Join John Helfen for an in-depth discussion in this video Create an extrusion to next face, part of Autodesk Inventor 2018 Essential Training.
- Let's go ahead and take another look at a different termination type within in the Extrude command. We're going to use the two next termination.IPT as a starting point. To begin, we need to right click and select New Sketch and we're going to select the interface here that we can see on the model. As that sketch is created, you can see it's rotated, but we have a problem. The geometry that is in front of it is blocking our view. If we rotate, you can see that all this geometry is blocking us seeing what's on this sketch plane.
If you right click in the graphics window, in the right click menu, you'll find an option that says Slice Graphics. It's also F7 on your keyboard. Go ahead and select that and you'll see that the geometry that was blocking our view has now been removed and this is a temporary option. The F7 on your keyboard will toggle that and each time you click, it will toggle either on or off depending on its previous state. We'll go ahead and leave it off and rotate back to a right view so we can see clearly. Now we're going to right click and select Center Point Circle and we're going to create a circle anywhere on this face above this line on the axis line.
It doesn't really matter where it's positioned or how big it is. We really just need something we can extrude. We can now finish the sketch. We can now go ahead and right click and select Extrude and what we'll find is Inventor selects the one profile we just drew and it extrudes that. By default, it extrudes it to one inch. Now, we can look at this from the front view and remain in the distance option and could simply use the heads up display to either drag it out to the next face or we could even drag it a little further so that it intersects with this piece of material.
If we select the green check mark, you can see the model looks correct. The shape we drew is extruded between this face and the next face. The problem we have here is while the model looks correct and it is, it actually accomplished what we want it to to extrude from one face to the next. Because Inventor's a history based modeler, we can go back in time and make changes to the features that existed before this Extrusion-3. For example, if we were to go to the browser and right click on Extrusion-1 and select edit sketch, we can return back in time to when this sketch was created and we can increase its distance to 2.5.
When we click enter, the geometry's updated and when we finish the sketch, so is the model. Now you can see the problem we have. When we were creating Extrusion-3, we set it to a distance and then we manually moved the distance so that it intersected. What we didn't account for is the fact that people could go back in time and modify Extrusion-1 essentially breaking Extrusion-3. To fix this, let's go ahead and right click on Extrusion-3 and select Edit Feature. This will return us to the heads up display that we used to create this feature in the first place and again, we can rotate to the front view.
We can go ahead and manually drag this out, but we really haven't solved the problem. The problem we have is we need to change the type of termination. In the heads up display, just to the left of the distance, is a drop down arrow and within this, we have the option to set distance which is what we have now, or we can choose other termination types. We can select To face and body, we could select To selected face and point, or even Between two faces or planes. They all will generally work here. We're going to focus on this one here, the To next face or body.
If we select this, you can see Inventor evaluates the previous features and finds the solid model and uses that as a way to solve the answer here. What it's done is essentially taken that shape and extruded until it hit another solid body or face. If we select Okay, or click the green check mark, and return to our home view, you can see that our model has now been updated. The nice thing now is if we return to Extrusion-1, right click and select Edit Sketch and this time bump this up to three inches, and hit enter, if we finish this sketch and return to the model, you'll see that the model updates appropriately and Extrusion-3 does extrude completely from one face to the next.
The nice thing about this is the first based feature isn't the only feature that could have effected this. We could, for example, edit Extrusion-2. If we right click on Extrusion-2 in the browser and select Edit Sketch, you'll see that we have several dimensions that we can modify. Two of these dimensions are driven by functions, you can see the FX label here indicating that, which means this is the dimesion that's the driving dimension. If we double click on it, we can set this to .25, hit enter on our keyboard and we've now essentially moved each side of the cut further away from where it started.
If we finish this sketch, you can see that the model updates still solving the problem that we originally ran into, even though this face moved back, the original sketch that we drew moved back with it, which theoretically should have, if we had used the distance termination, would have caused this to move back as well, but because we choose to extrude to the next face, the model automatically updated and we didn't have to rebuild things from scratch. Hopefully you can see how powerful this can be and you can keep this in mind as you're creating features because this will be the same for all features, not just the Extrude command but this is something you need to consider throughout the entire part modeling process.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers