay let's see what happens and see if it throws an error for us okay so you can see already that it's generating way too many tool paths because it's trying to go from the top of the stock so we need to actually limit that down so i'm going to show you what happens if you select the top of this right here so let's go edit and let's go back to our heights and then in the top height let's go selection because right now it says stock top but it thinks that stock is way up here so let's bring back our cam stock and we're going to select this top face as our top height and let's hit ok and let's see what happens simulate that might actually work okay this might be a larger issue on the 3d adaptive but sometimes what happens is fusion does not like to machine at a lower height than the top of the model right so the clearance height it basically what happens is when you start your tool path on your cnc it's going to try to travel up to the clearance height and travel over and then come down to your retract height and then go down to your top height and if your retract height is something significantly lower in fact that might be why it works so let's pull that up and check real quick let's go edit heights so it's coming from retract height and this one says stock top so let's change this to selection of the top of our cam stock here and hit ok of course this is probably still working again for us it does look like it might be trying to cut in okay so it is colliding with the stock let's see if we can pause that real quick so it's not actually touching anything right now but it's actually colliding with the stock and that's because it's trying too rapid at this point because as far as it as far as it knows you don't have a model here right because you put your clearance height as just slightly above this section not the top section and so what can end up happening is you end up generating a lot of errors in your tool path if you don't set your clearance height up really high up here now that presents a really big problem for us because this is taller than my z my cnc z height and so if i set my clearance height here the first thing my machine is going to do is travel up and crash at the top of my z height and i won't even get to my tool path and i'll hit the e-stop so what we'll probably have to do to avoid some of these errors is set our clearance height really high and then just go into our g code when we post process this find any numbers that are at our z height or not our z our clearance height and change those values so that way we can manually override this or you can deal with any of the collision errors if you'd like just pay really close attention to make sure it's not slamming into your fixture or into your model or anything like that so the way we're going to solve this is we're going to go back to our contour and hit edit and then in the heights tab let's do this one by one so let's check our bottom height our bottom height does need to be the bottom of the model our top height we only really want it to start cutting at the top of this cam stock and so we're fine with that and then our feed height so that is where the cutter stops doing a g0 rapid and starts applying our feed rate that we applied in our tool tab so this 90 inches per minute that is the point of where you will no longer get that error so we need to make sure that our feed height is above the start of our cut up on this headstock in the contour so let's go ahead and do from selection and then we'll say from our highest point that we selected in our contour which is this wing right here and we will say like 0.5 above that and then we will say our retract height is the same thing so it's going to retract to where we know we are safe so it's like a little safe zone both in the g0 rapid and in our retract and then in the clearance height we need to actually change this to the top of our stock the actual top of our stock over here so that way fusion doesn't throw an error for us and then we should be able to run the simulation without any errors and then we'll have to go back in once we've posted these and edit out these uh edit the g-code now you won't have to do this if you have the adequate z clearance for your machine in my particular case i don't but the top of this neck um or the top of this headstock is about two and a half inches for me that's taller than my zero my z clearance so this is what i have to do so let's just go and hit okay and let's try simulating this and see if we get any other errors so right click simulate let's hide the camstock and run it through okay so we were able to get rid of those errors so we're going to end up applying that same technique to all of the other tool paths we're going to do in this setup one last thing i forgot to do in the contour so let's go back to edit real quick and let's go to geometry we're going to add tabs to just the heel side because right now we are securing down the blank with double-sided tape which is fine for this operation the reason we're going to put in tabs is that once we take this off the blank or sorry off the fixture and we put it onto our 3d printed wedge we don't want this to be loose and be able to dangle inside of our stock so we actually still need our heel to be secured to our stock for the next operation so what we're going to do is we're going to turn on tabs and then we will go at points and we're going to say at this point and let's rotate the other model over and we'll say at this point now i am using my sketch selection still the one that i did for my contour to develop this when i had that turned off it didn't allow me to select these points on the heel and then i'll say from here here and here and let's make all of these like well that can stay point zero sixty five but our tab width we're gonna go ahead and make point seven five something pretty meaty so that way it's very unlikely for this to actually um snap off and let's go ahead and hit ok and we'll simulate one last time and then we'll move on okay let's just make sure the tabs show up the way we expect and let's hide our fixture make sure we go all the way through with our tabs yes we are good