iLogic Tutorial for the iDoor – 06

iLogic Tutorial – Creating the hinge bore extrusions

The first feature to be created will be the hinge cup bore at the small offset. The Sm Hinge Layout should be the only sketch visible, and you should rotate the model so that the right stile is towards you as shown below…

iLogic Tutorial for the iDoor Page Six Image 01 - Sketching features in Autodesk Inventor

We will be using the Hole tool for all of the holes we create, and will use previously created parameters for all of the dimension settings. The first one will be the large hinge cup hole directly in front of us. Grab the Hole tool from the Modify Panel. You will get something that looks similar to the image below…

iLogic Tutorial for the iDoor Page Six Image 02 - Using the Hole tool

…if the drop-down Placement selector on the Hole Dialog Box that pops up is set to From Sketch. If not, do so. All 12 points will be selected, and will show a preview hole based on the last hole created. You will also notice the right stile is selected as the solid that the operation will be performed on –which is correct. If yours isn’t selected as shown, click the Solids Button on the dialog, hold down the Ctrl key, and de-select the incorrect one and select the correct one.

With the Centers button active, use the same technique, holding down the Ctrl key and click the points of all of the previewed holes that shouldn’t be there, which is all but the larger one towards you.

iLogic Tutorial for the iDoor Page Six Image 03 - Using the Hole tool in Autodesk Inventor

iLogic Tutorial for the iDoor Page Six Image 04 - Sharing a Sketch    You should now have just the one point for the right hand hinge cup selected. We now need to set the width, depth, and hole bottom type. The top right drop-down box is for the depth. Select and delete the value present, and click on the arrow. Choose List Parameters, then choose Hinge_Bore_Depth from the list. Now go to the drop-down below that to set the diameter. again, clear whatever is listed in the window, and choose Hinge_Cup_Diam from the parameter list. The preview will update to show the hole now matching the large circle in the sketch. The last thing to do is change the drill point to a flat bottom. You will see this change in the preview as well. now click OK to accept the settings and create the feature. You will now have the hinge cup hole on the right hand side, and, depending on your settings, the sketch was likely consumed and disappeared.  We need the sketch, so expand the Hole feature just created in the browser, right click on the consumed sketch, and select Share Sketch from the list.

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