Industrial Design using SolidWorks

good morning everybody we're gonna take a look today at how SolidWorks can be very helpful for industrial design so we'll switch over the SolidWorks and we'll take a look the first thing I'm going to do is I'm just going to open a component or an assembly that has been finished let's say by the mechanical Department so you'll see on the screen here that we've got the mechanical elements of a carving knife here and just while we're in here SolidWorks is really good for mechanical designers a lot of you will already know you can see here that we can actually show how the mechanism of this carving knife works just by pulling particular components and that side of a sort of SolidWorks is very well covered in some other webcasts that we've been through before here at Inova what we're going to do today is we're going to take a look at how SolidWorks can give some really nice benefits to industrial design so first and foremost one of the things that industrial designers tend to do is create a sort of rendered sketches if you like so we'll we'll show one of these in SolidWorks and you can see here that we've got sort of the profile sketched out of this knife handle now what we can do in SolidWorks which has been done here is actually insert those sketches into active documents and use them as a basis to produce a 3d model and that's exactly what we're going to do here so this particular sketch has been inserted onto the right plane so we're going to start a new sketch on that right plane and we'll just take a look at that normal to now and what I'm going to do is I'm going to use a tool called spine here you'll be familiar with this one and we're going to just draw out a three-point spline sort of mimicking the top profile of this handle like so now splines are great when you want a nice curvy surface and some of the things that we can do with splines is show things like curvature so you can see if you've got nice curvature running across the top there you'll see it's quite hard to see when they're set to yellow like they are on mine but you can see here that we've got a nice even sort of curvature comb running across the top of spline what I also want to do is just link the end of this spline to the origin vertically and that just means that when I draw out a profile to sweep along that spline that the two are going to contact each other that's really all we need to do for the time being okay so we can exit that sketch the next thing we're going to do on the front plane here is we're going to draw out the profile that we want to sweep along that path so again we're just going to start a sketch I'm gonna use a three-point arc here we'll start there we'll come down to the bottom here and then just draw that out like so I'm just going to ensure that all these points are level so I'm just going to ctrl select these in the origin and make those vertical and then we'll just take a look at how far down this arc is going I really want to make sure that it intersects with the sort of employed intersection of that area there so we'll just just get it so that we can grab a point here and just move that down a little bit like so you can use dimensions here if you want to but we're just gonna work in a more fluid way we're going to use the sketches as a sort of guide for dimensioning so we won't need to add too many numbers to our sketches so we've now got the prerequisites to create to create a sweep so we'll go ahead into the surface section of SolidWorks and you can see we've got a number of tools that we can use we'll be using a few of these as we go along so the first one we're going to use is swept surface so within a sweep we need to define a profile and a path we've got both of those so this is our profile and we want to sweep it along that path like so and you can see that that does a decent job there but I'd really like to get the end of this to match the same as the start so underneath the options here you'll see there's a lot of options that we've got within here but I want to keep the normal constant and that will will maintain the arc across the spline path that we've defined you can also apply guide curves in here and start and end tangent sees if you want to we'll cross those subjects in a moment okay so we've added our first sweep and you can see that that looks pretty good we may need to refine this end profile a little bit just to sort of encompass that sketch there so if you do want to do that you can go back into any of these sketches at any point edit them drag it down a little bit and you'll see that the yellow line indicate indicating where the actual sweep is at the moment will sort of allow us to visualize where that's going to be so we'll start that now and you can see that we've captured that a little bit more now what we really want to do with this sweep is we want to modify this surface and make it so that it it sort of carries this belly shape along the knife handle as much as we can do and to do that we can use a tool called freeform in SolidWorks it's quite a nice fluid tool very much like what you would find in NURBS modelers like Rhino an alias we can start this tool all we need to do is define a face that we want to adjust you can adjust the transparency here so we can see through it a little bit easier and then we just need to set a couple of options here we want the orientation to be right related to the surface and we're just going to change some of the continuity at the ends of this surface as well so what that means is we just need to tell the system what we want to happen at these junctions so at the top here we're sort of working directly down a line of symmetry at the moment for this component so we really want to maintain a curvature across that edge over on the left and the right hand side we can make these moveable because they can adjust if we need them to and towards the bottom again we we want to really maintain curvature or at least tangency but we want to move that edge so the option we've got there is movable tangent so we'll add that one there so the next thing that we can do is we can either add control curves or control points I want to add some