Hex Bolt Design (CAD Tutorial)

hey what's up everybody tutal toy here and in today's on shape tutorial I'm going to show you how to create this setup now really I'm going to do this as a two-part series um and the this video is going to be a little bit on the longer side what I really wanted to do was create a true step-by-step tutorial that teachers or students could follow along with and create a hex bolt there's a lot of good lessons we can learn from modeling a hex bolt you know we can learn about how to create these nice rounded corners on the head of a hex bolt we can learn about what the proper way is to set up a helix and then to sweep a profile along that Helix and we're also going to talk about how to create this lead in here at the top of the hex bolt so that these two parts can in fact mate together or screw together now in the second video I'm going to show you how to create this hex nut and how to do what's called match threading which means you've got an existing part and the threads in that existing part work well now you want to create the mating component for it and you want to kind of transfer those threads into the mating component so I'm going to show you how to do that in the second video video but for now let's get into this first video this is going to be a true step-by-step tutorial on how to create the hex bolt so it's going to be a little bit on the longer side but I'll include bookmarks down below so you can just kind of Click into the different sections of this lesson and hopefully you will learn how to create a 3D printable hexol [Music] ow so here we are in our web browser in the totally free version of onshape on shape.com free if you want to sign up for that free account and we're going to choose to create a new document I'll call this 3D printed hex bolt and nut we're going to create the nut in the second part of this tutorial series but in on shape it's very easy to create multiple parts that interface with one another all in the same document so we're going to create this document here 3D printed hex bolt and nut and now we're going to create the hex bolt itself now this is not working from any existing standard of uh an existing off-the-shelf hexol this is a custom 3D printed part that I'm going to create and so with that in mind if you want to change any of these Dimensions to fit the project that you're working on you know feel free to do that but this should be a really nice step-by-step tutorial to help you create a hex bolt so I'll start out here by create by selecting the top plane pressing s and creating a new sketch on the top plane and then I'm going to press n to get normal two now I'm going to jump into the polygon command the inscribed polygon command you can see here that we've got the inscribed and circumscribed polygon we're going to use inscribed and you're going to see why in just a moment so the inscribed polygon command I'm going to single click on the origin move my mouse out I'm going to single click again and then as I move my mouse here kind of left and right you can see that I'm increasing and decreasing the number of sides on this polygon so if you've never used the polygon tool before now you kind of have a basic idea of how to use it once you decide on a size it works for you you can single click in the background let's say I I choose seven and I single click in the background and then I realize oh actually this is supposed to be six cuz it's a it's a hex bolt right so you just double click on that Dimension change it to six and there we go now we've got this nice hexagon so I'm going to take one of these lines of the hexagon and press h on my keyboard that makes that line horizontal and then I'm going to press the S key and jump into the smart Dimension command and for this 3D printed project I'm going to make the flat to Flat distance 40 mm so there we go we've got our 40 mm uh Dimension there for the flat to Flat we've got a circle here uh in in this polygon that's going to be important we're going to use that in the next step when we go to create our rounded Corners so now let's take that shape and let's extrude it so s key extrude and we're going to extrude that up to a height of 13 mm and again these are just kind of uh imaginary numbers that I came up with that look good but for your project they might be a little different and that's fine um you should be able to kind of follow along with this tutorial and then make changes as you see necessary so we're going to make that 13 mm High hit the green check mark hit okay and there we go we've created kind of the head for that hex bolt I like to rename my features so I'm going to use shift n here I'm going to say head for hex and now I'm going to show this original sketch so I'm going to show this sketch of that has a circle there and the reason why I'm doing this is because I want to create those nice rounded Corners around the perimeter of the hex bolt and one way that you can do this is you can start with a sketch here on the front plane so this is the plane that's going through these corners of the hex this corner and this corner of the hex um this this wouldn't work if I chose the right plane you'll see why in just a moment so I'm going to choose the front plane here and then on the front plane I'm going to choose to begin a new sketch so begin a new sketch there get normal to