Modeling Challenge: Puffy Cube
The winning blog post suggestion from the recent contest came from SolidWorm, and he suggested a monthly surfacing challenge. You all voted for him and agreed, so here we go. We’ll start this one off simple. This is a nice example of justification for surfacing. We will build up to more difficult surface modeling challenges as we go.
Sometimes instead of a flat face you need something with a little bulge to it. There could be many reasons for this, including general looks or even to increase stiffness.
The challenge here is to create a box with puffed out sides. Each side must have curvature in two directions, so they could be created by revolving an arc, but not by revolving a straight line.
Any method other than import is valid, and you can use any technique as long as a surface feature is used at some point. The finished puffy box must be a solid body.
Make the distance between adjacent corners 1 inch (25.4 mm), and make the part centered around the part origin. Each side should be the same size and shape, so I’m looking for something cube-ish.
Use the comments to ask for hints or suggestions.
Since this is an easy one, and SolidWorks World is a month from now, lets make this one end on Monday, Feb 2 – Ground Hog Day. Send in your model to me at matt (at) dezignstuff (dot) com. On Feb 2, I’ll post the way I would do it, but I’ll also post my favorite methods from models submitted. I always learn something when I see how other people model stuff, even something relatively simple like this.Â
There are no prizes this time, but I’ll be looking for:
- fewest features
- most robust through changes
- most novel approach
- most creative way to break the rules
Best of luck to every one!
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Entry 1 is from Kalpesh Navale. Click the feature manager to the left to download his part. This is a very interesting part. Extruded surfaces are used to create intersection split lines, which are lofted together to create the faces of the puffy box. Very interesting! How will you make the part?
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Entry 2 is from Charles Culp. Another interesting model. Charles made curved sketches forming a X and then used the Boundary feature to make the surface, patterned it, then trimmed.
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Entry 3 is from SolidWorm. Again, this is a solution I wouldn’t have thought of. Â This involves a solid as construction geometry, planes, sketches, and a boundary surface patterned around.
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Entry 4 from Clay Corbett. This one uses an extensive 3D sketch with planes to minimize features, and then makes the faces of the part with lofts. Clever, and nicely done.
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Entry 5 from Brian McElyea. Five entries and not a duplicate yet! Nice job on this one. Just a single surface creation feature, and the first Fill surface entry. Brian created a framework using a 3D sketch, and used a Fill to make a surface between the 3D sketch elements. Then pattern twice and knit.
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Entry 6 is from Garrett Brooks. This one uses another clever method that I wouldn’t have thought of. This is also the first to use a revolved surface. Garrett revolved a surface, then extruded a square with draft and used that to trim the revolve. Then the familiar pattern and knit.
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Entry 7 is from Steve Martin. Steve started with a 3D sketch, built planes, then sketches, and built a boundary from the sketches. Then he patterned the boundary, and built 2 more boundaries from the pattern. Very nice.
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Entry 8 from cgroh. Another boundary suface user, but this time with a twist- a Thicken and a Scale, presumably to get the dimensions correct.
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Entry 9 from Arthur Young-Spivey. Arthur made 2 versions, separated with folders and configurations within the same part file. The first uses a 3D sketch and a boundary surface, patterned, then two more boundaries, and finally knit.
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Entry 10 from Arthur Young-Spivey. Arthur’s second entry is called his “robust” version. It uses a layout sketch, a series of planes, a series of 2D sketches, a Boundary surface, circular pattern, then two lofts and a knit.
Two patterns seem to be employed in most of these parts, either patterning a face twice in opposite directions or once, then using additional features to cap off the first pattern. A variation on this is to make a single feature with 4 sides. 3D sketches are popular because they reduce feature count, but notice that Arthur doesn’t use the 3D sketch in the one that is “robust”. 3D sketches are prone to failing for reasons other than ones you might expect.
I think there is a lot to be learned from seeing how several people make these models. I will analyse in more depth after the end of the challenge.
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Entry 11 is from Mark Kaiser. Mark took a different approach, with straight sides on his box. He used a single loft created from a set of 2D and 3D sketches.
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Entry 12 is also Mark Kaiser. Similar to previous with a boundary surface instead of a loft.
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Entry 13 is from Mark Reader. Mark notes in his email:
“Something happens tolerance-wise if I replace the surface-revolve sketch with a single spline curve coincident with the wireframe cube corner. Â It builds find of course, but measure to the corners and it’s not 1.000Â consistently. Â Some measure just over and some under.”
