Fusion 360 Screwdriver Tutorial

[Music] hey everyone kevin from mechanicaladvantage.com today i wanted to do a video on how to model a phillips head screwdriver so that's what we're going to do and we're going to jump right into it the first thing i'm going to do with this file is save this i'm going to hit the save and i'm going to give it a name and i'll just call it screw driver and i'm going to hit save in that location right there that'll work for me and now i'm going to do a couple things before i get started i want to create two uh parameters so from the modify menu i'm going to go and choose change parameters and when this menu comes up i'm going to hit the plus and the two parameters i want to call are going to be handle height and i'll give this a value of 2 inches and i want to do another one of shaft height and i'm going to give this a value of 2.25 inches and i'll hit ok now we really should answer comments but what these do i'm going to skip that for the video and i'll hit ok we'll reference those parameters later on in the design process i know i'm going to have a handle component and i know i'm going to have a shaft component so right off the bat i'm going to start off by creating components and there's a couple ways you can do this you can go to the assemble menu and choose new component and because this is the way it's been done in fusion for a long time it's my missile memory a lot of times what i do is right click on my design name and i choose new component i'm going to use a standard component and the name of this component is going to be handle it's going to be uh underneath the parent which is the design and it's going to be activated once i hit ok the other thing i'm going to do right off the bat is i'm going to go to the assemble menu and do an as build joint and i'm going to click on the word handle in the browser the component and then the word origin and that's going to create a rigid joint between them now i get asked a lot why i do that well let's just hop into another file i'm just going to create a new component right off the bottom and i can even save it if i draw something here sort of like what we're going to do later on let's draw a circle and i'm going to extrude that when i do it this way you can see that i can take that circle this cylinder and move it anywhere i want to so i'm going to undo that and get it back to where it needs to go to revert that back if i were to roll back to the very end and say assemble and choose an as built join between the component and the origin and then i'll hit ok so that was the very first thing that i did roll this to the end now now i can't move that cylinder anymore so i know that handle i want it at the origin so i'm just doing an as built joint right away so that it can't move i'll close this out and go back to my original design file so i'm on my design file now i've seen the joint symbol bothers you you can just come and turn off the joints folder or you could turn off the individual individual joint that we just worked on i'm going to create a sketch now on the front plane and we're going to work on drawing the handle shape so i'm going to start the line command and i'm just going to kind of come over about maybe that far i'm going to come up angle in angle back out come straight up and don't worry but if you're not being you know completely perfect on these now oftentimes i'll do what i just did there to close shapes up i know i want this to be vertical when i'm done but i drew it kind of as an angled line so that i visually can remember to come back and say make sure to make that vertical so i've got that taken care of that's going to be my handle shape i didn't do a great job on the sizing but that's all right we'll be able to fix all that in a minute and i'm going to start another line command and this time i want to draw a center line uh not construction but center so i'm going to go to the origin and just drag down and that's going to make doing my dimensions a little bit easier so now i'm ready to start adding some dimension so i'm going to start the dimension command and i'm going to click on this center line and this outside dimension and what i do it's going to give me the total diameter of the part so i'm going to say that that's going to be 1.125 and i'll hit enter and that creates my uh diameter dimension there i'll click on that center line again and i'll click on this upside dimension here and i'm going to call this one inch so that gives me a one inch dimension to see that things are sort of flipping around that's okay i'll just drag this in a little bit and that's probably where i should have been a little bit more careful on getting the scale right on this but you can see it wasn't too big of a deal so i'll dimension this is going to be 0.2 inches and i'll dimension from here to here and i'll call this point six to five inches every time i move this around it's just going to come back with the next dimension so i should have probably just left it but you get the idea i'm going to add one more dimension between here and here and i'm going to call this 160 degrees and then i'm mostly black the only place i would what i have left is to define the total height and i'm going to do a dimension here and i'm going to click that but instead of typing that dimension in i'm going to call this handle and i'm going to reference that handle height parameter and i can hit enter now that i've got all my dimensions on here i can move these around and clean them up should i want to kind of move them and