Introduction to Surface Modelling in SolidWorks [Webcast]

now in this webinar we're going to have a look at some of the surfacing techniques within SolidWorks looking through a basic introduction to the the area in the software and and some of the techniques you can use to actually build up surfaces so to actually start off a model in this particular exercise we're going to look at this mouse and actually have a look at creating it within SolidWorks and using surfaces to to create some of the organic shapes within the design so the first thing I'm going to do is just to switch to SolidWorks I'm actually starting from a blank document to start with so I'm just going to create a new part now in this new design what I need to do first of all is just check that I've got the scale right and I've measured the part beforehand so I'm just going to do a basic sketch which is going to show how long the part is I measured the models hopefully about 120 millimeters and I'm going to fix that on to the to the origin with a midpoint relationship and that just helped me build up the design and make sure I've got it the right size so now what I'm going to do is actually bring in a picture within the model often when you're building a normal design of solid model women SolidWorks it's quite easy to go in and actually measure that particular elements you want trying to try to design when you're doing surface model it's a little little harder will be with your more organic shapes to actually measure what the or the item looks like so I actually going to insert a sketch picture from the sketch tools menu it allows me to take a picture from my machine and bring it in as a backdrop to model on to so it's just a case of scaling this down to the right size and bringing it into position there's panels on the left hand side when we can do this manually and also adjust the angle as well if we need to okay so I'll scale and I'm going to move it so it's roughly in the right position so this it's approximately over that that line that I created earlier on from measuring the model so I think that's about right there the next thing I'm going to do is to actually take away some of this white background from the picture I can use the transparency settings on the left to do that so I'm going to put in a user-defined transparency setting there and that allows you to select a color and increase the transparency of that color increasing the matching tolerance will increase the range of colors picked up and made transparent so with that created I've now got that to model on top of as a backdrop I just hide this first sketch and I'm going to cry which is going to be the outline of this sketch picture that putting because there currently I can't model with this backdrop but if I draw something around it I'll then be able to use it within my design okay so generally within this set within this webinar I'm going to be using some techniques using the spline tool in order to build up the complex shapes that I want the spline tool is quite useful within SolidWorks because it allows us to get a constantly-changing radius and quite an organic shape quite easily it's got these drag handles which allow us to change the angle of projection of the spline and we can increase the amount of influence by increasing the length of the drag handle so I'll increase it and put in a second spline around the top oops now what you know is with this spline I'm putting in the minimum amount of points possible you know in order to get that shape you'll find that you get a much better surface created if you decrease the amount of points you put throughout the spline it helps the spline to become more free-flowing so it's a case of adjusting those drag handles till we're getting the kind of shape we're looking for I tend not to adjust the drag handles in the middle too much but rather actually pull the points themselves in order to adjust the actual shape of the spline as soon as we adjust these drag handles again it will make the spline a bit more unnatural so just by adjusting the drag handles at either end we get a nice free-flowing shape in between now that's been created I'm going to go ahead and actually exit out the sketch so I've got a sketch which goes all the way around the perimeter of this set this profile and I'm going to use a planar surface first of all in order to create that so with that sketch selected the planar surface just fills the sketch area with a particular surface model so what we're left with is a surface body which matches perfectly the profile that we brought in from that sketch picture okay so much you're going to bring in a second sketch picture now and do that process again now rather than do it all over again I'm actually going to open up a model that I created earlier on so it's the same idea of just I've just brought in a second sketch picture if we hide both of those you see that the sketch picture of a line so it's got a nice symmetry down the middle and I've drawn out my second planar surface we have a look at that sketch just to see how that was created again that was using splines but the only thing I've made differently here is just to make sure I've got a horizontal relationship where it matches up with that symmetry plane and that's just making sure that when I actually go and mirror this part when I'm finished it will have nice symmetry in the middle area there's no real point in me modeling the whole design on both sides because it is a symmetrical model so I might as well just model half of it and then actually mirror it over okay the next change to make is to actually insert a sketch which matches this silver area around the edge of the model and that's actually flowing in in several directions essentially flowing it in sort of three directions