Inventor Tutorial for Designing a Shaker Table – 6 – Patterning the Solids

Now for some fun stuff, the patterning of the solids that were created in the previous Inventor Tutorial. All of the patterning will involve mirroring, and all of the mirrors will use the models origin planes as their center –which makes for a very robust model…

..but before we get to the patterning, I placed the one “out of the box” so-to-speak detail to the piece. The chamfer on the underside of the top. I went with a ½” chamfer for now, but will likely tweak things a bit later. Most things are not written in stone in parametric modeling (if things are done correctly). The Chamfer is pretty self-explanatory. Click on the Chamfer tool, then either start selecting edges then size, or vice versa…

 

With that out of the way, let the patterning begin. We’ll start by patterning the leg. Select the Mirror tool from the Pattern Panel. On the Mirror dialog that pops up, there are two choices on the left “Mirror individual features” is the default, and below that, “Mirror a solid”. Mirroring a solid gives you all of the features within that solid, and is the one to choose. After selecting the “Mirror a solid” option, the Solid selector becomes active. Select the leg in the modeling window. The selection is now outlined in a dashed magenta line. The Mirror plane selector is now active, so we will select the YZ plane in the Feature Browser (if the Origin folder is not open, it can be opened with the tool active). You should have an outline of the mirrored leg in the correct place at this point. Now go to the upper right corner of the Mirror dialog and select New Solid…

 

…click OK to create the new leg, and name the new Solid Body Leg B.

Now for the front apron. In this case, we will not be creating a new solid. We will be mirroring the half apron and the tenon. Because the tenon is buried in the leg, we will expand the Apron A solid body in the Solid Bodies folder of the Feature Browser so that the features can be selected there. Depending on your view settings (does not work in Ortho, you need the Perspective setting), you can also zoom inside the leg and select the tenon directly, or select the features down lower in the Feature Browser, or, you could make the leg invisible and select the tenon on-screen –or a combination of the above. Whatever tripps your trigger.

Now select the Mirror tool again, and this time we will use the default settings. Select both features within the Tenon A solid…

 

…now click on the Mirror Plane selector tool and select the YZ plane as the Mirror plane. You should have a green preview outline at this point…

 

 

 

 

 

Click OK to accept create the mirror. I generally name all of my features, even if, as is the case here, I really don’t need to. You may as well do the same. If you expand the Leg B and Apron A in the Solid Bodies folder, you will see the two mirrors that you just created. Rename them as seen in the image to the right…

 

 

 

 

 

 

 

 

Now mirror Apron B’s features in the same way, making sure you use the XZ Plane this time…

 

Name the new mirror feature Apron B Mirror. Now for the Corner Bracket A. We will be mirroring this solid body into a new solid as we did with the Leg A solid…

 

Name the new solid Corner Bracket B and the new mirror feature Corner Bracket B Mirror. Now it’s time to mirror the Apron B across to the other side as a new solid.

You know the routine…

 

Name the new solid Apron C and the new mirror feature Apron C Mirror. You should now have something like (or better yet, exactly like) this…

 

From here on in you are on your own. You need to create mirrors of both legs, both brackets, and Apron A to finish up the modeling. Rename the solids and features as per the schema we have been using, and save the model. If anyone gets stuck, I’ll help you out –but its not likely.

In the next installment of this Inventor tutorial, we will create a material called Yellow Pine and apply it to the model. We will then create two new colors, and use them to make the model look a bit more realistic. From there we will get into some iLogic coding and other stuff.

Until then play around with the parameters a bit and use the Measure tool (on the Measure Panel of the Inspect Tab) to assure that the mortise and tenon always match each other in size. Remember that if you go crazy with resizing, you can break the underlying sketch. One of the first iLogic routines we will write will set min/max values.

Later…

 

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