Creating Shop Drawings in Fusion 360 | Tutorial

want to learn how to make drawings like this in fusion 360. stick around welcome back to cloud42 i'm james if you've been around the channel for a while you know that i have a three-ring binder full of shop drawings like this anytime i make anything in the shop i always start with a drawing with all the dimensions i'll need it just helps me to keep track of things and reduces the number of mistakes and scrap parts doesn't eliminate scrap parts but it reduces the number of them that i make now i get a lot of questions about how i make these now sometimes i'll just sketch something out on a piece of paper with a pencil but more often than not i now model everything that i'm going to build in fusion 360. now this is a natural thing to do if it's a cnc project but even if it's a manual machining project i tend to model it first so that i can get a good idea of how everything's going to fit together be confident it's going to work before i start and more importantly so that i can then generate the drawings from the model so today we're going to talk about how to take a 3d model in fusion 360 like this and turn it into a set of shop drawings like this and maybe you'll pick up a tip or two along the way let's start with something simple this is a model of a chuck key that i'm going to make for my four jaw chuck and this consists of three components i've got the main body of the chuck key with the square drive on the end i've got a cross handle and i've got a 1032 screw that locks the handle in place let's start by making a drawing from this model so we go up to the file menu say new drawing from design and we get a dialog over here showing uh the parameters for creating the drawing now uh we'll talk about contents in a little bit we'll start by just putting the full assembly in there we'll make a new drawing from scratch and we can choose the standard asme is the default that i have selected and that has north american paper sizes in it you can also choose iso if you live elsewhere and you want to do drawings on a4 a3 all the way up to a0 if you like i am going to choose asme and because of the printer that i have i do the 11 by 8 and a half that will give me a landscape drawing click ok and we'll create the new drawing and i have the model stuck to the mouse pointer ready to place a base view now the most important parameter that you want to set over here is the scale right now it's set to one to five i'm going to change this to one to two that's a better fit for this part on this drawing and you have some other choices in here you can choose the orientation for the base view this is a view from the front i could change that and say i want the view from the top and now we're looking down from the top of the model and this all has to do with the orientation of the views in the model itself in the fusion 360 model in this case front makes sense and i can choose the style i want for the drawing when i put it down so right now it's showing shaded but when i click to place the base view and click ok we can now see that it's converted that into a line drawing now if i double click on this view it opens this dialog again and i can go back in and change things so the style right now is visible edges only so like where this handle goes through the main body you can't see any of the detail inside you can't see the screw if i go up here and mark visible and hidden edges now you can see the hidden edges that are not visible from the outside of the part there's some other options like shaded and shaded with hidden edges usually the visible and hidden edges is the most useful for what i'm trying to do now what we've placed here is called a base view and in a drawing typically you have more than one view of a part this is the base view and we can also put in projected views so i'll click the projected view button choose my base view and now i can pull out from that and place other views so if i want to view from the left end i pull it out to the left and click if one of you from the right end pull it out to the right and click if i want to view from the bottom pull down and click and you can even put in isometric views by pulling out at an angle so i'll go ahead and click that i've got all the views i want i'll hit enter now this is pretty busy but you can then go in and you can modify the settings on the individual views so down here where we see the screw the hidden screw there that makes sense that's useful here on the top end if i'm trying to see the detail of that screw hole all those hidden edges are make it hard so i'll double click on this to open the settings for this particular projected view and just click visible edges only and we'll do the same thing over here double click visible edges only and then we can easily see and dimension that square drive now often on a drawing like this you'll want a sort of an isometric view of the part just to identify what the part is in the drawing i can double click this yeah that's pretty big let's go ahead and make that smaller and you know maybe make it shaded and maybe then put that here so i mean that's a terrible example but it gives you an idea that you can actually take these multiple views and put them in your drawing for various purposes what happens though if i don't want the entire assembly like with the tool post grinder i don't want to focus on the entire assembly at once i want to focus on just one part at a time well let's create a new page for the drawing now it's good to note that in the fully licensed version of fusion 360 which is what i'm running here you can put as many pages as you like in a drawing in the free version you can only have one sheet per drawing file so if you need multiple views you just have to create multiple drawings but it works exactly the same so i've created a new sheet and in this new sheet i can insert a new base view so do the same one to two bring this in actually let's make it bigger one two one and bring this in here and place our base view click ok now what that's done is over here in the tree we have our document we have our sheet and then we have our model and then we have our components so i can come in here uncheck the screw and the handle and it leaves me just