123D Design – Several Ways to Skin an Advanced Cat
20 February 2019

Hello everyone,

Following on from where we left off with our last article but in a slightly different vein. Today we’re going to see how it’s possible to model a more challenging shape in several different ways, which each yields slightly different results.

The shape we’ll be modelling is your basic pipe segment but with triangular cut-outs extruded from its surface along its circumference. Immediately, two completely different ways of how this can be accomplished come to mind. One is additive and the other is subtractive. We can either begin with a pipe and extrude triangular cut-outs from it by different means so that we are left with the pillars in between each triangular extrusion or we can begin with nothing and just create the pillars before capping them with a top and bottom ring which can then be continued into un-extruded lengths of pipe of any desired length. We’ll go over both methods in this article.In this first video, we go over the first 4 approaches one can employ when trying to achieve the shape described above.

We begin by sketching some circles on the default sketch plane / ground plane (using the ‘Sketch Circle’ tool from the Sketch menu at the top of the 123D Design interface). These represent cross-sections of the pipe segments we’re going to be extruding triangular cut-outs from (the first three methods for achieving the intended shape are subtractive).

First approach

After sketching the profiles of the pipe segments we then sketch a circular arc which is 22.5° wide and concentric with the middle pipe profile sketch (with one endpoint on what, I believe, is the Y axis?). For sketching the arc we use the ‘Two Point Arc’ tool, likewise from the Sketch menu. This is actually half of the actual intended arc we are going for, which is 45°. We don’t have to go with this particular angle, we could just as well pick a wider or narrower angle if we were going for fewer or more triangular cut-outs along the circumference of the pipe. Or thinner or thicker pillars in between the same number of triangular cut-outs. And we’re sketching just one half of that actual intended arc at first so we can nicely align the arc we actually do want.

After sketching the 45° arc, we turn it into a circle sector by sketching the radii that touch its endpoints (using the Polyline tool from the Sketch menu). Then we turn the circle sector into a triangle by sketching the chord corresponding to its arc (by drawing a polyline that connects the arc’s endpoints) and deleting its arc (using the Trim tool from the Sketch menu, we could also delete it by simply selecting it and pressing the Del or Delete key). This particular step isn’t absolutely required though.

After selecting all of the areas of the triangle (by clicking one and then holding down the Shift key before selecting the others as well, so that the previously selected area is not un-selected when we pick another one), separated by the circles which depict the inner and outer diameter of the segment of pipe, we then extrude the triangle upwards specifying an extrusion deviation angle from the vertical of -30°. This means that the triangle shape we are extruding vertically will have its walls tilted inward by an angle of 30° from the vertical.

Again, this isn’t the only angle we can go with. If we opt for a greater angle here then the triangular extrusions we’ll end up with will be less tall and have a greater circumference span/width to height ratio, making them appear flattened out and the pillars in between them closer to horizontal than vertical. Feel free to experiment with the value of this angle.

Having extruded the triangle but not all the way into a complete pyramid (something which we could just as well have done), we simply select the frustum resulting from the Extrude operation we just performed (my first reflex was to do this using drag-select but then we remembered the triangle sketch underneath and that that would get selected as well so we click-selected the solid instead of using drag-select) and then choose the top surface and press the Delete key.

We then use the ‘Circular Pattern’ tool from the Pattern menu at the top to create a circular array of evenly spaced instances of the pyramid we just completed, which all automatically retain their orientation relative to the centre of the circle. Because we chose 45° as the arc angle when we were first designing the footprint of the pyramids we can now fit 8 pyramids around in a circle, with just their edges touching. But we don’t actually want to do that since we want to leave some space left over for the pillars in between the triangular cut-outs (the latter which we will actually be achieving by subtracting these pyramids from the pipe). So we choose to have 6 pyramids instead of 8.

