SOLIDWORKS World: Model Mania 2002

welcome to another video where we're going to take a look at the model mania design challenge from SolidWorks world 2002 if you're unfamiliar with model mania it's a design challenge held every year at SolidWorks world where you're given a drawing similar to this in your tasks with creating this part in SolidWorks both as fast and as accurately as possible and if that wasn't challenging enough once you're done with this part you're given a second drawing where you have to make a variety of changes to the part now we're going to hold off on looking at the second drawing until we get to that point there's some surprises there but let's go ahead and look at how we might tackle this one of the first things you'll notice is that this part is symmetrical both about section a a as shown in the top view so from left to right but also from top to bottom as we can see both in the section view itself and the front view now also unique is the direction of the two holes in this part the main 70 millimeter bore in this part appears in the front or right hand side view where the other bore of this part comes down from the top and yet we have to capture that relationship so let's go into SolidWorks and look at how we'll tackle this the first thing I want to do is start by capturing most of that profile keeping in mind that this is a a mirrored part or a symmetric part I'm going to start on my right plane and I'm going to start with one of the easiest features this big 70 millimeter diameter circle and while I'm at it I'm going to go ahead and capture that seven millimeter offset right now as well the next thing I know is there is a line that comes off from this circle that's tangent if you drag a line out from a circle while maintaining tangency you'll notice that that line will preserve that I'm going to go ahead and just drop this out here and then we'll go ahead and kind of draw the rest of this profile I'm going to kind of snap out here and out here now you've seen if you've watched the previous videos I like to use contour selection and we'll go ahead and do that again here I'm going to go ahead and just trim these arcs now I could go ahead and remove all that just like so as well but keep in mind you could have left this there's no reason you have to trim this now the next thing I need to do is I need to capture this angle that's 15 millimeters let's drag this in because I know that that pretty long so we'll set that to 15 and now we have to determine where the end of this is now the end of this is if we go back to the drawing is determined by the diameter of the bore on the top but also the seven millimeter offset to the outside so if we come back how do we capture that well there's a variety of ways you could do this you could do this doing some math so for example you could put a construction line in here and you could say well it's a hundred millimeters out to the center of this circle and then you know that well from here to here it's going to be half the diameter so we could type in 15 divided by two plus seven millimeters and we could get it that way but what happens at the diameter of the circle changes or the offset you'll have to go back in here and recalculate all that so this isn't a very efficient way of doing this so let's go ahead and delete this geometry and think of another way even though the circle is drawn from the top view there's no reason we can't use a circle and capture this information here in an earlier sketch so what I'm going to do is I'm going to do just that I'm going to dimension that 15 millimeter diameter circle 100 millimeters off from the primary bore and then what I'm going to do is I'm going to dimension from the end of the part and while holding the shift key snap to the tangency of that circle and specify that 7 millimeter dimension and now that the sketch is all black we know that it's fully defined we're not going to use this circle when we go to extrude this but we will reference it later and in fact I'm going to do a little trick here to save me some time later on and I'm going to drop a point on the quadrant of that circle you'll see in a minute where we go ahead and use that I'm going to go ahead and close this sketch and I'm going to choose to extrude it and because SolidWorks doesn't give us a preview you can also see by looking at its cursor it's looking for contours for us to use so I'm going to go ahead and choose the main contour here if we drag this out to the 70 millimeters it's supposed to be you can see that we get this arc from that circle well this is the real beauty of contour selection I can just select that circle and fill that in now I did choose to extrude the 770 millimeters but it is a symmetric part so it probably makes sense to maintain a midpoint relationship to keep all that geometry in the middle that will be especially important in just a minute here as you'll see so we've got this main body of our profile done the next thing I want to do is I want to look at bringing in those sides out to that tangency so a good place to do this we're going to draw a sketch on our top plane I'm going to draw a line from the vertex up here I'm going to bring it down and I'm going to use this trick that's inside of SolidWorks where well you're in the line tool if you go back to the endpoint of a line it'll actually snap and switch to an arc will draw another tangent line and you can see I didn't get it quite in the center that's okay I'm just going to drop this here and then we'll just drag that and snap that into place now I know that this arc needs to be tangent to the end here but I need to somehow calculate the diameter of this now again we could do a bunch of math but what we're going to do is we're going to use that geometry we created in that first sketch in the feature manager tree you can click on any sketch and