In this article we are going to be going over a few techniques employing the ‘Fillet’ tool in 123D Design to achieve smooth, circular edges, faces and corners as well as quickly and simply model pipes with easily defined, arbitrary paths and curvatures.
To begin showcasing these techniques, we’ll start with the video below:
wherein I go about modelling an irregular bathtub or, if you are feeling charitable, a fort with peculiar walls. Please forgive the results since our aim here is not realism or usability of that which we model but simply a demonstration of a few of the modelling techniques we can employ to end up with smooth rounded corners and edges in actual modelling projects.
We begin by sketching out the footprint of the ‘fort’ using the ‘Sketch Rectangle’ tool from the ‘Sketch’ menu. After designing what might conceivably be the outline of a fort’s wall perimeter, we switch to using the ‘Trim’ tool to clean up the sketch (parts of the edges of the various rectangles we drew which intrude into the perimeter).
We end up with a clean although boxy perimeter outline for our fort or irregular bathtub. We then use the ‘Extrude’ tool, from the contextual menu of the sketch we just drew, to downwards-extrude a solid from the fort perimeter outline. After having done that, we actually no longer need the original sketch so we can just select it again and delete it by pressing ‘Del’ on the keyboard.
Now we can use the ‘Fillet’ tool from the ‘Modify’ menu to round the vertical edges of the solid we just extruded (we quickly and easily select just the vertical edges of that shape by selecting the front view from the view selector box in the top, right hand corner of the interface and then using drag-box select from the right, careful to only touch vertical edges with the selection rectangle; it’s important to drag from the right since that way the software will select any edge touched by the selection rectangle instead of only edges fully contained in it – as would be the case if drag-box selecting by dragging from the left) and that lets us get rid of all the sharp corners on the fort perimeter (which is now expressed by the top and bottom faces of the solid we extruded). While this approach is neither essential nor indispensable when dealing with such rudimentary shapes as in this exercise, this technique is very powerful and useful when one needs to turn sharp-angled corners of flat faces of more complex solids into smoothly rounded corners.
After that we proceed to create a solid of whose’s faces one will serve as sketch plane for the cross-sectional profile of the fort’s wall. Which itself we begin creating by projecting the profile of the face unto its own surface before then cutting the sketch in half along the vertical by sketching a line down its middle. This is necessary because when I placed the parallelepiped which I went on to sketch the cross-sectional profile of the wall on one face of, the centre of its bottom surface acted as snap/anchor point and that only snapped at intervals of 5 mm along the ‘ground’ plane (default sketching plane) whereas I actually needed it to snap at intervals of 2.5 mm, if the box shape had been just 5 mm wide. And I wanted the thickness of the wall to only be 5 mm wide.
Once I’ve cut the wall profile sketch in half with a vertical line down the middle, I delete the parallelepiped – which I’d only created in the first place so as to use one of its vertical faces as sketch plane. I then extrude the half of the sketch closer to the fort perimeter into a new tall box shape.
At this point we get to try out a simple but effective technique for turning a flat face of a solid into a 180° degree arch by simply applying the ‘Fillet’ tool to two parallel edges of that flat face and choosing, as radius for the ‘Fillet’ to be applied to those two edges, a value which is half the distance between them. For this technique to produce its best results, the distance between the edges needs to be constant along their entire span. Which is indeed the case here.
By applying this technique to the new, narrower solid we just created we turn its top face into a rounded arch before using one of its side faces itself to define the cross-section profile of the fort wall. We don’t need to project a sketch of that face unto its own surface first to use that as ‘Profile’ input for the the ‘Sweep’ tool as that tool can also take as input for its ‘Profile’ parameter a flat face of an existing solid, not just sketch.
For its ‘Path’ input we just use the edge of the top face of the solid we extruded first, from the outline of the footprint of the fort wall or bathtub we sketched at the beginning, and which we rounded the vertical edges of previously.
We now have our irregular bathtub / fort perimeter wall with a nicely smoothed round edge on top and can get rid of the rounded top parallelepiped we used one of the faces of as cross-sectional profile for the wall as we no longer need it now.