control points and I want one here to define that sort of pushing of the belly and I want another to around here so that we can pull the base of that curve out once you've defined the points you can actually grab those collectively using the ctrl key and start to pull and manipulate the shape of this down so you can see here that I can start to pull the whole surface down to match up with the line that we've got at the bottom that we're using as our guide we can even adjust the the sort of influence of the end the end point as well as put in there by default and we'll just use this point here just to pull it back up a little bit at that end like so and you know you can fiddle around with this sort of shape a little bit more than I have at the moment adding some more control points and defining it a little bit better but that gives you a good idea of what can be achieved very very quickly okay so once we've got that drawn out like so one of the other things that I want to do is sort of introduce the top sketch which has been inserted into this component and if we take a look at a top view you'll see that our surface is currently where this blue edges but really needs to be out here so we need to do a little bit more work in terms of manipulating that surface out to match where the industrial designers sketch is is currently shown so to do that we what we can do is add in some control curves and I'm going to add one indirectly in the center here and then we will use that to manipulate the surface to pull it out so I'll click the add curves but I'm not going to add one there like so just hit escape and that will come out of that and then if I select that control curve what you'll see is I'll get the same control points that I'd added onto the original edge at the bottom so again I can control select these two points and start to manipulate this surface in terms of moving it out and refining its position so again we'll just sort of tweak this end point here a little bit like so we're going to leave this front edge pretty much as it is we'll just pull it back slightly there just to influence this sort of curve here but we're gonna retrospectively trim that section off in a little while as well so we'll leave that as it is okay so we've now sort of defined quite a nice surface but if we want to interrogate this for curvature we can actually turn on the curvature combs on the entire surface and you'll see those of you who deal with surfaces a lot you'll see that we've got quite a large amount of spikes running sort of top and bottom here which we really need to do something about so to do something about that we're going to add a curve in at the top here like so and we're going to use that curve and it's control points to start to pull those around and see if we can't refine those curve it just spikes just a little bit just to lessen their impact so you can see as I start to move these around we start to lose the massive spiking that we get and we'll follow the same procedure towards the bottom here as well so if I grab hold of that and then grab hold of these two points I can start to just pull and flesh out this surface a little bit just to try and refine those spikes just as much as I can with a few more curves and a little bit more time we could really adjust those for the better but for the time being they'll they'll serve the purpose that we need them to do okay so once we come out of the freeform command you can see that we now get a really nice surface on the screen that looks really really good okay so the next thing we want to do is we want to cut off this front section here just to try and again mimic the sketch that we're copying so we can do that by creating a sketch we'll just come into a top view here and start a sketch on the top plane and we can draw out just a single line here and then cut back across the component like so and we'll just add a couple of dimensions to this just to control it so we want an 18 degree angle and this wants to be 20 mil like so and this sketch really is just going to form a trimming boundary for us okay so SolidWorks is very versatile in terms of how you can trim you'll see that as we go through back on the surfaces toolbar we can use the trim surface tool here and we can use the sketch to trim and then we've got a couple of options here we can either choose to select what we want to keep or what we want to remove and you'll see that the sketch actually creates a defined boundary on that surface for us so we'll cut that section away and that's gonna form a nice straight portion on the front of that knife handle for us before we mirror this over to the other side we really need to fill this surface in so I'm gonna use a tool called film surface here and we're going to select a boundary like so at the moment it's not going to close that up a lot of systems sort of dictate that you would need to define a boundary between these two points here but within the field surface tool we can actually tell the lung the option to fix up the boundary and it's going to create that boundary for us which is quite nice so if we click the green tick there we end up with our sort of flat surface on that end okay the next stage for us is to mirror those two surfaces over to the other side and we'll just check the integrity of the surfaces that we've created so on the standard features toolbar here you'll see mirror and we just want to select the central plane here and we want to select some bodies to mirror which are these two like so and we can mirror those on to the other side now once we've mirrored them we may want to knit them together so in SolidWorks we end up with separate surface bodies and unless we knit them together so there's a tool for us to do that within the surfaces toolbar just at the top here we can select entities to knit together like so and you'll see that it will show us the if there are any gaps between the surfaces and the size of those we can see we've got some really small gaps here and I can just toggle on to allow the system to actually knit those gaps together and we end up with a combined surface body now so what I'm going to do I'm just gonna hide the two sketches and