Alibre - A First Attempt

Dave -

Nothing to do with faces/planes or 'mid-air' - Jason's diagnosis above nailed it.

Sketch was not closed due to containing a circle crossing the long side of the rectangle. If the projection of hole edge had been a reference figure, it would have worked.

Martin did show sketching on the face. Not sure what you mean by 'starting in mid-air'... If you mean on a plane, that is actually 'best practice' in 3D CAD. It is more robust than sketching on a face, but at expense of taking extra time.

Dave, regarding your floaters, I have added another rectangle that in the 2D sketching mode may look as though it is floating about in space

However when viewed from a different angle you should be able to see it is co-planar with the Xz plane as that is what I selected to initiate the 2D sketch so it is fixed in that dimension, if I constrain the sides of the rectangle in the sketch that will constrain the other two dimensions so it is then fixed in all three.

Even if the rectangle were sketched on a plane that is some distance from the previously created part

Provided the extruded cut were long enough it would still cut the edge off.

Thank you.

Jason -

Ah, not the PCD. That is fixed by needing to place a stud centrally in a web only 5/8" thick. What is variable is how many holes, but whether 5 or 6 studs, the cover's own PCD is still to that central stud.

The effect is important at the outer ends too, as it dictates the size and layout of the steam passages to avoid fastenings going though them.

This raises an aspect of CAD I learnt at work, even before trying it for the first time myself. You still need know designing things even though CAD lets you draw them efficiently, and examine how their assembled parts interact.

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David -

I'd not realised how deeply the matter of the grids and dimensions go. I remembered the term "parametric" as a type of equation - though did not understand them - so did not know if Alibre's meaning is part of the software's internal mathematics or is more immediately related to what the user sees and does.

I'd had a fright when seeing how that revolved cut cut goes about its business - the momentary swarm of triangles is a bit alarming - but I had noticed making the generating shape needs a planar elevation. My first attempt put the taper triangle at a strange angle to the outline, as I had a tilted view still on, but setting the column upright solved that.

I have come across IT terms not always matching the words' ordinary meanings, elsewhere, with MS 'Access' the worst offender; but it tends to make the software less intuitive.

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When I tried learning TurboCAD's 3D mode I'd often create single-topic exercises to examine individual tools - holes through rectangular blocks, and the like. Whereas CAD tutorials put a lot of action into a small space, so can look overwhelming for someone who finds complicated software hard to learn; and that deterrent effect can be reinforced by the impressive, rendered images on the publishers' web-site.

It took me a while to realise Alibre's Parts and Assemblies approach is not only of engineering significance. It eases that load problem by creating natural breaks. E.g., I'd not really appreciated that that MEW tutorial starts by modelling and saving what becomes a scribing-block base, not by modelling a scribing-block straight off.

So for a single-move exercise, for example, I could try that revolved-cut tool on a simple but fairly large-diameter cylinder, without worrying about what the cylinder might be for. It does help to be realistic though, such as the scribing-block parts on their own, other exercises like the boring-head or parts borrowed from some other plan-set, or by measuring actual metalwork.

(My realism point is from finding certain maths topics easier to learn if they have some real, physical "frame". I related 3D graphs [x, y, z] to the familiar Ordnance Survey maps' grid-references and contours.)

I like 'floaters', very descriptive!

We're starting to build a list of things that might baffle a beginner:

• Snapping to a grid rather than the required sketch feature
• Open loops
• Floaters
• Stuck in select mode
• Trying to edit a line that's in a different sketch, or editing the wrong sketch entirely
• Ploughing on into total confusion as a result of not recognising the symptoms of a simple mistake
• Ditto, as a result of not noticing or ignoring warning messages,
• Clicking wildly, hoping that something will work, not realising that each click could be stacking up a long list of daft actions for the software to resolve. Then baffled when the software throws a wobbler after clicking on something innocent forces it to implement a list of mistakes.
• Attempting to do too much in one step, leading to over-complicated sketches and hairy extrudes that the software might gag on. Several simple steps are safer than a single convoluted master stroke.
• Not recognising objects like Nigel's steam cover aren't as simple as they seem, needing a two or three step strategy, rather than attempting the whole thing in one go

Any other examples?

None of my list are peculiar to Alibre Atom, which I like the look of.

