SOLIDWORKS World: Model Mania 2008

in this video we're going to take a look at the model mania design challenge from 2008 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 in SolidWorks both as quickly and as accurately as possible now if that wasn't enough when they're finished with the part they'll be given a second drawing with a series of changes and in some cases such as this year in additional tasks to perform so we're going to create this part and it's actually fairly simple the real challenge comes in phase two we will look at simulation for this however though I am going to highlight the use of contour selections this is a great example where the entire front view of this part can really be drawn in one sketch and in fact it's quite useful because a lot of the geometry is contingent upon one another so let's go into SolidWorks and start doing that as I go ahead and create this geometry again keep in mind we will be using contour selection so we can bypass some of the trimming steps that might be necessary so in this case I'll create the cylinder diameter and the bore through it and then for the keyway I'm simply going to go ahead and I'll type that width and we'll drop this on here I'm going to locate this on the center by simply adding a midpoint relationship to the center for the length of it I'll dimension to the end of the keyway and while holding my shift key snap to the outside tangency of that circle now you could trim this up in some cases you'll want to do this but when you do that notice what happens it makes the keyway go under defined we can go ahead and add that dimension back that we removed the six but it's still not located on the center well this key way was centered keep in mind these two lines would be equal lengths likewise another way to capture that would be to make these two endpoints vertical to one another finally you can go ahead and also add a centerline to the midpoint of this line and make the center line horizontal there is one last way you can do this however without any construction geometry you can right mouse click on this line and choose to select its midpoint and then while holding the control key select the origin and make them horizontal to one another so as you can see there's several ways to accomplish that task and that's a very common task inside of SolidWorks I'm going to go ahead and start on the slot on the outside the slot tool inside of SolidWorks is perfect for this and in fact the center of this slotted arc happens to be right in the center of this part so we'll use a center point slot I'm gonna go ahead and drag this out and then just drag my slot up and then drag out the size you'll notice I had add dimensions enabled so a lot of the dimensions have been included but notice this fifteen point five nine that's not actually how we're going to call this out instead we're going to define this by a radius value so I'll just delete that and add a new dimension well update these values to their correct numbers and in this case the angle will be 30 degrees and you'll notice that this part this slot is still free to move around in the part well there's actually two here and what we're going to do is offset these now I could do the calculation and determine that the offset in this case will in fact be six millimeters and it'll add that dimension automatically but that's not how it's called out on the drawing so I'm gonna delete that and again I'm going to add a radius value the reason is is what if one of these ever had to change I don't want to have to go back through and continually update that offset value these were defined individually from one another so that's how I'm going to dimension them the next thing we want to do is capture this line on the bottom which is also tangent to the bottom of this arc will just window select those and make them tangent to one another and then finally there's an arc here on the top for this we're going to go ahead and use a three-point arc and attach it to the two pieces of geometry now you'll notice we will want to go in after the fact and make these tangent to one another to make sure that they they are in fact the tangent and then we'll go ahead and add this radius value of 175 now the next thing we want to do is create this pocket in the middle here and offset this is another great example of where we'd use it we will want to reverse the direction to go to the inside but notice I'm going to leave off the circle the reason I'm going to do that is I'm going to show another way to dimension two arcs so I'm going to drag these back and I'm going to create this tangent arc that goes from the bottom here to this line here now you'll notice when I go to create it they're obviously not tangent well SolidWorks actually presents you with the ability to I had a relationship between the entity you just sketched in the entity you attached it to in this case tangent to one another so that'll save you a few steps and not having to go back and add it later well we mentioned previously the ability to hold down the shift-key to dimension to the outside of an arc well it actually works from the inside to the inside as well in that case I just simply held down shift while I selected both of those arcs to capture that six millimeter offset between them the last thing I'm going to go ahead and do is trim off some of these extra pieces of geometry just to clean the sketch up a bit so we have this sketch that represents the entire front profile I want to now start creating geometry from this so I'm going to go ahead and do this I'm going to choose extrusion and because there's multiple profiles in the sketch SolidWorks automatically enables selected contours for the first feature I'm gonna just go ahead and select the cylindrical feature on the front and enter the 30 millimeter depth for it now you'll notice the sketch goes away it hides itself automatically but we can go back into the feature manager tree and just resit I'm then going to go ahead and choose extrusion again and in this case this extrusion is 16 millimeters wide I will go in and use the offset tool though to capture that 2 millimeter offset off from that back face we've talked about that in previous videos and we're going to do the same thing on this internal region here in this case we're going to make it 14 millimeters and we're going to offset this 3 we're just going to add up the 2 millimeter from the the second feature we created and the additional 1 millimeter that's needed so we've got the bulk of the geometry all that's left is to create a series of Philips and if you've watched the previous videos in this series you'll immediately know why I select faces because it allows me to capture a lot of geometry all at once but in this case we are going to do these Philips in two steps you'll notice that I create the Philips around the rib first and then the second set and that's just to ensure that they're able to solve the way that we want them to look finally there are a series of four millimeter Philips on these front edges and