3D-CAD Package Shootout - Cotton Reel Example

I have read a lot about comparisions between various 3D modeling packages, and there are some features that are suppose to make some packages better than others.

In the end, it is not really the features I have found that make or break a 3D package, since these days many 3D packages offer basically identical features/tools.

It is really stability that is important, at least to me anyway.

I looked at Alibre, Autodesk, and Solidworks with I was considering purchasing a package, and ended up going with Solidworks because it had a good reputation, was a very polished package, but more importantly (the most critical thing to me) SW did not have the annual subscription, but instead a perpetual liscense could be purchased one time, with no further fees.

I have seen Alibre do things as well as SW, or better, but at the time, SW seemed to be a more professional package, and I needed it work work, as well as hobby modeling.

I went with SW, and the only gripe I have with it is that the models are version-specific, ie; a model created in SW 2012 is not compatible with any other SW model that was created in a later version of SW, ie: I cannot open a model created in a later version of SW.

I don't exchange many 3D models, and so it is not a huge problem, but I cannot convert files with a conversion program like I can with 2D AutoCAD.

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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.

The fastest way to create a 3D model not necessarily the quickest model type, but rather the model type that can be most easily edited after it is created, especially when you get into complex models.

Some model shapes are more easily edited (stretched, etc) after they are created, and so sometimes I take a more modular approach, even if it takes a bit more time initially to configure.

It is a bit of an art, that much is for sure.

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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?

Very interesting, watching.

A version in Fusion 360

Cotton Reel

Another variation in MoI - sorry for dawdling part-way through, I had a slight distraction.

Martin.

Pat's comments are the ones that really matter here.

Making the body from 3 separate extruded cylinders looks simple but it doesn't make for a particularly good part, and is not easily editable if you need to change any dimensions. The same applies to creating the bore separately. And it's all so slow.

I used a single solid revolve originally, but the gaps had to be cut out using a more complicated sketch. The single spoke in an existing hole then patterned as a feature is easier to draw, easier to understand and all attributes can be changed simply. A major reason for using CAD is not having to do the calculations to decide on the angles or lengths of lines before drawing them.

Name the sketches and operations as you do them, because it's hard enough remembering what did what later in the day. You'll have no chance in six months when you want to make the part out of different material.

One example of using references is for a steam cylinder with flanges on it.

The first cylinder I 3D modeled went well enough, and then I decided I needed to make it longer, and so I edited the length. The flanges were not referenced from the ends of the cylinders, and so the flanges got larger, instead of remaining the same thickness.

I use revolve quite a bit, but I am not sure how well it stretches, or what that does to the references.

As I have gotten into some more comlex modeling, I often have to make up techniques as I go, and sometimes that works, and sometimes it does not.

Remembering what I did 40 steps back can be rather trying, although one can generally poke around and figure it out. What I do now for comlex parts is to hit the "print-screen" button after each step, and past that into a photoshop program.

Then all I have to do is flip back through the screen captures, and I can seen exactly what I did, even a year or more later, and very quickly figure it out.

But getting back to the basic question of the thread, if you can trade of some stability for cost, then there are some good inexpensive packages out there. I think all of the 3D packaged have improved over time.

I should note that I looked at one rather expensive 3D package, and then read the reviews, and professional users said it had stability issues, so this can occur across all price ranges.  Do your homework.

If you can't afford to have a part lock up in mid modeling, such as with a complex work project with a tight deadline, then you spend more money on a more stable product, since that is actually the cheapest route in a work project situation.

And Solidworks has a large number of features that I never use.

I do use motion studies to run steam engines virtually, and this is very helpful since if your model is not exactly correct, the program knows, and the engine will not run in simulation (which is very frustrating, so I test one part at a time, to keep track of which part makes it all stop running).

SW has some molding features, and since I do foundry work, this sometimes is handy.

I can make a model, draw a cube around it, and then create a mold cavity, such as would be used for a corebox, and then 3D print a corebox.

Generally speaking though, I use just a handful of tools over and over again, such as extrude boss, rotate boss, extrude cut, revolve cut, fillet, and draft angle since I 3D print patterns.

I would guess that 95% of my work uses the above commands only.

It took me a while to figure out how to add planes where needed them, and rotate those planes.

Once I figured that out, life was much easier.

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Edited By PatJ on 12/04/2022 12:07:02

Edited By PatJ on 12/04/2022 12:09:16

I used AutoCad as 2D then Inventor for 3D, quickly got in the habit with Inventor of creating parts as they would be made ie starting with a basic block or round. Doing it this way I was sure that the part could be machined. When I started as a self employed contractor with firms that had just took up Inventor I saw many occasions when some feature were just impossible to produce. Whilst my approach may not have used the minimum of key strokes I could still edit it at the end.

I hadn't intended anyone to do the spokes, thinking it was a useful next step. Gold star to all those who added them, though it's very naughty they copied the photograph rather than the drawing! The boss will be furious when she finds out: the reels are to be milled from stainless steel blanks, and machining sharp corners will push the price up!