reorganize them i usually leave this step for the very end so there's my original handle design i'm going to go ahead and finish my sketch i'm going to go to a home view click on the revolve command and choose my center line as my origin and i get the basis of my handle so far okay for step two i'm gonna put a little rounded corner down here so i'm gonna add a sketch and i'm gonna put that sketch on the front plane and once i get on the front plane i'm gonna slice this now i'm seeing wherever the solid body meets the plane that i put my sketch on but i can't reference any of the lines if i start the line command it's not picking up on any of those edges so i have to project those edges into my sketch first so from the create menu i'm going to go to project include and this time i want to use the intersect option in the filter over on the right i want to change it from specified to body so i'm going to go and change bodies and i'll just click ok and now what basically what's happened is fusion's projected in the outside profile of my handle and that allows me to go create an arc a three-point arc i'll click on this bottom line and somewhere on this edge and kind of pull down a little bit i do want to see that tangent symbol there i don't want a tangent symbol right there this isn't going to be a perfect tangent on each edge so i'll add some dimensions now and the dimension that i want is going to be from here to here is going to be 0.4375 and the radius is going to be 0.75 and it turns fully black and constrained because there's only one arc that can be tangent to this bottom line have a radius of 0.75 and a distance of 0.4375 away from the edge now a lot of times what we would do is we'd finish the sketch and do a revolve there are two closed profiles that fusion would have to we could choose between so it can't automatically make the choice for me so sometimes what i'll do here is i'll go right to the solid tab even though i'm still on sketch i can still go to the solid tab and choose the revolve command now makes it really easy to grab that profile right there and then i'll choose my access which i could choose the blue access or any solid round face will work and you'll see that i'll get my cut and i'll hit ok and now i put a little cut around the bottom to make my life a little bit easier i usually try to leave fillets in chamfers until the very end but i want to knock the edge off of this so i'm going to go to the modify menu and choose the fillet command click on this edge and i'm going to put a fillet radius on that edge of 0.25 and we'll hit ok so my handle starting to take shape pretty well i've got some holes that i want to you know kind of put some like little grips on the handle so i'm going to put a sketch up on the top face and i'm going to do a circle but i want to be construction i'm going to start from the origin and this diameter of the circle is going to be i'm going to go with i think two inches so put a two inch circle there and then i'm going to come over here and i'm going to draw another circle somewhere on the construction circle but i don't want this one to be construction so i'm just going to kind of come over here drag this out i'm not going to dimension it i'm just going to make it that size the reason i'm not going to make it that size is the rate the dimension that i've been given is a radius dimension and i can't add a radius at the same time as i'm creating the dimension so now i'm going to right click and choose radius i'll left click to place it and type in 0.5 and now i have my 0.5 inch circle and i probably need to change the diameter of that a little bit i don't want that to interfere with the top edge so i'm just going to call this 2.05 let's go just a little bit larger see now it's outside of that i'm going to add a horizontal vertical constraint between the origin and the dot in the center and now that moves it into place and you can see that everything is lined up where i want to go i'll finish my sketch i'm going to rotate slightly and i'm going to extrude this circle pull the direction i want to go until it starts to intersect and then i'm just going to say i want to go through all hit okay and there's one of the grip cuts that i'm going to have going through my handle right there now i'm going to add a couple more fillets on here at least one more to start out with so i'm going to fill it this edge and that phillip radius is going to be .05 and now we've got a nice fillet going around there okay i know i want six of these grips in total and now i don't want to do that six times so instead what i'm going to do is from the create menu i'm going to choose to do a pattern and a circular pattern right now my feature type or my pattern type is set to faces i gave the answer away there i wanted to be set to features so i'm going to go and select features and i can click those features on the model or i can select them from the timeline so i'm going to select mine from the timeline you can select yours however you want and again for the axis i just need to click on some round face so i'll click on that edge and tell fusion that i'd like six of those and we'll hit okay and now we get the uh the fill it and the cut for the grips going around i'm gonna do one more fill it across this so i'm gonna choose fill it one more time i'm gonna grab this bottom edge right here and i'm gonna call this point zero two five just to put it just around that corner off a little bit and i'll hit okay and now i get all those edges rounded over we'll do a different fill radius i