choose to show it once that's done you'll notice now I can take the center point of this arc and holding my control key select the center point of this arc and make those coincident to one another if you look at the top view you can see that what we did is we captured the center point of that circle in that very first sketch and we're reusing it here the next thing I'm going to do is I want to cut this out now you'll notice something unique about this sketch it's not closed in any way that's okay SolidWorks will allow you to use this when you go to the using ik an extruded cut with an open profile SolidWorks presents you with a few new options one of them is this little arrow with the flip side to cut and if we change this to a through all end condition what SolidWorks is actually going to do is remove all the material on the outside of that sketch geometry so we we could have gone in and drawn the rest of that geometry but there was no reason to now I'm going to reference that sketch again this time we're going to draw the actual cut that goes through here and you'll see how convenient that point we created is going to be I'm actually going to snap from the center of the circle to that point we created on that vertex and then all I need to do is go ahead and do a cut extrude I'm going to switch the direction and change that to a through all end condition now I'm done with that sketch so I can go ahead and hide it now and then easily we've created the top half of our part now if we go back to the drawing the next significant feature is going to be this pocket and you'll notice it's a seven millimeter offset from all the surfaces around it so let's go back here to the SolidWorks part and I'm going to show you two different ways you can tackle this the first way is actually using some surface geometry if I go up to my services tab on the command manager we can create an offset surface of seven millimeters and I'm going to offset this bottom face in this face here and I'm going to choose to reverse their direction to the inside now you might not be able to see those but if you'll notice a new folder has appeared in the property or in the feature manager containing this new surface body there you can get an outline of it let me show you how we're going to use this I'm going to start a sketch on the top plane and what we want to do is we want to offset several different pieces of geometry again seven millimeters so I'm going to offset that edge let's do that again to offset this edge and then one more time to offset this circle here finally I'm going to go ahead and clean this up by using power trim and we're just going to get rid of some of that excess material and in this case we are going to close the sketch off now you're probably wondering how are you going to use a sketch down here on the top surface to cut something up here this is another great feature inside of SolidWorks when you cut you can actually go in and choose to choose to do the cut from an offset now the diameter of this arc could change so we're just going to set this way out there in space like 100 millimeters and notice that the cut actually starts up here and then for the end condition we're going to change this to an up to surface cut condition and I'm going to pick that right out of the graphics area there and there we have it we've gone ahead and created that cut now at this point you could go ahead and you could you don't really need this surface anymore so you can either choose to hide it or I prefer if I really don't need it to just delete the surface out of the part altogether we just needed that for some reference geometry now the next thing we have to consider is all this draft on this part and I actually made a mistake intentionally here the first piece of draft were going to run into is along the outside of the part this needs to draft seven millimeters in and a neutral plane draft is a great way to accomplish this I could pick this face or the top plane I always like to use the system planes whenever possible and we just select the faces that we want to draft and when I right-click SolidWorks drafts those in but look what's happen the offset of our material wasn't right in this case this is actually very easily corrected you'll notice if I go over to the feature manager tree if the draft had happened before that cut well the cut would have been offset from the proper seven millimeter so you can see it's really easy to quickly manipulate the feature manager tree to make different changes there's no reason to go back and undo what we've already done now the second draft needs to start from here and go inwards so how do we capture that if we did a parting or if we did a neutral plane draft from the surface it would make this part way too thin this is where parting line really comes in and you heard me accidentally mention that parting line draft works in a similar manner in that you select a pole direction but instead of faces we're going to choose edges to draft from now I'm going to grab this edge and you'll notice this arrow that tells me it's going to draft this face you can change that but we don't want to draft that outside face we want to keep that down so let's go ahead and grab all these faces and we'll make sure that those arrows are all going in the right direction they're a little hard to see but when I hit okay SolidWorks just reverses the draft we didn't have to do the math and subtract seven and then another seven it just took care of it for us and that's it we've got that the next thing we could do is add some Phillips but I want to go back I mentioned there's a couple ways we could have created that pocket I did this with some surfacing I'm going to go ahead and delete this surface and we're going to go ahead and get rid of several of these other features here I'm not going to create a cut in this manner or