Good point about the importance of the operator. CAD doesn't have a magic button for drawing cotton reels and there are a number of strategies by which they can be modelled. We haven't seen them all yet! Some get a quick result whilst storing up trouble if a fundamental changes later. For example, starting with a sketch that models the spokes first creates a structure less resilient to change than one that cuts the spokes much later. Will the model break if the customer suddenly announces the reel's diameter should be bigger or smaller?

Dave

How about a quick computer mouse in MoI?

Martin.

Let's see what happens in Solid Edge Dave....taking my existing Cotton Reel model...

Used smart dimension to select the outside reel diameter and change it to 40mm (from 30mm). I can do this because it is not a dependent dimension.

So then do the same for the internal diameter... (radius from 12.25 to 18mm)

Spokes still look OK. Might not have been as predictable if I'd tried to increase the internal diameter to exceed the external one first though. To be clear, I've only changed the two diameters here - nothing else was altered.

Regards,

IanT

As others have pointed out, a 'quick and dirty' one off use model may be done a little differently to a model that will have the key dimensions re-set multiple times to produce variations on a theme (without throwing errors, or disrupting the topology).

Both have their place - there is no single 'correct' answer.

My poor attempt, just noticed I've only done 4 spokes. Solid edge, draw half the outer profile on one face, revolve it, draw the Sector holes and centre hole on the top face, cut extrude.

I've used SE 2D before (quite a while back), but never the 3D. It wil take some getting used to but there are a lot of features to say the least.

I think an interesting comparison would be to see which program(s) easily allow the modification of the various types of generated shapes, such as the spindle.

I have not kept track of such things, but I have noticed it from time to time, that I can't edit some shapes as easily as others.

I am not sure if this is due to limitations of Solidworks, or whether it is inherit in the way all 3D modeling programs work.

I have had situations where I extrude some shape, and it all works fine for a while, and then I have to add a few more shapes or cuts, and the whole thing gets balled up, to the point where I basically have to start over with a completely new approach.  Sort of like what I imagine a game of chess would be like (I don't play chess, but I can imagine).  Things tend to cascade, sometimes with very bad results.

Occasionally I can drag a feature up or down one or more levels, but this rarely works.

The places on the feature tree can be critical.

No two objects are exactly the same, and things like draft angle and tapered support legs can really throw some wrenches into the gears.  Compound curves can also be challenging for the best of 3D programs.

I definitely learn something new every day in 3D modeling, and have learned quite a bit already from this thread.

Discussion is definitely a good thing.

Sometimes I use a hybrid of all the methods shown.

3D modeling definitely forces creative thinging.

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Edited By PatJ on 13/04/2022 00:49:15

LOL, that would be "thinking".

Speed typing has its disadvantages.

But as I mentioned about chess, the first few moves can be critical, and may determine the win/loss outcome.

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Seeing as how the world and his dog are taking up the challenge, I might as well weigh in with my effort.

First, draw the cross-section of the main body, then extrude to 28mm

(I had to take some artistic licence with the diameter of the body as I couldn't see a dimension given)

Next, add the end "flange" by duplicating the original cross section and increasing the outside diameter before extruding it 1.5mm.

Mirror it onto the other end about the central plane, add a bit of filleting bling and render it without the joins:

John

Now I'm off to contemplate how many ways I can think of to kill a cat!

Edited to include facetious comment!

Edited By John Hinkley on 13/04/2022 10:04:13

'Creative thinging' is a pretty accurate description of my interest in Model Engineering!

I've learned from this thread too, and one factor is the different ways people approach solving the same problem. Even when modelling an object as simple as a cotton-reel! The difference between liking and hating a package might be how slickly the software caters for our individual mind-set, which we might not realise is ill-adapted to the problem. Learning is difficult!

So far all the packages have survived the shootout: they all do the job! I think only one has shown a clear reason why some people should avoid it. OpenSCAD models are built with mathematical scripts, which is a powerful technique, but a particular type of intelligence and skills are needed: maths and programming!

Adrian gets First Prize for the most direct answer, but the 'Programmers Solid 3D CAD Modeller' is a steep learning curve if you don't know a bit about set theory, coordinate systems, programming, and the language. Adrian's OpenSCAD solution:

$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
}

Although there are compelling reasons for modelling by writing code, I don't think they apply to the majority of mechanical engineers, especially hobbyists. Most of us, I think, are happier clicking buttons with a mouse. Programming is difficult. By the by, Adrian's cotton-reel in the picture above is missing its top: my fault - as an officious ex-C programmer, I added an extra semi-colon, which changed what the code does. Oops!

Dave

I know very little about other CAD systems Pat - but my understanding is that most use what is called "Ordered" mode - that is one based upon a build history. Solid Edge offers both "Ordered" and "Synchronous" modes and you can switch between them if required. Normally you set a default design mode and I decided from the outset to (learn to) use synchronous mode, as it seems to be preferable in general use.

More experienced CAD users (coming from other 3D systems) may find ordered mode more familiar. In terms of my general design work though, synchronous seems to be the better choice. This may be a feature unique to Solid Edge but I don't really know.

This short video explains the differences between the two modes better than I can.

(2) Synchronous vs Ordered Modes in Solid Edge - YouTube

Regards,

IanT