using x y&z axis so it's quite a complicated curve and in order to create that I'm going to use a 3d sketch tool for those of you who haven't used that before we can find that by dropping down under the sketch to find 3d sketch now it's quite hard to define a 3d sketch you might if you ever done it before it's quite hard to get them right so in order to draw this item and get it correct I'm going to bring myself into those standard planes by orientating myself in the top plane for example and limiting the amount of changes I'm making in that y-direction as we can see in that triad on the left hand side so it means that I can get quite an accurate curve but without having it going totally out of the way okay so I'll stop at this end I just draw it around just placing points wherever the spline changes direction and to finish the spline off I'm just going to attach it on to the curve that I created for that planer surface first of all okay so it's around about the right place from this direction I'll now bring myself round to the right plane and we can see the kind of sketch we've got in the other direction so in order to bring this into the right shape it's just a case of actually dragging these points into the right position okay you'll notice it doesn't perfectly match on this end that's just to do with the kind of sketch features that I've taken maybe they might be in a slight bit of lens distortion there that there's several reasons why it might not quite match up with those sketch pictures so you will get a slight amount of tolerance when working with those and it can be worth just taking a while long and just making sure you've got them correct when you first create it but it's not a problem I'll just take that into account when creating my design so now I switch back to this top view just to again manipulate the shape from this direction so it does involve a lot of suite switching between views in order to make sure that you're getting the correct shape in certain areas I will have to just manipulate the drag handle in between there in order to get the correct item up that I want and again it's the case of actually making sure we're going to get symmetry here so I want to make sure this drag handle is pointing nicely with a symmetrical relationship so I'm going to make it along X which means it's pointing in the X direction so when I mirror this item over but not have nice symmetry on this design okay so that's fairly fairly good from this angle now it looks quite accurate I just switched back to the right plane once more just a double check that it's right still on this direction and just to make a slight change I'll just drag this point up a little bit and slightly adjust the drag handle in this direction okay so I'm fairly pleased with that now and you can see we've actually come out with quite a complex 3d curve preview it from a isometric view for example so we can use that for the basis of our surface model so I'll hide these two sketch pictures out of the way now I don't need those anymore and in order to build up the next part of the design I'm going to loss from about here to this end profile here so in order to do that I need to do create a new sketch plane to draw on by using the ctrl key I can just drag out a new sketch plane too into the right position and I'll change that to a dimension of 30 draw out my spline again between these two points and by making sure they're in the right place you'll see as a rotate around I can tell that it's not passing through my 3d curve in the correct in the correct place so if I hold the endpoint down and then press control and select the 3d curve as well I can add in a PS relationship which will mean that the point is exactly on this 3d curve as it passes through the sketch plane and I'll do that same for the bottom as well so Pierce is quite useful relationship when working with splines and also make things make sure you've got the sketch items ending in the right position and just to finish it off just drag these drag handles out to get the kind of shape that I'm looking for so I know it's quite rounded on this back edge so I'm just gonna pull out quite a rounded shape on the on here to get the right profile so I'm fairly pleased with that and I'm actually going to hide the sketch plane away so I can go ahead and laugh between this profile now and this one here now using a surface loft is very similar to using a standard loft within SolidWorks the only difference being is that we don't have to select an enclosed profile we can just select a single line like this one so I can loft from this profile here to the end profile over here the important bit are this M profiles that I've split these splines of the two elements so I could select them separately we do have to make these show these green dots line up so I just drag one to the top if it's not in the right place and then we can select the guide curves to help influence this spline as it moves towards this end profile so the guide curve the bottom would be this edge and the guide curve at top is that 3d sketch that I created so you'll see that we get quite a nice profile as it moves along and it quite nicely matches the shape of the mouse if I hit the tick that'll create the kind of loft I'm looking for the only difference is I want to make sure it slightly undercuts a bit more around here I do that I do know the shape slight undercuts a little bit more from looking at the mouse so I need to put in another profile at this position I think in order to get that because you'll notice it's not quite matching the profile enough at that position now the great thing about loft with this older works when you're working with them is that you can insert a profile straight into it in order to do that I'm going to create a new sketch