Category Archives: Autodesk Inventor

Mass Customization and Fast Prototyping Age?

This article is less about technique and more about thoughts that I had while designing my last project. It was based on an idea I had a few days ago: a reminder that you place in top of a medicine tube to remember the last time you took your medicine. This design was published on Thingiverse.

pillReminder_assembled pillReminder_dissasembly

To get a practical design I had to go through multiples iterations and the 3D printer was a great way to directly have a confirmation that my changes were going in the right direction. In this case I just had to wait 50 minutes to see the alterations results…


So what are the consequences of these short prototype cycles? Can these 3D printer be used by the end customer to get exactly the right custom product?

When we think about the “2D” version of printing we can see and evolution with:

  1. Scribes and monks reproducing parchment by hand
  2. Gutenberg and the print press with mass production of books
  3. To reach mass customization with modern printer technologies like inkjet or laser

Images sources: [1] [2] [3]

Now if we look at the 3D object reproduction, we can see that the first step was sculpting to get a custom object. Then injection molding and casting helped to mass produce the same shape and now the 3D printers are opening the realm of mass customization…

3D_evolutionImage Sources: [1] [2] [3]

Note that I’m not trying the start a flame war when I make a parallel between hand-writing and CNC. Modern machining is in a sense the final step of evolution of sculpting. The helmet picture is one of the most impressive demonstration of 5 axis machining that I’ve seen so far. Built by Daishin, the speed and the details that this machine is capable of carving are absolutely stunning.

Now 3D printing is currently at his infancy slow and some time limited. But it as already access to many materials from plastics to metal and ceramic. New fields are opening with organ and organic tissues printing. So who can really know where it will stop?

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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.


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).
  • 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.
  • 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).
  • The final master sketch part should now look like the view under.
  • 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)
  • 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.
    Then extrude the left rectangle by height and keep only the intersection. to create the dove tail.
  • Now the main body can be created by Extruding the right rectangle by “height”.
    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.
  • To finish the piece you can add a fillet on the internal side of the dovetail.
  • The second piece is created the same way, from a derived part except you have to do the “negative” geometry.

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



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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First prints & lessons learned

After many tests print I finally got to print some real stuff these last day. The first object was something completely useless but full of gears and very cool (so by my standard indispensable).

One of the mistake I made, was to print the raft and the pin out of PLA. I could not get them to stick to the bed without but couldn’t separate the result so my yellow internal pieces have a black layer 🙂 GearCube_Assembly

The end result is a nice transformer like cube…GearCube_EndResult

My second print was one of my puzzle: double dovetail with a twist.

The pieces are large and I got warping as my bed is not heated… Nevertheless, the comb infill is nice to see…DoveTail_warping

The dovetails ended pretty flat, and just a little bit of sanding was necessary to allow a nice sliding between the parts. DoveTail_separated

And here is the final assembly 🙂 I need to design more puzzle!DoveTail_assembled

And here is the puzzle in action!

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Brain Teaser: Double Keys Box

Today’s puzzle is an other trick opening box. From the puzzle classification list by Slocum this is the family where the goal is to take apart the assembly. In this box you have a hidden mechanism that let you open it if certain steps are followed.

The box is rather plain for outside, but the interesting part is the internals. With 6 sliding pieces this is by far the most complex assembly I’ve built to date. As you can see, the master sketch part starts to be a bit crowded! In on of my next post I will probably describe the process of creating complex assembly and shapes with Inventor.master_doublekey

The assembly instruction gives a better overview of the different pieces.Instructions

The Main body (box) is were all the other pieces are sliding into. On both side a panel and a key have a round slot to catch one of the 1/2″ marbles. The pieces are symmetric so that the same geometry can be reused. Once everything is pushed inside, the door slide from the top.

To keep the door shut the pins have a spring bar that I saw in another Thingiverse object by Ttsalo.

As I do not have a printer yet, I use the schematics and cut views to make sure everything will work.


The Interesting part is to have a look at the lock pin cut:


In this cut one of the ball is placed in the slot. The pin is in locked position (note: the spring is not bent, so it’s going through the back wall). The door cannot slide up, the only way is to pull in the pin using the side panels. But unless both keys are activated at the same time, the door should not move…

As always I’ve uploaded the STL on Thingiverse here.

