Designing Consumer Products Using SolidWorks

hi everybody it's Jamie here from cat TEKsystems I'm just going to spend the next 30 minutes or so going through a demonstration that I've prepared just to show how SolidWorks can be used within the consumer product industry so any kind of product designers out there wanting to create kind of more organic shapes like the remote-control there that you see on the left hand side I'm going to show you some of the tools that you can use in SolidWorks to help you achieve that I break it into four sections today the first section is looking at how we can actually create some initial sketches and so that might be using kind of hand-drawn sketches that we might have drawn on a bit of paper or something that's going to take about ten minutes to look at then we're going to spend the next ten minutes after that looking at how we can create basic surfaces using those sketches that we've already created then we're going to spend five minutes looking at how SolidWorks has got some lovely features for adding kind of assembly features like maybe snapping grooves maybe snap hooks mounting bosses things like that we've got a great automated tool in SolidWorks to help us achieve some of those features really really quickly I'm going to spend the last five minutes looking at how we can create photorealistic images like the one that you see there on the left hand side so the first section is looking at initial sketching I always start my designs generally speaking with a bit of paper and I start sketching out what it might look like so on the left hand side there you just see a quick sketch that I've created of a suggested TV remote control and all I'm going to do in SolidWorks is actually take my hand sketch I'm going to scan it in I've actually created these already and I'm going to copy this into SolidWorks pick out the outlines so picking out the major kind of outlines there and then extracting them into SolidWorks then we can use those to create some of the surfacing so let's take a look at how we can actually create our initial sketches so every in SolidWorks I'm just going to start a brand new document and then on my front plane I'm actually just going to drop a sketch now this time I'm just going to insert a sketch picture so you can see here is a collection of the pictures that I've got my side sketch is going to go on to this front plane so I'm just going to open that up and then drop it into place now as you see here this is my origin this kind of red-crab that you see there and I'm I want my origin to be on this very corner point here of the sketch so I'm just going to drag it over something like that then just going to take this blue line and this is going to help me to scale the picture so I'm just going to drag that to the end point there I'm going to drag this out to approximately the end of my sketch something like that and then SolidWorks is prompting me to ask me how long that line is so I'm going to tell it is 185 which matches up with my sketch and it's automatically scaled my picture then also I'm just going to change the transparency of this as well just so we can be a bit clearer when I start sketching over it what I'm actually doing so again I can just hone this down just to get it into place so something like that and I'm happy with that so what I'm going to do is I'm going to rename it because SolidWorks is called this sketch one which doesn't really make too much sense to anybody so I'm just going to rename this side sketch so then what I'm going to do on my front plane again I'm just going to pick out some of those edges now using a three-point arc I'm just going to specify that there's my first point my second point is over here somewhere and then I'm just going to pick out that arc something like that now I've sketched that kind of freehand and that's the nice thing about SolidWorks is we can kind of do this stuff freehand but I now want to constrain it or actually dimension it so first of all I'm just going to tell SolidWorks these two points are horizontally aligned I'm also going to tell the SolidWorks that there is a distance involved and that's the hundred eighty-five if you remember so up there and it's going to specify that that arc has a total horizontal length of 185 and also I can mark out the radius as well so I'm going to go for 650ml radius it's gone black the sketch has gone black and down here it's telling me it's fully defined as well and that's really where I want to be with sketches in SolidWorks so then I'm just going to okay it then I'm going to drop another sketch onto this front plane and this time I'm going to pick out this suggestion of a split line so again using a three-point arc I'm going to go ahead and do that so doing this kind of haphazardly to start with all kind of quite quickly to start with I'm just going to tell SolidWorks a couple of things about this for example there's a vertical distance here around about 6 there's a vertical distance here of about 10 I'm just going to tell SolidWorks that these two points I want to be vertically aligned just to make sure that they fall in the same vertical orientation same with this one over here as well so just picking out these two points I can build a vertical relation between those and again I'm just going to pick out a radius for this so again I might go for about 650 and my sketch is gone black so I'm just going to okay that one the final sketch we want to create is the one that's going to follow this lovely sweeping edge down the bottom here so get on to that front plane I'm going to drop a sketch I'm going to use something called a style spline this is a new tool in 2014 as well and it just helps me to create