Dave

If number of holes in a pattern might change, use a 3D Feature Pattern instead of a Sketch Pattern to add copies of the seed hole. Similarly if the hole size might change.

Patterns in sketches can't easily be edited if you return to the sketch at a later time. Whereas Feature Patterns can easily be edited - say from 5 to 6 holes. Edit size of circle for seed hole, and other holes created by the Feature Pattern will update too.

Nigel - very sensible to practice simple steps and 'play' with individual tools to build understanding of how they behave. There are several options for even the simplest tools - which can often be glossed over. More complex tools have loads of options and hence many more ways to go wrong!

Edited By David Jupp on 10/05/2023 11:37:06

Some more:

Traditional drawing requires you to know where everything is and how they're related. If you don't, you won't be able to design or place new features. CAD is the opposite; it tracks the details, so you can just add to centres of edges or bores, on corners, 'drill' holes through four parts in one operation, view at a different angle, section a part at the click of a button etc. Which in turn enables you to concentrate on your actual design work, that the computer can't do.

There's usually more than one way of modelling parts. Considering how you're going to make the physical object often decides which is the best most efficient to use - the three concentric features of Nigel's cylinder cover strongly suggest a single revolve for the basic solid to me, just like they would for a complex spindle. The notch and hole pattern being so closely related would come from another sketch. This is where you start to get the benefits of 3D CAD, because this thinking is equally applicable to making the actual part.

Not understanding what the program expects from you. Intuitive is a word that gets thrown around a lot, but like common sense, its attributes are a long way from universal. This affects all complex programs, not just CAD, and is something the software industry handles really badly. Impenetrable or contradictory jargon, non-existent or terrible or out-of-date manuals, constant 'upgrades' to the user interface and useless error codes are just the start of a long list.

There are lots of features with specific uses that are really tempting to use willy-nilly - grid snaps, automatic projections, multi-point splines all need considerable care to not leave you wanting to put a hammer through the screen. A lot of my time is spent on car parts, where left and right is taken from the driver's seat not from the front view

These programs are advertised and sold as easy for everyone to use. That should be added to the list of The Great Lies of All Time.

Thanks to everyone for providing the solution - special mention to Lee for being first with the answer.

I didn't think to swap those two options because I can't remember changing them in the first place, but maybe I did that inadvertently.

I'll keep playing.

Thanks.

Martin.

Martin,

You didn't change the option - it defaults to Sketch Figure (which is often, but not always, what is needed).

If you get the wrong figure type, simply right click on it and 'Convert to Reference Figure' or 'Convert to Regular Figure' depending upon the offered option.

When they click for you then they are quite easy, but it depends on how your brain logic works

This is lucky-me from clueless 4 months ago to..

but it's not just about pretty pictures

Suddenly you can tackle entire projects in glorious 3D scale drawings

So the gain is definitely worth the pain

Who knows

in a couple of years the ME magazine could be flooded with new projects from its new army of CAD users and poor Neil is begging us all to stop submitting stuff

Martin,

The drawing you did with the rectangle and circle, would work in DesignSpark mechanical. DS makes each part of the sketch into a surface, the rectangle and two halves of the circle could be either extruded into a solid, or extruded as a cut. That's why I was unsure about Alibre.

Had another go at the Revolved Cut tool to see if I could cut a thread....

It's not an easy tool to use though the scribing-block exercise says it is.

The nut is still plain, but after a lot of mistakes, puzzlement, referring back to the tutorial document and experimenting I managed to make something looking like an M25 thread on the bolt. I've over-rounded the crest a touch but at least I managed to round it off.

(I had based this exercise on rule-measuring an M24 nut and bolt I have lying about. I found later that the actual ISO standard is indeed M24 not M25, but don't tell anyone I'd not looked at the thread-charts first.)

You are getting there

Well done, Nigel. Keep up the good work.

John

I've just had a very weird experience. Needed to revisit some old TurboCAD work I did many years ago. However, I didn't have TC loaded on my new laptop. So I dug out the USB stick with my TC16 stuff on it and (finally) found the email from Mr Tracy with the serial number and actvation code. All loaded OK and then up popped a window asking if I'd like the available update? Thought it might be a good idea, so downloaded that. All good - fired it up and....

I have no idea what I'm doing - it's like I'm looking at a completely alien CAD system. First, it seems to have defaulted to 3D mode (I don't remember that at all) and second - I've forgotton eveything I thought I knew so well about TC (after using it for some 20+ years! ) . I'm sure it will all come back but (after 3 years away) all I want to do right now is run back to Solid Edge as quickly as possible.