After that we extrude the segment of pipe from the ring sketch (to do that, like when we extruded the triangle into a pyramid frustum, we need to select one area of the ring then hold the Shift key before selecting the second one as well, so we can extrude both at once as a single solid). When extruding a sketch interferes with an existing 3D shape / solid, 123D Design will default to subtracting the solid we are extruding from a sketch from the existing solid. To avoid this, one must select ‘New Solid’ from the drop-down menu available when clicking the little button besides the input field for the height the sketch is to be extruded to, before completing the extrusion by clicking on empty space.

After extruding the ring / pipe segment as a solid, not to its final height yet, we switch to creating a copy of the first pyramid we created, by selecting it then pressing Ctrl+C and Ctrl+V. When we paste a copy of an object, 123D Design automatically pre-selects the Move tool for the copied instance of the object so that you can choose to relocate the copy or change its orientation from that of the original. And we make use of this feature to rotate the copy instance of the pyramid so that it is upside down.

This enables us to make use of another feature of 123D Design, whereby we can push or pull a surface of one object until it is flush with a different surface of the same object or one of the surfaces of a different object. The surface we are pushing or pulling and the surface we are using as reference must be parallel for this to work. After pulling the top surface of the ring / pipe segment up until it is flush with the top surface of the upside-down pyramid, we again select the pipe and pull out both its top and bottom surfaces 5 units. This is because we want a narrow section of full, un-extruded pipe above and below the section of pipe which actually has triangular cut-outs extruded from it.

We then use the ‘Circular Pattern’ tool again, this time on the downward pointing pyramid and choosing to only have two instances of it (one copy besides the original). We also switch from the ‘Full’ mode to the ‘Angle’ mode of the ‘Circular Pattern’ tool, which allows us to specify an angle of rotation. We then specify a rotation of 30° because we chose to have 6 instances of the upright pyramids, which means a 60° angle between any two neighbouring upright pyramids.

And as each upside-down pyramid has to fit in between two consecutive upright pyramids it follows that it has to be 30° offset from either of the neighbouring upright pyramids in order for it to sit squarely in between them, evenly spaced from each. We then select and delete the original downward pointing pyramid, which we obtained by turning a copy of the original upright pyramid upside down, and again use the ‘Circular Pattern’ tool to this time create a circular array of 6 evenly spaced downward pointing pyramids, offset 30° from the circular array of upright pyramids along the circumference of the pipe.

All of the pyramids, both the upright and upside-down ones, are then subtracted from the pipe section, which results in triangular extrusions being cut out from the pipe. Finally, we select the Fillet tool from the Modify menu and drag-select, using that tool, all of the edges of the triangular extrusions to collectively apply a fillet of radius 1 to all of their edges. And we’re now done with the first way we can go about modelling this particular shape.

Second approach

The second way we can go about achieving a similar (but not identical) shape differs from the first approach described in detail above only through what shape we use to create the triangular extrusions from the pipe by Boolean Subtraction. And also how we come by that particular shape. And that is through using the Loft tool from the ‘Construct’ menu at the top.

We begin the same, by drawing a circular arc 22.5° wide to be able to build the full, 45° arc from that. Then we make the full arc into a circle sector by sketching the radii corresponding to its endpoints. Then we convert the circle sector by sketching its corresponding chord and deleting its arc.

However, we then begin to diverge from the previously employed method as we sketch an additional line cutting across the triangle, parallel to the former chord line corresponding to the arc we just deleted but laying inside of the outline of the inner surface of the pipe on the sketch.

We then extrude the area of the triangle which lays outside the perimeter of the pipe’s external surface outline straight up, rather than inwards to form a pyramid or frustum. Then we make sure to pull the top surface of the extruded shape up until it is level with the top surface of an downward pointing triangular extrusion from the first pipe we created.

After this we use the Project tool from the Sketch menu to sketch the outline of the outward (from the centre of the circle) facing surface of the shape we just extruded right unto itself. Then we use the Polyline tool to draw the two sides of an upright triangle whose bottom corners touch the bottom corners of the rectangle that corresponds to the outline of the face of the shape we projected unto itself and whose top tip touches the midpoint of the top edge of that same rectangle.

