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!
I’ve not posted for a few days now, because I was experimenting with my new printer. I came across this 3D touch printer from Bits from Bytes and it was the perfect tool to start experimenting on 3D printer while waiting for the Form1.
It’s a Fused deposition modeling type that can print ABS and PLA plastics. Like any technology there is usually no silver bullet and these printer are quite complementary to stereolithographic ones:
Wild variety of printable materials, with different colors and mechanical properties. The main ones are PLA and ABS. PLA is a recyclable plastic made from corn than can be dissolved in hot water over the course of multiple days. ABS is stiffer and better for mechanical pieces but not as ‘green’. But you can find also ‘wood’ filament, nylon or even recently an elastic/flexible filament has been announced. From the way the extruder head works in this printer I don’t think I will be able to print this elastic filament.
The printing materials are “cheap”, the starting price is around ~$30 for a spool of 1kg of PLA. Specialized materials/colors are of course more expensive but at least the basic material is affordable. There are also initiative to build/sell filament extuders so you can even recycle your own trash plastic. I would be worried about the fumes that some plastics are releasing while melting and wouldn’t try these apparatus with PVC for example (but maybe HCl is only created when the plastic is burned?)…
With FDM you can print hollow or partially filled objects. The internal structure will add structural strength while keeping the weight down. It’s also a great way to save maters and produce cheaper parts.
The printer can have multiple extruder heads, so an object can be made out of different colors/materials. It’s also possible to print supports in PLA and the main object in ABS, so once the print is finished, the support can be dissolved without affecting the object.
The print accuracy & reliability can be difficult to reach. These printer are still not main stream and requires a lot of fiddling and tuning to get the best result. One of the main challenge is to have the first layers adhere to the print bed. If the temperature, calibration, surface state is not perfect the print will not work. Once the adhesion is working, the surface quality, over-hang and seams marks are some of the few challenges that needs to be cleared…
The laser curing enable high accuracy and reliability
The printer can have fewer moving parts, so it’s easier to calibrate/operate
Cost of the resins, even with the Kickstarter preferential cost, the liter of resin has been announced at ~$120. The materials are also usually not really nice and a bit toxic when uncured. The choice of resins are also more limited in color and mechanical properties.
With the ‘vat of resin’ design, it’s difficult to build an hollow object, unless there is an escape hole to flush the resin at the end. This will translate in higher cost of the final parts.
But enough talk, let’s have a look to my first prints 🙂 I’ve spend quite some time calibrating the bed to make sure it was horizontal to the head axis. The first print was one of the example given by BFB in ABS. While the layers were quite coarse, the end result is quite impressive, very sturdy and light.
For the second try I’ve selected the one piece Penrose triangle that I’ve put on Thingiverse.
The support was a bit difficult to remove (I might try to get it less dense next time), the final shape is a bit too curvy, but with the right angle the illusion is nearly working.
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.
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
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.
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.
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.
Exit the sketch, and build a sweep using the top square as the profile and the spline as the path.
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.
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:
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.
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.
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 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:
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).
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.
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.
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)
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.
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).
In this series of “Impossible Objects” articles we will use the magic of 3D printing to explore strange objects that are (maybe) totally useless but at the same time absolutely essential.
We will start with something that defy intuition: constant width shapes. It’s is a rather boring name for something very cool. Like circles/spheres you can roll them and they will always have the same width even if they are not “round”:
Every odd number of side regular polygon can be transform to fit this property by drawing arcs of constant radius as shown in the next figure:
This video shows multiple of these strange “wheels” in action:
These shapes make a perfect tutorial to start modeling in Inventor for example and play with the constraints. I’ve made a set of wheels (IPT Inventor file) and converted them to STL for your printer.
Start with a standard part and create a new 2D sketch
Create all the wheels shapes with parametric dimensions:
Create a circle and add a constraint with diameter name for the diameter
Create with the polygon tool the triangle/pentagon/Heptagon and fix their dimension using diameter name
Switch the initial shape to construction lines and add all center-point arcs. Make sure all the construction points are ‘snapped’ to the initial geometry (in blue). If they are not snapped, they will appears in green (under-constrained)
Exit the sketch and extrude the circle with parametric distance call thickness. The sketch will be “consumed” by the extrusion, to right click on the sketch in the model try and select “share sketch”. Now extrude all the shapes. If the full profile cannot be selected it’s probably because there is an open loop in the sketch. To solve it edit the sketch and in the right click menu select “sketch doctor”, search for open loop and let inventor resolve the issue. You should be able to extrude all the shape now.
We are nearly there! Add a small fillet on the front and back edges for the beauty. Save your part, then select export to “CAD format” in the File menu and create the .stl file. The preview let you adjust the precision of the triangle approximation.
Print your new wheels! I’m eager to get the Form1 to test…
So are Reuleaux polygons really useless?
The answer seems to be mostly… Beside a few coins, guitar picks and some signage the shape is not used in many applications. The Wankel engine uses a shape that is similar but with flatter sides. Maybe the fact that you can drill a square hole with them will finish to convince you?
In a coming post we’ll see the extension of these Reuleaux polygons in volume.