Surface creation for complex geometry

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Surface creation for complex geometry.

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In this video, we'll use delete for solids and surfaces.

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We use split face, create a lofted surface, a surface patch and use Stitch.

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In Fusion 360, we want to get started with the supplied dataset sandwich container.

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Oftentimes when we're working on new designs, we have to use surfacing tools to get the geometry just right.

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In this case, we're dealing with a plastic molded sandwich container.

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We need to add some indents features on the bottom to add a little bit of structure and give it away to nest into another container.

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In order to do this, I'm going to start by expanding my sketches and showing my split sketch.

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The split sketch is going to allow us to split the bottom face and this will give us an area to work in.

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This bottom sketch has an offset from the edge,

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and it allows us to see different areas where we're going to have a recess or an indent and a transition area.

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In order to do this, we're going to start by going to Modify and Split Face.

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We're going to select the bottom face of the container.

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And when we go to select our splitting tool, we're going to begin by selecting the outside and saying, OK.

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We'll need to bring that split sketch back and we'll need to use the split tool again.

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This time we're going to select the inside face and the tool is going to be this inside edge.

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And we'll repeat it one more time selecting the inside face again and this inside edge here.

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The reason that we need to do this is because we want to identify the areas that we want to modify the geometry.

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So the first thing that we want to do is we want to talk about the use of the delete tool,

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and how it's different when we're in our solid tool set versus our surfaces.

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For example, if I were to select this face and simply hit Delete, Fusion 360 patches the surrounding geometry for me.

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If I use Undo, navigate to my surface tools and I select that same face and hit Delete,

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it's going to remove the face from our geometry and it's going to turn this into a surface body.

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We expand our Bodies folder.

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You can now see that we have a surface body made up of 223 different faces.

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We're going to select and delete that other face as well.

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And then we're gonna use our offset tool under create to offset this small face.

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When we make that selection, notice it's trying to grab everything because chain selection is on by default, really we just want a single face.

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We're going to bring it down a distance of a 0.25 millimeter.

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That's very small.

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But oftentimes when we're dealing with molded plastic components, a small amount of geometry can add a huge amount of structural integrity.

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So with that new minus 0.25 offset I can then select the original face and delete it.

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When we're looking at this, we now have a small offset face that's on the inside.

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And when we hover our cursor over these edges because we originally split the faces up multiple times,

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what we now have is a division here or vertex that we can select when we're going to create the transition between these two.

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The next thing that we need to do is we need to consider whether or not this geometry needs draft.

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If it does need draft, then we need to reduce the size of the shape.

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There are tools such as extend that can be used to change the size or shape of different surfaces.

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If we select the edges of our surface, I'm going to grab the inside and outside edges.

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And begin to drag them in, notice that it's not allowing me to reduce the size.

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However, if I drag them out, it will allow me to extend them.

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So because of this, it's not allowing me to create that offset.

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I'm going to need to use split or trim to remove additional material.

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So I'm going to right click and create a sketch on this.

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Then I want to use my offset tool.

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I'm going to select the entire outside profile and I'm going to offset it in a small amount in this case, minus 0.125.

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That small amount, I also want to make sure that I take a line and I extend it out tangent all the way to the original edge.

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Because I do have that vertex selection on the outside, I want to make sure that I maintain that position.

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This needs to happen on the other side.

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Once again, I’m maintaining tangency with that original edge.

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I'm going to hit Escape.

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I'm going to select this line and I'm going to convert it to a construction line.

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We'll do the same thing on the other side, making sure that that is not going to be a valid selection.

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We'll finish the sketch and now we can use our tool such as trim to remove additional material.

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We're going to start with our selection being this edge and then we need to select the area to trim and say, OK.

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That sketch is still visible after the trim tool so we'll rotate slightly and we'll repeat the trim.

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We're going to use this as our trim tool and remove that small area on the outside and then we can hide that sketch.

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Now let's rotate around to a bottom view.

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And if we want to, we can also rotate this.

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Now we can see that this offset surface is slightly smaller and this gives us a great opportunity to create a loft between those faces.

