Create digital components

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Create digital components.

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After completing this video, you'll be able to

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create a fully dimensioned and constrained sketch,

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create a 3D model using features,

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modify a model with filets and champers and

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apply surface features to create or patch complex shapes

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to get started.

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We want to make sure that we have the supplied data sets,

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undefined flange and lofted bodies dot F 3D open.

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We're going to begin with the undefined flange and note that in the body's folder,

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this is currently a surface body.

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Some of the features have been removed and we need to

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begin by patching it and creating a solid body once more.

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For now, let's expand the sketches folder and hide the sweet path.

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When we rotate around to a right view,

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you'll notice that we can see the inside edge of this opening.

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But if we happen to rotate it around to a left view,

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you'll know that the opening is actually tapered.

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So we're gonna use our surface tools to fix this opening in this

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design and we're gonna make sure that the inside is no longer tapered,

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just like with everything in CAD.

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There are multiple ways that we can approach this design.

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For example, we can take this edge and we can try to use the extrude option.

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When we extrude this out,

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you'll notice that there is a gap because of the tapered opening.

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If we select the back face of our design

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fusion 3 60 will automatically measure that distance,

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it's going to continue to use the extent type distance.

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And we can also change it to object, select the same face.

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And now there's going to be a parametric link.

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Meaning if the design changes before this point in our timeline,

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the feature will also update.

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Let's go ahead and select. OK.

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The second thing that we want to note is there's a small gap here.

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And in order to fill that gap once again,

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there are many different ways we can approach this

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if we try to use the patch tool and select the outside border.

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Notice that we're not able to select the inside.

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This is OK because we can use this patch and trim away the section we don't need,

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we're gonna select trim

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using the inside cylinder as our trim tool.

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And we're gonna remove the inside section of that patch.

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This leaves a perfect intersection between all surfaces.

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Once again, there are multiple ways that this could be done.

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For example, you can use tools like extend or even create and ruled surface

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for now, let's go ahead and stitch all three of these together,

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the extruded cylinder,

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the patched face and the original body.

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Once we select all three of these, notice that as soon as we click, OK,

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we now have a solid body

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for this.

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We're gonna navigate over to our solid tools and

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take a look at this sketch bolt pattern.

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We can tell inside of the browser that bolt pattern

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is undefined because it doesn't have a lock icon.

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Instead it has a pencil icon.

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If we right click and edit this sketch,

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we'll also note that one of these holes has a diameter value,

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but all of them are displayed blue because their location is not set.

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What we're gonna do is we're going to begin using constraints

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and dimensions to fully define this sketch before creating our bolt holes

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using the equal constraint.

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We're going to select each hole as we move around,

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selecting the 15 millimeter diameter hole as our seed or first selection.

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Next, we're going to use the horizontal vertical constraint

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to make sure that the center points of these holes

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are always horizontal or vertical relative to each other.

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The next thing that we want to do is add a few dimensions

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with our sketch dimension tool.

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We'll dimension the center point of this upper left hole

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and we're going to set this at 15 millimeters,

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we're going to set the vertical distance

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by selecting the 15 millimeter dimension we just created,

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this is going to fully define the hole in the upper left hand corner as

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well as the vertical position of the hole in the upper right hand corner.

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However, we still need to give it a position to the right.

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Once again, we're going to select that 15 millimeters and say, OK,

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we need to add one more vertical constraint between the center points of these holes

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and then we can add one more dimension.

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We're going to add a vertical dimension

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once again, 15 millimeters and now all four holes are fully defined.

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We're gonna finish our sketch and use the extrude

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tool to create and extrude through our part.

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We'll select each of our profiles,

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we'll rotate the design around and select the option to object,

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selecting our back face.

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Once again,

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using two object will allow us to create those holes in

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a parametric relationship with the back face of our part.

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The next thing that we wanna do is we want to consider the sweep that we need to create,

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but we're gonna be creating a solid sweep off

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of a surface that hasn't been created yet.

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Once again, there are multiple ways that we can do this.