(Sorry - back to Nigel's Alibre adventures)

IanT

I too have now installed the trial version of Alibre Atom3D Nigel. At least I can now follow along with what you are doing.

Thank you Jason, John.

.

Ian - I think 3D is TurboCAD's default mode, probably because all its rivals are. It seems now the de facto CAD way; although CAD advertising shows still a strong professional market for 2D programmes.* You can still switch to 2D mode in TurboCAD - never switch in mid-drawing - certainly in TC 2021 Deluxe, which I have.

TC offers saving files in common CAD formats like DWF, and it is possible to transfer its 2D drawings into Alibre, presumably SE too, with the specifically-TC formatting bits rermoved. I have not yet found how to do it so they act as ready-made Part sketches; and I don't know about transferring 3D drawings.

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It is very different from SoldEdge and Alibre though, especially in 3D mode which in TC has at least two solid types ("solid" and surface). The other makes appear to tuck all that neatly away behind the screen - so saving we poor users what I've always found TurboCAD's biggest 3D headache!

Also be aware that IMSI does seem to change individual tools around from edition to edition, not just bung in more, and each edition has three different versions (Deluxe, Professional and Platinum) different by each step up offering more tools anyway. Deluxe is the rather disigenuously named basic version. So its primary functions should all still be there but you might need ferret some out: why leave a tool easily accessible when you can change its symbol and hide it to baffle users? Still, TC does that very useful toolbars and commands library, and I have often used it.

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Lee -

Good luck! What I found frustrating, and it is by no an Alibre problem, is the tutorials and general manuals don't warn you what can go wrong if you make a mistake or miss a step. So when you hit an obstacle you don't know where you went wrong.

On the other hand I like its Parts and Assembly modus operandii. It gives natural breaks to the process, but more importantly perhaps, if you go wrong drawing one new Part, you won't hurt the rest.

Also I like the way modifying a Part, including correcting errors in it, is reflected in the Assembly - with the proviso of due care and diligence in the Assembly's design, which is not a CAD matter.

Presumably, if you think you may need reverse the change, one would store the Part as two separate files suitably named, keeping the original intact; but I don't know how you break the Assembly link to the first used.

Whilst I'd not expected adding a repeated Part to an Assembly to be as simple as one mouse click per copy. That was a very pleasant surprise! My two generic CAD books, and TurboCAD, all work on complicated Groups and Blocks for things for that. Alibre seems to take care of that internally.

'''''

* Still a market too, for manual drawing-boards, and slide-rules! (All right, the latter are specialist trade ones, not ordinary times-sums tools.)

Nigel - be VERY careful here - it can all be done, but it's also easy to mess things up badly.

If you change the name of a part file outside of Alibre, this can have dire consequences. Use 'Save As' from inside Atom3D if you want to save a version of the file for archive/fall-back, or to edit it to produce a variant of the design.

For an explanation see this help topic

In Atom 3D, if you need to substitute one part for another in an assembly, you have to delete one and then insert/constrain the other. In higher levels of the software there is 'replace component' tool that can make this a bit easier to achieve.

Edited By David Jupp on 13/05/2023 11:14:48

Edited By David Jupp on 13/05/2023 11:15:08

Thank you David.

I had assumed saving copies within Alibre, but didn't know how you replace one Part with another version of itself in an existing assembly.

Another question, outside of actually using Alibre...

My trial licence ends in the next few days. What happens then: does Mintronics send an invitation to buy? I looked on the Alibre web-site but couldn't find anything about that.

How do I switch 3D "Off" Nigel? Looked last night but couldn't find it... (have to relearn my TC keyboard shortcuts again too). Part of problem is that I'd customised/simplified the TC UI quite a bit and cannot remember everything I did now (TC on my old laptop looks quite different to this 'reloaded' one)

I will be moving some of my 2D to SE - hence the need to tidy things up a bit before doing so...in a bit of a rush at the moment but I've certainly done this in the past.

Regards,

IanT

Typically the Sales channel for your region will follow up in one way or another. If that doesn't happen for any reason you can of course initiate contact.

At the follow up contact, it's a good idea to ask about any remaining concerns/uncertainties before you make any decision.