Alibre – A First Attempt

[David JuppParticipant @davidjupp51506]

Steve,

Top row are all about grid – Visibility, Snaps (ON/OFF), Grid size settings

Middle row, toggles in turn for DoF Colours, DoF Callouts, Real Time Dimensioning

Bottom Row – Visibility toggles for Dimensions, Constraint Symbols, Guide Lines

You have much more control of exactly what shows up in Pro or Expert, and easier to toggle stuff without jumping to System Options – BUT more to learn and remember.

 

DoF = Degrees of freedom, whether figures are fully defined or not.

 

Edited By David Jupp on 09/05/2023 15:51:48

[Ady1Participant @ady1]

I always use the snap grid, and even if it means changing the dimension by 1mm I always try to do divisible circles, 8mm, 12mm etc

Anything that makes things easier faster and simpler I embrace

[David JuppParticipant @davidjupp51506]

People can see that we all have our own different habits and preferences. There is no single 'correct' way!

[SillyOldDufferModerator @sillyoldduffer]

Posted by Ady1 on 09/05/2023 17:01:42:

I always use the snap grid, and even if it means changing the dimension by 1mm I always try to do divisible circles, 8mm, 12mm etc

Anything that makes things easier faster and simpler I embrace

In 3D I do it Nealeb's way with the grid switched off other than for special occasions. (Once every 70 years, like the Coronation.)

The reason is I rarely want to snap to grid points, and connecting to one by accident causes hard to spot bugs. Generally I want to snap to features on my sketch: circle and line centres, line ends, tangent points, and intersections.

Like Ady, I try to work in exact millimetres, which is easier with the grid off. Diagonal lines between grid points are rarely an exact number long.

Dave

Edited By SillyOldDuffer on 09/05/2023 17:52:13

[Nigel Graham 2Participant @nigelgraham2]

I know the Systems Options menu David Jupp shows above, with some visibility aids, but does Alibre Atom offer a Snaps choice other than the grid, or does it use an automatic snap function and the nodes?

Edited By Nigel Graham 2 on 09/05/2023 18:47:09

[David JuppParticipant @davidjupp51506]

Nigel

The snap threshold below the grid settings is for snapping to items other than the grid. See This help section

[blowlampParticipant @blowlamp]

I downloaded Atom and have been having a play.

I couldn't make any progress beyond drawing circles and other shapes for quite a while, which was frustrating, but eventually I realised that once you have completed a sketch in Atom, you need to apply some kind of Boss or Cut function, and from what I can presently tell, that function will act on all geometry within that particular sketch. I think this is why keeping a sketch simple is important and you probably shouldn't include geometry that isn't needed at that point.

Anyway, I made a video of where I keep getting stuck on Nigel's cylinder cover – it's the extruded rectangle that's used to slice off part of the flange that throws an error message for some reason. I can't think what I'm doing differently, because previously it just seemed to work.

Martin.

[lee websterParticipant @leewebster72680]

Just a guess Martin, but when you selected the project to sketch and clicked on the circle, you chose sketch figure instead reference figure. I think this confused Alibre because you were then trying to extrude cut the two of them. Try selecting the circle as a reference figure.

As I said, it's just a guess!

[JasonBModerator @jasonb]

When "project to sketch" was used that is a bit like copy and paste so your hole has become part of the sketch.and needs to be removed using "trim" so that you just have the rectangle to cut. You can see the red or blue outline of the sketch is a rectangle with one side slicing through the hole so it is not a solid outline.

Ticking the box when project to sketch comes up to use as a ref rather than part of the sketch will save having to trim the circle.

When that box popped up saying there were problems, if you clicked show rather than ignore it lists the errors and as you click the errors down the list they are highlighted in red so you know where to go looking for them

I seldom use project to sketch but put it there as it shows a practical use for it and it was in the article so again shows its use.

There are several ways that the part could be drawn as I mentioned earlier. You could do the circle place a line 30mm from ctr and trim to get the overall shape and also do the hole pattern in one sketch, the recess and spigot as two others. But for now Nigel is probably better doing each bit separately.

Also doing it the way I did will move the "cut" rectangle's edge if the PCD of the stud hole sis changed as it takes it's position from the stud hole. If it had just been dimensioned at 30mm from the ctr then it would nee dto have that dimension changed each time the PCD was changed and as the PCD seems a bit of a variable in Nigel's design that seems the best way to do it.