Happy brain teasing!

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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
  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.
  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.
  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.
  5. Exit the sketch, and build a sweep using the top square as the profile and the spline as the path.
  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.

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!



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Impossible Object 3 – Spheroforms Inventor and Matlab versions

July 2013 edit: I finaly printed the spheres see pictures [here]

Here we are back to our Impossible object series, and I promise this is the last time we are going to cover the Reuleaux polygons! Those constant witdth polygons can be extended to 3 dimensions to build non-regular spheres (I.E. spheroforms).

Here is a video of one ‘sphere’ based on a revolve of the Reuleau triangle:

Here is how to build these Reuleaux spheres:

  1. Build half of the Reuleau polygons (see here how), and define the vertical segment as a center line (optional, the revolve command will let you select it anyway). Before closing the sketch, make sure that all the loops are closed with the sketch doctor tool.
  2. Use full revolve for all the polygons and the circle (you will need to share the sketch). You can now export your spheroforms in STL and print.

The Inventor file is here, and the STL is here.

These spheroforms are relatively easy to build using Matlab. Here is a parametric script that:

  1. Build the regular polygon
  2. Build the Reuleaux polygon
  3. Rotate it through one axe of symmetry to get the cloud of points
  4. Tessellate and save the result as a STL file


Note: The Matlab  scripts are available HERE, Launch it with the start.m script. all code are copyrighted, only usable for non-commercial purpose and provided as is with no guaranty of any sort!

As a final note there are other spheroform like Meissner’s tetrahedron but I’ve covered enough the constant width solids for the moment. Maybe in the future…

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Impossible Object 2 – Non regular Reuleaux Wheels

In a previous post we’ve seen how to build Reuleaux polygons from regular polygons. While already intriguing they were still regular. Now we will see that in fact we can start from the same base and build non regular constant width 5 sided polygons (There is no degree of liberty with 3, and I’m not doing with 7+ but it would work the same). Here is how to build them with inventor.

The files for this tutorial are [here for the inventor file] and [here for the STL]

  1. The first step is from an empty part drawing, create a new 2D sketch and draw a 5 points star. Make sure you are not creating any constraints on the segments (like alignment with axis, relation with other points…). To check if any were created, press F8 (show all constraints), then remove any constraints using the small cross near each icon:
  2. Set the length of one segment with a name (I’ve used length = 40mm to get wheels compatible with the previous article). Then use equal constraint to fix all segment to the same length (You can hid the constraints back with F9).
  3. Pass all the segments to construction and draw thee points arcs from each vertices to get the outline of the Reuleaux polygon. Remark that, because of the constraints you can pull any vertex and deform the final shape.  You can copy multiple time the initial shape and deform it to have strange wheels. Before finishing the sketch, make sure to run a “sketch doctor” to close any open loops, otherwise you won’t be able to extrude the wheels.
  4. Now extrude the wheels. Now we will add on one face of the wheel a embossed version of the start. To do that (repeat for each wheel), create a new a 2D sketch on one face. If the face outline was not projected in the sketch, use project geometry to do it. Change all the line (and origin if available to construction then draw the 5 point star with the construction switch ON.
  5. Remove the construction switch and select the offset tool. Now select all 5 star lines and press enter to validate. You can now draw an offset version of the star “inside”. Repeat a second time and then fix the distance to 1mm and 2mm from original star. (after some try 0.5mm and 1.5mm work great to get the star closer to the border)
  6. The current profile are intersecting so to be able to extrude/emboss them you have to add “points” to all the intersections. Once done exit the sketch.nonReg_reuleaux_step6
  7. Extrude or emboss 0.5mm deep the star, then add a 0.5mm filet on the star and a 1mm fillet on the outside edges of the wheel. (if you select the ‘all fillets’ option, you can capture all the star filet at the same time so no need to select one after the other).

Here it is, you have a set of non regular wheels compatible with the previous ones.
The files for this tutorial are [here for the inventor file] and [here for the STL]

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