Join John Helfen for an in-depth discussion in this video Create splines, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to begin exploring the spline command. What we'll do is we'll take the steps we used in the previous movie when we learned about rectangles and arcs, and rather than using arcs to create the shapes on the mouse we'll replace those with splines. Splines are significantly more advanced than arcs, in the sense that rather than three points, you can use a large number of points to define an overall shape of the line. What I've done to speed the process a little is I've created a starting point cube so that we don't have to create that again. If you want to learn how we got to this point, you should review the rectangle and arcs movie.
To begin, we're going to select the face on the side of the model and use the heads up display to create a sketch. The button on the right is Create Sketch button. Once we do that, we're in a sketch again. We can pan over so that we can see the model clearly, and we're ready to begin. Now a spline is just a type of line. So we're going to go to the Sketch tab under the Create panel and we're going to click the expanded menu under the Line command. You'll see that we can create a line. We can create a spline with control vertex points. We can create a spline with interpolation, an equation curve or a bridge curve.
We're going to select the Spline Control Vertex. What this does is allows you to create a series of points that the line is going to flow between. This helps you get very nice, smooth-flowing lines. We're going to do things slightly different than we did in the previous movie too, rather than project all of these edges to this sketch. We even talked about an application option that would automatically do that. This time what we're going to do is look at a different path. Inventor will automatically project edges as needed. If we hover over the left vertical line, and we find its midpoint by hovering near it, and waiting for the green line to pop up, you'll see that the line has become black.
If we left click, we'll create a coincident point at the start point of this line. When we're finished, you will see that Inventor automatically projects that edge to the sketch, so that we can reference it. Next we need to create the control points. We can do this by simply hovering above the top horizontal line and left clicking. Then as we move our cursor, you'll see that the line is actually being curved, based on where we're placing the next control vertex point. We're going to select a point somewhere near the middle bottom of the model.
Then we'll repeat that process again up at the top right. Finally, we'll finish up by left clicking on the vertical edge on the right near the top. Once you've done that, you can click the green check mark, and the geometry is created. Just like I mentioned, the start point and end point that ended on those vertical lines were automatically projected to the sketch. They're the yellow lines on the vertical sides. To finish this up, we could do some fine tuning. Like I mentioned, we can left click and drag on these vertex points to adjust our spline.
We can also dimension these, both the construction geometry and vertex points if we need to, but I like the general shape that was created, so I'm going to stop here. The one thing we need to do before we finish this sketch is to either project this edge or draw another line that connects the end points of these two reference lines. Rather than project like we did in the previous movie, let's go ahead and just create a new line. We'll right click and select Create Line. We'll hover over the end point of that line, and then we'll hover on the end point of the other line.
We now have a closed loop between the spline and the reference geometry that we've created. We can go ahead and click Finish Sketch, and we're now ready to extrude that. If we right click in the graphics window, you can select Extrude. Inventor again, automatically will select the single profile that was available and it automatically tries to add geometry. Here, it's set the value one inch. We'll make a couple of changes here. We'll change the operation from a join to a cut. Then we'll also change the extense of this extrude from a Distance to a Through All by clicking the arrow to the left of the distance value.
When we finish this by clicking the green check mark, the changes are applied and you can see the overall shape of the mouse. If we look at it from the front view, you can see that is has a nice curvy shape to it. We'll return to the home view and we're now ready to create that same shape on each side of the mouse. To do that, we're going to left click on the bottom corner of the view cube so that we can see the bottom of the mouse. Then we're going to left click on the bottom face of the mouse and use the heads up display to create another sketch. Now I'm going to use the view cube to rotate this 90 degrees so that it's in the proper orientation and we're ready to continue the process.
We'll go ahead and return to the Create panel and select the Spline Control Vertex from the drop down menu under Line, and we'll repeat that process. This time rather than using the midpoint on the vertical line, I'm going to move up a little closer to the top and I'm going to left click to place the start point of the spline. Then we'll follow the same steps we did previously, placing the control vertex points. We'll left click above the horizontal line. We'll left click somewhere in the middle, below the horizontal line. Again above the horizontal line, and then we'll finish up on the right vertical edge.
Once you're done, you can click the green check mark, and your geometry is created. Now I'm going to make some minor adjustments here so that we see a little more curve to the side. I'm going to left click and drag the start point of the spline down a little bit. I'm going to drag the bottom control point down a little bit and I'm going to move the far right vertex up just a hair. I generally like this shape so I'm going to stop there. You can go ahead and fine tune as much as you'd like. The final step we need to do is close off this profile.
Right now it's open on either side. What we're going to do is either project this edge, or in this case let's go ahead and just draw a line that connects those two points. I'm going to right click and select Create Line from the Marking menu and then hover over the end point of the vertical reference line. Left click to start the line and then left click on the other vertical point in order to close that shape off. We can now finish the sketch. We have the geometry we need. So we can right click and select Ok to get out of the command and hit Finish Sketch on the ribbon bar.
We can now right click and select Extrude. Again, Inventor selects the default single profile. Adds geometry. We'll change the operation from a join to a cut. We'll change the extense from one inch Distance to Through All and select Ok. We now have the basic shape on the side as well, but we need to mirror that over. So at this point, we've learned how to create splines, and just like the previous movie, I'm going to use a few extra commands that we haven't looked at too much, and we're going to go ahead and finish this model off.
In the 3D Model tab, there's a Pattern panel that has a Mirror command. We're going to launch that. We're going to select the feature we just created, which is this curve on the side. Then in the dialogue, we're going to select the Mirror plane and we're going to go to the Origin Geometry, click the plus symbol to expand it, and select the XY Plane. This is the plane I sketched on originally to create the starting model, and it runs right through the center of this geometry. By selecting that, you can see a preview of the geometry mirrored and clicking Ok will mirror that geometry.
We can now finish this model up with some fillets. I'm going to go ahead and select the vertical line in the front, and then use the heads up display to create a fillet. We'll do the same by selecting each of the vertical edges around the model. I'll set this to .5, which gives us a nice rounded shape. I'll click the green check mark to finish that, and then we'll wrap this up by selecting the top edge, clicking the fillet from the heads up display, and in this case you see an error. .5 is a little too big for this, so we're going to go ahead and go to .25, which should shrink it down so that it fits nice and evenly around the model.
We'll go ahead and click the green check mark, and we've now completed this shape. If we rotate around a little bit, you can see the curvature in all directions.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers