SOLIDWORKS World: Model Mania 2011

in this video we're going to take a look at the model mania design challenge from 2011 if you're unfamiliar with model mania it's a design challenge held every year at SolidWorks world where attendees are given a drawing like this and they're tasked with creating the part inside a solid works both as quickly and as accurately as possible now if that wasn't enough when they're finished with a part they're given an additional drawing with a series of changes in additional tasks to perform so we're gonna go ahead and dive right in creating this part there's nothing really exceptional about this part I should point out there are several ways you could create this the order in which you could create the features all these things will have an impact on how you make the changes but I'm gonna go ahead and start by drawing on the top plane and I'm gonna create that top profile first now because the two circles are equally spaced from the center of the part this is a great use case for the midpoint line midpoint line was introduced in SolidWorks 2015 and it's a great way to quickly capture the distance from say the center of the origin and you'll notice here that the end points always stay that same distance so this way when I go ahead and I add these circles out to the end of this and they are 240 millimeter diameter circles I'm gonna dimension the first one and notice on the second one I'm gonna leave this alone and then I'm just gonna make it equal to this one then when I go ahead and add the 60 millimeter dimension between the two of them the sketch is fully defined at this point I'm also going to go ahead and add this arc that's going to be tangent to both of these circles so I'm going to do this using a three-point arc and then I'm gonna go back and add a tangency relationship after the fact now because we conveniently have a centerline here I can go ahead and just Muir that arc over to our side and like the circles when an entity is mirrored it always maintains the same geometry on the other side so when I add this dimension here notice it adds it to the other side as well I'm gonna go ahead and trim this up at this point I'm just gonna remove these entities here and I'm gonna go ahead and extrude this the 30 millimeters up so the next thing we're going to go ahead and do here is is there are some Phillips that go on the top of this so I'm gonna go ahead and I'm gonna choose my Philip command here and it's a six millimeter fill it on the outside now an important thing to keep in mind is that fill it is going to be offset the wall thickness of the shell that we're going to create in a minute so let's go ahead and do that now let's enter the three millimeter wall thickness for the shell and notice when I do that how it automatically offsets that geometry now the next thing I want to do is I do want to create a hole through this entire part right here so I'm going to go ahead and do this by sketching on the top plane and what I'm gonna go ahead and do is I'm gonna go ahead and make this concentric to the center of this fill it right here and this is going to be twenty two millimeters here and again I'm gonna just draw the circle and then I'm gonna select the other one and make them equal to one another then I'll just do a cut through all and you'll want to make sure that the direction is appropriate in that case there's also a boss that comes out from the side but notice that it doesn't intersect this now there are a few different ways you could approach this I'm going to show you two different ways you could do this you could draw the circle here it's a 26 millimeter diameter and it's tangent to the top here and it's vertical to the origin in this case and we have this now you could extrude this the two 20 millimeter directions so if I select the second direction let's go ahead and make that 20 as well you'll notice that you end up with this material on the inside of this and you'll notice I didn't do this before the shell and that's because the wall thickness is different that doesn't mean you can't use that though let's take a look when I show this notice that it will hollow that out but what we can do in this case is we could do the math the outside diameter is 26 the inside is 16 that's a difference of 10 divided by tooth that's 5 so in the shell there is an option to specify a different wall thickness and in this case we could select these two faces and they will have a different wall thickness and in fact we could in that shell feature itself select the two end faces as well and automatically create those holes with that to save us a few extra steps so kind of a unique way looking at doing that yes you could have created that as a boss and then as a cut and one of the other ways you could have done it would have been to extrude it from the outside into the part as well but there you have it we kind of have our part the last thing we need to do is specify the material to 1020 aisi is in my favorites list remember when you set the material on a part you're not only changing the physical appearance of the part but you're also changing the physical properties of the part so this will impact things such as the weight or the strength of the part when uh if you ever decide to do a simulation on this which we happen to need to do in Phase two speaking of let's go ahead and let's look at the phase two drawing the phase through two drawing shows two significant changes to the part the first is is we're going to add this arc across the top the next is we're going to add these bosses now this can get tricky so let's go ahead and let's start with the arc the best place to do this is the arc really happens before these Phillips were ever created here so we're going to go ahead and we're going to change this in this case and we're going to just go ahead and add a cut now this cut will have some bigger implications on this part than what we may anticipate I'll show you what we mean in a minute let's go ahead and quickly add the dimensions to this the other thing to notice when you add an arc like this is to make sure that it's centered on the part you could go zoom out find the center and make this vertical to the origin but keep in mind another quicker way sometimes is just to make these two endpoints horizontal to one another now I want to cut with this geometry and it's not a closed sketch notice when you choose to cut with a single line and I for instance choose through all in both directions it actually almost creates a surface cut and it just allows you to choose which side to remove so I could choose everything to the bottom or everything to the top in this case and when I do that it removes this but when I did that I completely remove the top face and all the original edges of that face so this is going to get a little bit tricky because most of our features are going to have failures that take place for example these Phillips can't find that edge that I selected when I choose edit it notice that there's a missing face that's okay we'll just select the new