this draft for that manner either so here we've we've rolled back we still have the draft on the outside of our part other way we could have tackled this if we know that the wall thickness is always going to stay seven millimeters we could have used a shell feature and by selecting this top face it shells and hollows that out to that phase now notice in this example because of the order of the draft these faces are tilted inwards they're offset from that outside face well that parting line draft actually works really well here and that all we have to do is specify that draft angle and SolidWorks will fix that orientation automatically for us now you seal I got that error that means that one of these edges is potentially going in the wrong way my errors disappears so we're going to go ahead there we go see how these arrows are pointing to the outside we need to correct that so I'm going to grab those edges and make sure that those are both pointing down and now when I press okay we get the same results as before so there you have it two different ways to look at a very similar problem shells probably the easiest but it requires that all the offsets always remain 7 the other way we did it we could change any one of them now the next thing we want to do is there are some fill it's on this part if we go back to the drawing you can see there's a bunch of fill it's on that inside pocket so we come back here how are we going to do this well if you've watched any of the previous videos you've probably seen that selecting faces provides a very powerful way to quickly grab a lot of edges with three faces I've grabbed all those edges that easily now I could create the Filat that goes around the outside but I do want to make sure that it blends to the second half so let's get to look at mirroring this so I'm going to go ahead and I'm going to choose the mirror feature and for the mirror face again we're going to use that top plane we've created everything off from it and we're going to use the bodies to mirror option and I'm going to grab the main body of this part and ensure that merge solid solids is checked in press ok and there you have the part with the last thing we need to be those additional fill 'its now I've talked about selecting faces here's an example where by selecting a face we get a lot more than we're bargaining for so here's an example where a face isn't necessarily a good choice but maybe an edge and you'll notice that the tangent propagation follows all the way around to the part to about here and that's because there's no tangency across that sharp vertex so we'll just go ahead and grab that additional edge on the bottom and you can see that it puts those together right there where they need to be so we have our part done now here's where the real challenge comes in we're given an additional drawing and in normal model manias your tasks with creating a changing several dimensions on the part in this example we've actually been tasked with creating several configurations of this part and this is typical to what you would see in a parts or a suppliers ordering catalog you see a table with several different dimensions that you could order the part in so we want to be able to capture the same type of thing so let's go into SolidWorks and figure out the best way to do this we're going to do this obviously using configurations but there's a really clever way we can accomplish this using something called a design table a design table is a great way inside of SolidWorks to quickly build up a variety of configurations and this can be accessed by going to insert tables design table now I'm going to go ahead and choose the auto create option because I want to kind of go through the process of selecting some information and I'm going to simply press ok SolidWorks then launches Microsoft Excel into the graphic serie and it's asking us which dimensions do we want to include well to be honest with you these names don't mean a whole lot to me so I'm going to go ahead and just hit OK at this point and kind of skip that process what we want to do is we want to capture some very specific dimensions so I'm going to just pick on this face and you'll notice all the dimensions appear this is because I have something called instant 3d enabled if we go back to the drawing we can see that we need the large diameter hole the distance between centers and the angle of that slope so let's go back to SolidWorks all I have to do is pick that diameter the distance between centers which we have in this first sketch and the angle of this slope that easily we were able to do this and then type in the other value so we have 60 125 and 10 oops I got a tab through this 60 125 and ten fifty a hundred and fifty and seven and forty a hundred and seventy five and five we do need to give these names as well and the names are B C and D let's not let Microsoft Excel automatically fill this in and this is the default configuration it actually should have filled the name in here we'll go ahead and just exit out of here and you'll see that solid works will tell us that it's created these configurations automatically for us so there we go we've got the default configuration in configurations B C in D using that design table made that whole process quite easy for us to do so there you have it the design challenge from model mania 2002 with a unique twist where we're not making one change in phase two but instead we had to make three completely unique parts I hope you enjoyed this and if you have any questions or want to post your times leave them in the comments below or use the hashtag sww 15

Channel: SOLIDWORKS

Views: 57,298

Keywords: solidworks, 3D CAD, Dassault Systemes, mechanical CAD, mechanical engineering, SOLIDWORKS World, Model Mania, Tips & Tricks

Id: p4aZb8AkZT8

Length: 16min 48sec (1008 seconds)

Published: Fri Nov 14 2014