plane at the right position so I'm just going to drag one out to 30 in this direction this time and that's just ensures that I can get the profile in the right place and then turn certain in profile to this loft I just right-click on it and select add loft section we can either choose to rotate and move this profile into the correct place to get a sketch where we want it or we can select a plane within the design so I'm going to select that new plane that I created but you'll notice because it's below the loft we can't select it so we need to make some adjustments to our design tree and actually drag this plane to above the loft in the design tree so that essentially it would be created before the loft and now you can actually use it in that selection okay so adding in this new sketch now it leaves me with a new profile that I can use in this loft so I'll just edit the sketch for that and then I can slightly adjust the profile a little bit to like to make it undercut a little bit more you can see the profile matches a bit more nicely so I'll just edit that loft and we can have a look at it okay so that's the loft profiles it moves along so the next thing to do is just to have a look at creating the next surface within this model so I'll just hide this surface away this plane away sorry and now I want to show you one of those sketches that 3d sketch one I'm going to use that for the construction of the next surface as well we've got quite a curved surface here and I have to bear in mind how that will influence the next surface that we create so it's quite an interesting thing to look at within SolidWorks so we'll just switch back to that PowerPoint and just have a look at this the types of continuity you can have between surfaces so when two surfaces touch up to each other we get a contact relationship or a c0 continuity tangency whether a line or curve meets another curve at a tangent we get c1 continuity and curvature continuous or c2 continuity is when the curvature continues straight from one curve straight into another and that will be done mainly with splines so we can see if we have zebra stripes on what that actually looks like so contact you can see a visible edge between the two surfaces with tangent these zebra stripes follow into the next surface quite nicely but there is again still a slight break in there but it's not too bad but then curvature you actually can't see the break between two surfaces Soaker which is particularly good for high quality renderings and things like that in this particular example we're going to go with either tangency or all curvature in order to get the result we're looking for so in order to get a tendency or curvature continuity from one surface to another I need to be able to select something as a reference we can actually create a sketch automatically on this this plane here at an intersection by just creating an intersection curve by selecting the front plane and this face here I can go to the tools menu under sex sketch tools and select intersection curve okay and that creates a new sketch for us at that intersection so now we can use that next reference so I'm going to create a new sketch on the front plane so I the front plane there and this again is just going to be a spline now I'm not fully defining these splines because it can take quite a while through this process to fully define a spline but you can do it within your own models it just means that this would be have slightly more less design intent so if you did want to make any changes to it afterwards be a little less easy to update so make the two ends coincident and then I can add in that curvature or tangency relationship by selecting both curves so I'll add in curvature there okay so it matches up and quite nicely follows the curvature from one to another and then I can just select the next edge okay I just want to make sure again I'm getting that relationship between the two edges so that it will it will mirror over nicely I want to make sure it be symmetrical on this edge so I'm going to add in a horizontal relationship about there and that quite nicely brings out you know quite a fluent curve from one edge to another the next item I'm going to insert in the next next surface I'm going to create is a boundary surface boundary surfaces are quite good for adding that yet adding in that continuity between different areas in the model so much like a loft I'm selecting the profiles in one direction so that will curve along and then I'll select the profile down here so we'll be essentially going across the model like that and you'll notice that I can select a whole edge all the way along and it doesn't seem to matter you know it's going to trim that back afterwards the next thing to do is select the profiles in the second direction which will be across the model like this so that will be this edge up here and at the moment you know it looks quite messy but you don't have to worry about it we can select all the edges and it does sort itself out in the end and we're still left with an area over here that we don't want to create within the surface but the options within a boundary surface allow us to trim them with trim the surface back by one of the edges so trim by Direction one cuts the surface in half and you can do that by Direction two as well if you've got it going across the model like that so next the neck make is to actually add in that curvature relationship without having it added in in the sketch beforehand we wouldn't now be able to add that between the two surfaces so we need to add it in to the sketches that help build up this design and we can increase the amount of influence that curvature is bringing across through the model the next relationship I'm going to bring on the other side and I want to make