Learning CAD with Alibre Atom3D

[David JuppParticipant @davidjupp51506]

Ah yes – Jason has it, I keep forgetting that the simplified interface for Atom3D does a few things differently from Alibre Design.

Edited By David Jupp on 15/03/2019 11:22:10

Edited By Neil Wyatt on 01/05/2019 13:54:46

[Neil WyattModerator @neilwyatt]

Posted by Nigel Graham 2 on 14/03/2019 23:01:08:

TurboCAD has a third way to generate solids: "Primitives", a few common solids like cuboids and cylinders you set to your own dimensions. These too, have their own characteristics.

I forgot those!

I think you might do well to set out exactly what you hope to gain from using CAD, whether 2D or 3D.

Fore some jobs, the back of an envelope is entirely adequate but if you want to design for a 3D printer or CNC tool, 3D CAD is virtually essential. And there's all sorts of things in bewteen.

Neil.

[Nigel Graham 2Participant @nigelgraham2]

Thank you Neil.

I can answer that: I knew what I hoped (and still wish to) gain from CAD before I started, and I always knew the envelope-sketches still have a place.

The main points for me were and are:

Orthogonal drawing techniques whose advantages over manual drawing, include:

– copying repeated features or even large parts of the drawing, readily and accurately, to another area or even a new drawing.

– making changes or corrections more readily and less messily than on the drawing-board (I saw parallels with word-processing v. typewriters here),

– accurate dimensioning, as the computer does the sums,

– consistent lines etc, admittedly more aesthetically than functionally important.

Also, Isometrically-based assembly-drawings readable from different sides, to help ensuring Part B will rotate freely on Part A without hitting Part C; or to make building & servicing notes for future reference.

I was vaguely aware of brochure-style CAD pictures, from works drawings having small pictures to help the machinists and fitters visualise the task. This though, was and is of lesser importance to me, and worse, I now know adds only considerable difficulty.

Although not a time-served, professional machinist I do have a general, somewhat sketchy, semi-skilled background in electrical and mechanical engineering trades. So as well as my model-engineering hobby, I already understood engineering-drawings, in both manual and CAD days.

Also, I had some 20 years computer experience: MS 'Word' and 'Excel', and using laboratory instruments controlled by BASIC and 'Labview' programmes.

My encouragement was a perhaps too-ambitious project to build a 4"-scale steam-wagon from the scanty publicity photographs and Commercial Motor magazine trade-reviews remaining of the original, introduced in 1908. It was and is a matter of design a bit, make it, design the next bit, make it… then a few years later find Part B will not only hit Part C, but would obstruct Parts D to H.

So I saw CAD as potentially very useful.

I even hoped that one day I could reclaim the dining-room from its resident, A0-size, industrial-pattern drawing-board!

My reasons for wanting to take up CAD, was clear, and still stands. I knew it is a lot to learn but unfortunately, not how difficult and non-intuitive it all is to learn, nor the lack of useful supporting literature.

[Colin HeseltineParticipant @colinheseltine48622]

I am drawing up a simple adaptor to connect dust port on a grinder to a vacuum. Once I am happy with it I wish to convert the 3D CAD data into a file my 3D printer can then use to print the required item. I have created my basic shape and changed diameters as required.

What I now need to do is cut the smaller diameter at 45 degrees and rotate the cut piece around to give me a 90 degree bend. What is the best way to achieve this. I have followed the MEW tutorial exercises but not found anything that covers what I want to do.

Any suggestions please.

Colin

[JasonBModerator @jasonb]

Bit hard to say without seeing what you actually have but rather than cut a bit off and try to rotate it I would draw the small diameter as a sketch and then draw another sketch with a 90degree bend, you can then "sweep" the circle along the bend which will give a mitred bend or if you fillet the path you will get a smooth flowing bend.

Draw circle and path

Select sweep, enter the circle as the sketch and the bent line as the path

Result

Here I am editing the path to follow a curve

Which gives this

 

Edited By JasonB on 18/03/2019 16:15:43

[Nick WheelerParticipant @nickwheeler]

Not having any training in 2D drawing(the 50 minutes a week 36 years ago just made my head hurt), I find the insistence that 3D CAD is counter-intuitive peculiar. Representing a 3d object on a plane requires all sorts of artificial constructions and although I can read them OK, drawing an existing object is really tricky. Designing and drawing that way is a step too far for me.

3D CAD is easier, because you are intended to get to a 3d representation as soon as possible. So you sketch(which is what Fusion calls your first step) a basic sized shape, and extrude it to 3d. Then you add or subtract features directly to/from its planes, faces and axes. This is how you fabricate or machine the intended object, so it gives you a good idea of how to make it too. Being able to design the additional parts is place is another big help, what could be more natural than designing a piston in its bore?