then we're going to turn on something in the display options called zebra stripes and that'll allow us to interrogate the surface in a little bit more detail so these zebra stripes just allow us to look at where surfaces cross each other so right at the top where we've mirrored these surfaces you can see that the zebra stripes are exactly in line that has occurred because of the curvature constraint we added to this top edge when we modified the surface so ideally on consumer products you know things that people are going to look at all highly reflective surfaces you want to maintain a good level of curvature across any sort of joins like we have here and you can see that because the zebra stripes line up exactly that indicates that we have a good match of curvature between the two halves anywhere where you get discrepancies or big changes in curvature you would see something like what we have here between these two surfaces so we've got a very large zebra stripe and a very small one this side and they don't line up exactly if we take a look at the bottom as well we should see that we've got a nice crossover at that at that intersection as well so that looks really good okay so we can turn off those zebra stripes you don't need those anymore okay so we're getting somewhere with with our sort of products here I'm just going to bring back the right sketch because the next thing we need to do is we need to put on this back end to the handle here you'll see that maybe we've come a little bit longer with our are sort of swept profile than we may have wanted to what we can do there is we could drag a reference plane maybe to about there we'll just define that a little bit more specifically with a with a size so I 175 and we can actually use that plane to trim the surface as well so we could remove that back portion if we wanted to just to give us a little bit more area to work with to create this back section alternatively we could have gone back in and modified the original sketches if we wanted to but it's quite nice quick process and it shows you in another way that we can trim in SolidWorks so we need to create this end here I've actually got a sketch defined already for the base of the sort of foot and really what we're doing here is we're creating a section so this carving knife handle can stand straight up and not roll around a work surface so we just need a flat foot for that to fit onto so we're going to introduce another tool here called boundary surface this is a really flexible tool that can be used for a lot of different situations it's quite nice here so what we're going to do is define some directions so some profiles for the directions we can use a tool in SolidWorks called the selection manager this'll allow us to select groups of entities open loops or closed loops we're going to use it for a closed loop here and select these two edges of this surface at the back so you'll see here using the closed group tool within the selection manager it allows me to select that as one entity I can just accept that and then choose the next profile that I want to create the boundary surface between and you'll see we get a very straight transition between the two now that would be fine in some situations but what we want to do is try and maintain a level of curvature between this surface so what I can do is select the first closed loop here and then define a an end condition on that so here we're going to maintain curvature to face like so and you'll see that that matches quite nicely up with the curvature defined in the original sketch now what we can do is manipulate that with a numerical value here or alternatively we can drag and pull that out and manipulate it a little bit more so maybe we just want to match slightly more than we were originally and you'll see that we get the curvature combs up on there as well which is really nice so once you're happy with that you can click the green tick and you'll see that we get a nice sort of sweeping handle shaped like sign so we can hide our sketch again we don't need that necessarily so the next thing we may need to do is close off the base of that and we can do that using the filled surface tool we've seen this tool already so we can just select the two ends there and close that off and it creates a flat surface for us okay so now that's done we just need to sort of knit this portion to the main surface body so we can use our knit surfaced tool again select those two and the original one just heal any gaps and we can join that together quite nicely ning that together just allows us to fill it this particular edge here so we could say we want a constant radius fill it of two millimeters for example and we can do it around that entire bottom portion like so and we end up with our nice soft flatfoot there now taking a look towards the front of this handle there's no sort of finger guard for the blade in this design at the moment and that is something that we are using from an external supplier the external supplier themselves use use Rhino as a product to design their components and they've sent through a file in Rhino format now one of the things that's good about SolidWorks is it's sort of data import from other systems so if I just open the open dialog here you'll see a range of file formats that we can open and one of those is Rhino so if we select the Rhino format we can see we've got a Rhino file here 3dm is the native extension of those files so we can select open and it will convert that file into a SolidWorks file it asks me if I want to run import Diagnostics which I don't so I can just say no and you can see here that we've got our Rhino files imported as she comes in as a surfaced body but we really only need to show it in our files so that's fine for what we're going to do so we can save that as a SolidWorks file now we'll just save it over the top of what we've got and then we'll just move back to our assembly here now what we're going to do is we're going to insert that guard into our assembly so we can just select that component you'll see we can place it anywhere on the screen but I've sort of configured this so the origin snaps it into position so we're going