As stated in a previous post, the scope of this Autodesk Inventor Tutorial was increased from showing how a mortise & tenon joint can be modeled so that they automatically match each other, to a full blown table design that incorporates the afore mentioned matching magic.
The correct way to model something like this in Inventor is by using layout parts containing multi-solid bodies. Several years back (or currently in some ERP systems) this would have been accomplished by separate parts that share global parameters e.g.: a mortise width in one part and the tenon width in another are both controlled by a common parameter called MT_Width. You also could have used cross part dependencies with adaptivity, but that schema was incredibly buggy and failure prone. It also ate up system resources If I remember correctly, but in any case, just don’t go there.On with this incredibly kick-butt Autodesk Inventor Tutorial…
I’m going to make this tutorial easy enough for a person with just a tad of Inventor experience can follow along. If you are a more advanced user, you may feel like skipping ahead –but you never know when you will pick up a new technique. There are numerous ways to accomplish almost anything in Inventor, and I try to mix my techniques up to show as many as I can.
To begin the model, start a sketch on the XY Plane (may have happened automatically), and name it Top Sketch. The only reason to add the “Sketch” part to the name is that you will later have both features and solid bodies that need to be named, (names must be unique) and I prefer to reserve, in this instance the name “Top” for the solid body. This way when the solid bodies are turned into parts, they will have the names I want without any further work.
Draw a rectangle around the center point with the Rectangle Tool, then grab the Vertical Constraint tool from the Constrain Panel, then click on the center point, then hover over the center of the top line until you get a green dot visible and click. The top line will jump over and center itself vertically to the center point. Do the same thing with the Horizontal Constraint and the center of the left line. The rectangle is now constrained horizontally and vertically to the origin of the model (very important). A couple of dimensions will fully constrain this sketch. We will create them as parameters, then pick them from the parameter list to apply them.
Open the Parameters table and add the following parameters:
Notice that the last parameter looks a bit different. When I add whole numbers to the parameter table, I simply type in the number and move on. Inventor will add unit designation based on the unit properties of the document you are working within. With fractions, I prefer to type in the fraction as opposed to decimals. Inventor recognizes the closing quote mark as being an inch unit.
There will be many, many more parameters to come, but these will do for now. Click Done to get rid of the Parameter list, then grab the Dimension tool from the Constrain Panel and add the Overall_Length parameter to the top or bottom line.
Now add the Overall_Width parameter to the left or right line to fully constrain the sketch. You can double check this by glancing at the progress bar (bottom of the program screen) on the right side. It should say “Fully Constrained”. If all is well, right click one of the dimensions and select “Dimension Properties…” from the context menu. On the “Document Settings” tab, in the drop-down selector for the Modeling Dimension Display, select “Show Expression”.
All of the parameters we will use here are named, so it’s a lot easier to just see the name on screen. Now right click anywhere in the design window and select “Finish 2D Sketch”. The first sketch is complete.
Now for a bit of orientation. If you look at your View Cube, you will see that it is calling the view you are working on the Front view. It’s not the front view. You are looking down on the top of the table. To change this, right click on the View Cube and select Set Current View as then select Top from the fly-out.
At this point, your screen should look like this…
In this model, the plane we started out on, the XY Plane lies at the surface of the table’s top. The majority of the design will be created at the plane that will be at the bottom of the top. We’ll create that plane now. Start by expanding the Origin Folder in the Feature Browser by clicking on the little plus sign dealie to the left of the folder. Right click the XY Plane and make it visible. Orient your model similar to how it is in the image below, then get the Plane tool from the Work Features Panel, click the plane in the modeling window, and drag downwards…
…now click on the little arrow to the right of the text box and select List Parameters from the list. From the Parameters list that pops up, select Top_Thickness…
The parameter Top_Thickness will now appear in the tiny little heads-up display window in a centered fashion. Select anywhere in the window and drag left, or select in the window and use the arrow keys to get to the beginning of the parameter’s text. Add a minus sign there…
Click the little green check mark to finish up the placement, then rename the plane “Sub Top Work Plane”. Grab the Create 2D Sketch tool from the Sketch Panel and click on the Sub Top Work Plane in the modeling window. Name the new sketch “Sub Top Sketch”. Now we are going to project some geometry. Select the Project Geometry tool from the Draw Panel and click on all four lines in the first sketch (Top Sketch). The projected lines will appear in the current sketch just below the first one. Now turn off the visibility of all planes and, if you are using the Presentation color scheme with a gradient, it should look like this…
Now shut off the visibility of the Top Sketch and click the Top of the view cube to align yourself for the next sketch. We will need to add a few more parameters which will be used to lay out the leg and apron portions of the design, so click on the Parameters tool…
…then add the following parameters:
That’s it for today. Stop back tomorrow for the next installment. Later.
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