iLogic Tutorial for the iDrawer – 18

iLogic Tutorial – 18 – Extruding Sketches and Mirroring Bodies

Now for the bottom. Turn the visibility of the Drawer Bottom Profile on, and arrange the view so that you can see at least one of the dado cuts. This will allow you to tell if you are extruding in the right direction.

iLogic Tutorial for the iDrawer Page Eighteen Image 01 - The bottom sketch

Use the Drawer_Dado_Thickness for the Extents, and select the New solid button. For some reason, selecting New solid always reverses the extrude direction, so if its now going the wrong way, change it back.

iLogic Tutorial for the iDrawer Page Eighteen Image 02 - The Inventor Extrude Dialog

Click OK to accept the new solid body, then rename the extrusion  Bottom Ext and the solid body Bottom. It should look like the image below…

iLogic Tutorial for the iDrawer Page Eighteen Image 03 - The Drawer Bottom

Save the file. From here on in, everything is mirrored from the origin planes. Grab the Mirror tool from the Pattern panel, and select the Mirror a solid button, which is the lower of the leftmost buttons on the Mirror dialog. This will bring up the extra options needed for mirroring a solid body. Now select the Right Side body in the Solid Bodies folder. Now click the XZ Plane in the Origin folder –you should get a preview at this point that looks like the one below…

iLogic Tutorial for the iDrawer Page Eighteen Image 04 - Mirroring

…the Magenta outline on the front section means that the new material will be added to it. Click OK to accept the mirror, and name the new feature Right Side Mirror. Now use the same process to mirror the right side again. This time you will use the YZ Origin plane, and you will need to click the New solid button as we are creating a whole new body on this one. The preview will look like the one below…

 

iLogic Tutorial for the iDrawer Page Eighteen Image 05 - Mirror a Solid Body

…click OK to accept. Rename the new mirror Left Side Mirror, and the new solid body Left Side.

 

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