to click OK and you'll see now that we have that guard in position now one of the sort of requirements that we have from a design perspective is to maintain the curvature that this guard has at the front of our knife handle and at the moment we don't have that we ever saw a flat flat front so we need to do something about that so I'm just going to edit this component again and start a sketch in the right plane what we can do which is really nice in SolidWorks is take data from other things and reuse it so here I'm just going to select this edge I'm going to toggle on the option to create no external references and all this means is that I'm basically going to copy this edge into my active part and I don't want it to create a relationship to this component because this component can move forwards and backwards with the knife handles we don't want the front of our knife guard moving front to back so if we just toggle that option on we can convert that and it gives me a little warning here and it's going to say the references will be broken which is fine we're just going to select that turn it into construction geometry and fix its position and that's fine and then we're going to offset a line from that in the reverse direction we're not going to add any dimensions and we're just going to say ok what that allows me to do now is maintain the curvature of that arc whilst being able to manipulate its size you'll see I can move it front to back round to wherever I want it and I'll roughly get it into position there and that's fine for how we want to sort of sculpt the front of this this handle so what I want to do is create a two directional surface for the front of this handle so I need to create the the direction curvature so I'm gonna do that on the top plane and we'll just put ourselves into a top view here and I'm going to use another three-point arc like so we'll just ensure that the center point is aligned with excuse me we'll just ensure the center line is aligned vertically with the center of our component and then we'll just add a relationship between those two endpoints to make those in line as well and again we could sort of add dimension to this art but we're going to leave it as it is I'm just going to add a point on to this here onto the center of that arc and then I can use that point to create what's called a pierced relationship between the two curves like so and all that insures is that the two curves contact each other and I can now start to manipulate the size of that curve around if I need to which is quite nice okay so once we're happy with the sort of general position of those two curves we can exit the sketches and we can use the boundary surface tool again here to create that two directional curve so well slightly different to what we did before here is going to select two directions so the first direction is going to be this line and the second direction is going to be this line here and you'll see we get that nice that nice curved surface on the front of our handle so I'm quite happy with that you can see the curvature combs on here as well just to give you an indication as to what the curvature is like so we'll just click the green tick to accept that and then what we can do here is again use trim surface we'll toggle on the option to use a mutual trim here and that allows us to select two surface bodies and then use those as the trimming boundary so I can select the items that I want to remove and we've now got the nice sculpted front the matches are guard on the front of our knife handle okay so I got is quite a fair way through that but there's there's just a couple of other bits that we want to do first as well I'm just gonna hide this surface body and just show the sketch again here so we just take a look at the right sketch you'll see there's a section of the design that's cut out for the operation button we just need to recreate that so we'll just bring our surface back and I've actually got a defined sketch for that which we're going to use to trim our design so if I just press select the sketch and the trim surface tool we need to go back onto standard trim you just select our sketch again I can then specify that I want to remove that section from our design like so now we need to fill this in with some kind of surface we're going to use filled surface again we can select the two edges that form the boundary and what you'll see is it that skins quite a nice surface across the top there that's pretty flat so that's fine we'll just click the green tick and we end up with that surface we'll just use our knit just to position those together and accept that and we're pretty much done in terms of what we want to do on here now but before we move on to the next stage which is to create a solid item out of this we really need to fill it some areas of our design just to make it a little bit smoother so we're gonna use our Phillip tool again gonna specify an 8 mil Phillip to run at the top here and at the bottom here and you'll see it pre selects the mirrored edges of those as well so we've created a nice rounded section to the front of that handle now I want less of a sort of sharp difference between these two surfaces so I want to fill it this area so if you click enter it'll repeat the last command I don't want to fill it give or take around 3 mil just running around this edge here and one of the things you'll notice when you do fill it's is that sometimes we can get this sort of tapering in of a Phillip when you have different angles of surfaces coming together and that's not something that I really want in this design so what I can do is I can use the face Villa option within SolidWorks and that allows me to select this face and this face here it will pick up all the faces around as well for us automatically you'll see there's no difference in terms of the fill it at the moment but one thing the face fill it gives you over a constant radius is we get some more options and we can toggle them the option to maintain a constant width fill it what SolidWorks will do is it will work out all the sections around the area where the fill it is changing modify the radius to suit our constant width so if