and the geometry that I'm going to create is going to look like this it's going to be a a line that comes over like so it's going to be another line that kind of comes up here like so let me delete that extra line and then it's going to be an arc which is tangent to that uh upper line so create an arc here you can see that this Arc has a tangency relationship to this upper line if you didn't get that tangency relationship just go back in and add it manually now I'm going to take this point of that sketch and this Arc from the inscribed polygon and I'm going to use What's called the Pierce constraint which means that wherever that Arc is passing through the sketch plane there's going to be a relationship so I'm going to pierce that point in the current sketch to the Arc of that external sketch and we can see that that locked in to where that uh where that circle is now I'm going to create a relationship here just a coincident relationship between these two so I'll press I on my keyboard for coincident and then finally I'm going to add a dimension here and the deeper this Dimension goes the the closer you're going to get to tangency so let's say I make that 1.5 and then I'm going to just press n to get normal two and uh then I'm going to examine that Dimension and I'm going to change that Dimension to two you can see that we're getting closer and closer to tangency here for this other Arc you can kind of Imagine That by seeing where this point is relative to this point the closer this gets to horizontal the closer you are getting to tangent now it doesn't have to be tangent um I like in this case with you know with this geometry that I've created here I like for this Dimension to be closer to to close to tangent but not quite perfectly tangent but if that's what you wanted you could take these two points and just make them horizontal to one another I'm going to use a dimension here of 2.5 I'm going to create a line that goes up through the middle of the model here like so and then going to perform a revolve command so revolve and for the revolve command I'm going to say this will be my revolve axis there you can see what that preview looks like it is showing up red uh because I'm probably going to end up getting like a zero thickness error if I try to make this as solid geometry but we're not trying to add geometry we're trying to remove geometry so we choose remove and there we go we hit the check mark we hide that original sketch and look at that thing that thing is looking good that is uh pretty much exactly what we wanted from this model uh nice little rounded off head there and you can you know you can see that when you 3D print that that side is going to be a nice smoother transition where this side here I'm going to leave this side sharp and that way when you 3D print your model you can kind of compare the two results and you'll see what I mean and this is basically what a a traditional hex bolt looks like it's got these rounded off Corners here well that's how you can create that geometry in on shape so now let's uh let's rename this feature shift n we'll call this um uh rounded corners on hex and let's move on now and create our next feature which is going to be the shaft for those threads so I'll pick this face here begin a sketch uh Orient my view I'll just leave the view oriented the way it currently is create a circle here and I'm going to give this circle a diameter of 20 mm and then I'm going to extrude that out to a height of 65 mm so I'll press tab tab tab 65 enter enter there we go nice quick way to uh to quickly create that geometry and we'll call this thing shift n here uh shaft for the Reds always good to rename your features kind of let you and your your co-workers know what's going on with those features now what I want from this thing let me do a shift one here to get into my front view what I want from this thing is I want to have a lead in so that when I go to to put this thing into the the nut or or engage the threads into the mating component uh it's it's very easy for the geometry to two mate together and the the intuitive way of creating this feature would be to create a chamfer so I could create a chamfer like this the problem is we're going to be adding material for the threads and once we add that material for the threads we're not really going to have a clean Edge that we can just chamfer so instead what we're going to do is we're going to create a sketch here that we're going to plan on using a little bit later in the design to create that lead in so I'm going to go to the front plane here and I'm going to begin a new sketch and I'm going to create some geometry that looks like this it's going to uh start here uh kind of at this this top edge of the model it's going to come down here at about a 45 degree angle it's going to come up like this uh we'll probably bring this up like 10 or 15 millim above the model it's going to come over like this uh same kind of idea 10 15 millim above the model and then we'll close this off here like so let's make that 10 mm that looks pretty good let's make that line vertical and let's create a coincident relationship between these two entities uh like I said we're going to have a uh an additional kind of offset here let's say we'll make this uh 12 mm uh really kind of arbitrary what that distance is and then we're going to Define what