Inventor Tutorial for the iDoor – 06 – Starting the Stile Profiles – Continued
Now shut off the visibility of the Stile Sketch Plane, then grab the Project Geometry tool from the Draw Panel . Click on both lower points to project them onto the sketch you are working in. Right click and choose “Finish Sketch” to exit the sketch environment, and rename the sketch just created to Stile Profiles. Now right click the Layout Sketch and shut off it’s visibility. Get the View Face tool from the navigation toolbox (below the View Cube), and click on the newly made Stile Profiles sketch. The sketch will rotate and center itself onscreen; which will make the next step easier.
Now to create the stile profiles. If you have been following along closely, you should have a center point and two projected points visible on your screen as shown below…
The parameters for the stiles can be added as-you-go, and the widths have already been established. I like to add parameters ahead of time when possible, and will add several more to describe the stiles now. Note: when adding the parameters, just add the Parameter and the Equation, the unit and Export will default to the correct setting, and you need not add the ‘in” after the Equation either as a the program will automatically add the default unit. The new parameters are as follows;
| User Parameters | Unit | Equation | Export? |
| Bead_Rad | in | .1875 in | No |
| Frame_Thickness | in | .75 in | No |
| Panel_Groove_Thickness | in | .25 in | No |
| Panel_Groove_Depth | in | .375 in | No |
| Panel_Gap_Top | in | .0625 in | No |
| Panel_Gap_Sides | in | .125 in | No |
| Tip: If any of your parameters seem to disappear, and you are sure you created them, look and see if the checkbox above the ‘Add” button (Display only parameters used in equations) is not checked. It can easily become checked simply by clicking in the blank space horizontal to the checkbox —even after the text. When checked, only parameters in use will be visible, which hides most of those made so-far. |
At this point it would also be helpful to change one of the settings in the program options. When you create sketches in inventor, you will notice a little image near the cursor, after beginning with any drawing tool called a Constraint Glyph.
The one shown in the image above is a vertical constraint glyph, and if I were to make the second click while it was visible, there would be a vertical constraint added to that line. The default setting is “Parallel and perpendicular“, which can cause numerous problems on large sketches. To change it to Horizontal and vertical, go to the Application Icon , and at the bottom of the menu select the little box titled Options, then go to the Sketch tab. At the top left there is a place to set Constraint placement priority that contains the settings just described. select the lower, “Horizontal and vertical” setting, hit the apply button on the lower right, then close the dialog box.
The next page begins the sketch of the right stile profile…
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