Notice that when I applied the ‘Sweep’ tool, it defaulted to offering to extrude the wall shape out of the parallelepiped with the rounded top, whose side face we used to define its cross-sectional profile. However, we don’t want to subtract the shape of the wall from that solid. This wouldn’t achieve anything and also deprive us of the solid we’re using to define the shape of our wall. We want our wall instead so we choose the ‘New Solid’ option. And after that, as the parallelepiped with the rounded top is no longer necessary, we can go ahead and delete that.
We now need to create a bottom surface or floor for our bathtub / fort perimeter wall. One approach for doing this is to slice the perimeter wall horizontally and then ‘delete the hole’ in the slice we obtained by manually selecting all of its inward facing surfaces (holding down the ‘Ctrl’ key while doing so) and pressing ‘Del’ on the keyboard to get rid of them once they’re all selected.
Something to be mindful of here is that it’s not always necessary to select all of the faces or sides of the hole before deleting them but not doing that can sometimes be misconstrued by 123D Design, with regard to what our intention is by doing that, and result in the software actually deleting part of the shape or the entire solid rather than the hole in it. What happens when deleting which or how many faces or surfaces of a shape is too complicated to explain here and is simply something we need to develop an intuitive feeling for through trial and error.
To actually slice the wall in the first place I created a small cube which is 5 mm wide, long as well as high (placing it on the default sketching plane) so as to use its top face as section plane for cutting the wall. Then I use the ‘Split Solid’ tool from the ‘Modify’ menu picking the wall as the solid to cut and the top face of the cube as the ‘Splitting Entity’. Which results in a slice of the entire wall which is 5 mm high.
After obtaining the slice of the perimeter wall, I go in and manually select (holding the ‘Ctrl’ key down on the keyboard) all of the inward facing vertical surfaces of the slice before choosing to delete them, which causes the top and bottom faces of the shape to get extended to cover the hole, yielding a solid surface with no punctures or breakthroughs. We can then use the ‘Merge’ tool from the ‘Combine’ menu to recombine the newly obtained solid floor with the remaining height of the wall we cut a slice for the floor out of and get our nicely enclosed bathtub fort.
Unsurprisingly, this method can be quite tedious and time consuming so a different approach may be preferable in most cases (I nevertheless showed this technique here because it’s important to be aware of all of the tools available in one’s modelling toolbox, even if some of them will only rarely be used). And, luckily, there is indeed a quicker, easier approach.
We just use the ‘Project’ tool from the ‘Sketch’ menu to project the profile of the bottom face of the wall on the default sketching plane. When you choose the ‘Project’ tool, you first need to let it know what surface to project to, by clicking on that surface (so I click on the default sketching plane), and then the face profile or edge or segment thereof to project to that surface. So I then click on the bottom face of the wall. If I didn’t want the profile of the footprint of the entire wall perimeter I could have chosen just the specific line or arc segments which I wanted to project by clicking on them one by one.
Once we obtained our sketch of the horizontal profile of the wall, we simply need to delete a single segment of the outline on that sketch which corresponds to the perimeter of the inner surface of the wall and that gets 123D Design to no longer regard that area, formerly cordoned off from the rest of the sketch, as an enclosed area. Meaning we can can extrude the sketch as one single unbroken surface with no holes or islands but just the contiguous outline of the wall’s outer surface alone defining the shape of the prism solid we will be obtaining, ridding us of the empty space we’d otherwise end up in the middle.
In 123D Design, when extruding a solid from a sketch and the top face of that shape touches the bottom face of an already existing solid (which is not set to hidden at that time), 123D pre-selects the option of merging the freshly extruded shape with the already existing solid (solids we extrude from sketches can either be created as new, stand-alone shapes, be merged to visible existing solids or be extruded from visible existing solids).
If we were to extrude further up than just 5 mm (to where the floor is actually intruding into the remaining height of the existing wall shape) 123D Design would instead default to assuming that we want to subtract the solid we are extruding upwards from the already existing one above it. We can, of course, override the pre-selected option of subtraction from (or merger to) an existing shape. In this case, I choose to create a new solid, not extrude from (or merge) to an existing one.