let's check the bottom side yes okay that's looking good we're green on all sides of the contour and we have our tabs and we were able to avoid those clearance issues so now let's close out of the simulation and let's do our big 3d adaptive to clear out most of the material on the neck so we will go 3d adaptive clearing and then we want our quarter inch flat still so we're good there and in the geometry tab we're only going to machine up to here let me close out of this real quick we're only going to machine these surfaces and the heel we're not going to go into the headstock transition because what will happen later is as we flip the part up on this angle that's going to really complicate our selections and what we're able to machine and clean up this surface so we actually want to machine this entire surface of the transition from this angled view and and that's because that's at the point where we have access to all of that geometry and we don't want to end up really cutting that twice because if we end up cutting that section twice we might end up with little errors or misalignment issues things like that so we're going to cut this transition on the angled face and we're going to cut everything else in this orientation so let's go back to 3d adaptive clearing and we've still got our tool and stock contours i've got a selection or a sketch here that basically starts from that point and so that's this is the area that we're going to be machining and then let's turn off rest machining and check model we want to make sure that it's not trying to machine anything else so we're going to say we want to select all of the surfaces on the top of our model right here and we don't want to select any of these contours because those ones are already green those are already solved from the contour and then our machining boundary will be selection we're going to use the exact same selection and tool can go outside of boundary that's just fine we might need to add an additional offset but let's see in a moment and then in the geometry tab we're going to do the same thing we did before except in this case there is no feed height so our retract height needs to be our feed height essentially so we're going to say the bottom needs to go to the model bottom which is totally fine and then our top height needs to be from selection not stock top because remember our stock top is technically up here so let's bring back our cam stock and our top height is going to be the top of this area right here and then our retract height is going to be from selection let's hide our camstock and let's go from right here and do the same thing we did before 0.5 above that and then you might not need to go that high in this particular case because we're not machining anything over here but we already know from the previous operation that that's a pretty safe value and then let's go clearance height is from our top of our cam stock and we'll say zero that turned this back to black because it didn't like that the clearance height was lower than the retract height so that should be good let's double check this again so we are going from bring back our model i think i selected the wrong thing we want to go from here to 0.5 there we go that looks a little better and then in the passes tab what we want to do is we want to go to both ways keep our optimal load at point one that's fine and then we will do our maximum roughing step down of a sixteenth of an inch so that each layer that we're going to leave for our ball nose end mill will be a sixteenth inch deep and then we will leave we'll definitely leave stock to leave and let's go ahead and say order by depth that might not that might be unnecessary but that will allow our tool to stay in a concentrated area based on the depth that we're currently at and then let me just double check do we have anything else we need let's go to our linking tab and scroll down let's take off any lead in or lead out transition and let's assign at least one entry position so that way we can make sure as much as possible that we're not starting in an area that we don't want it to machine like the transition so we'll say from that point right there we can also say if it lets us sometimes the selections here kind of suck and then we'll say like right here right here and right here so those are the areas that the program is technically allowed to enter the stock from but there are certain circumstances where it no longer is going to be cutting that area and it's going to come in down on the side and so we still might run into some issues but let's hit okay and see what happens might take a second to generate okay so let's simulate this let's see if we have any errors we still do so we might not have perfectly solved that but let's go and hit play let's make sure we have stop on collision checked so it's going to go through that contour and it's going to enter in from that first spot that we designated and start clearing out material do the first layer same thing on the second layer keep going whittling away this material and then our first one is over here so let's back that up just a little bit and play it pretty slowly and let's make sure that what's happening is something we're okay with because we've already set up our clearance heights etc and we won't really get another opportunity to solve some of these in this particular type of model so as long as we're okay with what the cutter is happening so i'm typically okay if it's plunging into the material like that but what i don't like is if it's side loading the cutter if it's side loading the cutter really hard that can cause my cnc to lose steps and i'll need to find a different solution so let's slow it down and hit play okay it's coming in here let's see what this is going to do i'm gonna turn off stop on collision and slow this down okay so you can see it's still not touching anything but that's because we don't have a feed height so we're still getting an error of rapid collision into stock but let's see it's just gonna plunge down and i'm actually okay with that because my my cutter or my cnc can handle plunging what it can't handle is major side loading of the