the body and i can go ahead and place another view if i want that also appears in the tree and i can come down here and i can turn off the body and the screw and that will leave me just the handle now this is too big for the sheet but you get the idea so now i have two views in here and then each one of these can be used to pull out projected views so then you can create drawings of just individual parts and this is exactly what i did with the tool post grinder where i have a bunch of sheets with a bunch of different individual parts the models are all over here in this tree on the left and you can see in this case i've turned off everything except the bearing spacer and that's this particular view right down here now the other way to focus on a single part is when you make the drawing initially from the design you can check in the contents instead of full assembly you can say either visible only or select so if i click select select one part click ok then it opens up a new drawing and i have only that one part uh in selected but ultimately it does exactly the same thing it builds the tree over here and it just inserts the model with the other parts disabled so that they're not visible and if you create a new base drawing and bring that in and drop it it will have all those parts and you would have to go in and you know uncheck if i just wanted a drawing of the screw for some reason so now we have a basic drawing with a part in it let's add some dimensions to it if i just grab the dimension tool and start clicking around there are lots of different kinds of dimensions that i can place if i for example just click a line in here it will add a dimension that gives me the length of that line in the drawing if instead i click a line and then come over and click a second line then it gives me a dimension between those two so if i wanted the overall length of the part i can just come in here select the line on one end and then come over here select the line on the other end and then click to place it and i get the length of the part which in this case is eight inches if i want the width of the part click those two lines and i get three quarters of an inch now another way to get it this same three quarters of an inch here because this is a round part is from this projected view if i just click on the circle then it will place a diameter dimension which happens to be the same the width of the part and the diameter of the outside of the part in this case are exactly the same and so in this case that is a diameter if i wanted a radius i can go into dimensions and select specifically that i want a radius dimension click that same circle and i get a radius dimension now for something like this radius probably doesn't matter that much for something like this where i have an actual radius on the part if i just click the dimension tool since it's not a full circle it automatically figures out that what i wanted there was a radius dimension and it places that so you have the r for radius and the diameter symbol for diameter another thing is handy if you want a whole bunch of dimensions that are coming from the same point is what's called a baseline dimension so i will start by placing a dimension over to this shoulder so i now have a base dimension here of 0.52 inches and i want to also take the dimension to this transition and to the center of this hole and to the end of the part so under dimensions i can just choose baseline dimension choose this dimension that i already have there and then reach over and start clicking on these other locations now in that case i selected the side of the circle and it automatically snapped to the center and i'll choose that point and so then i will hit enter because i'm done and i have now placed a dimension here the 4.52 then 1.52 to this point seven and a half inches to here and eight inches to here and apparently i didn't select something reassociate that there we go and now i have a stacked set of dimensions and i didn't have to place them physically in space and it automatically lined them all up so now if i'm working from this end of the part i have all the dimensions back to the various uh the various points that i need to work with now on this particular drawing this seven and a half inch dimension here is probably not that useful because i'm not going to measure from this end of the part to place that hole i'm going to measure from this end of the part so i can always just come in here and place another dimension i'm having trouble getting to the center of this there we go the reason i'm having trouble selecting the center of this circle is because remember this part is round so that's a round hole through a round part and so it's not a nice clean circle it's actually a bunch of different compound radii there are also some other kinds of dimensions that you might want one of these is an angular dimension now with the dem i can go in and select that specifically an angular dimension or if the lines that i select are not parallel it'll automatically assume that's what i want so if i click this line and this line it'll automatically put an angular dimension between them another kind of dimension that is interesting is what's called an aligned dimension so in this case if i want to know the length of this line not the width in the x-axis but the actual the actual length of that line i can choose the dimension tool select that line and depending on where i pull out if i pull directly up i can get the x dimension here if i pull at an angle i get the aligned dimension and if i pull far enough over i'll get the y dimension and so you can sort of work this back and forth and depending on where you click choose the dimension you want you can also go in here and say specifically i want an aligned dimension and then click two points and it will give me the aligned dimension between those two points the last kind of basic dimension or i guess in this case annotation that's really useful is if you use the whole tool in fusion 360 to create a hole so in the case of the chuck handle here that's exactly how i made the hole for this screw so the screws in here if i hide the screw this is a threaded hole created with the hole tool in fusion 360. so when i created that hole i gave it