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I'm going to rotate this around and take a look at my create tools.

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Loft will allow us to go between two selections.

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So first I'm going to select this rail but we need to keep in mind that we have these small sections on the outside.

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So I want to make sure that I grab all three sections for that initial profile,

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and then I'm going to hit plus to create a new profile selection and grab this edge.

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When I take a look at this, you'll notice that it is creating a new surface.

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We'll have to rotate around to see it because of the colors.

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But you'll notice that it's creating that new surface.

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It's connected at the top and bottom.

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But if we want to have a smooth transition, we can add tangency to both of those or curvature.

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In this case, I'm not going to add curvature,

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simply because the faces that I'm dealing with are flat or planar on the bottom of the container in this offset.

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But notice that when we do have that small amount of transition, we can also affect things like the tangency weight.

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To reduce that if we only want a very small amount of that transition.

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We can also go back and we can increase the offset where we were creating that transition.

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Instead of using an eighth of a millimeter, we could go back and make it a larger offset.

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If we want to do that, we simply need to go back to Sketch9, edit the sketch and take a look at that dimension.

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So in this case, that minus 0.125, I'm going to go to minus 0.3.

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I'm going to finish the sketch and then I can go back to my loft, select those tangencies,

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and now I can increase that back to one or make it even larger if I wish.

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I’m going to increase this to one as well and say OK.

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We're going to follow that same procedure on the other side creating a new loft.

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Once again we need to make sure that we select all three of those sections for that profile.

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And then for our second profile, we simply need to select that inside edge and make sure that they are tangent.

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Now that we have those two selections, let's go ahead and use a tool called Stitch.

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We're going to stitch these three sections together and we want to combine them with the bottom of the housing.

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This leaves some open areas and that's okay because we still need to fill those in.

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Once we combine those, we can go back and create a new loft.

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We're going to select this edge as well as this edge and note if we view this from the bottom, we bring this into focus.

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We can actually take the endpoints and drag them in.

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So that way the loft isn't going all the way to the edges.

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When we do that we also want to make sure that we are adding tangency.

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When we drag those edges in and we say OK, what we've actually done is we've created a division,

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a division that we can select and delete, leaving just that small section.

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Once again, we want to stitch, selecting everything to combine it together.

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And now we can use another tool called patch to fill in this open area.

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We're going to group all the edges together so that way tangency applies to all of them and say, OK.

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Repeat the process by repeating the patch on the other side.

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All the edges are grouped and we'll add tangency and say, OK.

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So now we've added these smooth transitions, we want to stitch those together.

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And then repeat the process one more time on the other side.

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As you can see, the process of creating this geometry does take a little bit of time.

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The good news is that once you create these surfaces,

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you can go back and you can create patterns or mirrors based on the way your original geometry was created.

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I'm going to say, OK, I'm going to delete these edges.

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I'm going to stitch everything together and then I can use my patch tool to create that surface patch in that area.

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Once again, it's important that we always go back and we remember that when we create this loft,

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we always want to be mindful of how it connects to our surrounding surfaces.

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If you forget to create that tangency, what's going to happen is downstream.

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You're going to get areas of your surfaces that are not going to be smooth.

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Once again, we'll make sure that everything has tangency.

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We’ll repeat the process one more time on this side and then we'll stitch everything together.

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Once we stitch the main body back together with these two surfaces, let's pay close attention to what happens in our Bodies folder.

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Once we say, OK, because we've now created a closed region, it converts it back into a solid body.

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This means that we can come to Inspect, take a look at a section analysis.

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In my case, I'm going to select the YZ plane.

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I'm gonna drag it over until we get into that geometry.

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Now, we can take a look at how far into our container that goes whether or not we need to create the same sort of indent on the inside.

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If we want to do that, we can use our offset tool and we can take our surfaces that we’re interested in,

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and we can offset them inward and then repeat the same process, creating those splits and those new lofts and patches on the inside of our container.

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For our purposes however, I want to go back, hide the analysis.

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Make sure I navigate back to my solid tools, minimize my sketches folder and I want to save this design before moving on.