splines that the curvature is really really nice so first of all I'm just going to draw it so you'll notice here as well when I start drawing I'm not actually drawing the spline as you might do with other packages I'm actually drawing what we call the control polygon and this basically helps me to actually control it without picking on the spline itself I can I can actually control it better using this control polygon now the reason we do that is if I just show what we have is called curvature combs and that basically you can see here that it gives me like a comb on the top and this is showing me the curvature now what we're after is something that sweeps nicely from negative 3 to positive and into negative again which is what we've got here and you can see that because it's nice and smooth this is the reason that we use the style spline as opposed to just a regular spline tool so first of all I'm just going to tell SolidWorks I can actually hide off those curvature combs now I'm just going to tell SolidWorks at these two edges or these two lines of my control polygon are vertical that just means that not horizontal as I just said there are vertical that just means that when they flow up into this edge here it's going to be completely tangent so I'm forcing tangency here to make sure that it's going to sweep into the any other surfaces that go ahead with it it's going to sweep into it nice and tan gently so you can see here I'm just tweaking this control polygon just to shape this particular edge and you can see here that we can get it really quite tight something like that so I'm kind of happy with that and I'm just going to go get it now on this top edge here I want to create a center plane running right through the center so if I just go back over to this sketch I'm just going to drop a control point on it so the point is going to be right in the center which SolidWorks identifies for me and also want to create a plane that is in line with this kind of narrowest part down here and the thickest part down here somewhere so around about here somewhere I want to create a point vertically above it and the aim for the narrowest part which is roundabout kind of here somewhere make a bit more sense when I start drawing it what I've actually put these points in here but this mid point here I'm going to use straight away so first of all I'm just going to hide off my side sketch because I don't really need to see that anymore so I'm left with my sketches from my side view so next I want to do is to take my my right plane which is currently at the end here where my origin was I want to copy this right plane to this midpoint here so to do that I'm just holding my control key down I'm just dragging one of those kind of pimples in the top corners here and then I'm going to pick another reference which is going to be my point and you can see here then that it creates me a center plane right in the middle over there I'm just going to rename that as well so I always like to name my planes and my features over here just that it makes a bit more sense so I'm going to call this mid plane and then onto here I'm actually going to create a sketch first of all I'm going to insert my sketch picture so this is looking down at the end of it now and I'm going to bring this in so again the first thing I need to do is just to give SolidWorks an idea of scale of this sketch picture so using this line this blue line I can just drag it out roughly where I want it sort of works and prompts me to say how big is that line I'm going to say it's around about 60 mil and I'm also just going to change the transparency of this as well so over here I can change the transparency just to make it a bit more transparent and then I can move this and where I'm after is basically this top point you see here so this top point here is where I'm trying to locate the top arc of my image so something like about there I think and then again I'm just going to rename that particular sketch with my picture on it just so that I can hide it off at a later stage so I'm going to call this n sketch okay so next I want to do is to actually draw on to that plane again and pick out this very very top edge that you see here this top arc so again I'm going to use a three-point arc to do this I'm just going to pick out a corner and another corner just going to draw it kind of quite haphazardly to start with just going to pick out this point here that you see I want to be in the middle of my particular arc something like that and then I'm just going to drag this to look a bit more sensible so all I'm just going to specify these two end points need to be horizontally aligned you can see now that it starts to behave a bit more symmetrically then I'm just going to specify a distance so between here and here you can see my image here is telling me it's around about 60 mil and then also I'm going to pick out a radius as well so I'm going to say that's got a radius of a hundred so I'd use some nice hole numbers for this so that's that particular part done I like actually hide off that sketch as well now my own sketch just to make it a bit clearer last thing I need to do is to pick out the top shape as well so onto my top plane I'm just going to go ahead and drop a sketch picture of my top and you can see it's right there and again all I need to do is to set tell SolidWorks or give SolidWorks an idea of scale so I'm just going to say that from here down to this bottom is around about 185 also going to change the transparency just so that it's a bit easier to see what I'm doing and then I'm just going to get down to position so again I'm just going to drop this mid point here on my origin something like about that and then