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But let's explore our surface tools. Once more,

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we're gonna go to create an offset,

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select the inside face and create a five millimeter offset surface.

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This is going to represent the id of the new

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piece that we're gonna use as the base for our sweep

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to turn this into a solid body. I can select, create and thicken

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and thicken this in the outward direction minus five millimeters

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and select the new body for the operation.

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This is gonna contain the original offset surface

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as well as the new thickened solid body.

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From here. We're gonna be using the face of that solid body as the basis for our sweet.

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So from our create menu and our solid tools, we're gonna select Sweet.

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Our profile will be the face of the new solo we created

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and the path is going to be the sketch.

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Notice when we do this,

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that there are areas where we do have some of the geometry bunching up

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for. Now, let's go ahead and select. OK. But go back to our sweet path.

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I'm going to right, click on the sweet path sketch and select show dimensions.

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I'm gonna modify the radius of 25 millimeters to 30 millimeters,

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increasing that radius and removing the bunch in the corner

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by using this show dimensions.

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We'll be able to see the updates in real time on

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the screen without having to edit the sketch that was created.

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Well before all of these features,

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let's go ahead and hide the sweet path sketch and take a look at our results

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because the sweet path had joined turned on and our thickened

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solid body had an intersection with the original extruded block.

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All the solid bodies were joined together,

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that's OK in this instance.

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But this is something that we should pay close

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attention to any time we're creating new bodies.

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And we do want to join them to specific entities

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rather than all of the solid bodies in the design.

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One way that we can fix this is by hiding the original solid body.

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When the sweep is getting created.

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Now, you can see we preserved two bodies.

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We have the original body and then we have

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the sweep with that five millimeter thick extension.

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Once again,

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these are just things that we should pay

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attention to when we're creating our designs.

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The last thing that we want to take a look at

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in this design is a sketch that's called key cut.

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We wanna right click and edit this sketch and hide the bodies inside of the browser.

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When we take a look at sketches with projected edges,

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even if the bodies are hidden inside of our browser,

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we still can maintain closed profiles by using

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the overlap between these projected or intersection curves.

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This can be extremely helpful,

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especially when creating sketches that are inside of complex bodies.

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Before we save this design,

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let's go ahead and apply a couple filets and champers to the model now.

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So to do this, we're going to go up to modify and select either file or chamfer

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first, we'll select file

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and notice that the type of file is set to fill it.

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But we also have rule and full round filets.

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The rule filet will allow us to apply

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filets that are at the edges of selected features

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as it is extremely handy when you have an extrude that has a lot of internal edges,

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you can determine whether or not you want them

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applied to a specific feature such as an extrude.

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And then you can determine whether those are all edges or just

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between certain faces and features such as internal filets or external radii.

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We also have full round filet which will allow us to select

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a face and create a full round filet based on the adjacent faces

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for our example.

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However,

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we want to select file and then begin selecting and

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applying filets to the outside edges of our plate.

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We're going to select the edges and note that if you can't select through your model,

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oftentimes double checking your selection filters to

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make sure that select through is toggled on

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will allow you to easily select all the edges without having to rotate.

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I'm gonna apply a 10 millimeter filet hit the plus to add the selection set

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and then we can select an additional edge and

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apply an additional filet feature at a different size.

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We're gonna say OK for that filet feature. And then we're going to apply a champ

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champ for has a similar dialog box.

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In this case, we can use equal distance, two distance or distance and angle.

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We can also toggle different types of corners.

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If we're using three intersecting edges.

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For this example,

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we're just going to place a small chamfer on the outside of one millimeter and say,

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OK,

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applying fits and champers to a model can finish off the

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design and you can always go back and make adjustments.

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For example, if we want this radius to be smaller,

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we can reduce it to one millimeter and then select OK.

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It's important to play around with all the various options inside of

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filets and champers to make sure you're comfortable with all of them.

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Now, let's do a quick save

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and then let's move on to our lofted bodies.

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For this example, we're gonna be using the create a solid loft tool.

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We're going to select loft and we want to

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go from the bottom profile to the upper profile

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using just the two profiles will create a

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solid loft without needing any additional rails.

