The Phys Ed director approached me at the school before the break asking if I could fix some parts of their Frisbee Golf equipment and explained they no longer make the kit so they can’t purchase parts any more and a new kit would be over $1000.
I said I’d give it a try and try to design the parts in CAD then see if 3D printed printed parts will hold up. The first part I’m attempting is an adapter between 2 different sized square tubing.
The adapter is tapered smaller by 1mm at the ends so that the square tubing slips on better.
The adapter has tapered ribs along each side which taper toward the ends of the adapter.
There is an interface between the 2 ends of the adapter which is also tapered.
Here’s a picture of a good adapter:
I’ve setup a bunch of parameters in a VarSet and tried to experiment with a loft between a square and a square with a bunch of notches in it to see if it would loft and it didn’t.
So my current approach is to create 3 parts which are all tapered. The large end, small end and the interface between them. I lofted the large end negative to the XY plane, lofted the interface above the XY plane then lofted the small end adjusting the Attachement Offset of both sketches by the height of the lofted interface.
For a stab at the ribs, I selected a side plane of the top/small side and drew a sketch of one tapered rib then I padded it followed by applying a Linear Pattern. I now have to do that 7 more time. Here’s what it looks like with just one side with ribs. Oh and I tried 6 ribs but for some reason the geometry went bonkers between the first and 2nd rib so I reduced the count to 5 and it looks like it’ll work.
Probably not very helpful but this is a way to do it in Blender (same in Zbrush and 3dCoat). I have 4 or 5 CAD programs on my computer but my brain just doesn’t work well with them.
It’s a little bit trickier in that not only are there 2 sizes of tubing going over this(smaller on top, larger on bottom) but there is a taper between the center stop-edge and each end of adapter PLUS those tapers on the ribs. This is why I was trying to use the loft tool between 2 drawing/sketches. It could be that the taper, which is only 1mm, is there for mold release in the injection molding process but I’m not sure so I’m trying to be faithful to replicate the original.
I’m guessing you did a lot of copy and pasting to get the ribbed design to extrude. In FreeCAD it’s a bit more tedious with line drawing and then sizing all of the line segments. I was thinking I could put in the initial effort of one sketch drawing and then copy/paste resize and loft between 2 sketches but my test wouldn’t work and I ended up lofting squares of the inner diameter/size and then adding on ribs. Took me a few hours. ugh.
And while the original is hollow, the adapter only has parts fitting over the outside of the 2 ends so I’m making it a solid and will print it horizontal with 6-8 perimeters and 5% infill.
It is a completely different way to create a 3d model as compared to CAD. One reason I have such a problem working with CAD.
Made a square.
Extruded the square to create thickness.
Subdivided by 13, selected alternating outside edges on one side and extruded for the ribs.
Deleted the other three sides and then revolved the side around the center origin.
Joined the geometry and deleted the additional points created by joining. Ready to extrude on z axis.
I could have done it parametrically using a circular array command. Probably half a dozen other ways to create the base.
The different sizes for top and bottom would literally be one resize command for the geometry.
For any folks that want to play with a hybrid system, there is a branch of Blender that is attempting to add CAD-like functions called Blender CAD Sketcher.
Could you post a couple of pics from different angles? Like, straight from the side and another view? This looks doable in Solidworks if I have the exact dimensions.
I’ve not figured out how to get the VarSet data out into plain text but here’s a pic of the parameters I used for most of it. The radius of 8mm didn’t work because I have the ribs too close to the corners so I used 7mm hardcoded which now seems dumb because I could have used the parameter name, switched to the tree view, changed it to 7mm then back to the Fillet Data window. The taper parameters are as follows:
Rib taper is across the length from the interface(center element) so it’s 3.5mm wide at the interface and 2.5mm at the ends.
Side Tapers are measured on the outside of the ribs so the total outside dimension at the interface(center element) is 80mm for the large side with 79mm at it’s end, then 74mm for the small side and 73mm at the small side end.
SideH is how long each section is from the interface(center element).
I’d be interested in your technique/steps you’d use to create the model. I’ve skipped making it hollow since there’s nothing interfacing with the interior and a little 3DP infill will add some strength since 2 4’or 5’ sections of square tubing fit over this adapter to hold the Frisbee Golf basket. There is also a base section I have to reproduce which uses the large size square of the adapter and has 4 horizontal studs fitted so some extension footing tubes can be added.
That’s an elegant way to do it Oscar! I’ve only dabbled in Blender and wouldn’t have been able to guess at that method nor figured out how to get all the geometry stacked. Literally everything is tapered to some extent.