what I can do is obviously rename it so that it makes a bit more sense so over here I can just call this top sketch and then onto that plane I'm actually going to go ahead and pick out this outline so the first thing I'm going to do is just to use some mirroring technique sort of center line just to draw a center line from here to here that just means that I only really have to draw kind of half of it but I'm actually going to pick out these points first so again using a three-point arc you see I'm drawing this really quickly I always describe this as kind of sketching with a pencil something like that and then just going to tell SolidWorks that these two points here are vertically aligned so this is now me just kind of honing my sketch down or constraining it in in sensible way so I'm just going to say that those are vertically aligned as well just going to say that the end point and my arc I want to be in the middle I'm just going to specify I want my mid line to be that 185 millimeters I'm also going to tell the SolidWorks over here that exactly the same so that's a midpoint that I want to have there and again I'm just going to that Ark something like that and I can start to shape this to look more like my sketch then I'm just going to start adding some dimensions so first of all from here to here we're going to go for about say 24 something like that we'll go for radius here maybe a hundred radius on this back arc of say 50 again you can see that it's just allowing me to control it a bit better now next I'd like to do is to pick out the highest point you can see if I hover over this line I've got a yellow point in the middle or a square kind of point and that is basically telling me the midpoint but also I've got this rhombus shaped point and this is the highest point of that arc so I'm just going to dimension from there so if I just drop a point down there first of all on the highest point and then I can dimension from there down to my center line and that's going to be 30 which is half of my 60 obviously and then I'm just going to pick out a radius for this particular arc and we're going to go for 500 so as I said we'll use some nice round numbers for this and you can see I've picked out the edges quite nicely they're part of this bottom one but what I can do is just take this line that I've create at the top and my center line that goes through the middle and then just mirror it onto the side something like that well then need to do is just to hide off my top sketch and you can see here now that we've got all the sketches that we need to start creating these shapes so looking at how we've created our initial sketch we're easily and quickly able to define our boundaries so using sketch pictures we can do that again there's some nice tools in 2014 that allow us to kind of scale our pictures a lot easier we've looked at arcs and style splines that's how we can create really nice curvature based style splines we've also looked at tangency and curvature and also how we can use mirroring as well to kind of split our design time in half if you like okay so we've had a look at the initial sketching now we're going to have a look at basic surfacing so that's how we can actually create some surfaces from our initial sketches so let's take a look at how we can actually create our surfaces so over in SolidWorks all I'm going to do is take my initial sketches that I've just created in the last session and then to ink operate that into a surface model so first of all I'm just going to use quite a simple tool which is the extruded surface all I'm going to do is just to click on my outline and then I can actually extrude that surface now I'm going to extrude that mid plane around about 30 millimeters so you can see here I've got a 30 mil depth extrusion I'm doing this mid plane simply because if I just look at it from my right view I want to create this surface here that runs from my top edge down to my split line so as long as my surface spans that gap which it does then I'm happy so I'm just going to accept that whilst I'm there I'm actually going to radius the sharp internal corners as well so using our Phillip tool I can just select an edge so loic's prompts me that it's located other edges that I might want to radius at the same time so I'm just going to select that it's the four corners that I want to radius and we're going to go for a radius of around about eight millimeters for that term for those four corners there next I want to use is a slightly more complex surface called a boundary surface and basically this creates a surface between two profiles in different directions so first of all I'm just going to select one direction which is going to be basically the top surface I'm creating now so my first sketch is going to be that line which denotes at the top and then the second sketch is the one that was picked off of the end sketch so that's creating the surface like that so you can see it's created a really nice surface there a couple of things I'd like to do is a bit of trimming I want to get rid of some of the surfaces now so I'm just going to trim first of all need to pick a trim tool so I'm just going to pick that very top surface that I've just created that one there and then I can either cut everything away from it on the top or on the bottom so I'm just going to select that I want to trim everything that's above that particular face then I'm going to do the exactly the same so I'm going to trim surface and this time I'm using this outer surface is my trimmer or is my cutter kind of guide if you like and then I'm just going to remove these four corners at the bottom then you can see what we end up with it's a nice set of surfaces that are