Inventor Tutorial for Designing a Shaker Table – 4 – The Final Sketching

In the last installment of this Inventor Tutorial, we finished up with Tenon Profile Sketch –which will wrap up the sketches on the Sub Top Work Plane, but before we create new planes to draw the legs on, it’s time to create the two planes that describe the top and bottom of the mortise and tenon joint.

We could leave things as they are and create tenons without top and bottom shoulders, but that would create a crappy joint. The mortise in the leg would come through the top of the leg and weaken the table dramatically. This is why the driven dimension Tenon_Shoulder was created in our last installment. We will now use that parameter to create an offset plane that will be used as the starting plane for both the additive and subtractive extrusions that make up the mortise and tenon.

To begin, make the Sub Top Work Plane visible and rotate your model similar to what you see in the image below. Grab the Plane tool, click the plane in the modeling window, and drag downwards just like you did to create the Sub Top Work Plane. Add the Tenon_Shoulder parameter, and make sure you add the little minus sign again as we want the plane in the Z- direction…

 

Name the new plane Tenon Top Plane. Now for the bottom plane. Shut off the visibility of the Sub Top Work Plane, and use the Plane tool to create another plane in the Z- direction. Accept any dimension in the incredibly small, non-resizable heads-up text box. Name the new plane Tenon Bottom Plane, then double click on the name in the feature browser to bring up the old-school text box which can be resized. Enter the formula seen to the right. Note that the distance formula is separated with parenthesis from the direction (the minus sign at the beginning). If you don’t write it this way, the minus at the beginning will be applied to the distance formula, which would suck.

 

 

The formula simply states that the tenon should be the width of the apron minus the two shoulders. Click the check mark to accept the formula and rename the new plane Tenon Bottom Plane. Notice that if you expand the Tenon Bottom Plane in the browser, the three planes it is dependent on are listed. The Tenon Top Plane is actually consumed by this new plane because it was not used for anything else before the offset. Now measure between the two planes to make sure you have the formula right. You should have two inches…

 

…if not, go back and try again.

Now we will use the line and point method to create the plane for the leg profile on the front. Start by making everything invisible except the Sub Top Sketch. Orient the sketch as shown below, then use the Plane tool to click on the line shown, then click the endpoint of the line. A small plane will appear as seen here…

 

Now for the leg sketch. Start a new sketch on the new plane using the 2D sketch tool. Name the plane Leg Plane A and the sketch Leg Profile A. Turn off the visibility of the plane, then use the Project Geometry tool to project the line that represents the front of the leg (use the View Cube for orientation if needed)…

 

Now click the FRONT of the View Cube to align the drawing, and turn off the visibility of the Sub Top Sketch. Using the projected line as the top, finish sketching a rectangle as shown below and give the geometry a dimension using the formula: Overall_Height – Top Thickness…

 

Now we need to add a couple of parameters that will be used to define the taper on the legs. Open the Parameters editor and add the two taper parameters and their respective formulas…

 

The taper is created by drawing an angled line as shown below. Using the Line tool, move your curser over the right vertical line somewhere near the top until you see a little Coincident Constraint glyph. Click while the glyph is visible. Now click on the lower line anywhere but the center (green dot will show). Add the parameters you just created to fully constrain the sketch…

 

Now for a step that shouldn’t be necessary in my opinion, but you need to do nonetheless. Grab the Split tool from the Modify Panel and hover over the right vertical line. When you have the indicator present that shows that a split will be made at the intersection of the line just created an the vertical line, click to split the line…

 

Do the same where the new line meets the horizontal line –which completes the sketch. The reason for splitting the lines is that Inventor will sometimes not recognize areas such as this as a closed loop… which would mean we could not extrude the profile we need.

Now to finish up the sketching, do the same thing you just did to create the other leg profile on the LEFT orientation of the View Cube…

 

That’s it for today. The next installment of this fine Inventor Tutorial (tomorrowish) will begin the extrusions to create a multi-solid body. See you then.

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