Create Pier Model

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Hello, my name is Thom Tremblay.

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In this course, we'll be taking a look at an overall bridge design workflow.

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And in these lessons, we'll be focusing on how Autodesk Inventor can be used to create custom components,

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to be used in InfraWorks for your bridge designs.

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In this lesson, we'll focus on preparing a pier component for use in InfraWorks.

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We'll focus first on building a component using parameters that are already included in the file.

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When creating complex designs in Inventor,

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it's ideal to include named parameters that tell users and editors down the line what those parameters are being used for.

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You can create these parameters on demand, use sources like spreadsheets to import them in mass, and share them through multiple files.

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Or you can even prepare templates that already include the parameters that you'll need to prepare your model.

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To prepare this model, we're going to start with the Hammerhead Pier Parameter Template.ipt file.

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This is a template that has all of the parameters that you'll need included in it,

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including three parameters that are required by InfraWorks to be able to import a pier.

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Pier height, pier cap left Width, and pier cap right width.

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In addition to being able to open a file that has the parameters,

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you also have the option of using the "Save As" tool to save any file as a template.

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This is a great way to start building up a library of the type of components that you need to create and have them accessible at any time.

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A pier component needs us to create the primary sketches on the xz-plane.

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So, I'll use the view cube to align the xz-plane normal to my screen.

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To make it easier to reference, we can rename this point of view to be front.

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And we can even set up a home view that will make it easier for us to review our work as we go through the process.

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We'll want to expand the origin folder, and turn on the visibility of the planes, axes and center-point there.

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Then we're going to create a UCS.

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A UCS allows us to establish additional coordinate systems within a model.

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These coordinate systems can be related to any other coordinate system and be able to reorient any sketch or feature based on them.

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We'll start the UCS tool and then enter a parameter that's already loaded into the model.

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For that delta x value, we'll use pier lateral offset for this value.

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Then using the Tab key, set the delta y and delta z to zero.

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Right clicking and selecting "Finish", we'll generate the UCS.

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And a double-click of the mouse wheel will zoom all so that we can see our original origin planes and the new UCS that's been created.

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Now, let's create a new sketch based on the model's original xz-plane.

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In this sketch, we'll begin to create construction lines.

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We'll start out with a short horizontal line, well above the origin, that's roughly 20 inches wide.

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Don't worry about centering it immediately,

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because once that's placed, we'll be adding another line from the origin to the midpoint of that horizontal line.

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Next, we'll project the origin center of the UCS that we created and create a vertical line based on that UCS point,

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roughly the same height as the last line we created.

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Then we'll apply a vertical constraint to the line that was drawn from the part of origin to the midpoint of the short line.

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This horizontal line will be used to reference the top of the pier.

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So, we'll establish a dimension from the origin to that line, we'll expand the dialogue,

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select "List Parameters" and choose the pure height plus vertical adjustment parameter for the dimension value.

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With the zoom all, we can see that this is increased to 520 inches.

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We can extend our construction lines to keep them in view as we zoom in.

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And now we'll begin framing the outline of the pier.

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We'll start the line tool and turn off the construction override.

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Then we'll start a line at the midpoint of the short horizontal line, drawing it down to the left at an angle.

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Then we need a short vertical line, roughly 20 inches.

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A chamfer at an angle.

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And a bottom line that goes to the construction line based on the UCS.

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Then we'll create the same geometry on the other side.

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Because I don't want to lock this into parallel with the vertical line on the left, I'll skew it slightly and then complete the geometry.

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Then we can add a vertical constraint.

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Now it's time to start adding dimensions.

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Again, all of the parameters that we'll need are already built into the part.

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So, as we place dimensions, we can place the angle.

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And we'll just start applying the dimensions.

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So, the first one will be the pier cap top left slope dimension.

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Then we'll use the pier cap right slope.

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And we'll go back and forth between these pairs of dimensions.

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Using the left pier vertical face and its mate on the right side,

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we can use the left pier chamfer vertical, the left pier chamfer horizontal, and then its opposite on the right side as well.

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Now we'll apply the pier vertical cap extent parameter to get the overall height of the cap.

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And then using one of the critical dimensions,

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the pier cap left total length and the pier cap right total length to complete the dimensions of the cap.

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Now we can finish the sketch.

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If you want, you can rename your sketch to keep things more manageable.

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And then we'll extrude the cap.

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We'll use the parameter, 'pier cap thickness', to create a symmetrical extrusion.

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This will shut the visibility of the sketch off.

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Now we'll create another new sketch based on xz-plane of the component.

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We'll need to, again, project the origin of the UCS.

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And then draw a line from that origin to the left, using the pier column left width parameter.

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Note that we can type in the names of the parameters, rather than using list parameter.

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And I'll draw another to the right, using the peer column right width value.

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Drawing a vertical line, we can gesture over the bottom edge of the cap to project that bottom edge into the sketch.

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We'll do it for the right and then for the left.

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To close off the sketch, we'll draw two lines from the vertical lines we've drawn down to the bottom point of the cap.

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And back up to the vertical line.

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We can then extrude using, again, the symmetry to create our column using the pier column thickness parameter.

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And then apply a fillet to the bottom edge of each side, using the fillet radius parameter for the value.

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In the next lesson, we'll be exercising the model to make sure that the parameters perform the way we need them to.