we click the green tick there we get our nice constant width fill it running around there and we'll just do the same over on the other side so face fill it select one face and then the second place and just toggle on the constant width option there and we end up with our very nice-looking handle okay so we're pretty much finished with the sort of sculptural design element of this handle now we really want to turn this into a solid item so we can use a tool called thicken in SolidWorks at the moment this is a surfaced body so just before we do thicken if we just take a section through this you'll see the surface itself has no thickness compare that against a solid item like the blades and you'll see there is a thickness there so we need to give this a thickness so the thicken tool is used for that we just need to define a wall thickness here so that's going to be two mil and you can also predefined a direction to thicken it in so side two typically is inside side one is outside and this one is mid plane so we're going to select our surface and then that's going to thicken internally and we'll just check that by using our section tool here and picking a particular direction and you can see now that we've got a thickness all the way around our handle so one of the things this section tool is very good for is sort of visually checking for interferences so you can see here that we've got a good clearance around that motor element and the mechanism at the front end of that knife handle so that's quite good we want to be a little bit more specific with our interference detection we can using tools within SolidWorks to do that so under the evaluate tool while we've got interference detection we can just calculate any interferences within here and you'll see that we end up with two interferences that are highlighted in red and you can see that's where the blade actually comes through the front end of that handle we haven't done anything for that so a good check just to confirm there are no interferences in the main body of it so we've done a good job of shaping the body of our handle there but we do need to rectify these little issues here so now they've been pointed out to us we can come out of the interference detection tool and we can edit the part and just do something about that so a nice tool that we have in SolidWorks is called indent that allows us to create a cut using other geometry so other parts things like that so this is our target body and we want to use these two blades here to cut on the front of our knife handle and we can specify an offset size within here so maybe we've put a point five offset around those just to give it a little bit clearance just click the ok' button and you'll see there that we create those two cutouts just to allow those blades to move okay so that's that's worked really well so we're sort of done now in terms of error checking so we're going to open this part in its own window and just check a couple of other things just before we move on to the next stage so once you've done a design like this one of the things may be worth doing is using a draft analysis tool here we have one in SolidWorks to do that so all you need to do is specify a direction that the pulls going to go in and an angle that you're your recommended minimum for the draft angle and you can see that we've done a pretty good job here in terms of making sure the surfaces are all drafted so this can pull out of the mold so we've got a good split line running across that component as well so a good visual check here and it will show you the draft angles as you move around which is quite nice as well so if you leave that draft tool on it will display so if you do need to make any modifications you can keep that color up if you want to but we're okay so what we're gonna do now is we're going to split this component so to do something like that we can use a tool in SolidWorks called split which we have here so if we start the tool we can select a plane to cut the part and then just click cut part that could be a sketch if you wanted it to and it's going to show us the two bodies that we've created in that component so I can toggle on those two bodies to keep and it's going to define the names of those bodies for me and we end up with two halves of our component like so two halves of our solid component now because this is a molded part we may want some kind of jointing detail between these two items to allow them to be fitted together easily and a really nice tool within SolidWorks is called lip and groove so we're gonna use the lip and groove tool here all we need to do is select a body that we want the lip or the groove to be on so the first one is the groove and we'll select the second body for the lip component so the groove face is going to be the inside face here and the groove edge is going to be the inside edge of that component because what we don't want to do is effect too much the external display of this component so we'll just select these edges here like so and that will create the lip on that come all the groove on that component the lip selection is is pretty much the same so we just select a face to use and the edges so we can select the same inside edges and this tool was brought in a couple of years ago and because these these type of features typically used two takes or three or four features to create which is quite time-consuming but they've been conglomerated here into one command so just towards the bottom here we've got some controls over how that lip and groove in terms of its size is that kind of thing draft angles bits and pieces like that we're going to leave those as they are and SolidWorks will do the rest for is so we just get a small message about some drafting problems which we could rectify manually but we'll just use the section tool here just to have a look and see what the lip and were Taal has done and if we take a look you can see that it's actually doing a really good job there of making those two halves for us okay so we're gonna move on to the next stage I'm just going to hide both of these bodies here and just bring back the original sketch so we can take a look and you can see that