I then choose ‘Show Solids/Meshes’ from the menu on the right to get all solids in the scene to display. I do this to then clearly show that there are two different identical floors present and in the same location by then hiding one of them and having the other remain visible seemingly without anything having changed despite my hiding one of the two floors.
Because I created two identical floors through the two different approaches outlined above, when I go ahead and hide one of them by clicking on the floors (they’re identical so one of them gets picked at quasi-random, by z-buffer noise determining that at that particular pixel on the screen either one or the other of the two floors was closer than the other when that’s actually not the case; it doesn’t really matter which one gets picked) and then on the ‘Hide’ button, the one with a stylized eye symbol, the other floor – which looks the same – remains visible.
I then use the ‘Merge’ tool from the ‘Combine’ menu to merge one of the two identical floors to the remaining height of the wall. As explained above, I could have actually done this at the time I extruded the second of the two identical floors I created.
Once that’s done, it’s time to use the ‘Fillet’ tool from the ‘Modify’ menu again, this time to fillet the inner seam between the inside face of the wall and the top surface of the floor. I arbitrarily choose a fillet radius of 2.5 mm. After that I go on to also fillet the join between the outward facing side of the wall and the bottom face of the floor.
Because I deliberately made both the wall and the floor 5 mm thick, I now likewise deliberately choose a fillet radius of 7.5 mm (2.5 mm radius of the inner fillet + 5 mm thickness of both wall and floor). The reason for this being to get the curvatures of the inner and outer filleted edges to be concentric, which we get to see is clearly the case at the end of the video. This is another powerful technique which is all the more useful the more complex the shape it’s applied to is.
I temporarily slice the bathtub to show a cross-sectional profile of it before undoing that action and making the other floor I created visible again before sliding that 125 mm to the right. I then use the ‘Project’ tool from the ‘Sketch’ menu again, this time to project the top face of the floor solid on the default sketch plane.
I then delete the floor and get started on creating a profile to use with the ‘Sweep’ tool again. It’s at this time I recognize I dun goofed with this approach as inward pointing corners get an outer radius of 0 mm, making them sharp, 90° corners. Which simply won’t do.
So it’s time to reconsider and slide the rectangular parallelepiped 5 mm towards the inside of the bathtub outline, enough to straddle it evenly, before narrowing the rectangular shape 5 mm overall by pushing its side faces inward 2.5 mm each (same as before, the snap point for shapes is the centre of their bottom surface and the snap increment, on the default sketching plane, is 5mm, facts which, together, won’t really do when modelling a wall just 5 mm thick).
As before, we don’t actually need to project a sketch of a face of the shape unto itself so as to use it as ‘Profile’ input for the ‘Sweep’ tool. We can just use one of the solid’s own flat faces itself instead. Which is just what I do next, before finally deleting the parallelepiped as it’s no longer needed.
This second bathtub needs its floor as well, so it’s time to extrude the floor outline sketch upwards into a new solid that’s merged with the existing perimeter wall. After which I prematurely delete the floor outline sketch not realizing I still needed it. I then go on to apply the same filleting to the inner and outer seams between the walls and floor as I did for the first fort / bathtub, before realizing I still needed the sketch I’d deleted and undoing the last 3 actions to recover it before redoing the seam fillets.
I now slide the second bathtub to the right 125 mm and extrude the bathtub floor plan up the full height of the walls (20 mm) rather than just the floor thickness (5 mm) before applying the ‘Shell’ tool, from the ‘Modify’ menu, to its top face to hollow it out.
I choose a wall thickness of 5 mm (the bottom of the shape is regarded as a wall as well and has the same thickness applied). This yields the same wall and floor thickness as the first two bathtub forts modelled. It’s then a simple matter of filleting the seam between the inner surface of the perimeter wall and the top face of the floor and the seam between the outside surface of the wall and the bottom surface of the floor (to radii of 2.5 mm and 7.5 mm, respectively, just like before) as well as filleting edges of the top face of the bathtub wall to a radius of 2.5 mm to turn the wall’s previously flat top surface into a curved edge spanning its entire length.