because they're only applied to those edges that's what I'm going to select so we've created the part rather rapidly but if you look at the drawing there's one other thing that's specified but the material has to be applied to this part well let's go ahead and do this applying the material in SolidWorks is actually pretty easy you simply right click on the materials node in the feature manager tree and you can select one from your favorites in the aisi 1020 that specified is here but let's look at the Edit materials library it's a big library in SolidWorks but it does more than just say what the material is you'll notice that it also captures all the physical properties of the part including things such as the yield strength and the tensile strength which we'll be using in a moment to perform simulation additionally it's also going to change the appearance of the part to look like that material and it will automatically define the crosshatch used in a drawing so a lot of things are set when you set the material not just the name or just the color but a lot of different properties so as we pressed OK you can see that the part look does indeed look the way it was supposed to so let's go ahead and save this I'm gonna overwrite a previous example that I did of this and we're going to go ahead and flip the phase two now when we look at the phase two drawing we can see that the part itself doesn't change a whole lot but there are some very unique notes at the bottom we're going to be working with configurations to create a second version of this part then with these two versions we're going to perform a simulation in our example using simulation Express to analyze the two configurations in determine which one is strongest so let's start by going back into SolidWorks and making the new configuration we're going to go to the configuration manager and simply right click and choose to add a new one and give it a name in this case we're going to go ahead and call this phase 2 and simply press ENTER we want to keep the appearance that we did before so I'll choose no there and we need now need to make some changes so I'm gonna double click on this feature and one of the first changes is these web the thickness of this change so for example this one changes from 6 to 14 now you might think just update the value and hit enter and this new configurations updated but be careful when you do that you'll notice that I've actually changed it in both configurations of the part when you're changing two engines for the first time you'll want to be aware of the pulldown to the right of the dimension this pulldown is where you can specify which configurations have this dimension and by default they're always set to all configurations so we're going to change this to this configuration and reset our default configuration now notice when I toggle between the two there's a noticeable difference let's go ahead and do that to a few of the other dimensions on this in this case we're going to change this 14 millimeters over here to be eight millimeters and the offset value from the back we're going to go ahead and again only in this configuration change it to six now when we rebuild the part you can see it's drastically different from the first configuration so within one file we have two slightly different versions of the same part but now comes the interesting piece we need to perform an analysis on this part to determine which is strongest and capture the factor of safety for this we're going to go ahead and use SolidWorks Simulation Express which is available in every version of SolidWorks you may have to register it if it's the first time you've used it but it's free of charged anybody using SolidWorks it'll guide you through the process step by step but we're going to go rather quickly and just show how to do this the first thing we need to do is add a fixture where will the part become strained and in this case we're going to choose this bore going through the part then we'll go ahead and apply that by pressing ok and choose next we could have added more if we wanted to next thing we want to do is add a force and in this case we're going to apply a force of 400 Newton's to the face selected here the next step we'll see is where we can choose our material now we already specified this so notice that simulation automatic automatically captured the Youngs modulus and the yield strength of the part so we can bypass the step and go right to running the simulation this will go rather quickly and when it's finished SolidWorks will give you a preview of how those forces will act on the part if it's unexpected results you can go back and change how you entered the parameters but in this case it looks good so when we look at the results immediately we can that the factor of safety for phase two is two point eight three eight three now one of the other things we might be interested in is looking at the von Mises stresses of this part here we can kind of see how the stresses are actually acting and where most of the load has been applied to the part and we can see it it's kind of down in this area here likewise if we go back to the factor of safety we can actually say show me anywhere where that factor of safety falls below three in this case and we can see that the weakest area of that part is about right there so that was really that was pretty easy to solve but we need to compare this to the other version so let's go ahead and say done viewing results and I'm we could generate a report but I'm simply going to close this for right now and save my settings all that's needed to check the results on the default configuration we made originally is to activate it restart simulation Express and we literally can just skip through these steps because all the properties and specification we've defined are exactly the same we just need to rerun the results so again very quickly SolidWorks shows us what it's looking like we'll say yes and continue show me the results and we can see that this part is significantly stronger with a factor safety of four point four three six four so in this case if we were to look for anything below a factor of safety of three nothing shows up again you could see the von Mises stresses and we can see that they've moved further down that web as well and this is because the way we've designed the web we've changed the cross section to better handle the way the loads been applied to this part so we're done with that as you can see we went through this model mania design contest and not only made the part rather quickly we were able to see how strong it was fairly rapidly as well and compared the two different results to one another if you'd like to learn more about model mania or SolidWorks world I highly encourage you to visit the links in the video and below the video or on the blog page depending on where you're watching this

Channel: SOLIDWORKS

Views: 38,440

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

Id: bpREvDAYc3w

Length: 13min 11sec (791 seconds)

Published: Fri Dec 26 2014