bit because then it can cause it to lose steps so let's just check each one of these as we're going through and make sure that's what's going to be happening in the cut otherwise we might need to change something okay we've got this one which looks like it's going to be the same we teleported to the other one okay it's going to come in here in a second okay just double check this yes that one's plunging as well we're okay with that then we'll check this one as well so it's going to retract up come back down nope didn't hit that yet that's further forward okay yes it's gonna plunge there again so let's go to this one if you didn't know you cannot zoom in on the timeline here if you just scroll while your mouse is over it and that's actually quite helpful for getting getting in on some of these longer operations yes that one is plunging as well let's check this one that one is as well i think that's going to be the same for all of these so let's just check again we're almost done here it does look like i messed up on my step over um yeah that one was plunging as well the step over here looks like it's trying to apply a fine step over on some of these shallow areas so i probably forgot to make my fine step over the same as my large step over so i'll have to take care of that in a second and let's check this one last one and then we'll make that adjustment and simulate same thing but this one look it's just barely clipping that material it's totally okay and let's run it through the rest of this real quick that's looking pretty good to me so let's zoom up and make sure that everything that we want touched is touched before we go back in and make our changes so we didn't touch these outer walls we're good there we look at this our tool was allowed to go outside of this boundary so that way we left a clean surface here for our bonnel's end mill but we're not actually still cutting into our model at this point so that's totally material we were going to end up removing anyway so we're fine that this went outside the boundary a little bit so that looks good so what we're going to do is we're going to right click and change our step over so adaptive edit and then go into our passes tab and so our maximum roughing step over is point zero sixty five but our fine step down is point zero zero six two five so we just need to make those the same hit okay this should load significantly quicker now because there's so many less tool paths yes and let's go ahead and hit simulate one last time just run it through and double check there's our errors okay so that's looking more like what i was expecting these ridges here are significantly taller and we cleared out all the material that we need to and so i think we're good to move on to our ball nose uh parallel path so let's close this out actually before we move on to the ball nose one thing we forgot to do is clean up this face because we did leave stock to leave on this face so let's do a 2d facing operation while we still have our quarter inch flat end mill and then in our geometry tab we're going to select this contour right here and then in the heights we're going to say instead of model bottom we're going to go to that surface right there and then our top height is going to be the same cam top cam stock top and then this in this case we have a feed height as well and so we will go selection again the highest section that maybe may or may not be machined and we'll do 0.5 as our feed height there retract height is going to be the same as from this selection plus 0.5 and then our clearance height so selection is going to be from the top of that stock so right there and we'll make that zero and then in passes it typically orients in a horizontal fashion so let's go ahead and switch it to 90 degrees so passive our pass direction we'll switch to 90 and then we will apply a extension of 0.125 actually 0.0625 so that way it cleans up this tiny little area right there and our step over let's go ahead and make .125 so half of our bit no multiple depths no stock to leave let's check that real quick and so we'll just simulate that operation let's hide our cam stock okay and let's make sure that it's not going to hit that side wall here so let's watch this cutter as it comes through okay we're good we probably could have applied a little bit longer of an offset so if this doesn't clean up very nicely we might be able to do that coming through okay so we do have a little bit i don't know if we're going to be able to get all of that but we have a little bit more breathing room here because we applied finishing passes on the contour so let's make that offset just a little bit larger so let's go 0.125 and let's make sure that our bit doesn't end up crashing so simulate okay and let's slow it down in this corner make sure we're okay yes we're okay it didn't hit the sidewall so let's see what that end up corner ends up looking like okay i'm okay with that there's a tiny little piece there and that's going to end up getting cut off by the ball nose end mill anyway but we don't have a giant you know piece that was unmachined so that looks good to me let's go and move on to the ball nose end mill so let's set up a 3d parallel pass and we're going to change our tool to our quarter inch ball end mill and then we're going to go to geometry tab and our machining boundary is going to be that same selection that we did for the roughing so we're only cutting this part of the neck not the transition and then we are going to say avoid touch surfaces and what this allows you to do is say you can machine everything within this boundary except these surfaces you the tool path has to work around them and or what you could do is you could select touch surfaces and say well within this boundary it has to touch these surfaces so you can have either or so we're going to say avoid and we're going to avoid these all the areas on the neck pocket so like that make sure we have this face not touched because that's already done as well and that looks pretty good so we want to make sure the tool is on center boundary so if it's outside the boundary it's going to have the same limitations as the roughing one