I struggled for years with various versions of Turbocad, yet had a respectable model of a QCTP within a couple of hours of installing Alibre. Then the computer does the complicated bit of forcing the 3d into flat drawings to make the part. None of my stuff is going to be rendered into a pretty picture!

[Colin HeseltineParticipant @colinheseltine48622]

Jason,

Thanks for that. Can you use do the same thing for a duct (i.e. hollow pipe).

Colin

[JasonBModerator @jasonb]

Yes, just draw two concentric circles to represent the inside and outside diameters

[David JuppParticipant @davidjupp51506]

Or produce the solid, then apply a Shell command to hollow it out (removing both end faces).

[JasonBModerator @jasonb]

Or do a thin sweep if Atom has that.

[Nigel Graham 2Participant @nigelgraham2]

Re Nicholas Wheeler.

It's interesting how different people have very different perspectives (!) on CAD depending on previous experience. I think all draughting skill depends on how easy you find it to visualise a real object from a drawing, and vice-versa.

Mine's the opposite way round, nearly. My only school-leaving GCE A-Level was in Technical Drawing, long pre-CAD; and not that many years after The Eagle comic published those superb, manually-drawn, pictorial cut-away views to explain ocean-liners and such-like. I worked at low levels in various engineering-related trades for many years. So I am used to orthographic drawings, which anyway you still need for workshop use, and isometric part- and assembly- drawings.

And I've been a model-engineer, sort of, since my teens, so over half a century ago.

I took a GCE A-Level course in Geology some years ago, and that can make your head spin sometimes, trying to read a geology map and visualise what's what below the land surface from the plan of the outcrops and the angles of dip (the slope of the strata). Nature does not build hills to neat regular geometry! Recently, I prepared a geological section projected from the map for a particular project in which I'm involved, and that is only possible manually, on the parallel-motion drawing-board.

Trying to learn therefore, to create a 3D model then take off the elevations for actually making the thing – reverses my thinking. And baffles me, mainly due to the software's complexity but also because I cannot visualise co-ordinate sets and work-planes floating in an abstract infinity.

Manually, I might start from a rough pictorial sketch but draw in orthographic-only. You can in TurboCAD, but I don't know if Alibre and Fusion offer that choice.

My last 3D attempt was of one of the two cross-heads for my steam-wagon engine, having measured the "adopted" pair of raw castings. I have to accept my rough drawing quality; but more importantly, what then? It's merely a non-dimensioned picture of one disembodied cross-head lying on its side, in free space.

So I suppose in the end what matters is what and for whom you want CAD drawings for, to what complexity and quality – and whether their help in your making physical items, sufficiently repays hundreds of hours trying to learn to draw them!

[Colin HeseltineParticipant @colinheseltine48622]

I cannot get the sweep to work whether I have a singe solid or a thin walled tube.

It just refuses to create. If I look at the status of the line which the sweep should follow it says the Sketch is Open, No. of loops 1.

When I look at the sketch the point where the line (supposedly) intersects with the circle it looks a little different to your picture. The cross and circle look at lot larger on your schematic.

Any thoughts?

Thanks,

Colin

[JasonBModerator @jasonb]

In this case an "open" sketch is usual for a path unless you are sweeping a complete loop.

The circle needs to be drawn with the path starting on it's ctr so you may be better creating a plane where you want to draw the circle rather than placing on the surface of your existing diameter and make sure you draw the path sketch on one of the other planes that passes through the ctr of the circle.

If you can post a screen shot or photo of the screen showing the part and the path sketch that would help us to see whats wrong.

[David JuppParticipant @davidjupp51506]

Colin,

Jason started his sweep path that the origin by the look of it, and drew his profile (circle) on one of the principal planes that intersects the origin.

The sweep path must at least reach, or can pass through, the plane on which the profile is sketched.

As Jason said – the path sketch can be open (the warning about this is a standard thing, most sketches do have to be closed, but there are a few exceptions).

Is any error or status message displayed for the attempted sweep?

[John HinkleyParticipant @johnhinkley26699]

Spurred on by the discussion about sweeping objects, I have revisited my copy of Stefan Gotteswinter's cylindrical grinding attachment. I used the sweep tool to produce the drive belt profile. I admit to initially drawing the sketch in QCAD and then opening the DXF file with Alibre, before copying it to a new part drawing in Atom. That method suited me fine, but now that I've done it that way, I can see that it would be just as quick to create it directly in Atom

Originally I modelled it as an exercise in Atom 3D, but now that I've bought a surface grinder, it has become a future project

John

Edited to clarify

Edited By John Hinkley on 19/03/2019 10:24:17

[Neil WyattModerator @neilwyatt]

Posted by David Jupp on 19/03/2019 07:37:21:

Colin,

Jason started his sweep path that the origin by the look of it, and drew his profile (circle) on one of the principal planes that intersects the origin.

