3D-CAD Package Shootout - Cotton Reel Example

All too often a question about choosing 3D-CAD software descends into a confusing exchange of conflicting personal opinions, leaving no one the wiser! Name a package and some swear by it, while others swear at it.

This thread asks CAD jockeys to show how their preferred product produces a the same common object. It's purpose is to show the steps necessary to go from a set of dimensions to a finished object. By keeping the object simple, we can concentrate on how each CAD package gets to the goal, and compare how they each do an actual job. I suggest this is more informative than a generalised discussion because newcomers will see the look and feel and how well or not they tune into the workflow. Let's demystify!

The target is a plastic cotton reel, and the model could be 3D-printed in plastic or turned on a lathe. This is the original:

Dimensions given in this drawing to no particular standard. QCAD used, back of envelope would do. Note the inner fins aren't called for, yet!

The 3D model should look like this:

I'll start with FreeCAD;s Part Design Workbench, then do the same with Fusion360. As will be seen when both are published the workflow for producing a cotton-reel with these two is almost identical: the difference is mainly look and feel. If you can drive Part Design, you should be OK with F360 and vice versa, at least for simple objects. In practice, F360 is slightly slicker, but they take about the same time to do this job. I like them both.

How to with FreeCAD next post.

Dave

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

Exactly; created this in five minutes in Alibre:

I suspect my method is a bit involved, as it includes extrusions, revolutions, circular patterns and a mirror operation.

Andrew

FreeCAD latest version is 0.20, but this is still a bit experimental guv, so I'm still using the current stable version v0.19.3 (Linux AppImage on Ubuntu 20.10). FreeCAD is available from here, installation should be straightforward.

Start the package by clicking a desktop icon or finding it with a search.

Select 'Part Design' top right next to the red button and click on the big plus Create New Button, opening a 'Create Part Window:

Click on 'Start part', which opens a window asking which plane you want to draw in. Doesn't matter much, select XY:

Click OK, and note the Task Bar on the right now allows new options:

Click Create Sketch to start the sketcher and draw a circle on the centre point with the circle tool (button with two red dots and a circle). Set the diameter to 30.56mm with the red ⌀ button. My screen has constraints vertically listed on the left, by default it's on top with the others.

The circle goes green to indicate it is fully constrained, i.e. it's centre coordinates and diameter are both fixed and won't move. Press the Close Button in the Task Pane to get a set of options that can operate on the circle.

More in next post

Dave

Hi Dave,

I don't think that the diameter of the inner cylinder is specified in your drawing. Apologies if I am being dim. I'll use 28mm for no good reason

Here it is in OpenSCAD, for the programmers in our midst (a small contingent here, perhaps).

$fn=360; // Set number of segments in a circle
difference(){
union(){cylinder(1.5,15.28,15.28); cylinder(31,14,14); translate([0,0,29.5]) cylinder(1.5,15.28,15.28);}
cylinder(32,2.8,3.8); // Remove the cental hole from the rest of the reel
}

Quick plug: if you are a railway modeller interested in 3D printing you will find lots of useful advice and CAD models in our Gauge One 3D circle forum which you can find here: **LINK** and you'll find a tutorial on OpenSCAD that I wrote for my students here: **LINK**

Adrian

Click Pad and set the pad dimension to 1.5mm. Click to update the screen This pad creates the bottom of the cotton reel.

Click OK to close the Pad dialog, then select the top face of the cotton reel to select it. Should change colour:

The option to Create Sketch has reappeared, so click on it allowing allowing a new sketch to be added to the object. Draw another circle and constrain it to 28.00mm Closing the sketch allows this one to be padded as well. Press pad and set the dimension to 28mm as well. OK the Pad, to reveal:

In the same way, select the top face again by clicking it, create a new sketch with a circle diameter of 30.56mm, close the sketch, and Pad to 1.5mm:

To add the hole, select the top face and create another sketch, this time making it 7.6mm diameter. Close the sketch:

This time select the Pocket tool (Pad adds, Pocket subtracts). Set Type to 'Through All' and the hole is drilled.

Closing Pocket leaves us with a completed model cotton reel. FreeCAD understands it to represent a solid and can use it to generate the usual 2D projections, to which the user can add dimensions, notes and sections:

Or to export the object as a mesh or STL. These define the outer envelope of the solid and are used by other software to generate the additive g-code needed by a printer or the subtractive g-code needed by a CNC machine to cut metal.

Takes much longer to describe than do.