Before also extruding the area of the triangle sketched on the default sketching plane which lays inside the outline of the inner surface of the pipe on that same sketching plane and which is sectioned off from the rest of the triangle by the line cutting across it which we drew earlier, and which is parallel to the outward facing side of the triangle. We take care to extrude this second shape to the exact same height as the first one, by choosing the top face of that solid as reference surface to have the top surface of this new shape be flush / coplanar with.

We can now delete the shape we extruded earlier as we no longer need it and it will encumber us later. The Project tool is again applied now, this time to the outward facing surface of the triangular prism we just extruded, and so as to project the outline of that face unto itself, the same way we did with the outward facing surface of the first shape we extruded from the triangle on the default sketching plane. We can then use the Polyline tool again, in the same manner as before, to again draw an upright isosceles triangle bound by the outlines of the outward facing surface of the inner prism shape.

All of this has been a setup for being able to use the Loft tool to generate a shape from the two upright isosceles triangles we sketched on the outward facing shapes of the two shapes we extruded earlier. Because the shape generated by the Loft tool just touches the outward surface of the triangular prism, the tool defaults to merging the newly created shape to the existing upright triangular prism and we have to instruct it to create the new shape as a ‘New Solid’ instead of merging it with the existing shape.

And we can now delete the extruded prism as well, as it’s no longer required either. It was actually no longer required after we completed the sketch of the second upright isosceles triangle and we could have deleted it then and there. And had we done so and deleted it before using the Loft tool on the two upright isosceles triangle, this would have also spared us having to tell 123D Design that we do not want it to marge the shape resulting from the Loft operation with the existing upright triangular prism.

We are left with a triangular frustum of sorts, laying on its side, which we simply proceed with exactly the same with as we did with the upright extruded pyramids used in the first approach.

First take on the third approach

The third approach is the first one truly different, and is the one I fumble and stumble a bit experimenting with as it’s the very first time I employed this modelling technique which I’d thought about using before but never got around to.

With this approach, we sketch two lines parallel to a radius of the circle which is itself parallel to the Y axis. We do this using the Offset tool from the Sketch menu. This results in an enclosed area on the sketch, cordoned off by the corresponding outlines of the inner and outer surfaces of the pipe and also the two parallel lines offset from a radius of the circle. We extrude this enclosed outline downwards to obtain a 3D solid. Then copy, paste and translate a copy instance of that same solid upwards some ways before also pulling it’s top face upwards until it is coplanar with the top surface of an upside-down triangular extrusion in the first pipe.

Then create another copy of that translated copy of the originally extruded solid which is itself also rotated around the centre of the sketched profile of the pipe. As before, we do this using the ‘Circular Pattern’ tool in Angle mode again, and set it to two instances. I then ill-advisedly use the Fillet tool from the Modify menu to fillet all of the vertical edges of both solids before using the Project tool, similar to the way we did before, to project a face of each of the two solids unto itself. In this case, we project the top face of either solid unto itself.

Immediately after, I delete the two solids and apply the Loft tool to the two sketches of the desired profile of the pillar. This really isn’t the proper way to employ this approach, for a number of reasons. The first of which is that the Fillet operation is best left as a final, touching up operation and should generally *NOT* be performed before the Loft operation or in a way which will alter the output produced by Loft operations performed afterwards.

This is because you cannot remove or modify edge fillets built into the unitary surface of the shape itself, as a result of using the Loft tool on profile sketches which have already had their corners filleted. Surfaces of solids produced through lofting will not have seams or will have far fewer seams and will not be composed of primitive sub-surfaces such as flat, circular or spherical / spheroid surfaces or rotation surfaces produced by revolving a profile curve around a rotation axis. Which means you cannot remove or alter the filleting from the edges of the pillar if you perform the Loft operation on horizontal profile sections of the pillar which have already had their corners filleted instead of filleting the edges of the actual 3D shape of the pillar after generating it using the Loft tool.