 

Edited By JasonB on 10/05/2023 07:41:51

[Nigel Graham 2Participant @nigelgraham2]

Why did having the Grid Snap on, give me so many problems including objects locking onto the origin? Does it affect some other setting I'd not spotted?

Jason –

I don't know why you thought the PCD was a variable in my design, unless I'd inadvertently changed between attempts. There are two sizes of cover (HP and LP) so each with 1/4" diameter bolt holes and its own set of diameters of all other circular features, but not variable otherwise.

…

I re-visited the scribing-block exercise last night, with the grid snap off, and this time succeeded in tapering the end of the column, and assembling it to a new base with tapered hole base (with a few wrong moves).

[JasonBModerator @jasonb]

Your lines, circles etc would have snapped to the grid and that could have been holding them there so you could not subsequently move them.

By variable I meant from what you said the PCD had not yet been decided. But my reasoning still stands as the cut needs to go through the middle of a hole it is best referenced to that hole rather than a fixed dimension.

[lee websterParticipant @leewebster72680]

Nigel,

I have disabled snap to grid on all the cad programmes I have used. When using sketch in SolidEdge, pressing a key, I can't remember which key, will disable snap. I think pressing it again might re-enable snap, but I am not sure.

Edited By lee webster on 10/05/2023 08:42:51

[David JuppParticipant @davidjupp51506]

Nigel,

If grid snaps are on, lines can only start and end on grid nodes, not between them. That's why I never use it (but some people do find it helpful for some kinds of work). With grid snaps on, the angle for taper of the column probably wasn't compatible with the grid.

Very glad to hear you are making better progress now.

Just a note on 'variables' (or parameters) – any dimension that you apply in Atom3D gets a name (which you can alter) and is held in the 'Equation Editor'. Even if a value is not intended to change, you can use it to help define other values in the design. Instead of entering an explicit value, you can set things such as 'D6 = 3 x D3' , then if you alter the value for D3, D6 will also change to satisfy the equation – or you might decide later that 3.5 x D3 gives more pleasing proportions to the eye for the finished part.

[David JuppParticipant @davidjupp51506]

If you hadn't already noticed, terminology in CAD has some very specific meanings that may not entirely match everyday usage. Usage of names may even vary a little between different products.

Often a big problem is working out exactly what a user is actually trying to describe if they don't use terminology in quite the same way as we expect.

This is just one reason why getting hold of screenshots, and/or the actual files is so valuable when diagnosing issues.

[SillyOldDufferModerator @sillyoldduffer]

Posted by blowlamp on 09/05/2023 23:29:43:

…I keep getting stuck on Nigel's cylinder cover – it's the extruded rectangle that's used to slice off part of the flange that throws an error message for some reason. I can't think what I'm doing differently, because previously it just seemed to work.

…

Just a guess based on doing similar with other CAD but sketches usually have to be attached to a Face, and your rectangle might not be. I notice the rectangle starts being drawn in mid-air is mapped to the face later. (Terminology varies! By mapping I mean a tool that takes a sketch drawn in one face or plane and sticks to another.)

The technique is useful, but – in other CAD – it can create a situation where the sketch looks right, but it hasn't attached properly to the face, perhaps hovering a few microns above it. When asked to take a cut, the program knows the sketch isn't attached to a solid, and can't cut empty space.

For that reason, I prefer to sketch directly on faces, not starting them in mid-air. This ensures the sketch really is on the face and not floating nearby.

Dave

[JasonBModerator @jasonb]

Dave, Lee and myself have identified the problem, Martin did not click "create reference figure" so the circle became part of the sketch

See me select the ref on the video, the circle does not become red like it did on Martins as it is not part of the sketch

 

To initiate the 2D sketching you have to select the surface or plane first so the rectangle may look to be in mid air but is actually co planar to that surface/plane

Edited By JasonB on 10/05/2023 09:13:33

Edited By JasonB on 10/05/2023 09:15:29

Edited By JasonB on 10/05/2023 09:21:20

[David JuppParticipant @davidjupp51506]

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.

[JasonBModerator @jasonb]

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.

[Nigel Graham 2Participant @nigelgraham2]

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.

.

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.

.

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.)

[SillyOldDufferModerator @sillyoldduffer]

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

[David JuppParticipant @davidjupp51506]

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

[Nick WheelerParticipant @nickwheeler]

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.

[blowlampParticipant @blowlamp]

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.

[David JuppParticipant @davidjupp51506]

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.

[Ady1Participant @ady1]

Posted by Nick Wheeler on 10/05/2023 11:46:01:

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.

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

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