Fusion 360 next, after a nap and strong coffee. Delighted to see others submit the same job in Alibre, TurboCAD, MOI, Draftsight, Solidworks or any other favourite. Please don't cheat by doing it with one sketch and a rotate: I want to show how pad/extrude work with a succession of sketches.

Dave

A slap in the face with a wet fish is in order.

The original post asks how a preferred CAD package would create the given part. The latest post then says don't "cheat" by using revolve. The object is round so revolve is a logical operation; how is that cheating? I'd use two operations to create the "simple" shape; revolve followed by mirror.

Andrew

Yes, I know Alibre is a big hitter, but can you explain step by step how you did it!

Trivial to do in FreeCAD (and F360), though I haven't done the cut out properly.

Dave

My mistake Adrian, it is 28mm.

OpenSCAD is bundled with FreeCAD. I've never used it and will report back if I can get your code to run!

PS.  I guessed how it might be done and got errors:

16:06:57 Parser Loaded
16:06:57 Start Parser
16:06:57 Syntax error in input!
16:06:57 LexToken(ID,'$fn',1,0)
16:06:57 Syntax error in input!
16:06:57 LexToken(NUMBER,'1.5',2,79)
16:06:57 End Parser
16:06:57 None
16:06:57 End processing CSG file

Pretty sure this is due to me loading the program incorrectly.

Edited By SillyOldDuffer on 11/04/2022 16:20:48

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

Like it! Is that Alibre?

Yes

Here's Fusion, and there is no way I wouldn't use revolve:

Draw a construction line vertical from the origin, and a centreline centred to the origin. Add three rectangles, constrained symmetrically around the construction line, and make the two longest lengths equal.

Add the lengths

And the diameters from the centreline so no radius calculations are needed

Finish the sketch, and select both profiles. Click on Revolve, and Fusion automatically picks up that the centreline is a suitable axis, which is why it was defined as such

The resulting body, with the sketch still active

That's a new sketch, on the midplane; with the two diameters projected from the body, a vertical construction line from the origin, and a rectangle symmetrical to the line, tangent to the bigger circle, colinear to the small one and 1.5mm thick

Extrude the spoke profile symmetrically to the end of the body, ensuring that it is a join.

Use the spoke feature in a circular pattern, around the axis to create the other spokes.

Apparently, it will weigh 6grammes if made from ABS plastic....

Edited By Nicholas Wheeler 1 on 11/04/2022 18:31:51

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

This is Cotton Reel produced by Fusion360 using the same sequence of sketches and extrusions as I did with FreeCAD.

First start the package. Then click the start sketch button circled ib blue below:

Next screen, click on a pane to select the plane:

That done, draw a circle and set its diameter to 30.56mm:

Right clicking inside the circle opens a dialog with a Pull option. Pull's big blue arrow can extrude positively ('Pad', or make a negative hole. Pull positively and make the dimension 28mm:

Finish the sketch and open a new one on the end of the bobbin. Draw a circle of 30.56mm dia and pull by 1.5mm to add the reel's top end. Start another sketch on the latest end and draw a cirle diameter 7.6mm. Pull this one back through the body of the reel to make a hole:

Close the Puil, job done.

Dave

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

Didn't bother taking snapshots as I went along & I also think this can be done in a number of ways. Nor do I really see the point of this exercise quite frankly, because to a large extent - a) the result must depend on the skill of the user (and I'm certainly not the most skilled SE user, so certainly not the best to champion it) and b) I'm pretty sure most CAD systems could do this quite easily.

However, in Solid Edge, I did the following;

Sketched the basic reel outline (circles by centre) & then dimensioned them, added a spoke (two lines). Extruded the spoke and used circular pattern to create six of them. Extruded circular elements to length. As an after thought added the two outside rims and rounded them. Could have used mirroring but didn't.

Regards,

IanT

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

I'd be grateful if you could post snapshots Ian because you''re the Solid Edge ambassador! Without your help we have no idea what Solid Edge looks like, or what steps are needed to get to the answer.

Not a high-skill exercise because a Cotton Reel is pretty simple, and a few interesting ways of doing it have been demonstrated: Adrian's SCAD code is very different from Andrew's mirroring, Nicholas's revolve, and my Pad and Paste.

So far Solid Edge remains a mystery compared with OpenSCAD, Fusion, FreeCAD, MOI and Alibre. And thanks to Blowlamp video I now understand why people like MOI, and must have a play with it.

Go on, convert me to Solid Edge, pretty please with a cherry on top!

Dave

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