the lead in angle is here now I'm going to make this at 45 you might decide to make it a little bit more or a little bit less I'm going to make that lead in angle at 45 there and then I'm going to finish up by creating a vertical line here and this vertical line is going to serve two purposes it really is going to be used for construction so I'm going to take that line and just uh click on it and press Q to turn it into a for construction line and then I'm going to add some dimensions I'm going to add a dimension here to represent what the diameter of that leadin is and I'm going to make that diameter uh 14 mm uh to work with this geometry and then I'm also going to create a dimension here that goes from this point to the top of the model and I'm going to make that at 5 mm so basically this is at 1/2 of this distance here and the the significance of that is that that's going to become the end point of our Helix in just a couple of steps you'll see that in just a couple of steps so just kind of kind of bear with me but the reason we're creating that with a dimension instead of just leaving it free is because if the length of this shaft changes we want the Helix to update with that length change so that's why we're assigning a relationship uh between the the top of the shaft and this end point here so I think that sketch looks pretty good and eventually what I'm going to do with that is a revolve cut uh or a revolve and remove material but I'm not going to do that yet so I'm just going to hit the check mark here and I'm going to rename this to uh sketch uh for lead in chamfer call it that sketch for lead in chamfer so I'm going to be using that sketch a little bit later in the tree but I wanted to create it now while I have nice sharp geometry before I get in and actually create the threads all right so uh now what I'm going to do is I'm going to hide these uh front top and right planes uh I'll just hide them using the the traditional hide command instead of pressing P because I do still want to see some of my planes and one of those planes that I do still want to see is going to be a new plane that I'm going to create here so I'm going to pick on this face here and I'm going to go into the plane creation command that's going to automatically take me into an offset plane command and I'm just going to offset that 3 mm and that 3 mm is going to go down underneath that head of the bolt and this is where my Helix is going to begin and uh that way my threads kind of immediately begin here at the bottom and I don't have to do any cleanup we could there's other ways that we could resolve this issue but this I think is a a fine way if you're going to be 3D printing to to create the transition between the threads and the underside of the head so I'm going to create a plane here which is down 3 millimeters down underneath and there we go and that is going to be I'll do a rename there that'll be plane for Helix uh base Circle call that all right so now let's create that Helix base Circle so I'm going to pick this plane I'm going to choose to create a new sketch and I'm going to pick this uh edge here of the model and use a a convert or a project use command in on shape and just kind of project that Circle down onto that lower uh that lower plane and that is going to be my circle for the Helix base so now we're going to get into the Helix command now if you don't know where the Helix command is that's fine in on shape we can always use the search tools command here so I could search for Helix and there we go and you can just launch the command right from the search results so I'll launch the Helix command and then how am I going to create this Helix am I going to pick a centrical face am I going to pick an Axis or am I going to pick a circle I am going to pick a circle so here where we choose our circular Edge I'll choose this sketch that we've created and then for the height of this thing you can see that I can Define this with a height well I'm going to make that height end condition an end point so the end point of this Helix is going to be this point here that we created in our layout sketch and there we go now we can see what that Helix looks like now there's a lot of ways that you can Define your Helix you could Define it by the number of turns in Helix so you can see here that the target Revolution here I'm going to I'm going to increase this to 12 and press enter and there you go you can see how that's changing but typically when you're doing thread design you're more concerned with what's called pitch which is basically the distance between the thread the you know the same point on consecutive threads or in this case the distance between two revolutions on the Helix so in order to Define that what I'm going to do is I'm going to change this option from input type to pitch so we'll change this to pitch here and we're going to say that the pitch between each of these threads is going to be 5 millimet 5 millimeters and again this is just for this design kind of as a tutorial in in your example you might change you might tweak some of these dimensions and that's totally fine you you know you do you you work with whatever works for you if you like the ability to be flexible and to kind of create designs that work for you take a minute hit the like button on this video uh very important that we always remember