want to grab this underside this edge and this edge and i'm going to give those a phillip radius of 0.05 and you can see i get a pretty aesthetically pleasing shape right there i think and so we'll hit okay and click on my home button and really one of the last things i want to do to this handle is put a hole in it where the shaft is going to go so i'm going to use the whole command to do that and i'm just going to click somewhere on this face now again a lot of times what people try to do is they try to click right at the center and i'm going to encourage you to try to click off of where you want the hole to go so you can easily move the hole where you do want it to go so let's click right there if i click on the blue dot a white dot appears in the center i'll drag those two together kind of snaps together and now i can go start answering some of the questions i want the bottom of this hole to be flat so i'm going to set that to be flat and i want the depth of the hole to be 0.75 i'm also going to set the the diameter of this hole to be 0.125 so there's my 0.75 deep that actually looks a little on the on the deep side so let let's just come and change this to be like a half of an inch deep that should be enough and i'll hit okay um so that's the basics for the geometry of the handle now one of the things i note a lot too when i'm seeing things out on youtube or instagram or whatever is all the models are always gray our models don't always have to be gray we can give them colors so i'd like to change the appearance of this model by going to the modify menu and then i want to choose the appearance when this comes up i want to go find any appearance that i want i'm going to use paint for this and i think i'll go to the glossy and i can drag on any color that i want to onto my handle so i'm going to go just grab this yellow color and drag it on and now you can see that my handle changes color to match i can give individual faces colors if i want to so i just switch my selection filter to faces if if i really wanted to i could go drag a color onto an individual face rather than having it applied to the entire body i'll just undo that i don't want that one face to be colored so there's our handle handle's good now it's time to start working on the shaft so i'm going to activate my top level design again and this time from the assemble menu i'll say new component and this component is going to be named shaft and i'll hit okay and now i'm ready to start doing some sketching for this so i'm going to say that i'd like to create a sketch on the face at the bottom of that hole right there and once i get that done i'm going to finish my sketch and now i can just extrude that and i'm going to give this a a shaft height dimension and i'll hit okay so i've just created a relationship between the screwdriver shaft and and the the handle itself the handles driving the geometry so that the shaft always fits in the handle but again if i click on the shaft and i drag it it can move around anywhere it wants to so i'm going to revert it and i'm going to go to the assemble menu one more time and do an as built joint and as build joint means that this thing is drawn exactly where i want it to be there's no need to move it it is where it needs to be so i'm just going to click on the thing that can move and i want to click on the thing that can't move so i'm going to click on the shaft and then i'm going to click on the handle and it's going to add a joint between those two now i can't move that around anymore i want to put kind of a point on the end of the shaft so i'm going to create a sketch and i'm going to put it again on the front plane and once i get that located on the front plane i'm going to slice my geometry and one more time i'm going to go to the create project include intersect and it should be already set to bodies for my last time and i'll just click on this and i'll hit okay now for this i'm just going to draw a line from the edge and down the only place i don't want to be is exactly at the middle of this line so you see i'm off by a little bit and i want the distance from the center point of this edge to the endpoint of that line to be ten thousands of an inch now it's a little tricky because there's nothing there that i can dimension to so what a lot of people i will see do is they'll come and sell put a point or they'll draw a line or something and put the midpoint there's a maybe a faster way you can do this it's more automated i'm just going to start the dimension command and i'm going to hold down my shift button as i scrub along this edge and eventually what will happen is fusion will find the midpoint i'm going to click on there and i'm going to click on the endpoint of the line and i'll set this to be 0.01 and fusion will automatically add that point to me for me 0.01 is what i meant it'll automatically add that point and put it at the midpoint all in one shot so i didn't have to do anything to make that happen it just sort of did i have one more dimension that i have to do so i'm going to do a dimension between i did d for dimension there to get in the dimension command i'm going to click on that point and that point and that value is going to be 0.125 and that's going to be fully block blocking defined and again if i want to i can just go back to the solid tab choose a revolve command pick my profile pick on my outside face and fusion is going to rotate that around and cut the the end of that so we're starting to get a little closer to the shape of the screwdriver that i want i'm going