the the industrial design is sort of indicated an over molding a sort of type of a rubber section on the component for grip so we're gonna go ahead and recreate that now so if we bring back our our solid bodies here just bring those two back and we'll just bring our original sketch back as well we'll take a look in a a right view here and we'll just create a sketch on the right plane as well we'll just hide one of these bodies the way just so we can see the original sketch and then I'm just going to use a two-point spline here just defined at the two end points and the nice thing about two-point splines is we get manipulation handles at either end so we can start to pull and manipulate that spline around so it works quite nicely in that situation there and it will also work really well for us here as well so if we just create our spline at those two points we can actually pull and manipulate that around to match the contours of that sketch maybe if we just use this handle here we'll just pull that around a little bit and we can start to create that that sort of shape now over on the back here we have some new functionality introduced in this release of SolidWorks which allows us to create conics so we can actually use the conic functionality here just to create a nice shape there as well these comics are really controllable you can actually control them with row values if you want to and manipulate them afterwards like so but that'll that'll do just to sort of showcase what we've got there like so so we've created that sketch all I need to do now is just create a surface that I want to trim so I'm going to select this face here when you use the offset surface tool and offset that by one millimeter like so then what we're gonna do is we're going to use trim surface again with our standard trim and that sketch line and we're going to select to keep this middle section like so so if we keep that middle section we can then thicken this internally by one mill like so and we'll just toggle off the option to merge the results and we end up with our sort of over molding section just gonna use the Phillip tool here and we'll just use a one mil fill it just to round off some of these edges and within this fill until you actually get what's called a smart selection so here this is gonna grab all the corners for me with without me having to pick those and we can just add that on like so and maybe we just put a sort of 0.25 Phillip running around this top edge as well so we'll just let that figure itself out and it establishes it can't do it that big so we'll just make a change there to 0.25 and add that fill it all the way around the outside there and then maybe what we need to do here because we want this on both sides is we'll just use the mirror tool again on the right plane and select that body and mirror it about to the other side and we end up with our two halves of our molding over the top okay so if we just switch back to our assembly we've got a couple of other things we can do at this point as well we're sort of finished on the design side but in terms of visualization SolidWorks is really good at visualizing what the products is going to look like we can go into the right-hand side here I'm just going to pin this down we can take a look at the appearances that we can apply in SolidWorks so maybe we drag a map rubber onto this item and onto the other side here because they're two separate bodies and maybe we want a particular plastic color just shown on this item so we use a medium gloss plastic let's say yellow and we can drag and drop that onto the component as a whole and we can get an idea of what that look looks like in SolidWorks you've got something called real view which sort of adds a more real stick reflective appearance to items like so one of the other nice things that we can do is actually define cameras within SolidWorks as well so here I'm just going to define a camera on the left hand side you control where you're looking at so maybe we want to just zoom in a little bit and focus on the handle a little bit more than anything else you can use this little red dot source or focusing on on particular areas and we can define a camera like so and then view that camera and we've got our nice dist defined view of what we're looking at set up in SolidWorks once we've defined appearances we can also place the object in scenes and SolidWorks comes with a number of default scenes these really define the the sort of lighting environment that you're working in so you'll see as we toggle through some of these that the lighting will change the reflective nature of the material sort of has different high and low spots on it so we can start to see in which environment our object looks very good as a as a nice way just to sort of show this to you know people that you want to demonstrate the product to before actually making it so once you're happy with the scene you can you can adjust all acts aspects of this scene within the property manager on the left hand side so we can start to adjust whether or not we have floor reflections how high the floor is in which rotation the environments in which can affect the reflectivity and bits and pieces like that you can also adjust the influence of the lights in here as well but once you're happy with how the project the product looks we can use a particular atom called photo View 360 which is one of the add-ins we have in SolidWorks professional which will allow us to create a rendered image of this item so the first thing normally that you would do is open a preview window and get an idea of whether or not the appearance is you've defined make the product look okay so whether you've chosen the right rubber that kind of thing and if you hover your mouse over certain areas it will focus in on rendering that area first so you can see here we're starting to move over the rubber and it's refining those areas once you're happy with the preview window you can then go to the options page and specify sort of pixels sizes of your images I'm just going to do minor 800 by 600 just to allow this to run very quickly once you've set all that options up you can then go to the final render and