to hit the like button on these types of tutorial videos all right so we've got our just a review here we started at the top we said we're going to do a circle we said we're going to pick the edge of that sketch that we created we said our input type is going to be pitch our start angle is going to be 0 degrees that's fine uh our end condition is going to be an end point and that end point is going to be this end point here of that layout sketch that we created for the lead him and then our Target pitch is going to be 5 mm the uh direction of the thread or the direction of the Helix is going to be clockwise standard you know righty tidy type of thread so I think this all looks good and we hit the green check mark and boom there is our Helix we have now successfully created a helix for this design and you can see that the Helix does in fact go all the way down into the model it ends up way down here now in order to see that end point um because I am going to want to select that end point to use it for plane creation I'm just going to temporarily change here to a wireframe option so we'll do hidden edges visible that makes it a little bit easier for me to see the helix and the end point of the Helix I am going to select the Helix I'm going to select the end point of the Helix and I'm going to create a new plane which is perpendicular to the curve at that end point now fortunately all I need to do is launch the plane command the plane command is now buried here underneath the Helix command from earlier so we've got a lot of different types of reference geometry in here so I'm going to choose the plane command and on shape is smart enough to realize that what I want is a curve at a point we talked about this in an early quick tip video about how to create planes quickly so I'm going to hit the check mark there and that's going to create a new plane now you'll notice this plane is not exactly vertical and we can kind of compare it to the uh the front plane here you can see what the front plane looks like and here you can see what the new plane looks like and this is important because we don't want our threads to be created on a skew and and if we were to create the sketch for the threads here on the uh on the front plane that's what we would end up with we would end up with kind of a skew you might end up with expected binding when you try to interact between the two components between the hex bolt and the nut so this is why it's always important whenever you're doing a sweep so the the Helix that we created here is the sweep path and we always want to create our profile plane on a plane which is perpendicular to that path at the end point so I'm going to rename this here I'm going to rename this plane so shift n I'm going to rename this to uh profile plane for Threads and we are now ready to take that that sketch plane so we'll select that plane we're going to begin a new sketch let's get normal to and now we're going to create the profile for our thread now for the profile for this thread we're going to once again reference the end point of the Helix here so here you can see the Helix here you can see the endpoint and we're going to start out by creating a line from that endpoint I know it's a little bit hard to see it's a little bit hard to select but we're going to create a line from that endpoint and we can make that line horizontal for this example um I'm not going to get too deep into the the theory of thread cre for this uh tutorial that could almost be it its own video in entirety but what I am going to do is I'm going to take this Helix so you can see that I'm selecting a curve and I'm going to take this point and then I'm going to once again use the Pierce constraint because the Pierce constraint is going to lock that point down wherever that curve is passing through the sketch plane so I'm going to pierce that that that end point of my line to this curve so wherever this is passing through the sketch plane that's where the Pierce takes place now with the Helix it's a little tricky because it's actually passing through it in multiple locations right the Helix is passing through my sketch plane down here it's passing through it over here over here over here so it's usually you know whichever Pierce constraint is closest will be the one that is solved but just keep that in mind if this line was up here I might accidentally actually pierce it to to this location and that's not what I want I want to pierce it down here so for the Pierce we pick the curve pick the point in our current 2D sketch and that allows us to pierce that geometry this is going to become the center line for my thread so I'm going to uh change that geometry I'm going to press q and change that geometry and then I'm going to create the geometry for the thread and the geometry for the thread is going to look something like this I'm going to start out with a line command here going to create a line which is perpendicular to that uh original line that I created uh I'll get in there and just add a perpendicular or I can make a vertical here I'm going to create a line that comes down here and kind of overshoots that original line that I created and then I'm going to put in a a mirror of that geometry so I'll just window select that geometry and Mirror to mirror it across and now that I have created that mirror geometry I'm ready to