nicely trimmed as well now I want to trim everything from underneath my split line as well which is this line that runs to the center here so I can actually use that I'm just going to select the actual sketch itself and I can use that as a trim tool then you can see by highlighting this surface here I can either trim everything away from it sorry below it or everything above so I'm just going to trim everything that is below that particular line now you can see this is what we end up with next I want to do is to create the complex surface that's on the bottom there to utilize mirroring I'm just going to do half of it but what I need to do first of all is to draw cross-sections of what I want that surface to look like at certain points so the first thing I'm going to do is just to bring back a sketch that I've already created actually which is that top one and on that top sketch if you remember I picked out a point where the narrowest area was an appoint where the kind of widest or fattest area was as well so I'm just going to draw profiles at those points but also my mid point as well so my mid point is the one that runs right through the center of my remote control and onto that surface my mid plane I'm just going to drop a sketch so I'm going to use a style spline again by using a style spline remember that I can just make sure that my parts or my surfaces are nicely controlled in a curvature way first of all I'm just going to say that my control polygon I want this particular edge to be vertical which is going to make sure that when it meets this surface here that is going to be tangent I'm also going to select this one and say that it should be horizontal again because I'm just doing half a surface here where I match the two surfaces up together I want to make sure that across the split line that they are perfectly tangent as well by selecting this line and forcing it to be horizontal that's exactly what I'm doing then I'm going to specify that I want my endpoint to be on this particular edge and I'm just going to specify that this endpoint should be on that particular edge and now you can see that's what we've got if I look straight down on it I can actually start playing with this and making it as I want to so you can see here that very simply we able to affect the shape of this particular part at that section now I want to do exactly the same something's going to take my right plane and I'm going to then create a sketch for the narrowest part on that plane and then I'm going to take that plane I'm going to copy that again over to where my widest part is which is that point there now we'll start by drawing the cross section the narrowest part so again using a style spline you can see that I normally start out with these style splines by sketching them away from the actual geometry that just means that I'm not picking up on things that I shouldn't be so that line and that point I want to be piercing so it's just make sure that it is on this edge again this point I want to pierce this particular bottom sweepy curve this line I'm going to say that I want it to be horizontal and this line I want it to be vertical again that's just going to make sure that my tangency is okay you can see I've got a bit of work here just to make sure that this does exactly as I want to so something like about that I think might look quite nice so that's at my narrowest point you can see my profile there or half the profile then I just need to do the one at the widest point so just picking that plane I can sketch on it then I'll just use another style spline again just clicking away from it just to make sure that I'm not highlighting anything that I shouldn't want to this line horizontal same as before vertical this point I want to be piercing my edge and this point I want to be piercing my underside curve something like that and then again just looking straight down on it I can start tweaking it getting it to look how I want so I want this to belly quite nice at the bottom there so something like that I'm quite happy with and obviously being parametric I can come back and edit this at any stage as well which is great next I want to do is to pick out this edge here so this edge that runs all the way around the top I'll actually want to pick that out now that doesn't exist at the moment but you can see I've got an edge there so I just need to convert that edge into a sketch so to do that I'm just going to create a 3d sketch select right hand mouse button on that particular edge and I can actually select the tangency so you can see it's highlighted all the way around there and then I'm going to convert it but because I'm doing half of it we're only creating half a surface all of that at the top there I can just delete you can see that then we end up with a sketch that runs just around half of it okay so the first we want to do is to create this complex surface then so under my surfaces I'm going to create another boundary surface I need to pick the sketches that run in two different directions so the first one is going to be this top one now because this is half a surface I want to make sure as I said before that where they meet in the middle is going to be perfectly tangent so I'm just going to select a direction vector for that now there's a couple of ways of doing this and to make sure that you've got curvature continuous and you've got tangency at these points and this is just one way so I'm going to pick a direction vector for that then I just going to select my second curve which is that one I've just extracted from that edge and again I'm going to use a direction vector as I said there are different ways of doing this but this is my preferred method then I'm