Another very important reason why this isn’t the way I should have applied this approach is that you want to use more than just two profiles sketches with the Loft tool. In fact, the more guide sketches you use, the better, more accurate results you’ll obtain when using this tool. And it’s best to not just also use intermediary profiles in-between the beginning and ending profile, but also additional profiles after the beginning and shape of the actual length of shape you’re interested in. The Loft tool appreciates its freedom and will use every bit of leash you grant it, possibly producing quirky or undesirable results in the process. Whereas I myself only used a beginning and end profile sketch for the shape I was going for.

This means that the shape I create by Lofting may be free not to nicely curve around the circumference of the pipe but instead try and shortcut through the inside of the pipe to achieve the shortest span possible between the beginning and end profiles. This can actually be observed to have happened if we look at the pillar from above and see that, along its length, it spills inside of the circular outline of the inner surface of the pipe (pause the video at 14:49~16:05 to see what I mean). It also falls short of following the curvature of the outline of the outside surface of the pipe, which is also pretty bad.

After obtaining the pillar shape, I pull the top and bottom surfaces out a little so I can be sure I’ll obtain an interference fit with the top and bottom contiguous rings of the pipe surface above and below the section with the triangular extrusions. I then prematurely use the ‘Circular Pattern’ tool on the diagonal pillar I’d just created using the Loft tool before attempting to use the ‘Mirror’ tool from the Pattern menu to create another diagonal pillar leaning the opposite way around the pipe to then also apply the ‘Circular Pattern’ tool to that one as well.

This fails because shapes created using the Loft tool are complex (not comprised of simply primitive sub-surfaces stitched together) and the way the Mirror tool works is that if the mirrored instance of the original solid actually intersects the original shape, the original solid is subtracted (without being deleted as a result) from its mirrored instance before its mirrored twin is actually created. And because shapes created using the Loft tool are nastily complex and can perplex and bewilder the Boolean Subtract or Boolean Intersect tools from time to time, including this time too, the Boolean Subtract operation of the original pillar from its mirrored twin fails, which causes the Mirror operation to, in turn, fail as well (hence, the red banner near the top centre of the window reading ‘Invalid operation.’). The cube I created was just to use one of its faces as input for the mirroring plane parameter of the Mirror tool.

I briefly consider chopping the pillar along the plane defined by the same face of the cube I’d intended to use as mirroring plane (so as to avoid any intersections between the reference pillar and its mirrored twin when attempting to apply the Mirror tool again), before realising I’d either have to do that manually for the other pillars as well (which I’d created earlier by using the ‘Circular Pattern’ tool), or delete the pillars created earlier then have to apply the ‘Circular Pattern’ again later, which was actually the correct play.

I then choose ‘Hide Solids/Meshes’ from the visibility menu on the sidebar and begin monkeying about with sketches as I think about how to proceed. I get my bearings straight again at 17:10 again and sketch a line I’ll be using as splitting entity. Then I choose ‘Show Solids/Meshes’ from the visibility menu on the sidebar and chop off the part of the original slanted pillar which extents beyond the clipping and mirroring plane, defined by the line I’d just sketched. I then delete a neighbouring pillar to prevent it intersecting with the mirrored instance of the first pillar (didn’t remember whether other solids in the scene would likewise subtract from the mirrored instance of the pillar, not just the reference 3D shape it is a mirror of). I then merge the mirrored pillar with the original pillar. And proceed to delete the other pillars as well.

Then I attempt extrude the pipe profile. Which, as mentioned before happens when a sketch we are fixing to extrude intersects with an existing 3D shape, the Extrude tool defaults to subtracting the shape we are about to extrude from the existing V shaped 3D solids.