we can take a look at the final render screen so depending on the number of calls your computer has depends on the number of orange squares you'll get on the screen but you'll see the can process images quite quickly - quite a high level of realism you know I've spent literally next to no time on that image just to give you an idea of what can be done ok so once you've presented the product to somebody you know maybe it's the owners of the company or the client and they're really happy with what you've done you may want to just check your design for its manufacturability so the next thing we're going to do is take a look at a product in SolidWorks called called solidworks plastics so what we're going to do is we're going to we're just going to save out one of these bodies in this particular component so we're going to save out one half of this molding just to try and get an idea of whether or not it is moldable so we'll just give that a name and we'll save that and then we're going to take a look of whether or not we can mold this so again another adding that we have available for SolidWorks is solidworks plastics so we'll turn that on and it will load a different sections of the software this allows us to understand whether or not the product can be molded so the first thing we need to do in solidworks plastics is give the component a mesh to allow the study to run and there's two types of meshes in solidworks plastics the first one is a solid mesh which will mesh the void and every external face now these types of meshes can take a little bit longer to generate but are more accurate in terms of their results the second option we've got is a shell mesh these are a lot quicker and they will mesh every external face and every and internal face and then leave the void of the product as a void so these can be a lot faster to run more efficient for you system to generate by the end the results are a little less accurate so we're going to use the automatic settings for the shell mesh so all we need to do is right-click on that shell mesh and say Auto and then it's going to calculate and work out what it thinks the best size machine is so those of you who are familiar with simulation tools will know that the meshing can take a little while depending on the refinement level and if we went into the manual settings and define those we could refine the mesh a lot further so the next thing we need to do is juice choose a material so we're just going to open the database that solidworks plastics has and this contains around 4,000 materials now we can sort either by family so in terms of plastic family or by the company that produces the material so Dow Chemicals BASF typical ones in there those kind of things we're going to choose the generic grade of ABS but if you have a look through this list you'll see there's a load of you're sort of familiar materials that people will use for plastic components these contain all the temperature readings for the plastics the viscosity and certain temperatures and they just allow us to create an accurate mold flow of what's going on so once you've chosen your material we can just click OK and the next thing we need to do is define how the plastic is going to be injected into the components so it's more a how and where so we need to define a gate location so if you just open the gate section we can just click on an edge and define a gate so just add that gate on and then the system is going to use that as the injection point the plastic that's really all we need to do in a sort of simplest forms we can let the system do the rest and start to run the analysis okay so once the studies completed we get some really nice plots to help us visualize what's actually happening when this component is molded the first one is a fill time plot so it'll allow us to see the flow of plastic through the cavity and understand which bits are going to be moulded last and which ones first and then the system will calculate things like world lines so where the flow of molten plastic moves past an obstacle and rejoins we get weld lines created and these can sometimes impact the strength of the component so it's quite important as a designer to understand where those are possibly going to be along a similar line we also get indications of where air traps occur so because we're forcing molten plastic into a cavity that contains air we're effectively compressing that air down into a very small area and if we keep compressing that without venting the mold we can cause explosions which will you know can sort of blackened the plastic at that point and cause sort of you know cosmetic degredation so again it's important to understand those where those are as a designer we're quite lucky in this instance because the air trap is created right on where the split line of the mold is so it sort of it gets some natural venting so to speak you can see also we'll get an idea of the cycle time so the fill time for this particular component we'll also be able to see cooling time and quite a large amount of other plots that we can review there are some specific webinars on this product this product as a whole so it would be worth looking at those if you're interested in this side of things but a very useful product nonetheless ok that sort of brings us to the end of our presentation so if I just come back to our PowerPoint slide here I just want to say thank you very much for watching there are some future webinars that we're running listed up there for you at the moment so if you are interested in in nose then please have a look at our website for more details in terms of costing and sales of SolidWorks it would be worthwhile you getting a hold of your account manager who is Andrew nori so I've put his email and his contact details at the bottom there so if you are interested in pricing or looking at the different packages available then please get in contact with him once again thanks very much for watching we'll see you again next time

Channel: Innova Systems - Experts in SOLIDWORKS Training & Support

Views: 95,943

Keywords: solidworks, tutorial, tips

Id: N20UVv5Zb8E

Length: 47min 9sec (2829 seconds)

Published: Mon Feb 03 2014