going to select my other profiles in the other direction so there's my first one there's my second one and there's my third one going back to these vectors I just want to make sure that they are maximum tangency so it's just going to mean that they flow into the other surfaces really really nicely and that's my surface complete now because I want to onto the other side I can utilize a mirror so if I just select my front plane I can actually use that to mirror across this particular face and now you can see that we've got two now a great way of seeing whether we have coach continuous or really nice flowing surfaces is by using zipper stripes and in effect it makes it look like if we were just showing kind of strip lighting on it and this is how say in the car industry or the automotive industry we actually get really nice surfaces by using things like the zebra stripe tool just to evaluate those surfaces and you can see here that basically where we've got convergence is bad so you can see that there aren't really any areas of convergence there which is great so we've got some really nice flowing shapes there okay so the first thing I want to do is just to basically knit all of these surfaces together so by doing this I can knit all of those surfaces together I can try and form the solid as well so I can ask SolidWorks to try and make that into a solid body and now by doing that if I just section it you can see that what we actually got there is now a solid body and not a series of surfaces which is great there are some other nice tools that we can use as well there's a free-form tool all I do is I pick the surface that I want to freeform I then kind of split it up into areas so I'm just going to draw say I want to maybe lift this particular area at the bottom if I just draw a line there I can add a point to it maybe in the middle and that what's nice if I just pick that particular point you just keep your eye on this surface as I start to drag it you can actually create some really nice shapes and freeform shapes by using this tool now there's not too many CAD tools out there they've got this tool but SolidWorks has and it's great for being able to affect the overall shape of the surface by simply just splitting it into control areas there and using points on there to drag them around and reshape it so really nice tool also we've got a nice Phillip tool as well you saw me use the Phillip tool in a second ago just around those sharp corners but we can do is if I just select this edge here what a radius does by all by all kind of definition is just to apply a continuous radius around that edge so if I just zoom into it we have to go for a slightly smaller radius okay for a tumor radius that we actually get a radius that starts to minin from this edge starts to minim from this edge as well me just get this nice gentle curve but what we can do is use something called a conic fill it and this basically by affecting the conical row we can affect the shape of that Phillips so you can see here we can actually make it quite tight up in this area now that's just another great way of making sure that we can create some surfaces that have certain geometries like that so for example we've got that fill it tool and are using a conic row there so I'm just going to accept that we get a nice fill it all the way around it's just a nicer looking Phillip and a regular flat fill it so just to recap what we've covered there we've had a look at how we can create basic but also complex surfaces as well so looking at extruded surfaces how we can actually create just extruded surfaces in one direction using a curve then we've looked at boundary surfaces that's creating a surface between two curves in two different directions we've had a look at how to trim and extend our services as well using either surfaces or just sketches we've had a look at mirroring as well mirroring that complex surface on the bottom over to the other side we've had a look at the freeform tool as well so how we can actually pick a surface and just manipulate it as we wish and then also looking at some of our more advanced Phillips such as the conical Phillip okay so the next section is how to add features so adding features to our may be injection molded parts like as you can see on the left there graphic of a lip and groove so we can do that using automated features so let's have a look how we can actually get on and do that so back over in SolidWorks you can see that I've just got my surface body here the moma solid body I should say if I just do a quick section you can see that it's just a little lump so what I'm going to do is to give it a uniform wall thickness first so using my shell command I can actually just say that I want to create a two mil overall kind of general wall thickness for that and if I just do a quick section through that body now you can see that we've got a two mil wall thickness to that next I want to do is to split this into a lower half and an upper half I've got a suggestion of a split line there but I'm just going to choose a slightly different one on my front plain I'm just going to sketch just going to take that split line that I've already sketched and convert it and then I can actually offset it so I'm just going to say that one to offset it's a two mil above it and just select the first one I didn't turn it into construction geometry so basically SolidWorks ignores that so all you can see now is this black edge that runs to mil offset from this initial split line that I indicated up here I can then search for commands so if i just type splits into this box it brings up a list of of all the things it can find to do with split so as a new user SolidWorks this is a great