The video ends with a cross-section of all of the ‘bathtubs’ created. I use the ‘Project’ tool to project the cross-sectional profile of each bathtub’s section face unto itself, to conclusively show that the curvature of the seam between the inner sides of the wall and the top surface of the floor and the outer sides of the wall and the bottom surface of the floor are concentric.
Let us now move on to another interesting and useful application of the ‘Fillet’ tool, which we promised we’ll talk about as well at the beginning of this piece. Namely to turn faceted shapes with sharp edges into accurately modelled, smoothly curved pipes. The following video will show us how it’s done :
We begin by sketching the footprint of the pipe (as seen from above), on the default sketching plane (which, in 123D Design, we can think of as the ‘ground’). For this method to work, it’s important that the pipe have the same diameter or thickness throughout its entire span and also that the pipe’s various curves flow neatly from and into one another. This is why we sketch the pipe’s footprint using concentric and tangent circles.
However, even though I didn’t use any straight lines in this simple example, we aren’t required to sketch pipes using only circles or circle arcs alone. We can also employ straight lines for sketching spans of the pipe which are straight. But those lines need to be tangent to the circles which portray the bends and bended corners of the pipe.
The ‘Trim’ tool gets extensive use here for removing the parts of the sketched circles which we do not require to define the pipe’s footprint or which intrude into that or are otherwise a hindrance or unpleasant clutter.
Once we’re done sketching on the default sketch plane and we have a neat and clean outline of the pipe’s footprint on the ‘ground’ we can go ahead and extrude that upwards, into a curved wall of sorts. However, before we can have our pipe, we need to also draw its projection’s outline on a vertical plane as well.
And to that end we lay down a cube to use one of its vertical faces as sketching plane, as we’ve also done before. The sketching process is much the same as the one used for the pipe’s footprint on the ‘ground’ so I won’t go over it again. When done, we need to use the ‘Split Solid’ tool to employ the sketch of the pipe’s projection’s outline on the vertical plane as a ‘Splitting Entity’ for the shape we’d just extruded upwards from the outline of the pipe’s footprint on the ‘ground’ a little earlier.
We’re only interested in the shape which can be obtained from the intersection of the respective extrusions of the sketches of the outline of the pipe’s projection on the horizontal and the vertical planes so we delete the rest of the curved vertical wall after having applied the ‘Split Solid’ tool to it.
We’re now, at last, ready to apply the ‘Fillet’ tool to the shape so as to finally turn it into an actual, smoothly bent pipe. I try doing just that by selecting all of the long edges of the shape before applying the ‘Fillet’ operation to them. Unfortunately, there seems to be a slight bug at play causing one of the selected edges not to be filleted despite having been selected and having had the operation applied to it as well.
I get around the issue by manually selecting each of the edges individually rather than just using drag-box select. If that hadn’t worked then just selecting and filleting the last remaining shape separately, after filleting the first 3 edges of the shape, would have surely resolved the issue.
I end the video by admiring and toying around with the newly achieved shape a little, briefly considering applying the ‘Circular Pattern’ tool to it (from the ‘Pattern’ menu) before changing my mind and settling on creating a cylinder at each end of the pipe and merging them to it before filleting the join seams as well.
Let’s now conclude this walk-through with two comparison videos showing the much neater and cleaner results yielded by the technique outlined above, which employs the ‘Fillet’ tool rather than the ‘Sweep’ tool – even though using the latter is the more intuitive (although clearly inferior) approach for obtaining such a shape, and probably the first which would come to mind when one first attempts it.
This just goes to show that your results when modelling with 123D Design will usually only be as strong as your modelling technique repertoire and your knowledge of the capabilities and limitations, strong suites and weak points as well as the respective recommended applications of the various tools in the palette provided by this software.
Because 123D Design puts the onus on the user’s technique and ability to visualize, imagine and fore-plan to achieve shapes thought of in their mind before being achieved in software, learning to use this tool to its fullest cannot not carry over to more complex software, with wider selections of more complex tools. And will be a useful and rewarding exercise to any CAD software user.