The sweep path must at least reach, or can pass through, the plane on which the profile is sketched.

As Jason said – the path sketch can be open (the warning about this is a standard thing, most sketches do have to be closed, but there are a few exceptions).

Is any error or status message displayed for the attempted sweep?

I found that if you do a sweep that intersects with itself (e.g. turn radius less than the swept shape's radius) it will fail.

Neil

[David JuppParticipant @davidjupp51506]

Neil – that would normally give a 'self intersection' error – basically the part of the profile on the inside of the curve reverses direction of movement as it moves along the path, due to the too sharp curvature of the path.

[Neil WyattModerator @neilwyatt]

Posted by David Jupp on 19/03/2019 16:36:46:

Neil – that would normally give a 'self intersection' error – basically the part of the profile on the inside of the curve reverses direction of movement as it moves along the path, due to the too sharp curvature of the path.

Yes, took me a long time to work out what self-intersection was.

[Stephen Williams 6Participant @stephenwilliams6]

Hi all, just getting started with Atom and have a couple of general questions.

I want to design a dividing head. To draw an internal Morse taper should I just use the chamfer tool or is a different way recommended? I'm making the spindle with the extruding circles method.

What is the basic mechanism for bolting two parts together? Are constraints used in this case? The support for threads, threading and fastners seems rather weak. I'm a little confused how to go about introducing screws to an assembly. Any general pointers in the right direction would be much appreciated.

One final point. The threads (feed screw etc.) in the example boring head seem to have been done with a more advanced version of the software. When I load it in Atom it says there are features which aren't supported.

Anyway thanks for any help, this thread is a great resource

Steve

[JasonBModerator @jasonb]

You can either use the chamfer tool and specify the angle and length of one of the edges or you can draw a sketch which would effectively be a section through the tapered hole and then use the cut rotate to remove a cone shape from the solid table/spindle. There is a third way but given your method so far the two suggested would be the ones to use.

Generally it is not worth showing decorative threads and ATOM does not have the option from tapped holes and external threads, best option is to probably draw clearance size holes in parts that will have the fixings pass through and tapping size holes in parts that will be threaded as this makes dimensioning the 2D drawings easier.

Check what version you have as helical cuts and extrusions were added part way through the trial, you can use that to form the worm wheel. You can also use this to thread all your fixing holes but it takes time and memory which may slow things down.

Ask if you need more details on any of these points

Edited By JasonB on 20/03/2019 07:58:00

[David JuppParticipant @davidjupp51506]

Steve,

Mechanism for joining any parts together is assembly constraints – bolts are just additional parts in the assembly.

If you want quick way to get hold of bolts/screws for your design, take a look here and choose Mechanical Hardware as the category.  It isn't comprehensive, but it can be quite handy.

Edited By David Jupp on 20/03/2019 08:34:23

[Stephen Williams 6Participant @stephenwilliams6]

Thanks Jason and David, I really appreciate your generous help.

Jason, I will follow your advice re. the tapped and clearance holes. I do have the new version with the extrusion and helix, and I'm making good progress. I gave things a good bash today and managed to get the taper using the cut rotate method and put a thread on the spindle nose. So I have managed to get a drawing of the spindle for my dividing head. I'm starting to like this software quite a bit as it's doing most of the things I want, and I've never really had much success with CAD in the past.

David, I thought that might be how it worked. Starting to get the picture, thanks

No doubt I'll be back with more questions soon enough

Cheers, Steve

[Neil WyattModerator @neilwyatt]

Posted by David Jupp on 20/03/2019 08:27:50:

Steve,

Mechanism for joining any parts together is assembly constraints – bolts are just additional parts in the assembly.

If you want quick way to get hold of bolts/screws for your design, take a look here and choose Mechanical Hardware as the category. It isn't comprehensive, but it can be quite handy.

Edited By David Jupp on 20/03/2019 08:34:23

Useful resource, although I couldn't directly edit gears as SAT files, I found that by extruding a cut I could modify a 15mm gear to a smaller thickness.

[David JuppParticipant @davidjupp51506]

Neil – that is an old collection of 'dumb solid' models (most on-line catalogues offer dumb solids). You can apply additional features on top of the imported file – so adding keyways, cutting thinner, extruding thicker (use project to sketch for the outline) are all possible. Alibre Design Expert does have 'direct editing' tools – they largely make things easier / quicker, you can make most changes in Atom3D with a bit more work.

I like the Alibre part library if I'm in a hurry, as there aren't hundreds of categories to search through.

[JasonBModerator @jasonb]

OK provided you use UNC fixings

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