way of going to define the tools that you need so I'm going to split that particular body using that sketch so I'm just going to cut apart and SolidWorks is now defined top section and a bottom section I can actually save those out into individual files if I want to so if I just hide off this top body you can see that we're just left with our our bottom molding if you like so bringing back that what I'd like to do now is to actually create a lip and groove now I could do this manually but it's going to take me quite a long time we've actually got a specific tool for creating lips and grooves as well so this is particularly using I guess plastic designs but it allows us to work on both bodies at the same time so I'm just going to work my way through this feature manager hit over here so the first thing it's asking me to do is to select the body on which I want to create the groove now the groove is going to go on the bottom part so I'm just going to select the bottom bit which means that my lip is going to go on the top component or the top body then just need to specify a plane that is perpendicular to the direction of pull so I'm just going to say my top plane is that particular direction then I'm just going to specify my groove as sitting on that face and on this outside edges at the moment is asking me now if I just roll my mouse over these blue boxes it says here to select inner or outer edge for groove to remove the material so I want to remove the material on the outside of that edge so I'm just going to click on that I've got this tangent box ticked as well so it falls all the way around and then I can just select my lip so my lip you'll see that it hides out the bottom component as well which is really nice so my lip selection I just need to select the face first and then again I'm selecting the out the inner or outer edge for the lip to add material so because I've taken it away from the outside edge I need to add it to the outside edge of my top compart then scrolling down here all I need to then do is just to fill out this box with all the parameters so you can see here it's a really nice graphic of what we're actually going to get and then I just fill out this box here punching in some of the numbers that I want for my for the parameters of my lip and groove and I just accept it so it takes a couple of seconds just to go ahead and create the lip and the groove for these particular parts but it does a really nice job and quite quickly as well I've actually creating those if I just change the display ever so slightly it make it a bit clearer when I just do a section of what it's actually done it's created that groove detail it's done all of this additional work in here all the way around as you can see all the way down to the bottom all the way around this part very very very quickly so there you saw me how to create or showing you how to create lip and grooves for your particular parts but we've also got other automated manufacturing kind of bits and pieces as well such as mounting bosses snap hooks snap grooves and also vents as well so vents can be really quite tricky to do manually but we've got a great tool that allows you to be able to do that okay so finally we're just going to have a look at how we can actually render our model so that's that's creating photorealistic high-quality images like the one you see on the left hand side there so let's see how that's done so back over in SolidWorks you can see this is the model that we've just created but I'm just going to open up a part that I've completed and so in true Blue Peter style this is one that I created earlier and it's going to have all the buttons and stuff as you can see there and but I've removed some of the material appearances just apart from the buttons so the buttons have would have been colored but I just want to color the other bits and pieces you can see I've finished this model off I've added a bit more kind of detail and added a battery cover and bits and pieces on there but this is the model that I'm going to use so first of all I'm just going to open up my appearances tab so in here you can see we've got different materials different types of materials I'm just going to pin this open very quickly so you can see under here we've got high gloss medium and low gloss plastics we've got textured plastics and soft touch this is a new thing in 2014 as well so a really nice material this particular one I'm going to go for a low gloss plastic to start with you can see here then we've got a series of low dose plastic colors and I'm going to take my dark gray low gloss plastic and I'm going to drag it onto this bottom body here so you can see here never places it like a like a charcoal low gloss plastic appearance onto that particular body I can then copy that appearance and then just paste it onto the top here so this top body I also want to have the same color I could have painted them different colors obviously but I'm just going to leave those the same color but the battery cover I'm going to do in a slightly different material now I've got a remote control some around the house that's actually got a year a soft touch or a textured battery cover so I'm just going to take my textured folder over here and I can drag across some of these just to see what these look like so there's quite a fine texture you can see here maybe we can go for a slightly more coarse texture so here this is actually what we call a bump map so this is just going to make sure that when we start rendering this so it's actually going to look like it would do in reality so you can see here we've got a different couple of different appearances and then to finish it off I'm just going to select these