Learning CAD with Alibre Atom3D

Jason,

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

Colin

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

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

Or do a thin sweep if Atom has that.

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!

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

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.

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?

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

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

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.

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

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

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

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

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.

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.

OK provided you use UNC fixings

Today I paid for my licence for Atom3D. Now that I'm a paid-up Atomiser, I want try to customise it a bit. To start with, is it possible to alter the default font for 2D drawings? Exporting them to another CAD program alters the size dramatically, too, so much so that they are unreadable and require resizing. Any ideas what would cause that, aside from the way the 2D CAD program parses the ATOM output?

Over to you.......

John