This time, I didn’t bother selecting all of the closed off areas of the sketch of the pipe profile and instead just opted to delete its end faces to close off the open 3D solid ring once extruded. As mentioned at times before, when choosing to delete a facet or surface of a 3D solid in 123D design, the software automatically attempts to extend faces or surfaces of that shape neighbouring the one(s) which have been deleted so that to close off the holes resulting from the deletion of one or more of its surfaces of facets.

I now create a copy of the ring I’d just extruded and closed off and move the copy instance of the shape upwards. I then use the ‘Split Solid’ tool from the Modify menu to cut the translated ring using the the top face of the first pipe segment as cutting plane. I pull the bottom face of the top ring down until it is flush with the top surface of the downward pointing triangular extrusions in the first pipe.

I then make the same mistake as before and try to apply Boolean Merge to the V shapes resulting from joining the mirrored pillars I which I’d applied the ‘Circular Pattern’ tool to earlier. I can scarcely believe my folly and try to rule out a few possible causes of the Boolean Merge operation failing before accepting that it is indeed due not having had the foresight to prepare mating surfaces by lobbing off the ends of the tips of the V shape before applying the Circular Pattern to it.

I see myself forced to use the Undo feature to return to the point where I had just one V shaped 3D solid, intending to use the ‘Two Point Arc’ tool to measure 22.5° one way and 22.5° the other way, along the circumference of the pipe – concentric with its profile, to then sketch radii from those arc endpoints to use as cutting planes for the top ends of the V shape. I manage to fail a little with that as well before succeeding and finally actually being ready to apply the ‘Circular Pattern’ tool to the now polished V shape.

This time the Boolean Merge operation has no trouble at all but I’m still concerned it will fail and so take my time, merging just two solids at any one time, even though this wouldn’t really have any effect whatsoever on the tool actually failing or not, in this particular application. We notice that a circular array of 8 V shapes fit together perfectly. This is because, remember, we rotated the top 3D solid whose top surface we used to project a profile sketch of the top end of the first tilted pillar by 22.5° relative to the solid whose bottom surface we used to project a profile sketch of the bottom end of the same pillar. A single V shape has an arm tilted 22.5° in one direction and it’s twin leaning 22.5° the other way, for a total span of 45°. And 8 · 45° = 360°.

After merging all of the pillars together it’s smooth sailing making the top and bottom ring. I ten use the outward surface of the top ring as cutting plane for the shape resulting from merging the circular array of V shapes. I need to do this because, remember, I extended the first pillar I create a short distance upwards and downwards beyond its original length, immediately after creating it by applying the Loft profile to its beginning and the end profile sketches.

And, as mentioned above, skimping on guide sketches is a no-no with the Loft tool as it will take any freedom you give it with pleasure and take the liberty of not producing the exact shape you intended. In this instance, skimping on intermediary and auxiliary profile sketches, in-between and beyond the end caps of the actual desired pillar shape, means that the Loft tool will take a shortcut through the inside of the pipe and fall short of touching the curved outline of the outside of the pipe along the entire length of each pillar. This also means that extending the pillars after lofting them, as I did, results in the ends of the pillars spilling out beyond the outer cylindrical surface of the pipe. Which makes the additional follow-up step of using the ‘Split Solid’ tool necessary to correct this.

I now actually need to apply the ‘Split Solid’ tool to the pillars yet again, to also trim out the portions of the pillars which spilled out on the inside of the pipe, beyond the outline of its inner surface. This leaves us with leftover shavings we have to delete after selecting them using drag-select having first hid the pillars and rings. Quite shoddy, untidy and unseemly work but that’s the way it is when experimenting with new techniques for the first time. We continue by applying Boolean Merge to merge the upper and lower ring with the section comprised of the leaning pillars before concluding with the Fillet tool, likewise using drag-select to choose all edges of all of the triangular cut-outs to apply this tool to.