a thread and gave it dimensions and so if i come back over here this is that same hole i can choose the annotation tool in this case the text note and when i come in and click on that hole and choose that edge and click to place it it will automatically fill in the details that it picked up from that hole in this case it's a diet the diameter is 150 thou it's a half an inch deep and it is threaded 1032 unf2b because those are the parameters that were placed on that hole when i created it in the model so this is super handy for tapped holes in a drawing you don't have to go figure out what it is and type all this stuff in yourself it picks it up automatically okay so now we have a nice messy drawing with a whole bunch of dimensions on it what happens if we change something in the model now fortunately when we view when we create a drawing from the design the drawing is linked still to the model so we do have to save it first now i've saved this file and we can go back over to the model and edit it and so i've got to find the sketch that defines okay so let's start with this dimension right here this is half an inch from the end of the part to the hole if i go back in the model and find the sketch that defined that i can come in here and here is that dimension so let me just go ahead and move this down so now i've moved that part so now it is that feature is now further from the end of the part now if i save this and then go back into the drawing you can see up here in the corner there's this symbol with the yellow triangle and there's a warning down here saying the changes have been made to the reference design so if i just come up here and click on this button it will re-import you can see that feature has moved and the dimension has automatically been updated and we can do this you know as as much as we want i'm gonna go put this back because i actually did want it the dimension that i had it okay save that and you can do this as much as you want uh now it is possible as you move things around like if this if i move this hole far enough that it actually clipped out of the edge of the part then that will actually change the geometry of the drawing and so sometimes you can lose your dimensions like if you move two holes so that they overlap now you no longer have a complete circle in the part and so some things can happen that mess it up but in general you can update the model as much as you want and the dimensions in the drawing will update automatically now sometimes in fusion 360 you want geometry that is actually not a part of the model a classic example of this might be a center line if i needed a center line down this part in order to dimension something off of it you know i don't in this particular model but in another one i might so in this part i may want to dimension everything off of a center line so i can just choose center line here and now i can pick two edges i'll pick that edge and that edge and it will automatically put a center line on the part between them now it's good to note that center line can go between things that are not parallel so if i wanted to select this angle and this angle it's still going to put a center line mark between those so then if i wanted to come in here and dimension some of these things off the center line i can click the center line and then i can select these points you can see where this is half an inch off of the center line as opposed to having to dimension it from something on the outside of the part another thing that's sometimes handy especially for round parts or round features is a center point or a center mark so i can click center mark here click any curved surface and it will place a center mark in the center and then that gives me something i can dimension off of this is also really useful if you just have a radius and you want a to mark the center of that radius for some reason like if i'm going to cut this with a circular cutter and i need to dimension over how far that cutter has to come in from the end i can do that by placing a center mark on the radius another situation that comes up often is wanting to dimension from an imaginary corner of a part now this part when i machined it i machined it out of a rectangular block of aluminum and so i need to cut away this corner well that's easy if i just put this in the vise at an angle touch off on this corner and then lower my tool and machine away that surface but what's the dimension i can't put that on the drawing because there's nothing there to dimension from but i can choose the edge extension tool click this edge and this edge and it will put in those edge extension dimensions so that i now have that point so i can take a dimension grab this line grab that point and i can see that it is 0.41 inches so now i can bring my tool down touch off lower at 0.41 and machine off that material now there are a couple of other drawing tools over here that we haven't touched yet and that's the section view and the detail view let's start with the detail view so in this case i've got my model i've got a view here in my drawing and i would like to put some dimensions on this end part but if i come in here and start drawing these dimensions they're going to be pretty small in the diagram so i can click the detail view then come down here choose a center choose the parent view for the detail view so i'll choose this view and then i want to choose the center point for the detail boundary so i'll pick this that's pretty handy and then i can pull out the size of the detail view now i just want to focus on the tip here so i'll pull it out to here and click and now what that gives me is a larger version of that view so this is one to one i'm actually going to say two to one so we'll magnify it and then place that right here and click ok now this is detail a scale is two to one and this is the so you can see where this is it's marked on the original drawing with the a and over here it's identified and you can move this stuff around but it's identified as being detail a so you can see where it came from and so now we have a much bigger version of this if we wanted to come in and do some more dimensions so like if i wanted to show how i was going to cut this i can put a center mark here and i know that