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We also have the option to change the starting

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and ending profiles by driving them based on a direction

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simply using direction or if you've selected an edge

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of a solid or a surface tang agency or

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curvature continuity can drive the shape that you're looking

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for without the need for additional rails or constraints.

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However, in this example,

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let's go ahead and take a look at adding

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additional rails since we have them in the sketch.

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When we add a single rail, notice that it pushes the entire loft design to the right.

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If we add a secondary rail,

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it will allow us to maintain more of a symmetric relationship.

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When we're creating lofted bodies such as these,

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we need to consider various factors when determining

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what our loft inputs are gonna be,

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whether or not the design needs to be shelled. In this case, a thin wall body

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will determine how these lofts come together.

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As you can see, it looks like we've got a small crease in this area.

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Let's go ahead and select, OK,

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and take a look at the shell tool, selecting the upper and lower faces of this design

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and using a two millimeter thickness.

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When we select a two millimeter thickness,

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we've now created a thin wall body based on those lofts,

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we can go back at any point in time and add additional constraints or curves.

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So for example, we have these guides.

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But inside of the sketch browser, we also have a second set of guides.

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Even though we've added a shell in the timeline, we can double click the loft tool,

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go back to add additional rails

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and drive the shape on the front and the back.

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This will help relieve some of those bunches or

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creases that we saw happening on these outside faces.

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We're gonna select OK. And note that the shell updates properly

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using additional guide rails or working with symmetry.

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Whenever you're creating lofts.

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In this case, a solid or a surface loft can be valuable to the overall design goal.

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In this case, our lofted guides were symmetric about the origin,

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which means that we could have worked with just a quarter section of this design.

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Next,

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let's work on rolling the timeline marker back before the

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shell and make some additional modifications to the design.

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We have a sketch called split profile.

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The split profile sketch is going to be used to split the body.

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When we're looking at the splitt tools, we have three options, splitt face,

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split body and silhouette, split.

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In this case, we're gonna explore the split face and splitt body tools,

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split body will allow us to use planes,

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surfaces or sketches to separate solid bodies.

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For example, in this case, we want to split the solid body

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using our sketch profile.

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When we take a look in the browser under the body's folder,

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you can see here that we've got body two and body three.

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If we hide body three, we're left with just this rectangular profile.

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If we hide body two, you can see that we've cut all the way through the solid.

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If this wasn't the intention, then let's go ahead select and delete the split.

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We'll show the solid body. And this time we want to take a look at using split face.

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We want to make sure that we bring the split profile sketch back.

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And this time instead of selecting the entire solid body,

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we're going to use the splitting tool just to separate the top face.

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If we hide the split profile sketch,

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you can see now we still have a single solid body,

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but we're able to divide the top face.

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We also have another body in this design called plug.

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This plug design is going to be removed from the bottom of

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our design and this can be done with a couple of different tools

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we can use, modify and combine

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or we can also use the option to create a boundary fill

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for this design. It's going to be easier for us to use combine

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selecting our target body,

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our tool body

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and the operation type of cut

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note that we can use the keep tools option to keep the plug in the design.

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And this case will toggle that on and say, OK.

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Now, if we hide the plug, that geometry has been removed,

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we've made some changes to the design and altered the

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faces that were used for the initial shell selection.

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So if we drag the timeline marker forward,

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you'll notice that we might not get the appropriate result.

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Let's right click and let's edit the shell feature.

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Instead of selecting this wall, I'm going to hold down the control key,

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remove that selection and then hold down control

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again and reelect the interface of that plug.

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Now, if we take a look at the results,

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we've removed material from the inside of the design.

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However, the outside of the design isn't working well either.

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So let's go ahead and edit this one more time,

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holding down the control key and selecting this inside face.

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Now,

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you can see we've removed all the material as intended from the inside of the part,

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the selection process is extremely important,

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especially when you make changes to a model before a timeline feature has happened.

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So make sure that you do understand the

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implications of when features happen in a timeline

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and how to use those tools appropriately

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at this point. Let's make sure that we do save the design before moving on.