Learning CAD with Alibre Atom3D

Thank you Jason and David. as far as computing goes I live in a fog. Jason I found your ref previously but the choice of fast or mulicore looses me. I assume an ssd is a usb stick. Presumably I have to install the grapics first. I am looking for guidance on what card to search for/purchse/install.

John, graphics - just try what is in your computer first. It might well manage OK, and if you decide to upgrade later there's no need to re-install Atom3D. If you try Atom and the workspace is grey with nothing happening in it, you'll have to update graphics drivers.

An SSD is a disk drive without moving parts (like a USB stick but as main storage inside the computer).

The fast vs multi-core stuff refers to the fact that most of what happens inside CAD has to be done in sequence, so it doesn't benefit much from having multiple core processors. So if you had the choice, faster clock speed (More GHz) would be your preference over slower clock speed with more cores. Not really worth worrying about as computers are rarely built for a single task.

Edited By David Jupp on 06/12/2018 14:54:00

Thank you David the fog begins to clear.

I'm trying to put a dome end onto an air cylinder but cannot find the information in the help files. Can you point me in the right direction. I have been trying to adapt the instructions on page 20 of MEW but getting nowhere!

A written manual or book on the Atom 3D would be really helpful - I know I'm expecting too much but any ideas please!!

Paul, If you mean a simple hemi-spherical dome (or similar) - I'd probably just add a fillet of appropriate size to the edge of the cylinder.

If it need to be hollow I'd make sure to fillet the inside 'corner' before the outside one.

Sketching a half cross section and revolving it around the axis of the cylinder is another obvious way - but requires a bit more proficiency with the sketch tools.

If I've mis-understood your requirement, can you post here or PM me an image of roughly what you want to achieve?

The easiest way is to use "Fillet" as that will put a curved fillet into internal corners or round over external ones.

Select fillet from the bar along the top, then you can either select the end face of the cylinder or it's edge where it meets the side followed by entering the radius which should be half the diameter of the cylinder.

This is a similar function to the chamfer to the base that was shown in part one of the series, if you want to look at that as a guide.

Draw two circles to create the right thickness, use two lines and trim to make a 90-degree segment of the right thickness, then rotate it into a hemisphere.

Neil

Paul if you follow this link it will take you to the Atom Tutorial Manual which covers a lot more than the mag articles can. Page 59 shows the end of a solid cylinder being rounded.

If you want a spout or end fitting to the cylinder then drawing a half section and rotating will be the better option

Hello Jason..........I did originally put a fillet on the edge but needed a more 'bulbous' end to which I can then still fillet the edge afterwards. I didn't want a flat end filleted or a 'rounded end. Doesn't sound as if it's possible?

I am also having problems with converting to a Cura file (stl). A simple Atom 3D drawing converted ends up in Cura as a 535mb stl file to which it is too big to load or send a copy as an attachment on an email.

Paul

If you want something other than a pure radius than it will be best to draw a section and then revolve it, something like this where I use circles at the top and elipses at the bottom.

STL output from Atom - make sure that Binary rather than ASCII is set as Format the Interoperability options for STL/ZPR (binary file will be a lot smaller). You can additionally adjust any of the 3 Faceting Parameters to balance file size with 'smoothness' of model. You'll probably get away with adjusting Normal Deviation - you have to check the Custom Box to change from the default value.

If your cylinder has uniform thickness, you can simplify the construction by only sketching the external (half) profile. Revolve that to create a solid, then used Shell command to 'hollow out' the solid and put a hole in the neck.

You could make the hole as a separate operation.

Thanks Jason and Neil......I think it is two steps forward and one back. I've changed the ASC11 to Binary & the 5% works OK on the faceting. That problem solved.

I had already gone through the Atom Tutorial Manual (inches not in mm) but it is a step by step guide and no way to find individual queries. The 'HELP' button doesn't allow for finding things easy either.

Your drawing of the bottle shape comes from a different starting point than the way I was approaching the problem. I was doing it step by step as per the MEW and Manual instructions. This Atom 3D programme looks very promising and hopefully the MEW course will go further than the four months envisaged. Unfortunately age is not on my side and I need to know it all now!!

Paul

Paul,

Check your "Inbox" I have sent you a message that might interest you.

Nick.

Hi David and Jason,

I have a couple of questions related to the second MEW article:

1. I assume he only used 'revolve cut' to teach us the technique, as it would have been easier to use extrude with a draft angle, as we did for the tapered hole in part 1.

2. At the assembly stage, is it not possible in Alibre to 'mate' the two conical surfaces, rather than just align them? That would better reflect the physical reality of the situation.

Thanks,

John

John,

1. Yes Rob was trying to show a range of modelling methods. There are actually more ways the taper could have been added (chamfer tool for one).

2. Mate works for planar surfaces. Cylindrical or Conical surfaces have their axis picked up, which can be used for Align, but doesn't make any sense for Mate. Rob uses the align of the end face with underside of base to achieve final position.

Alibre Design does offer additional constraint types - but even they don't help much in this example.

Edited By David Jupp on 10/12/2018 11:34:08

Yes, I've just discovered you can define a chamfer by a length and an angle. That would be a very good method.

Directions please for changing from inches to metric.

John

Follow this tutorial to see how to change units and how many decimal places etc.

If you have it set to metric you can still enter an imperial size if you want, just put " at theend of any size you enter and it will drawing to the inch size but display in metric. I tend to use it more the other way round with say a metric tapping hole on an imperial drawing.

Thank you Jason, the tutorial is easy to follow but at stage 7 the APPLY box is just visible half off the screen.

Clicking on that un does the previous stage 6 so no change ( I am working on lap top with 14" screen)

John