Pick a plane that allows you to put a vertical line from the origin straight up (or down, it doesn’t matter since it will be a revolve axis and direction isn’t important - only the location and angle). I used the “Front” plane. Exit sketch and hide it for now, or not.
I was laying this out and planned on padding out the ribs, but realized that you cut away the material between the ribs, so you can do one of two things:
You can make the square 1.4mm narrower on each side, so that when you pad out the ribs, it is the proper outer dimension (easiest to do).
You can do what I am doing below, and basically dimension where the rib would be padded out, and then modify it to remove the material around it.
Create two vertical construction lines: One that is [74mm / 12] (half of the 74mm / 6 rib spacing because it is at the edge, and only needs to be spaced 1/2 the normal rib spacing from the edge), and one that is [74mm / 6], the regular rib spacing.
Then make your trapezoid that is 3.50mm at the bottom, and 2.50mm at the top, centered on the vertical construction line. Now make the left half of the next one, so we can get the spacing needed to remove the area between them.
So, now we can remove the area between the ribs, but if you do a regular cut, it will make the cut normal to the sketch face, which will result in something like this - a little slice left at the top, because of our 1mm draft.
Ok, I see that. Nice. Listing just so it’s more ‘in my head’.
Draw one simple sketch on XY plane of one end element of the adapter, centered and extrude.
Create a sketch along the Z axis(any one works) draw a line vertically through the origin. hide
Create sketch on one face and draw 2 right-triangles to cut the taper.
Cut the taper sketch followed by a circular pattern of 90 deg around the vertical center line.
Got it. Since you used the full 74mm of the outside dimension of the small end I’m thinking you will also do a similar thing, cutting and rotating to cut out the grooves which will create the tapered ribs.
Ok, I see that. Nice. Listing just so it’s more ‘in my head’.
Draw one simple sketch on XY plane of one end element of the adapter, centered and extrude. Yes
Create a sketch along the Z axis(any one works) draw a line vertically through the origin. hide. Yes
Create sketch on one face and draw 2 right-triangles to cut the taper. Yes
Cut the taper sketch followed by a circular pattern of 90 deg around the vertical center line. Yes
Got it. Since you used the full 74mm of the outside dimension of the small end I’m thinking you will also do a similar thing, cutting and rotating to cut out the grooves which will create the tapered ribs. Yes
Forgot to do the little chamfer on the ribs at the end. Did like before, made a sketch on the side of one of the ribs, and made a triangle. I just used 3mm for the long edge because it looked about right.
Like before, this is on an angled surface, so an extruded cut wil not get you what you want. You will have to pick the direction of the cut, which is along the top edge, so pick the top edge.
Here is the cut if it were normal to the sketch surface.
The center interface (adapter interface I assume) does not have to have a specific shape, other than a taper, so you could do a regular pad, and then chamfer one edge.
This is the part of doing CAD I believe is often overlooked in tutorials. ie the approach to the task can make things easier or even just more intuitive along with sometimes painting the designer into a corner.
As you can tell from my approach, my first thought was using the loft tool to sweep between 2 different sized sketches which I figured would be a little work on the first sketch and then some copy/paste/scaling work. That wasn’t working so I saw it as an additive process. But that did require me to have all dimensions of the base rectangles a function of the measured outside width minus the depth of the ribs.
And I just saw how you also used the subtractive method to make the chamfers on the ends.
Those are way more controllable than how I used a Chamfer tool and had to deal with the rib thickness and where I’d ended the rib. Nice!
I will practice a walk though of the subtraction method you used just for the experience.
I’ve done some cleanup of my rib locations and spacing and adjusted the corner radii to 8mm. ExtensionAdapterV2.FCStd (2.1 MB) ExtensionAdapterV2.step (1.4 MB) ExtensionAdapterV2.stl (4.6 MB)
Yeah, I didn’t notice initially, but the rib spacing was not what I thought it was, so when I got to the 8mm fillet, it wouldn’t work, so then I went back and looked closer and saw that the rib spacing appears to be uniform - same spacing from edge as is from center to center. Nothing wrong with that, I just typically do it such that the edge spacing is half that of the center-to-center spacing. Usually, it is because I may be assembling more of whatever I am designing into a larger assembly, and doing it that way allows for the proper spacing between sub-assemblies when they are aligned next to each other.
Lofting definitely has a place, but I reserve that for when I need to extrude from one shape to another shape - square to circle - or the like. Otherwise, creating a linear taper is more easily done with the cut I demonstrated, or if you want a specific angle, using the “Draft” feature.
The draft is nice because it tapers the full edge length, unlike a chamfer where you have to specify the length.