i want to bring that over and i know that tool that i want let's do a diameter dimension this is a quarter inch tool that i'm going to bring over to that center point and then i can dimension from the end of the part and now i have the detail here of how i'm going to actually machine this part i'm going to use a quarter inch tool and i'm going to come in 0.39 from the end and that will place that radius in the right place and i can do you know whatever else i need to do in here that makes sense on the blown up version of the diagram now another view that's sometimes handy is what's called the section view and this is very similar to the section analysis view in the fusion 360 model but i can just click this and now i choose my parent view now in this case we're looking straight down on the end of the handle and i can come up here choose a point at the top and draw a line and you can see it's going to place this view b and you can see where the arrows are it's going to show us a view slicing it along this line looking in the direction of those arrows so i've placed those click ok click here to place and now i have a cross section of this part taken through that line looking in that direction and here it is and i can do whatever i need to dimension this up as well and it's actually placed a little title down here and i can move that wherever it makes sense so here's my section bbc and then scale is one to two which is the same as the overall scale of the drawing and so you can use this to place a section analysis so on the tool post grinder i did this on the front page i've got my view from the end of the tool post grinder i've got my section d and then over here i've got the cross section that just gives a good overview on the first page showing everything that's going on inside and then all of these parts that are identified here with annotations are going to appear on other sheets of the drawing so far we've been working on these drawings and we have just been accepting the default format for all of the dimensions so in this case this dimension is eight this dimension is seven and a half this one is .38 now i i know that the radius of a three-quarter inch part is actually 0.375 and so it's just sort of chosen some default dimensions but we can modify those so over here in the tree on the left there's a document settings area that we can open up and this has all of the default information for all of these so we've got the font and text height the dimension units in this case these are all inches i can click to edit any one of those and it will open up the settings over here so dimension units are in inches i can change that to millimeters if i want click ok and all of the dimensions on the drawing will change to millimeters so what else can we change this is natively in inches i'm using each material so we'll do that dimension format is in decimal uh you can also do fractional if that makes sense so fractional so there's three quarters one-half it's almost like we're woodwork doing woodworking here which would be a great application for this i'm going to leave decimal and then we have linear dimension precision so it's set to two digits i can set how many digits i want i want three because i generally work in thousandths of an inch and there's some other things here display leading zeros display trailing zeros so without those that's what we're seeing here so now we've got three digits of precision so this now says 0.375 which is what we want because that's 3 8 of an inch but like this 0.5 and this .75 don't have their additional zeros on them so we can edit that as well we can display leading zeros we can display trailing zeros we can even display the units if we want so now we've got a leading zero and we have our trailing zeros and we have the dimension the actual units on there and so that if we went back and changed those they would you know change to millimeters but i'm going to simplify this a little bit and take off the dimension unit and take off the leading zeros that cleans it up gives us a pretty nice drawing but still gives me all the precision that i want so 8.000 do i really need that no but i like it so this is how i want the drawing this is how i'll set it up now you probably also notice that down here in the corner of the drawing there is a title block with a bunch of information in it now we can actually edit this just uh double click on it and it opens up and then we can go in and click on the individual fields now interestingly enough like if i want to change this title if i click here nothing happens but if i actually click on the solid part of the text it highlights it i think it's just using the same text tool it uses for sketches and that's how it works and but you can just come in here and you can just edit any of this that you want put in whatever information you like you can you know put weight information information about the sheet approval check who drew it dates you can edit all of this stuff and so that allows you then to title these up you know any way you want on your drawings okay so now i have my beautiful shop drawing and i need to output it how do i do that well there's a couple of ways uh first up here is i can output it as pdf so i just click the output as pdf it wants to know what sheets i want in this case i'll just say the current sheet and i'll say i do want to open the pdf and there's this additional check box of called line weights and what this does is when you check the line weights it actually outputs heavier lines in which i tend to prefer that particular look so i'll click ok and save this drawing and it'll open the pdf so here's the pdf viewer with our pdf document and this is what it looks like with the line weights now i can save this i can print it i can do whatever i want with it let's do another one without the line weights so that you can see the difference and without the line weights you can see the lines are just a little bit lighter and like i said i don't prefer this particular style but either way i can save this i can publish it i can print it now if you have the free version of fusion 360 the pdf output button will be disabled it's one of the features that they nerfed in the free version of fusion but you can still output