to put a sketch up on this top face and now what i want to do is i want to draw the cut uh where this is going to go into the bit so for this a couple of different ways we could do this but i'm just going to kind of draw a triangle so i'm going to bring a triangle in when i get to where i want this to end i'm going to have a radius end on it i'm going to left click and hold and i'm going to swing into an arc don't worry that our arc is really large compared to what i want right now and i'll just kind of drag this back out i know this is going to go down pretty far so i'm going to drag both sides back out and then i want a line that connects them i don't really care if it's horizontal or vertical or anything right now i'll fix that with a horizontal constraint to get that where i want it to and i know that the center of this is going to be lined up with the origin so i'm just going to put that on there now and i fully expect it i thought would have broken a little bit more and stayed together pretty well i also know i want a tangent constraint right there so we're good there okay so i can kind of just start dragging these things around a little bit get a little bit more into place i'm going to add a dimension so d for dimension between the origin and the bottom line here and that dimension is going to be 0.875 that moves that around i can just uh drag things back if i need to so i can just grab that whole thing and drag it a little bit closer to where i want it to be maybe i'll start adding some dimensions so i'm going to dimension between the origin and i want to dimension to the tangent point of this arc to do that i'm going to right click and say pick circle arctangent and i'm going to click on that arc and i will say .005 is what i want to do for that distance and i also want the radius of this arc to be .005 so i'll click on that so things are starting to work pretty well okay so i know i want this to be perfectly symmetrical on each side of the green line so to do that i'm just going to add another horizontal vertical between the origin dot and i'm going to hold down my shift button as i scrub across this bottom line until i find the midpoint and click on that now no matter how i change this it's going to change it symmetrically on both sides i'll add a dimension so i did d for dimension i'll click on this line and this line and it's going to be 92.5 degrees and i'll hit enter and now we'll see that everything is black and fully defined so that's going to be what's going to make my phillips head on this bit on this shaft i'm going to finish my sketch and i'm going to kind of rotate around now this time i want to do the revolve command one more time i'm going to click on that profile make sure you zoom in and you get this little chunk right there as well we need both of those for this to work actually we probably only need that one down there but we're going to use both of them and now for the axis i'm just going to click on this edge right here so lots of people think that the rotation edge also has to be on the model but any edge will work so i'll just click on that and we'll do a full 360 degrees of rotation and i'll hit ok and there we get one of the cuts that we're going to do to complete this shaft i'm going to say modify i'm sorry i'm going to say create pattern and circular pattern again i want to pattern features i can grab the cut right on the model i could have grabbed it on the timeline as well and for the axis i'll just click on the shaft and tell fusion that i'd like four of these this time and i'll hit okay and there we have our phillips head screwdriver i don't know if the dimensions for this phillips head are exactly right but the methodology of creating the jams right here should work out um so we've got our little phillips head screwdriver and that's the way that i go about creating it now in the very beginning you may have remembered that i added some i'm going to go back and activate my top level design i added some parameters because i might want to make variations of this so i'm going to hit save i can do a file save as i'm not going to i'm just going to go change the original if i want to modify and change parameters i could come to this handle height and maybe i could change this to be 3. and now if i hit okay you see that my handle got taller if i said modify change parameters one more time i could go to my shaft height and say that i want that to be 3.5 and i'll hit okay and now with those changing those two dimensions i got uh somewhat the same shape to the screwdriver but i got different lengths for the shaft and different lengths for the handle but the rest of the geometry all kind of matches so if you've ever looked at a uh if you've ever looked at a screwdriver set they all sort of have the same profile they just have different sizes we could change the diameters we could do anything we want to at this point just have to add more parameters if we wanted to do a more automated way so that wraps up my screwdriver tutorial hopefully you guys enjoyed this one if you have any questions or comments please leave them below if you have any other ideas or common objects you'd like to see drawn like this drop me a line kevin mechanicaladvantage.com and we'll see what we can do for a future video as always thanks for watching

Channel: Mechanical Advantage

Views: 836

Keywords: Autodesk, Fusion, Fusion 360, screwdriver, tutorial, phillips, modeling, Autodesk CAM, solidworks, Inventor

Id: DvoJwYgywic

Length: 22min 7sec (1327 seconds)

Published: Tue Jul 20 2021