earlier but we actually don't care about that what we care about is that the cutter is cutting everything that's within this boundary but is also allowed to go just outside of it excuse me it's allowed to go just outside of it down on this bottom corner here so we're going to turn on contact point boundary and what that does is that allows the tool to extend past the boundary line so long as it still has material to cut so we're going to go ahead and do that and hit ok if you don't do that what ends up happening is sometimes you get a little flat spot on the bottom here and then in our heights tab we're going to apply the same thing we did before so exact same thing here top height is going to be the top of our stock so let's bring back our cam stock right there and then our retract height selection let's hide this is from here plus 0.5 and our clearance height selection is from the top of here and no additional offset and then in the passes tab we want our step over to be pretty fine so we're going to do 32nd of an inch in this case i learned from the last episode that i'm going i don't need to change the past direction and i don't think we'll need to change any of these here so let's go and hit ok and see what happens i didn't disable coolant so let's do that hit okay let it generate and then we'll just simulate the adaptive and that one let's hide the cam stock and simulate okay so oh i had the facing operation the roughing one was already done okay so we did get one error right at the beginning everything else looks pretty good let's just double check and let's look at our boundary here so yes our sketch is right here everything on the this side of that boundary was machined everything on this side just kind of got clipped but that will get taken care of later just make sure we don't run into any other issues and we'll look at that error at the beginning yep it did clean off that little that little piece left over from the facing operation so we are good on this side let's just go back to the beginning to that little piece right here let's say stop on collision right here and what does this have what is happening here rapid collision with stock so let's zoom in a little bit bring it right before it started way too fast okay i don't know why that one's triggering that one looks perfect to me so let's speed this up turn it off of stop on collision okay i think that's fine that's doing exactly what we want it to do but it's detecting that some part of the stock it's cl colliding with but looking at how the the end mill is interacting with the material i think that's totally safe and i'm fine with that yeah okay we're going to leave that be and now we're going to move on to our last setup and then we'll be able to be done okay so setting up for the final operations let's go and create a new setup and in here we're only going to select this part of the scarf joint because everything that we're machining that's up on this area right here has basically mostly been machined already so let's go to our stock and we'll do from solid and then in here let's bring up our operation five and we want to select this as our stock right here this will help us avoid a really really tall clearance height now the other one is already really bad but we in this case it's even worse because we've angled it up this way so and i'll show you that in a minute but let's go to stock point to model box point right let's go to this front corner right here or sorry selected point right there select x and y axes here and here and then flip our x-axis so we're good there our model is going to be this right there and then our fixture is this and our 3d printed wedge so let's go ahead and hit okay that should be good and then we'll set up for a 2d contouring to come in and clean up this side of the transition because we already did cut this contour right here but what that didn't hit was this flat spot right here so we need to go ahead and just run another contouring operation which will also have the added benefit of giving us more room for our 3d adaptives to come in and work with so let's do 2d contour and then what we will select as a geometry let's see if we can so we're going to go up to this line right here so we should be able to select everything going around so we need to switch our tool back to our quarter inch flat and then in the geometry tab hold the alt key and we're going to select everything going around up until that point turn our model around there we go and right here and right here make sure all the arrows are on the correct side it looks like they are okay we don't need any stock contours or anything like that we do want tabs for the same reason as before is because this has been cleared out and we are going to be holding on to our stock with shoulder bolts here but we're not going to really be able to hold on to the model itself once we cut once we cut through this we will be able to hold on to the front face with blue sided tape if you'd like in this case i'm just going to opt to use tabs so let's go at points and we'll say here and here and then we will say here and here and let's make those 0.75 wide let's make those a little bit taller there we go again we can always pair these away with a chisel or anything and then in the heights tab because we selected our stock that doesn't extend way up here we don't really have to do the same trick anymore so let's do top height is stock top that's fine our feed height in fact i think we can leave all of these the same we might have to check that in a minute and then in the passes tab we want multiple depths of 0.065 because our bit is going to be plunging all the way around and then we want two finishing passes of 0.125 wide and then in our linking we're going to turn off any lead in or lead out because we're just going to plunge down a 16th of an inch and start cutting that should work so let's check that real quick now i wanted to show you guys the material that is still left over that isn't within this stock it's pretty minor and so i don't think it's going to be an issue for this contouring operation so let's see if i can pull up this one right here and let's just