Inventor Tutorial for Designing a Shaker Table – 3 – Sketching More Stuff

We left off in this Inventor Tutorial yesterday with the corner bracket drawn, but not constrained to the projected geometry. We’ll start today by projecting the other two lines that make up the square that represents the top of the leg, then window select all of the projected lines and click on the Construction icon on the Format Panel.

Making these projected lines construction lines will make sure they are not interpreted by the program as closed loops and thereby avoiding their auto selection when performing modeling operations that require same (such as extruding).

With that done, create a dimension between the inner point of the table’s leg and the back face of the bracket. Use the Bracket_Offset parameter here. To fully constrain the sketch (and get the bracket where it needs to go), use the Collinear Constraint tool to constrain each of the angled end lines of the bracket sketch to the closest line that represents an apron. The sketch should now look like this…

 

The last thing to do here is to add a driven dimension between the front of the bracket and the outer corner of the leg. To do so, grab the Dimension tool from the Constrain Panel and click the outside corner of the leg, then click the front face of the bracket. Inventor should be trying to give you a dimension either horizontally or vertically by default, so you need to right click and choose “Aligned” from the context menu. When you click to place the dimension, the program will give you a warning about an over constrained sketch. Choose to create “Driven Dimension”.

 

Note: You can set the default behavior apply a driven dimension by clicking the Application Icon, Options (at the bottom) Sketch Tab, then set the Overconstrained dimensions option to Apply a driven dimension.

 

The new, driven dimension will be named something like d12. You need to change it. Open the Parameters editor and scroll to the center where the Reference Parameters live. Change the name of the reference parameter to Hanger_Bolt_Length then click done.

 

That’s it for this sketch, right click and choose “Finish Sketch or Finish 2D Sketch”, then save your work.

Now turn of the visibility of the Corner Bracket Sketch (and any others that may be visible), and turn on the visibility of the Sub Top Sketch. Now create a new sketch on the Sub Top Work Plane by grabbing the Create 2D Sketch tool and clicking on it’s name in the feature browser. Name the new sketch “Tenon Profile Sketch”. Use the Project Geometry tool to project all of the leg and apron lines into your new sketch. Make sure you include both apron shoulders (apron end lines) as seen below…

 

Now shut off the visibility of the Sub Top Sketch and switch the view to TOP. Window select the entire sketch and change the line type to Construction. We are now going to create the part of this sketch that will auto resize the mortise and tenons automatically as the thickness of the aprons change. This can also be handled via a parameter and/or via iLogic, but for this tutorial we will have the joint’s thickness always be 1/3 of the apron stock thickness.
We will create this automation with a three segment line. Zoom into the leg portion of the sketch as shown below, then draw a vertical line, clicking three times to create the segments. Make sure the Vertical glyph is visible before each click so the segments are constrained vertically…

 

…then, get the Equal constraint from, of all places, the Constrain Panel. Click the bottom segment, then the middle segment. Go back to the bottom segment, then the top segment. All three line segments are now the same length. The reason for starting with the same line segment each time (no matter how many segments there may be), is that you want to avoid “daisy chaining” (A-B, B-C, C-D) constraints. I’ll post something more in-depth on the reason why later, but for now you just need to take my word for it

 

With the three segment line done, you need to attach it to its home at the shoulder of the lower apron. To do so, get the Coincident Constraint tool from the Constrain Panel, and click on the endpoint at the bottom of the line. Then, as can be seen below, select the point at the intersection of the leg and the lower corner of the shoulder. If Inventor tries to select the wrong thing, just wait for the little selection drop-down to appear and choose the point (must be a red dot, not a larger green one)…

 

 

 

 

… then right click and choose “Done” from the context menu, and grab the upper end of the line and drag it shorter so that you can see the upper shoulder of the apron. If this is not done, it will be very hard to attach the upper end of the line. Now get the Coincident Constraint tool again and select the top point of the line and the upper end of the apron’s shoulder…

 

Now, whatever size the apron becomes, the tenon (and later, the mortise), will remain exactly 1/3 of its thickness. To finish up, create the same setup for the other apron, then make the outer line segments of both into construction lines…

 

Now we can create the actual tenon profiles (which are also the mortise profiles). To do so, get the Line tool from the Draw Panel and start your line at the lower end of the vertical line to the right (make sure you have a green dot before clicking). Move leftwards until you see the little dashed line indicating you are directly under the far end of the upper line segment, and make sure the Horizontal glyph is present, then click to create the segment…

 

…then go straight up and click on the outer end of the upper line. Finish up the sketch as shown below…

 

The last thing to do in this sketch is create another driven dimension. It will be used to keep the shoulder cuts at the top and bottom of the apron the same as the ones on the sides. Again, this could be controlled in a more complicated way, but we aren’t going to go there in this tutorial. Grab the Dimension tool and dimension one of the equalized line segments as shown below…

 

…then go to the Parameters editor and rename the driven dimension Tenon_Shoulder. Finish the sketch and save. That’s it for today. Tomorrow’s post will wrap up the sketching (I think). See you then.

 

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