face here and reapply that fill it we go ahead and we create this extrusion likewise the tangency is going to be missing here to that original edge and we can see this when we select on this arc that's okay I'm just gonna go ahead and remove this and I'm gonna reapply the tangent relationship there now when I scroll down you'll see that the shell does update itself with no issues there so that was okay the cut that we created it in the part there is a warning here one of the things that's happened with this cut is that we had made this center to the original Philips while we changed those Philips so in this case I'm gonna go ahead and select this and notice this red dot I'm just gonna drag this out to this arc on the outside and we'll reattach this or maybe not maybe I'll just click and drag this and we'll just do this the easy way I'm just gonna reattach this in this case and want to do this to both of these arcs and then that will update and then finally in those Philips but remember there is this other new feature these bosses that go into the part now there's a few different ways of approaching this the first one is is you could always add this after the fact I'm gonna go ahead and just draw these on my top plane and I'm gonna draw the diameters here that we need to work with these are going to be 28 millimeters in diameter and I'm gonna draw two of these also here same thing like we did before we're going to go ahead and make those equal to one another now when I choose to extrude this we all we don't want to remove this inside material so I'll use convert entities to capture those edges and copy that geometry down now you may be looking at this going wow they're in the wrong place well actually when you choose to do an extrusion you can choose an offset option and in this case we're given a dimension value of 30 millimeters and then all I have to do is reverse the direction and choose up the body to join this together let's flip that direction around again and we get what we need - the Phillips that need to be added there was another way I mentioned we could have approached this and we actually could have changed the way we did this altogether I'm gonna I had and I'm gonna delete that sketch as well one of the things SolidWorks allows you to do is create the features in a different order than the actual sketch entities themselves so here's what I'm gonna do I'm gonna roll back to this feature here we're going to create a sketch on the top of this part and I'm gonna go ahead and I'm gonna draw the 28 millimeter diameter circle here and the 22 millimeter diameter circle here we just want to do the same thing on the other side remember Mir might be another way you want to accomplish this I'm gonna go ahead and just do this by drawing the geometry and then adding the actual relationships between the two so it created my sketch but notice I'm not going to do anything with it right now I'm gonna go ahead and just continue to allow the part to rebuild as normal and right now is a pretty good spot to do this I could do this after the fill it even but I'm gonna save that for later and I'll show you why in a minute what we can do here is we can take a sketch that exists earlier in our tree and we can go ahead and choose to extrude this and then choose an up to next in condition in this case notice the whole doesn't go through the part we can again reuse this sketch later if we want and we can choose to do a cut and with selected contours we could select just the whole piece in the center and choose a through all end condition in this case so that's another completely different way you can do that and something we haven't shown before and that's that you can create a sketch anytime you want and then act with it or use it later on in the feature manager tree so I'm gonna roll this back for it and the reason I saved the fill for the end is the fill that actually goes on the outside here is the same radius so we'll just go ahead and apply that there as opposed to creating an additional Phillip so we created our part there's one additional step we need to do it and that's we have to perform a simulation on this we look at the drawing it gives us all the information we need we need to fix the two faces that are kind of in that center cylinder and then we need to apply a low to the tops of those new bosses that we just added so in SolidWorks we could do this with SolidWorks Simulation or SolidWorks Simulation Express Express is great because it's inside at every version of SolidWorks in a kind of walks you through the process for example the first thing we need to do is add those fixed faces we do this by adding a fixture and simply choosing those faces fixed basically means that this geometry isn't going to move this is where we're going to hold the part down we could choose to add more fixtures but we're going to go ahead and move on to adding a force in this case and here we want to apply a force to these two faces on the top of this part now keep in mind when we do this we'll want to be careful of the option here we want to apply a 3000 Newton load but do we want to apply it to each item or overall and in this case we want to apply 3,000 Newton's to each face the next part of the step we've actually already completed completed when we specify the material earlier on if we hadn't we could define the material now by clicking the change material button I'm going to go ahead and click Next and then choose to run the simulation it takes our works a few seconds to give us the results that we're looking for and after it solves it it gives us a preview of how those forces act on that part in an exaggerated fashion here you can see it's exaggerated by 200 19.7 times this is just to confirm is this what we anticipated yes it is so let's continue and look at the actual results when we look at the results one of the first things we see is the factor of safety here it's showing us that what we're seeing is a factor safety below one but it also specifies the lowest factor of safety in the design is 2.76 to 1/9 you could probably just round that to 2.76 to be safe one of the nice things about this however is it for example we wanted to see a factor safety below 4 this would help us understand where the weakest parts in our design are granted plenty strong for the forces that we're applying to it likewise we can also if we wanted calculate the deformation of the part by showing the displacement and in this case we can see the maximum and the minimum displacement on this part so SolidWorks Simulation gives us some great results and there you have it the completion of the model mania design challenge from 2011 if you're interested in learning more about model mania or Moore's specifically SolidWorks world it's rapidly approaching I recommend visiting the link below this video or in the blog post for this is hosted

Channel: SOLIDWORKS

Views: 29,160

Keywords: solidworks, 3D CAD, Dassault Systemes, mechanical CAD, mechanical engineering

Id: nq2P4OBXN3s

Length: 13min 30sec (810 seconds)

Published: Fri Jan 16 2015