your drawings just come over to the file menu select print now normally i would use this to print to my printer but i can also come in here because i have the adobe tools installed i have the adobe pdf driver if you don't have that on windows you'll have the microsoft print to pdf driver so i'll choose that i want my current sheet and i have the same line weights checkbox i can click print and let's save this my drawing let me open that and here is the pdf file in this case uh you know it happens to be rotated that's just how the microsoft driver generates it but i can then take this drawing and i can rotate it edit it see i should be able to rotate that again because i've got the pdf editor here and you can print that out you can distribute it do whatever you want just like you would if you were actually outputting it as a pdf i think that's all the features that i wanted to show here in fusion 360. let's take a look at a complex set of drawings this is the tool post grinder that i did back in looks like 2018 and this is uh you know it's a fairly complex design with you know a dozen parts or or more in it and i put together a complete set of shop drawings for this so this has got multiple sheets we talked about that and on the front i just have a shaded view and i have a section view so this is just an overall orientation and i use the section view just to give an idea to the person looking at the drawing what they're going to be looking at on the subsequent pages and put labels on all of the individual parts to identify their names so that when they show up elsewhere in the drawing it's clear what they are and the second page here is just a line drawing with the only the visible edges with some of the overall basic dimensions now these are not the dimensions you're going to need if you're going to make the thing but it gives you an idea of the physical size of the thing for when you want to put it on your lathe how big is the tool post block how high is the spindle center above the bottom of the axa tool post holder what are the overall dimensions so that you could use this to decide if it's going to fit on your machine i also have a view from the outside shaded that i put down here in the title block just to make it look professional because i thought it looked good moving on we start to get into individual parts that are separated out got the spindle housing see we have a bunch of diameter dimensions we've got thread dimensions called out here now i didn't know at the time that i could have done this with the hole tool so i actually edited and typed in this dimension but you could just as easily if you'd made this hole and identified the thread with the hole tool that call out would have been automatic now here is an eccentric part where i've actually got two circles that are offset and i just use the geometry to put in a center mark on the inner circle and a center mark on the outer circle and then put a dimension between those two center marks and this gives me the offset dimension i need to set up in the four jaw chuck and the lathe to actually cut that over here on the bearing cap here's another use of the section so i've got a section detail e and it's a cross section here so that i could dimension up clearly the inside parts of this cap to show how the bearing register fits uh here's another uh case of a detail view so here i've got my tool post clamp i wanted to put a bunch of dimensions in here close so i ultimately used a detail a and brought that out so that i can zoom that up two to one now in this case what i was trying to show is how to dimension the inside of the dovetail in this case i've had i've placed in here a quarter inch pin and a 249 pin obviously you would be better off using two quarter inch pins to dimension this but my gauge pin set only has one quarter inch pin so i went ahead and drew the dimension with a quarter inch and a 249 and then put a note in here for what the spacing is between the pins so that as you're machining this you can measure the dovetail and here's a good example on this motor clamp showing the screws this is a case of showing hidden lines and so you can see the placement of the screws and where they fit inside the motor clamp but then i've actually got all the dimensions that are needed in this case like the bottoms of these counter bores are dimensioned off the center line of the part which is useful because there really is no dimension on the outside that's easy to pick up here are the detailed drawings of the pulleys and in order to dimension the pulleys i have actually included in the original model a thread wire an 063 thread wire and shown on the detail views here so here's the uh the actual scale drawing of the pulley and then i have a blown up detail view showing where that fits and the demand and with a note for the dimensions across the wire so that i could cut these v's to the proper depth and here's a case of edge extension because i needed to locate the center of the groove but there was nothing here that was easy to dimension off of so i went ahead and put in the edge extension geometry and that gave me something to attach my dimensions to i think that's pretty much all of the tools there's really not that much to it when you put together something like this with a lot of parts it can get quite complex but really it's just the same techniques over and over and over again i'm just pulling in the parts one by one laying out the views that i think are going to be necessary in order to machine or actually manufacture the parts and getting the dimensions on there and there is something of an art to spreading this stuff out and making the drawings readable i will not claim to be an expert at that but i was able to make drawings here relatively easily that gave me what i needed to machine the parts in the shop well i hope you found that interesting and maybe even a little bit useful if you did give the video a thumbs up feel free to subscribe to the channel and leave me a comment i'd like to know what you think thank you for watching [Music] you

Channel: Clough42

Views: 24,729

Keywords: Fusion 360, Drawings, Mechanical, Machine Shop, Machining, Tutorial

Id: GUDhet2TKHQ

Length: 35min 29sec (2129 seconds)

Published: Sat Mar 13 2021