Something to look into here… Also notice that all of the Origin icons in the FeatureManagers for these parts are red except for this one. Odd.
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Entry 14 comes from John Travis. John starts from a solid cube, makes some planes, then sketches, then patterns, knits a solid and combines solids. Nice job!
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Entry 15 comes from Jason Knox. This one is actually the closest to what I would have done. Revolve, pattern, pattern, trim. I have another trick up my sleeve if no one comes up with it, where I can get away with making a single face and a single pattern, no mirror or additional face features.
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Entry 16 again fron Steve Martin. An interesting method that copies a face of a 4 sided Boundary surface to pattern around and close off the open ends.
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Entry 17 from Chris Cole. All solid, but creative use of the Combine/Common feature.
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Entry 18 again from Chris Cole. I think this is the first one to start from a triangular slice.
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Entry 19 from Matt (me). The key to minimizing features is to use a 3D sketch, but there is a huge price to pay. Reliability and ease of use are not the best traits of 3D sketches.
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Entry 20 from the one and only Phil Sluder. Wow, this is exactly the way I did this originally, for the model shown at the very top of the article. Revolve, pattern, pattern, trim, thicken.
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Entry 21 from Ken Kronholm. Revolve, 2 patterns, series of trims. Nice alteration – Ken has a series of configurations from 1 to 36 that change the box from squarish to almost spherical.
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Entry 22 from Keven Bouwman. Kevin starts with a solid and makes surfaces to cut the solid. It’s getting difficult to make unique solutions after this many entries, but this is unique.
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Entry 23 comes from R. Paul Waddington. RPW used AutoCAD to create the shape. The two blue blocks are solid, and the varicolored one is surfaces. The DWG file is linked to the image above. Most of what’s interesting with this challenge is seeing how people did it, which we don’t get to see with the Acad data, but it is interesting that he was able to do it at all. RPW is a frequent and valued contributor to this site, although he is an AutoCAD reseller.
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Entry 24 is from Mark Landsaat. This is another version of the part I made for the image at the top of this article.
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Entry 25 is from Matt Lombard. In honor of Thomas Edison who discovered many ways to not make a light bulb before he discovered a way that worked, this is a failed attempt at using fewer features to make the puffy cube.
Here’s how the concept works: the only kind of pattern that can pattern all the faces of the cube at once in a single 3D pattern (instead of using 2 2D patterns or a circular pattern and a mirror) is a curve driven pattern where the curve is on a 3D face. I had to first make the face, which required making a 3D sketch with a lot of planes in it in order to use the sketch entities (with the selection manager) and the Boundary feature. Then I made a sphere, and placed 3D sketch points where each of the XYZ axes would intersect the surface, then I drew a Spline On Surface through all of the points, using the Tangent To Curve option, and a Face Normal selection.
The concept is great, except that it doesn’t account for the alignment of each face. In order for this to work, the Spline On Surface would have to go through each of the 3D sketch points in a particular direction, in addition to being a controllable length, because the Curve Driven Pattern only enables you to place pattern instances either equally distributed along the entire curve or at a given spacing along the curve.
I also tried this with a series of straight lines in a 3D sketch where the 3D sketch points were the midpoints of each line. Â I just can’t get it to work. I’m sure there’s a way to do it, but I haven’t found it yet.
I thought a Sketch Driven Pattern would work, but it wouldn’t do a 3D pattern, only a 2D pattern. Any ideas for this? I don’t think it’s impossible, just really difficult.
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Entry 26 from Mike Wilson. Yes, THAT Mike Wilson. And just as you’d expect from Mike, this solution is creative but simple, and different from what anyone else has come up with to this point. Mike starts with a revolved surface, then extrudes up to surface, then patterns the body twice with the Move/Copy feature. It’s getting harder and harder to add something no one else has done, but Mike pulls it off.
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Entry 27 is from Stacy Abel. Stacy’s differentiator is the use of several projected curves to create the surface. Nice job, Stacy!
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Entry 28 from Dan O’Neill. Another unique solution! This one uses extruded surface as reference geometry from which to build a Boundary surf.
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Entry 29 from Matt Cummins of Tacton Works. This is probably the model with the fewest features. It uses all solid features, which is a little surprising. Revolved solid, patterned bodies, then Combine. Nice job. Also, check out the download for this method. Matt has included a movie of Tacton Works controlling the cube.