Inventor Tutorial for the iDoor – 05 – Adding Parameters and Starting the Stile Profiles…
If you look at the status bar at the bottom of the window it should read “2 dimensions needed”. The top point in reality only needs one dimension to fulfill its purpose; the dimension between it and the top line. But we will add the other constraint somewhat arbitrarily to achieve a fully constrained sketch. It is good practice to always fully constrain sketches unless there is a good reason not to. So, the first step will be to add a Vertical constraint between the point and the center of the top line. The center was chosen because this point will be used later as the end point for both of the stiles, which will be created using the lower points.
Click the Vertical constraint tool and constrain the topmost point to the center of the top line. Now, add a Dimension between the same point and line, and use the Insert_Gap parameter for the distance. The top point should now look like the image to the right, and the status bar should indicate that the sketch is “Fully constrained”.
We now have independent controls for the widths of all four gaps around the door. In most cases, the gaps would all be the same; just as we have set it up, but if the need arises, one, or even all of the gaps can be different—an example of which will be shown later…
If you do not ‘get’ how this will work, never fear, it will be explained as we progress. Now its time to create the Work Plane that the stile profiles will be created on. If you have not already exited out of the sketch, do so now (you can also do this by right click: “Finish Sketch”). Open the Origin folder to expose the origin geometry, right click on the XY Plane and chose “Visibility” to make it visible. You will need to rotate the sketch so that the lower right corner is facing you, and the XY Plane is visible as shown. Now zoom in a bit so that you can see the lower right point, grab the Work Plane
tool, and select the point and the XY Plane . You should now have a plane at the location of the point that is parallel to the XY Origin plane as shown in the image below. If not, you screwed up and need to do it over…..
If everything looks good, rename the new plane from “Work Plane 1” to “Stile Sketch Plane”, and make the XY origin plane invisible by reversing the steps you took to make it visible. Now create a sketch on the Stile Sketch Plane by choosing the ‘ Create 2D Sketch’ tool and clicking on the Stile Sketch Plane just created..
| Tip: you can create a new sketch by either clicking on a visible plane in the workspace or by clicking on it’s name in the browser. |
Inventor Tutorial for the iDoor Navigation
Intro – 1 – 2 – 3 – 4 – 5 – 6 – 7 – 8 – 9 – 10 – 11 – 12 – 13 – 14 – 15
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