But there are many ways to produce that in all 3D CAD packages – there is no 'preferred method' for each CAD package, only preferred method of the person driving the system (and the limits of his/her knowledge of the system being used).

Personally I might even tackle that slightly differently each time I try, as no one method jumps out at me as being simpler, faster, or more versatile.

Could use revolutions, or Extrudes, or a mixture. Could do it all as additive, or could do some subtraction.

I presume the 'pie slice shaped' hollows were omitted to keep things simple.

Edited By David Jupp on 11/04/2022 14:44:50

Took me longer to snip and name the images then model the reel.

The spokes on mine are flush with the ends so I could have had one less operation if diameters and spokes done as one sketch but often it is better to split things up for easier editing.

Start by drawing the inner ring and outer ring

Extrude equally either side of the mid plane

Draw a single spoke set central to the vertical axis and then use circular pattern to add the other 5

Extrude spokes as before

Draw the "D" section flange, top edge of flange set on same plane a stop of reel

Rotate profile around central axis

Mirror to get one on the other end

Job done

Edited By JasonB on 11/04/2022 16:53:55

Yes

Similar to other examples, except I used the Inset feature as another way to make the ends.

First analyse the part and work out a geometric design sequence in one's head. We can see that the part has symmetry around mid-depth (ends are mirror images) and also has rotational symmetry around the vertical axis. First sketch creates the outer rim and cylinder, and the inner cylinder, which are then revolved around the Y axis:

I'm using the XZ plane for mirroring. If I was going to 3D print or CNC mill the part i would have taken care to orient the part with respect to the XY plane, as that makes it simpler when importing the part into a slicer or CAM program. Only half of the part is modelled. There's no point in drawing, and dimensioning, both ends. Although not obvious in the above picture the inner cylinder is lower than the outer as per the original part. Add a spoke using the top of the inner cylinder as a reference plane and extrude to the XZ plane. The spoke is constrained to be symmetric about the X-axis and the width is dimensioned. The length of the spoke is unimportant (not dimensioned) as long as it overlaps the inner and outer cylinders:

Use the circular pattern function on the spoke extrusion to create the remaining spokes:

Add fillets:

Mirror everything about the XZ plane:

Andrew

PS – When I first started 3D Printing, a friend suggested Open SCAD for my design tool.

It's very easy to get into but does benefit from a more 'programmatic' way of thinking. I'm a bit more 'visual' in nature and also need engineering drawing capability, so moved on to Solid Edge. However, I've written a few simple SCAD models that can be easily modified to suit different applications – and it's very easy to share them too – just a text file.

Adrian's SCAD model was a simple cut n' paste and worked fine in Open SCAD itself – I've no idea about using the FreeCAD version I'm afraid.

Regards,

IanT

Edited By IanT on 11/04/2022 21:44:50

It's way past my bedtime Dave!

However – here we are. Circles by centre – just click and enter the dims (or size it later)

Did this a bit differently, drew a reference line and then rectangle by centre, then trimmed. Think it was quicker using lines…

Then extruded the spoke to length…

Used Pattern by Circle to make six spokes…

Then extruded cylinders to length (forgot to turn off extrude symmetry for screen grab – but corrected it)

Which gave me the basic reel shape

Set my working plane to the end face (note F3 padlock icon) and sketched new rim.

Extruded this sketch and repeated at both ends. Could have done half model and mirrored – but didn't.

Selected rim edge to round it….

And clicked to round it – same at other end…and that finished it…

Edited By IanT on 12/04/2022 00:11:55

There seem to be a large number of approaches to modeling any given 3D part, and my approach has evolved a lot over time.

In the beginning, my approach was to make models in any way possible.

I have since discovered that the "editability" (can we make new words here?) of a model varies greatly with how you create it.

Some models look great, but basicaly self-destruct when you try to modify them.

I generally draw a sketch in Autocad 2D first, and then import that skeetch into SW.

I prefer Autocad for 2D work, although SW will also do 2D work.

Here is my approach. Just a few steps to create it.

As for Solidworks, I find it quite polished and refined, and very stable; definitely not perfect by any measure though.

As has been said by others a lot depends on the user rather than the actual CAD package. Interesting that of all the various reels posted Dave's all look the least like the photo he first posted so who if firing blanks? Can't be three programs that can't get the spokes right can it?