Because of the shoddy nature of my work so far, we cannot use a large fillet radius value with the Fillet tool as the outside faces of the pillars aren’t flush with the circular external surface of the pipe as well as due to other reasons. As such, I have to settle for a smaller fillet radius value to use with the Fillet tool. I could probably get away with a higher fillet radius if I were to choose and apply the Fillet tool to edges individually. But that would create mismatches and prevent me being able to also seamlessly filet corners where 3 filleted edges meet, which is something I always strive for and the main reason for using drag-select with the Fillet tool and filleting all edges at once.

Second take on the third approach

The last pipe segment I begin working on is actually the exact same approach I used for the previous one, the third one. Except with fewer mistakes (no longer applying Fillet or rounding profile sketch corners before applying the Loft tool) and more foresight. But, being as lazy as I am, I do still skimp on creating the necessary additional intermediary and auxiliary profile sketches for the Loft tool when using that to create the first leaning pillar. Instead, I employ the workaround of pulling that pillar’s outward facing and inward facing faces out so that they extend cleanly and completely inside and outside of the outlines of the inner and outer surfaces of the pipe, respectively, before cutting them down to be perfectly flush with the pipe’s surfaces.

This is good enough though, as we don’t need or care about obtaining the inward and outward facing surfaces of the pillars from the Loft tool – we can just get those from the respective outlines of the inner and outer surfaces of the pipe and thereby implicitly and inherently also ensure that the pillars’s own inward and outward facing surfaces will be flush with and seamless blend in with the pipe’s own.

Testing the accuracy of the Loft tool

As such, it actually doesn’t matter that the inward and outward facing surfaces of the pillar created by the Loft tool aren’t correct and don’t adhere to the curvature of the inner and outer surfaces of the pipe. We only care for and want the sideways facing surfaces of the pillars as produced using the Loft tool. And those should be, for all intents and purposes, correct even when using only two profile sketches for the Loft tool. I’ve actually tested this out and, as you can see in this screenshot :

and as long as you are not using an overly broad sweep angle for the pillar (such as more than 30°, especially when the pillar is not very tall and this results in excessive lateral lean) the sideways facing surfaces of the pillar produced by the Loft tool will be quite accurate even using just two profile sketches.

In the screenshot above we can see that I sketched a profile of a pipe and then the outline of the pillar inscribed in the the outline of the pipe wall, with curved inward facing and outward facing faces of the pillar profile exactly coinciding with the outlines of the inner and outer surfaces of the pipe. One wall of the pillar (the leftward one) is exactly aligned with the radius of the curvature of the pipe and the opposite one is parallel with it while being slightly offset laterally, towards the right.

I then created a leaning pillar shape from that profile by using the Loft tool on two profile surfaces I obtained via the same method already described above. As likewise described above, we notice a fair amount of deviation of the pillar’s inward and outward facing surfaces from the respective outlines of the inner and outer surfaces of the actual pipe wall. However, as mentioned above as well, we don’t really care about that since we can simply pull out the inward and outward surfaces of the pillar until they are cleanly and completely outside of the bounds of the outlines of the pipe wall’s inner and outer surfaces then just trim away the excess using the ‘Split Solid’ tool.

And in the test I conducted and included a screenshot of above, after creating the pillar with the Loft tool using just a beginning and end profile sketch, I cut the resulting pillar in two exactly half-way along its height (using a cutting plane parallel to the default sketch plane) then set the colours of the resulting two halves to red and blue and projected the outline of the profile of the pillar along mid-height cut on the sketch of the outline of the pipe (which itself is on the default sketch plane) and we can see that the left facing sideways surface of the wall (at the point I cut it in half at) is still perfectly on the radius of the curvature of the pipe.

And the right facing sideways surface of the pillar is still clearly parallel to its left facing sideways surface as well (I actually tried measuring the angle between the outlines of the two on the sketch and no measured angle was displayed at all, indicating that, at least within the constraints of the limits of floating point precision and as far as 123D Design is concerned, the lines are perfectly parallel). I then made doubly sure of that by also measuring the angles between the edges of the profile of the pillar along the incision plane which correspond to the sideways facing surfaces of the pillar and those edges likewise showed no measurable angle between them either, just as their projection on the ground plane doesn’t.

