Learning CAD with Alibre Atom3D

According to my interpretation of the blurb, you can install on several computers, but have to use the key with the computer you want to actually utilise. Not really a problem, as you cannot be in two places at once.

Pete

You can install Atom3D on multiple computers, but only have it activated on one at any time. You can switch activations between computers as described here.

The non-activated computers will operate in View Only mode. This is also what will happen on you activated installation after your extended trial expires, if you choose not to buy a licence.

Yes!

You need to click 'release licence' (on the start screen utilities tab) on the old computer before it will work on the new one.

Neil

Thank you Neil, David & Pete I'll have a go !

John

JohnF - though not officially supported on Mac, there are people out there successfully running Alibre software on (Intel based) Macs using Parallels (for example) - obviously you need a Windows licence.

Duncan,

Centre of Mass - Click on 'Viewing and Analysis' tab - click 'Physical Properties' - that will give co-ordiantes of the Centre of Mass. If you have defined the material, it'll tell you part weight too.

David,
If you have defined the material...…..HOW I can't find a way. I've found the calculation bit.
You have to import DXF into the 2D drawing workspace..... you might see some icons that you don't have access to....... I can't find any icons referring to import. Google is singularly unhelpful, just refers to the full version
I've worked through part 2. Keep it coming! I'm actually getting faster, or perhaps less glacial

Wow, Just found the 'centre of mass' calcs, handy if I ever design a ship...

Also 'create drawing from part'!

Neil

And another question. Having made an assembly of 2 parts, if I then modify one of the parts in the part drawing, how do I make the assembly update itself? Again the stuff on Google refers to icons/menus I can't find on Atom

The assembly will update the next time you open it so if you have both open close the assembly.

To set material click the Atom gem then at the bottom of that drop down click "Properties" and the tab that comes up has the material options.

Duncan - as I mentioned before, where it says Import in the video, use Open. There used to be separate Import and Open options for files - but they really did the same thing, just listing different file types. The 2 were consolidated into the file Open icon.

So click Atom2D icon at top left of screen -> click open, or just click Open on the Home Window and choose the DXF file.

OR from Windows, right click DXF file, choose 'Open With', then choose Atom3D.

At the risk of monopolising this thread and clogging it with photos, I present my attempt at assembling various parts:

This is not the first effort - I tried fitting the block and crankshaft together, only to find that I'd made a couple of fundamental dimensional errors in the block design. I thought that I would have to start all over again, but luckily I realised that Atom allows you to make alterations to the sketches, which meant it only took a short while to remedy things. It also reiterated the fact that, with a large and/or complicated drawings, it makes sense to give each sketch an identifying name. It makes finding it subsequently in the explorer that much easier. I learned the hard way!

Once I've put the conrods and pistons "in", I'll investigate the motion system.

John

Still on the foothills of the learning curve!

Updating Assemblies after editing parts - it's just like Jason said a couple of posts above.

There are other options that can shortcut this, and give you very powerful capabilities; see this video.

'Edit Here' and 'Edit in Separate Window' allow you to alter parts in the assembly whilst the assembly is open and see the results immediately. There some pitfalls to be aware of though.

Thanks, David, I'll have a look later.

John

John, I would suggest making a separate assembly of the Conrod, cap, any bearing shells and wrist pin. You can this bring this assembly into your main one which makes life a bit easier.

You may also find it helps to set the crankcase to semi transparent so it is easier to see what is going on.

One other general comment for anyone is that if you go back to alter one of the sketches that make up a part do make sure you click on the "generate to last feature" before saving as the part will get saved at the point where that sketch is down the list on the left. You won't loose any subsequent sketches but the actions won't be shown.

This can also be taken advantage of by putting all of your cosmetic actions such as fillets, chamfers, visual threads etc at the end so they can be left off when doing assemblies or drawings to make files load faster and keep the drawings clearer.

It is also possible to "suppress" any item which removes it from the model but still has it in the list, just right click in the list and click suppress.

Thanks David,

I can now set properties and update assemblies. I've also opened a dxf of a section through a disc wheel, but I think I'm going to have wait for a future episode to find how to then rotate the shape to form a 3D model. Probably getting a bit in front of myself.

Thanks again

On a completely different tack, MEW seems to have taken a great leap forwards in the last few issues. I was thinking of stopping my subscription, but the last few have changed my mind.

Jason, re: the conrod assembly - I have been doing just as you have suggested while you were typing! I can't see how to mate the gudgeon pin to the little end bush such that it is central. Any suggestions? Ditto the big end bearing shells, which should extend 0.5mm either side of the big end of the connecting rod, but I can only align it with one outer face or the other. Perhaps use the placement tool? I'm sure there is a simple solution, if only I could work it out.

John

I usually do it with Mate but enter the amount it sticks out or -ve if it is a recessed part

Just a quick example to show how I have used angled planes to put embossed text on a curved surface (the text isn't curved, just a shallow extruded cut). For each text I created a new plane at an angles through the main Z-axis, then a parallel plane at the radius of the curve.

If there's a way of doing this in one step (rotating a plan around an axis not on the plane) please point it out to me!

Duncan. Once you have your rim profile on the screen you need to set one part of the sketch the right distance from an axis of rotation. Here I have done a rough section and then using dimension entered 50mm from the x-axis to the OD of the running surface.

If you now go back to part modeling and select "revolve boss" if your sketch does not automatically come up in the box then click it down the L/H side and then click the axis you want to rotate around, in this case X-axis and as you enter it you will get a rough indication of whats going to happen

If all looks OK the click OK and you will have your rim.