Tag Archives: tutorial

Impossible Dovetail Joint

For this week Impossible object, we will revisit the dovetail joints and have a look at some interesting variation on the theme. This time we will use the “master sketch” technique in Inventor to build our different pieces.

 

This technique is using a single part with all the sketches required to model the whole assembly. Each piece is then derived from the master. To update the model, you just have to update the master sketch, and if everything is properly built, your whole assembly should follow.

Result_picture1

The inventor result files links are at the end, with the STL and the thingiverse link.

  • To start, create a part with a bunch of user parameters to control the design. Then on the horizontal plan XY create a sketch with the outline of the 2 main blocks (length*width).
    impossibleDovetail_01_userParam
  • The dovetails are extruded on a non-vertical plan, so the easiest way to control the result is to create a sketch in XZ plan and draw a segment with ‘Tilt’ angle from the horizontal. Then use this segment and the origin point to create the work plane using “Normal to axis through Point” tool.
    impossibleDovetail_02_TiltPlan
  • The next sketch will be on this newly created plan. The left triangle and the left side of the center one are drawn and the rest is a mirror copy. The base of the left triangle is at length/5=10mm. To allow some clearance in the pieces, all triangle have been “offset” inside by “clearance” parameter (0.25mm here).
    impossibleDovetail_03_DovetailSketch
  • The final master sketch part should now look like the view under.
    impossibleDovetail_04_Mastersketch
  • Now we create a new part to model the first piece. From the manage tab, select the “Derive” tool and choose the master sketch part. Then make sure that the User parameters and the Sketches are shared (yellow plus) and validate. The master sketches will appear in you new part. Now any change in the master sketch will update the part (you will have to press the update button / thunder bolt)
    impossibleDovetail_05_Derive
  • Each sketch will be used multiple time to build the piece, so don;t forget to make them “visible” again once they have been used by an operation. The first thing will be to create the “male” dovetail in the center, so the first step is to extrude the small version of the center triangle by a very large amount on both side.
    impossibleDovetail_06_Centerdovetail
    Then extrude the left rectangle by height and keep only the intersection. to create the dove tail.
    impossibleDovetail_07_CenterdovetailFinished
    impossibleDovetail_08_CenterdovetailFinished2
  • Now the main body can be created by Extruding the right rectangle by “height”.
    impossibleDovetail_09_body
    To create the 2 side female dovetails, just select both the external rim and the internal triangle on both side and cut into the main piece.
    impossibleDovetail_10_body
  • To finish the piece you can add a fillet on the internal side of the dovetail.
    impossibleDovetail_11_finish
  • The second piece is created the same way, from a derived part except you have to do the “negative” geometry.
    impossibleDovetail_12_PieceB

And here is the result assembled with a “wood” finish 🙂

impossibleDovetail_Result01

impossibleDovetail_Result02

I’ve printed the result to check that the piece would indeed fit and yes it works!

The STL files are available in Thingiverse here and the Inventor files are here.

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Impossible objects: The Penrose Triangle

The Penrose triangle is one of these shapes that seems impossible to build but that you can model for fun and then print. Theres are aready a few version on thingiverse but they are with an open loop (here or there). I will here go over a short tutorial with Autodesk Inventor to build one version of the said triangle with a closed loop.

  1. On a new part file we will first draw the “L” outline of the triangle with 2 square on each end with diagonal as construction lines. I try to keep most of the distance parametric so i can update the object faster after (in this case length=40mm, & side=5mm). Then extrude the whole profile by side amount
    penrose_step1
  2. On the bottom side of the L, create a sketch then project one of the center point that will be used for the next construction step and as a profile of the final loft.
    penrose_step2
  3. Create a three points plan using 2 opposite corners of one square of the first sketch and the center point from the sketch under the L shape.
    penrose_step3
  4. To build the sweep of the third side for the Penrose triangle, we need a profile. Add a sketch on the plane we just created. Project the 2 square center points and draw a construction line in between. Then add a three points spline that goes from one center to the middle point to the next center point. Activate the handle of one of the end points and add a vertical constraint on the handle. The spline should make a nice symmetric curve.
    penrose_step4
  5. Exit the sketch, and build a sweep using the top square as the profile and the spline as the path.
    penrose_step5
  6. Enjoy your new Penrose triangle. You may want to experiment with the length and the side to get a good looking result. Try to minimize the curve of the spline without creating a self intersecting profile.
    penrose_final

The STL file is available on Thingiverse here, the Inventor part file is here.

Edit 4/19, I’ve finally printed this object, see here!

penrose_final

penrose_final_side

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