click on our stock so this right here this yellow portion is the stock that we selected this is the stock that kind of overhangs some of that and this is the this is the point of which we machined in the previous setup so if you extended this line up to right here there's just a tiny little wedge here that it has remained unmachined from that previous one but the added benefit of not having to go through all of these clearance and just plunge through like an extra 16th inch of material just on this side right here i think is well worth it so i'm okay with that but we can simulate it if we'd like but let's go ahead and do our 3d adaptives and then we'll come in and clean and clean everything up so let's do 3d adaptive clearing and then let's make sure we still have our quarter inch flat we're good there and then machining boundary is going to be selection and we're going to select both of these contours right here because we want it to machine everything that's within here as well because there is material left over from the previous op and then no stock actually no we do want stock contours so we're going to select the exact same thing hold on sorry about that i didn't mean to hit escape quarter inch flat machining boundary is these two and our stock contours are those same two and then turn off rest machining and then in model we're going to select the faces that we want it to cut with this but not these side faces because we just did a contouring operation there so we're going to select the transition and these top faces right here and include setup model is fine to leave on because that will help us detect these holes and then we can say our bottom height is model bottom so that's good there our top height is going to be the top top of the stock that we selected our retract height let's give ourselves a little bit more room on top of that and our clearance height will be the same as our retract height so we can go from retract height zero that way they'll be the same and then in the passes tab we want to machine both ways with a 0.1 optimal load in both directions and then we want to set our maximum roughing step down and our fine step down like we did before 2.0625 and then we do want stock to leave because we're going to come back in with that same flat end mill trick that we did in the last video and then in linking there's no lead in lead outs but we can turn these to zero that should be okay we did get an error so let's see what happens okay z clearance is too low for the surface so that tells me that we still have a problem with that clearance that we set up and that is likely due to the fact that the model is extending far beyond our stock and again fusion doesn't like to have clearances or anything that is not above the model so contrary to what i said earlier i think we are gonna have to go back in and make that extremely high clearance height and we're just gonna have to edit it out in the g code so let's do clearance height from selection and let's bring back our heel side of the stock to right here and then our retract height should be able to stay the same let's find out yes it is generating now so you can tell that that immediately solved the problem we needed our clearance height to be above the model and because our model went all the way up here that we are kind of pushing the boundaries here of what fusion finds acceptable types of machining because most machines that we're going to be performing this type of stuff on is like a big five axis machine and they won't have those z clearance problems and so a professional machining center they won't need to go through all this extra work we're just having to do that to force our machine or force fusion to work with this on our limited z-height little x-carve that i've got so let's simulate these two make sure we don't run into any problems before we move on to cleaning everything up so let's hide that heel scarf okay so we're doing our contour first we do have another error of rapid collision with stock so we might not have put enough of a boundary there so we'll check that let's go through the contour make sure it leaves the tabs yes it did leave the tabs so we're good there okay and let's make sure that everything's okay with the clearing so it is important to remember that right at the beginning of this clearing it's going to be plunging a little bit extra so it's going to be going like an eighth of an inch plunge at this point because we have that little wedge sticking over okay stop on collision so let's zoom in on this real quick make sure that's okay and see if we actually need to come back in and change it okay it's just gonna plunge so i'm okay with that yep it's just gonna plunge down and then keep going i'm okay with that let's zoom out go to this one double check the same thing should be plunging again just like before yes i'm okay with that let's just check all of these real quick i apologize this is the nature of doing this kind of machining it's going to plunge as well so i have a feeling that's going to do the same thing for the rest of these let's just check the location of each one of these if it's in the same location we'll assume it's doing the same thing yes it's just moving further out so that's okay let's speed it up okay so let's show our model well i guess it's already showing so this should be on the same area of the boundary now we left stock to leave and so remember these might not actually even be plunging or touching anything it might just be doing that simply because we were simulating a part of the process that's not outside of the context of the previous operation and so we might actually these plunges might even be less severe than what we're looking at here so i'm not terribly worried about it so now we're going to clean up the top side or this back side of the headstock and then we will switch to a ball nose end mill to do our final operation so let's go to 3d parallel we've still got our quarter inch flat so we are good there and then in our boundary machining boundary we're going to select this back contour right here and then we're going to choose these surfaces that we're going to be machining and