get in here and start creating some Dimensions so at the peak of that thread I'm going to use a dimension here of 1.2 mm at the base of that thread I'm going to use a dimension here of 4.2 millim you know maybe you don't want to use those Dimensions maybe you want to use an angle instead that's totally fine uh I'm going to create a dimension here from this point to the the base of the thread and it's just going to be a small dimension and the reason that this this overlap exists is because the Helix is running right along the outer face of the the shaft well I want there to be just a little bit of overlap so I don't end up with like a zero thickness error or a gap or any kind of a problem with that thread so that's why we create just a little bit of overlap now if you uh if you wanted to control this Dimension a little bit more accurately what you could consider doing would be to create a a line that goes from this point to here a vertical line and then also creating a line that goes from this point to here a vertical line and then dimensioning between those two points and uh that way your 4.2 would be a little less arbitrary a little bit uh easier to accurately control what the the width is where the thread is touching the shaft of the hex bolt but you know again this is these are nuances that each person is going to decide as they're creating their geometry you know what works best for them the final Dimension I'm going to add here is just going to be the distance that the thread is sticking out from the shaft this might be considered your thread diameter in in traditional mechanical engineering terms and you might create this Dimension to the actual Center Line of the model but in this case I'm just going to be creating this as more of a a theoretical exercise a training exercise so I'm going to make that at 3 millimet and now that I've got that thread profile created I'm ready to sweep that along that Helix let's now take that that sketch and exit that sketch that is our thread profile so sketch the red profile and now we are ready to sweep that thread profile along our path so we jump into the sweep command here in on shape and we're going to say that we're going to sweep This Thread profile along this path and there we go I love the preview that on shape gives us for that that sweep that looks fantastic that's exactly what we were hoping for so let's hit the green check mark and that creates our hex bolt I'm going to switch back here to a shaded view oh yeah that is looking good so we can see here that the the way that we created our Helix was that it kind of overshot the top of the shaft because it went up to that that end point on that layout sketch that we created that uh sketch that we created for the the lead in chamfer there and so what that means is that we now need to use that sketch to remove that excess material and so that's why we created that sketch the way that we did we created it intending to remove this excess material and to leave ourselves with a nice lead in so let's take that sketch so here we can see our sketch for lead in chamfer and let's do a revolve and this is going to be a revolve about this axis here and we are going to be doing a remove and look at that you can already see how nice that looks so I'm going to hit the check mark there and I'm going to hide that sketch so we'll hide the sketch for the lead in chamfer I'm going to do a right Mouse button here on the Helix and choose to hide that the Helix does show up as an item down here in our part Studio down here kind of like its own extra body so if you want to completely get rid of that Helix you can WR Mouse button down here and choose delete and you might just do this just for cleanup just so if somebody else sees it they don't see an extra body in the tree and now we can do some final renaming so I'll rename this one to uh thread sweep I will rename this one here to uh lead in chamfer so uh cut revolve lead in chamfer and then I will rename this feature here to uh Delete helix and there we go that gives us a pretty nice result there I can press p on my keyboard to hide all my planes we can rotate this thing around we can take a look at it and if you're if you're feeling good about this what you can do is a right Mouse button down down here on part one and you can choose export and that's going to allow you to export that as an STL we'll call this hex bolt uh test one and you can export that as an STL send it over to your 3D printer and you two can 3D print one of these hex bolts so I think that's where we're going to stop with our tutorial today if you enjoyed this tutorial be sure to like the video be sure to subscribe and of course be sure to come back for the next video where I'm going to show you how to create the mating hex nut and the match threads so that these two components can actually thread [Music] together

Channel: Onshape

Views: 18,389

Keywords: CAD, Onshape tutorial, Onshape improvements, 3D design, 3D Modeling, Onshape Update, Onshape New Update, Onshape Modeling, 2D Modeling, Onshape features, Onshape Tips and Tricks, Cloud CAD, CAD Data Management, CAD for Mac, onshape, onshape inc, onshape cad, on shape, onshape cloud, onshape browser, browser cad, online cad, cad tutorial, future of cad, solidworks tutorials

Id: S9ZPcZ8osMY

Length: 23min 52sec (1432 seconds)

Published: Sun Feb 18 2024