sure that I've got symmetry across from this plane here so we can add in a direction vector in order to make sure the surface will be pointing in the right direction so I'm going to use this plane here and that will build up again that symmetry in the design I'm not going to add in any kind of continuity in the other direction direction one because I don't really need it across the surfaces this way so that will actually complete and create my surface now so get quite a nice boundary between the two surfaces okay now that's been career sketches away get rid of them the next thing to do is to actually create the next set of surfaces to actually finish off the shape now what we're left with are a set of three-sided surfaces as you'll notice all the surfaces we created so far these two within the design have both been four-sided which works quite well within SolidWorks we do get slight problems when we're creating three-sided surfaces and it's just to do with the way that sort of which creates the surface so it's worth having a look at that now so as you notice in this picture we've got surfaces being created with what's known as UV curves a grid that that helps describe the surface so obviously we need four sides to be able to construct that grid when we get a design with say more or less than four sides it can cause slight problems within SolidWorks you will be able to create these surfaces but but you will get what's known as a singularity where the curves in one direction or join up to each other and this is known as a degenerate surface so in order to get around this we can use slight techniques to make sure that the surfaces we're creating are quite nice and have that underlying structure built up quite well so we can use the trim or surface fill command in order to get a nice result out of our surfaces and we'll have a look at how to use those now the first one I'm going to do is just to trim this surface back to create four sides normally I'd do that just by creating a 2d sketch but in this example I'm just going to go in actually create a 3d sketch again to show off one of the other techniques so when we're creating splines we can also create what's known as a spline on surface which allows me to draw a spline which perfectly follows the curvature of a surface as you'll see there so it's a real useful tool when you're creating curves within SolidWorks and you want to match Mach two surfaces perfectly so I'll create a second one now in order to make sure a nice curve on this section I'm going to add in a long X relationship here again for that symmetry and just drag out this drag handle to get a nicer curve there okay so I'm going to go ahead and actually trim the surface back using that edge so I'll exit the sketch and from the surfaces toolbar we can use the trimmed surface tool it allows us to select a particular trim tool like this sketch and then in the sections to remove or keep box which is below we can then choose the areas of the surface that we want to get rid of okay so we've got a standard and a mutual trim type standard just let's use a trim tool to trim one surface Mutual allows you to trim two surfaces against each other so it is quite useful way of doing it so I'm in this particular example I'm removing this area in purple here and that actually means I've created a four sided surface from what was a three sided gap there so it means that when we go to create the surface it will have nice UV curves across it to actually construct the design the next example is using the fill command I'm going to do that in this particular area here at the moment to use the trim the the fill tool sorry we need an edge it will go along the design and stop at the boundaries between the three edges at the moment these edges follow it all all the way along the design and that's because these services aren't joined together they're just booting up to each other essentially in order to join the walk we need to use the knit surface command at the moment we've got four surface bodies by using the knit surface we can turn those into one so on it items together and we can close any gaps that are created by sliding consistencies in the way that surfaces are created and that then creates one surface body and it means that the edges here will stop where we want them to okay so then I can use that filled surface tool in order to create my surface okay now in here you think a good thing about it is that we can apply that continuity between the surfaces on the two edges that I've got across here you can see highlighting I'm going to apply a curvature relationship which pulls the surface into position I don't need curvature or tangency on this bottom edge I'm going to leave it as a contact relationship we're going to have a look at the other options in this area later on the only thing I'm going to do is to turn on this optimized surface tick box which is mainly used for four-sided surfaces but then we do get a resolution control pop-up this allows us to increase the quality of the surface but it also increases the rebuild time with the design so you'll see the filter is actually creates a surface for us we don't have to worry about going in and creating ourselves it does all the work for us and actually sorts out the surface itself so it automatically creates a surface has a four-sided item and trims it back to create a nice face curves on there okay so the next area is to create a loft in this area at the top I'm going to open a model that I created earlier on to do that because I'm already shown how to actually create a loft within SolidWorks okay and it just leaves us with a design you can see the curves created nicely across this surface the only thing to point out is the start and end constraints that have been applied we've got