two surfaces here and just go for a low gloss white plastic onto those so that's our materials applied to our particular part really really simply then we can have a look at where we want to render this now we've got a series of environments now the first few are kind of standard environments if you like these are kind of out the box or this this three-point faded one this is our default out of the box Solid Works works like this so you can see we've got some of the studio environs and then we've actually got some background images that we can use as well so some urban and also solar landscapes as well but I think this is going to be a studio render I'm going to do so I'm just happy to leave in our three point faded next thing I need to do is to add a bit of perspective I've got a shortcut to do that so I'm just going to initiate a bit of a bit of perspective it's best to have perspective on when you're doing your renders and then I just need to have a look at some of the so first of all we just need to specify the image size now I'm going to go for let's go for about a thousand wide by about 560 tall or 562 I've just fixed aspect ratio initially that was at widescreen so in 1920 by 1080 I'm just going to go for a thousand by 562 and I can render it live and you can see how quickly it does this down here we can just specify the kind of qualities that we want and also whether we want this to be kind of cartoon like or not now I don't want it to be cartoon so I'm just going to turn that off okay so then if I just do a quick preview I can actually just see what this thing is roughly going to look like so gone are the days when I first started doing rendering it kind of hit render you'd go home and the next day you'd come back and if you were lucky you'd get something you want well nowadays what we do is we just do a little preview and this window here just shows us roughly what we're going to get you can see it's starting out quite coarse at the moment but this should get clearer and clearer as you can see there it's just getting a bit bit sharper and this is a great indication is this roughly what I'm after yes it is so I can close this down and I can actually go ahead and do a final render and again rendering tools typically they take quite a long time you can see here all it's going to do first of all is just going to create a preview and then it's going to go ahead and actually create the main render itself now you can see here that each of those little squares you can see moving around there's a processor so I've got eight processors on my machine so the more processors you we got the quicker it's going to do it but you can see very quickly it's created us almost a finished render there so total time to do that was 21 point 4 seconds it gives me a readout here of the speed so 20 seconds to do a fairly decent render fairly high quality as well not I think I probably up the resolution of this if I was doing it in anger but certainly that's good enough for web so you saw out there how we can apply different materials different textures we have a look at environments within those environments we've got different sets of lighting that we can do as well so we can play and tweak with the lighting if we choose to it's not something I do a lot of I'll be honest because the environments hold quite a lot of the year the kind of lighting that I would like to use anyway within them and we've also got the ability to preview as well so it's really important before doing a final render just hit the preview button just to make sure that it's going to look roughly how you wanted see okay so just to recap what we've done we've had a look at how we can use our initial sketches to create the boundaries of our particular part then we've had a look at how to create some basic surfaces add features like the lip and groove detail and then finished on the render there to create the high quality image that you see on the left hand side so why choose SolidWorks as a CAD package there's plenty of CAD packages out there but by up by far SolidWorks is becoming the most popular one so currently over two and a half million users worldwide in over two hundred thousand companies across 80 different countries and in the UK just to bring that more localized to ourselves 160 1000 plus UK commercial licenses as a lot of people in commerce using sort of works to create the design work in over 12,000 UK companies why would you choose Cal Tech where you can't buy SolidWorks directly from SolidWorks you have to buy it through a series of value-added resellers Khattak being one of them well last year we were ranked number one for customer support satisfaction in Northern Europe which were obviously really really proud of and at the moment with the UK's only elite reseller as well so hopefully if you decide to go down the route of SolidWorks then you'll feel comfortable and helping you along with that journey if you want to see more of SolidWorks then we hold nationwide seminars and hands-on test drive events as well as if you just want to come along and watch you can but also you can come along and have a play with the software as well and there's nationwide we do that as well so hopefully you'll be able to find a an event happening near you if you don't want to get involved with that give us a call on oh one double six three seven four one four zero five or visit our website it's WWE tech comm thanks very much for your time

Channel: Cadtek Systems - SolidWorks Elite Training and Support

Views: 244,572

Keywords: Design (Industry), SolidWorks (Software), Engineering (Industry), Products Consumer Products

Id: HHBUHyikC1Y

Length: 35min 14sec (2114 seconds)

Published: Mon Sep 15 2014