I still goof a little early in this re-do though (when preparing for using the Loft tool – which I now use directly with the respective top faces of the two bodies I use to define the profile of the leaning pillars rather than going through the intermediary step of projecting those respective faces unto themselves (which would be necessary if I wanted to use more than two guide profiles) – I make the top surface of the top solid flush with the very top surface of the first pipe segment rather than, as I should have, the top surface of one of its downward facing triangular cut-outs, which is lower), and so this pipe segment ultimately ends up being taller than the others. Realising my mistake, I roll with and make this pipe segment taller.

Caveats, cost and considerations of the most difficult but best(?) approach

Also, the upright and downward facing triangular cut-outs produced by this approach aren’t perfectly aligned vertically, with the tips of the upright triangular cut-outs not reaching the same height as the top edges of the downward facing triangular cut-outs and viceversa. This is because, with the other approaches outlined above, neighbouring pillars don’t actually join into one at the top and bottom of the vertical span of the triangular cut-outs. Whereas with this approach, we did merge neighbouring pillars meeting at the top and the bottom of the overall vertical span of the triangular extrusions. Which squeezes out the triangular extrusion from between any two neighbouring pillars.

This can be corrected by just choosing to have 6 rather than 8 instances of the V shapes we arrange in an evenly spaced array using the ‘Circular Pattern’ tool. But had we gone that route we would have also needed to make the edges of the cross-sectional profile of the pillars corresponding to their sideways facing surfaces defined by two radii rather than two parallel lines evenly spaced from a radius of the curvature of the pipe (making the cross-sectional profile of the pillars the shape of a sector of a ring).

If we do not make the cross-section profile of the pillars the shape of a ring sector and we still model the pillars such that neighbouring pillars do not join together at the top and bottom, we’ll have extrusions which are the triangular shaped on the inside surface of the pipe and of a trapezoidal form on the outside surface. Which is most likely undesirable.

And we would have also needed to make sure that every pillar spans exactly 7.5° along the curvature of the pipe wall (because 6 · 45° = 270°; 360°-270° = 90°; 90° / 12 pillars for 6 pairs of non-joined pillars = 7.5°).

So, as we can see, this approach, while having the potential to be the best and, indeed, the only perfectly accurate / correct approach, is also the most complex, cumbersome, work intensive and time consuming as well. And it’s also the most mathematics heavy and requires the most concentration and attention to detail to avoid errors and it’s up to you to decide whether your intended result and the application you need it for require the accuracy of this method and are worth the additional hassle and time it requires. Finally, when all of the actual modelling is done, I take the time to set each pipe to a different colour.

A different take on the first approach

And now that we’ve concluded our review and analysis of the first three approaches to modelling this shape shown in the video above, it’s time to move on to the 4th approach we’ll discuss, showcased in the following additional video :

After creating the first video above, I recorded this follow-up to document a slightly different take on one of the approaches already shown in the first video, which is a subtractive method whereby we extrude material from the pipe rather than building the pillars from scratch.

The only difference between this 4th approach (I took a second attempt at the 3rd approach showcased above as I pretty much botched my first crack at it) and the very first one of those we’ve already gone over above is simply that we extrude the pyramid shapes horizontally rather than vertically. And that I had trouble with the Radeon Overly not showing up so I could select Region Capture from 123D Design and had to instead use the hotkey combo for starting and stopping recording using Radeon Relive not realising it would also record the Windows taskbar. Sorry about that.

This approach is pretty Mathematics heavy as well, because we’ll want to pick an inward deviation angle for the extrusion that results in the tip of the pyramid we extrude horizontally ending up (as close as we can get it to) being right above the centre of the curvature of the pipe. Of course, we can wing it and just manually close in on the appropriate angle by trial and error. Or we can try finding an online calculator that will enable us to accurately compute the dihedral angle between the isosceles triangle sides of a 3 sided pyramid and its equilateral triangle bottom face such that we achieve a desired height of the pyramid for a given radius of the base (the circle which circumscribes its equilateral triangle base).