tangency to face applied on edge one and on edge two we've got a direction vector to again keep that model SILS it will mirror across nicely at this point I do want to actually create a knit surface from this I'm actually left with three surface bodies once more because of the new surfaces that I created so I want to create one surface body out of them and that allows me to go on and then create a solid model so I use the knit surface command once more in order to knit these together and I can form a solid form them now with this new tick box that appeared my pair can also merge those entities so forming a solid is the ultimate objective of any surface model so seeing is a way of creating the more complex organic geometry but you do want to create a solid model from it eventually and by using the knit command we can do that the other way to do it is to use a thicken command which allows us again to create a solid model from the design if we've already got one surface body the next thing to do is to actually mirror this item over before I do though I want to create one more part of the model if we bring back that sketch picture we can see there's a slight concave area here where the scroll wheel is on this mouse so I'm going to create that on the design I'm going to actually put that in before we move the surface over in order to make it easier to create so I'm going to do a new sketch on my top plane I'm going to split this face into two I'm adding in horizontal relationships on these curves here by dragging out those drag handles and then I'm going to actually take away that solid body so I can see the escaped picture underneath and then I can match up my spline a bit more accurately to that sketch picture okay so fairly happy with that actually it looks like it matches up with the profile nicely so now I can project this sketch directly onto the surface to split it into two to do that I use a split surface tool using a split line so select the sky in the top box and then I can select the face that I want to split in the second one by having unprotected it allows us to project the sketch onto the surface and then split it into two okay and now our position where I want to mirror the surface over so I'm going to go to my features toolbar and mirror it like any other just using the mirror tool I'm going to select this planar face that I created first of all as the face to mirror with and then I'm going to mirror a body rather than a feature because it's far more robust it means that we go in and make changes to this original design say deleting a feature then the mirror in the model will still be created okay so that's nicely created the mouse now is actually looking a bit more like what we intended it to the last thing to do is to actually create this surface I'm going to put in some more curves in order to control the shape of it though so I'm going to do one get on here and that's going to go from the end of that split face okay and join up at the top there and I'll just adjust the profile slightly of that okay just drag out the drag handles okay so that gives me a curve something close to what I'm looking for and then I'm going to similar curve in the other direction so I've already got a sketch plane I can draw in that sketch plane too and I'm going to use another spline in that direction to define that again I'm going to use that Pierce relationship to join it in in the right place so Pierce it on either side and I'll also Pierce it to that sketch that I've just created in the middle so I've got curves which define the internal shape of that concave area and I've got the split face which defines the external shape of it so now I can use the surface tools again in order to create a filled surface here to match up to that so again in my boundary boxes you select those two edges and using constraint curves I can add in those two sketches that I've made and they will help define the surface shape okay so that at this that would just create the surface but it's not actually going to merge up or trim them up in the model at all in order to do that I can tick the merge results box and it will actually cook the design we may have to just flip the direction by hitting this box though so let's see how that looks we can see let's trim the model quite nicely so the only thing left to do would just add on a small Philip just to finish it off okay so that's that actually looks quite close to the design we're going for now so hopefully that's given you a good idea of the kind of tools you can use when you go to create a nice surface within SolidWorks and the kind of ways that you might apply surfacing to help your design thanks very much for watching and I'll just point out at this point the future webinars that we've got coming up we've got one on the 19th of April setting up the workgroup volt we've got one on the 26th of April and performing a clean uninstall and they've got we've got one on the 3rd of May by an introduction to flow simulation so again thanks very much and I will just stay on the line for a few minutes just for any questions that anyone's got okay I've got one question here asking is if there's any easy way to actually define a spline within the model one of the best ways of doing is actually just drawing your sketch out normally with with lines and arcs and then using the fit spying command you'll find that under tools and spline tools it allows you to then define your sketch normally and fit a spline around those entities okay if there's no more questions we'll end the webinar there thanks very much for watching

Channel: Innova Systems - Experts in SOLIDWORKS Training & Support

Views: 655,399

Keywords: SolidWorks (Software), surfacing

Id: fA2-i34UVUo

Length: 37min 27sec (2247 seconds)

Published: Mon Apr 16 2012