leaving includes that model checked and i have a suspicion that it's going to try to go into these holes so we'll take a look at that in a second and i can show you how to compensate for that tool on centering on center on boundary so we're good there and again we're going to have to do our little trick as we found out so stock top is fine here but our retract height is going to be from stocktop 0.5 and our clearance height is going to be from the top of this heel stock at zero again it's really annoying but because again because of how this is interacting with our z height we have to deal with this so then in our passes we're going to do pass direction as 90 degrees because if i don't do that it's going to go this way but we want our parallel to be going this way that heel side and then our step over is going to be 0.03125 so really fine little step over and that should be good let's hit play or ok and see what happens okay yes so it is trying to jump into these holes here and those have already been machined in like our very first setup operation so we need this to pass over those and for some reason when i was developing this i couldn't get it to pass over those and i had to go finding i had to go find a solution for this and i wanted to share kind of with the with the class of what's a really neat trick you can use for this so in slope what this allows you to define is what is the minimum and maximum angle on your model that it will detect and machine and so for example we have an angle here that's about 45 degrees roughly from our bottom surface here so if you drew a line up but we don't want it to machine anything that's 90 degrees and that's what these holes represent they represent a 90 degree change in direction of our cutter so we can say from slope angle we we're allowing it to machine from zero to like let's say 60 degrees we won't let it go like beyond 90 or anything like that let's in fact let's do something smaller and see if it doesn't touch this front surface you can see it left a little section where it's detecting that oh it can't cut that because of the slope angle so let's go back to edit and let's change this to 60 degrees hit ok and yes now it's actually machining everything and it's passing over these holes and that's exactly what we want in fact it kind of looks like it's going over our volute a little bit let's pull up our model and then go back to the setup back to model actually no it's not it just looks like that because of the stock to leave so let's simulate this real quick make sure we're okay and then we will do our final ball and mill clean up we still have those errors from the previous one that we're okay with the last operation that we just put in there's no errors so we are good there let's zoom through this contour and then clearing out the material turn off stop on collision and then yes it's coming in and cleaning up that area let's slow it down and yes it is just simply passing over those holes which is perfect it's not trying to enter in so we can speed that up and now we've cleaned up that back side now all we need to do is just switch over to our ball end mill and do another parallel pass on this surface right here and then we'll be done okay so let's go to 3d parallel and let's switch over to our quarter inch ball end mill and then what we'll do is we it looks like our feeds and speeds are a bit wrong so 16 000 rpm and we'll do 75 inches per minute and then go to our geometry tab and machining boundary will be selection now we can either select each side of these which may cause problems well we'll have to take a look or we can do silhouette which will basically create a line around the entire um around the entire model so let's try it this way and then we will do avoid touch surfaces and we're going to check touch because with this machining boundary it will basically try to detect all of this as well and we want to say no we only want it to touch these two surfaces okay and then selection we will select our machining boundary we will select these two and let's see if that works if it doesn't we might try silhouette or something and that should be good and then model bottom is the fixture our top height is the top of our stock so let's bring back our stock here the headstock side and then we do retract from stocktop 0.5 and our clearance height again is our top of this right there and let's make that zero and then in passes we do want it to stay going in this direction rather than 90 degrees like we did on the previous op so we'll leave that b but we want our step over to be 0.03125 inches and that should that should work if not we might have to change our machining boundary so let's see what happens okay it looks like we're not hitting everything so we're only getting about halfway down so let's try changing our machining boundary to silhouette which basically projects the entire body surface um onto the machining tool path and let's see if that solves it for us nope so let's go back and hit edit and let's turn on contact point boundary because right now it's trying to stay within that boundary um that it's projecting but we're not allowing it to go slightly outside to make sure that it touches some of these areas hit okay there we go that's looking a little bit better so we're actually reaching this full extent of this wing here so let's right click and hit simulate and let's see what we got okay we have some tool collides with fixture we'll need to take a look at that as well tool collides with fixture yep okay i have a feeling i know where that's coming from so we'll take a look at that in a second okay bringing out most of the material and then we're going to do our cleanup on the back side of the headstock and turn on stop on collision and let's take a look real quick okay and this is a tool collides with fixture so that means that you can see here the little channel that i put here didn't take into account this little part of the neck and so it's actually crashing into that and it might crash into it right here as well i will go ahead and update that later on but basically what you guys will need to do if you want to avoid that unless you're fine