I didn’t find such a calculator within a few minutes of Googling. The calculators I did find all took as input the side length of the pyramid base rather than the base radius. And the ‘Sketch Polygon’ tool in the Sketch tools menu in 123D Design only takes as input parameters the numbers of sides of the regular polygon you sketch using it and its radius. That is to say, the distance of its tips from the centre of the circle which circumscribes that particular polygon.

Pros and Cons of each approach

Let us now review an additional video comparing the cross-sectional profiles of the kind of pillars each approach of the ones we’ve gone over above produces :

  1. The first approach produces decent results. It’s clearly easier and quicker than the second (though not by much) and certainly the third approach. Its main drawback is that the cross-sectional profile of the pillars it produces is highly trapezoidal and thicker on the inside of the pipe wall than the outside, the opposite of how it should be. This could be corrected or mitigated at the sketch phase by making the tip of the triangular sketch we extrude the pyramid shape from (that we afterwards use to cut out the triangular openings in the pipe wall) extend beyond the centre of the circle and possibly even touch the outline of the inside surface of the opposite side of the pipe wall. Or maybe even further? This is something that would require trial and error testing to perfect. Another important drawback of this method (and related to the one already touched upon above) is that the respective tips and bases of the triangular cut-outs from the pipe wall are not aligned vertically (or along the axis of the pipe) with one another, on either face of the pipe wall and also across the pipe wall.
  2. Good mix of accuracy and ease of use / application. The pillars it produces are likewise trapezoidal in shape, but thinner on the inside than the outside of the pipe wall, which is fine and natural, actually, if one wants the tips and bases of the triangular windows in the pipe wall to be aligned vertically, both between themselves on the same side of the pipe wall and across the pipe wall as well.The only real drawback of this method is that it appears to produce pillars which thin out a little towards the middle of their span / height slightly.
  3. Potentially the best approach, if you take the time and hassle to apply it to its fullest. Also the most flexible. The drawbacks of this method are the considerable amount of work, time and hassle it requires as well as how error-prone it is owing to its complexity.
  4. A different take on the first approach. Still produces trapezoidal profile pillars which are thicker on the inside than the outside (rather than the other way around, as would be desirable) but much less so. The cross-sectional profile of the pillars is much closer to a rectangle but it still exhibits vertical misalignment of the upwards and downwards pointing triangular extrusions.

Conclusions and closing remarks

Finally, let us outline some closing notes and conclusions.

As the article title hints, there are often more than one way to achieve an overall similar (but not exactly the same shape) shape, especially when one is modelling somewhat of a more challenging shape. The various different approaches available will vary in their  difficulty, complexity, time required and may produce slightly different results, when working on a complex shape such as the one modelled in this article. As such, it’s important to put thought into exactly what shape and how we could go about trying to achieve it as that will inform the modelling process, the tools which need to be used and the steps necessary to get through to reach the desired shape.

If you’re willing to put the time into the planning stage, 123D is a very powerful tool capable of producing very noteworthy results. As 123D design is very much focused on technique and geometry focused modelling rather than modelling using pre-made modelling tools, it always pays to experiment with new modelling techniques and approaches, which can expand one’s toolbox of techniques and approaches not just with this modelling software but also much more complex ones. Other, more complex modelling software can unfortunately stymie their users’ growth and development of their own modelling technique toolbox due to fostering an over-reliance on pre-made tools and functions, which make the software itself more difficult to learn to use than a simpler software which relies more on user technique by providing only essential modelling functionality.

To be able to devise ways of modelling various different shapes, we must be comfortable with and aware of the respective capabilities of all of the modelling tools available in 123D Design, so we should be well acquainted with all of them, even if some will only be very seldom used.

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