with the with the tool actually plunging into that a little bit it doesn't go very far it only goes like maybe like a 32nd of an inch or something it's not a huge deal but basically you'd have to provide a little bit of clearance like i did with this slot here for that tool and yep same thing on each side and then it works its way through because now it's got the clearance and then this is a tool collides with fixture again because it's going all the way down to the bottom yep so that's all i would need to do to resolve these is create an extra little channel around for this flipped operation and we would be fine so let's just make sure all surfaces are green it does look like we have a little bit of a challenge here so we might need to come back in and resolve that let's play through the rest of this turn off stop on collision okay so we have a little flat spot here and we have a little flat spot here so let's see if we can resolve that real quick so the first thing we're going to try is right clicking and do edit and then in the passes tab we'll try machining steep areas because what this allows to do is it allows this tool path to have a varying degree of step over depending on these how steep of an area it's attempting to machine so we can say the absolute minimum that we will allow it to have right now it's point zero zero three so just like three thousandths of an inch let's make that point zero zero five that'll be the absolute minimum and then the maximum will be the one we set before and let's see if that resolves it so you can see in these areas it's going to take more passes it looks like it might still be leaving a little flat spot there so let's just simulate that and double check okay yep it's still leaving a flat spot there so i'm not sure how well we'll be able to adjust this but let me try okay so i spent a little bit of time working on this and i was able to get it to clean up most of that surface although there is still a tiny little section here that i just can't seem to figure out no matter what options i choose so i'm gonna have to at least in my model deal with that and just sand it out but let me show you what i did instead so if i go back to edit on the parallel and i go back to my geometry tab let's bring back our model here what i did was i flipped my avoid touch surfaces and used model selection so i said i want to machine these surfaces and i included the setup model so that way it's not trying to machine the other surfaces or machine over it and then on avoid touch surfaces instead of using touch to touch these ones i selected a void and selected everything else outside of that what that allowed me to do is basically allows my tool path to continue all the way over to the edge whereas the way i had it selected before is just the way the programming works it wasn't liking it very well and then i tried doing machine steep areas it didn't really help so i'm not going to apply that and if i hit okay and we simulate the whole thing you'll see what we're left with it's not perfect but it's pretty dang good and very easy to sand out again these errors that we have right here are ones that we've already tested and are okay with and these ones are tool collides with fixture and we know how to solve that so we did the contour then the roughing and now we're cleaning up the back of the headstock and then we are cleaning up this and it goes all the way to the edge which is great but it leaves a tiny little flat spot right here and that should be i mean what you're seeing here is a couple thousands of an inch so it's not a big deal we should be able to easily sand those out without much trouble so i'm i'm okay with that um but if in your model if you if you just want it dead on perfect right off the cnc you might have to play around with the options some more i wasn't able to solve that at least in my particular model so in summary we processed our stock cleaned up our scarf joint cut the truss slot and then flipped it over and machined the primary surfaces and then flipped it over one last time and cleaned up the headstock all on a cnc with a limited z clearance and a low cost fixture with just a 3d print to help us along the way we had to do some workarounds with our clearance heights to allow fusion to generate the tool paths but ultimately we came out with solid tool paths and a nearly perfect model i do want to stress here that we are somewhat pushing the boundaries of what fusion finds acceptable machining methods most companies that would produce these parts full time would invest in larger machines and more robust fixtures to make this process more bulletproof and fusioncam is primarily targeted towards those applications however i am confident that this process we produce today can allow just about anyone with a cnc to produce a good part there is always room for improvement however so if you have any suggestions i would love to hear from you down in the comments if you'd like to support my channel i would like to download this project file including the fixture toolpaths and even the animation at the beginning of the video you can find me on patreon.com forward slash austin shainer if you have any questions regarding this process or would like to submit a request for my channel you can send me an email or join our discord server to get help from myself or other viewers on projects you are working on links will be in the description below that's about all i have for today so thank you so much for coming and sticking with me through this hour and a half this is austin signing out

Channel: Austin Shaner

Views: 1,647

Keywords: Autodesk Fusion 360, CAD, CAD Modeling, CAM, CAM Basics, CNC, CNC Router, DIY, Fusion 360, Fusion 360 Beginner, Fusion 360 CAM, Fusion 360 CAM Guitars, Fusion 360 CAM Tutorial, Fusion 360 Tutorials, Guitars in Fusion 360, Tutorials, Xcarve, fusion 360 tutorial, Autodesk, 2D Toolpaths, 3D Toolpaths, CAM Toolpaths for Guitars, CAM for Guitars, 2 Sided Machining, CAM for Guitar Necks, Guitar Necks Fusion 360, CAM Guitar Necks, Scarf Joint CAM, Toolpaths for angled guitar necks

Id: HwBBoSaiepQ

Length: 95min 10sec (5710 seconds)

Published: Mon Sep 06 2021