Alibre – A First Attempt

[David JuppParticipant @davidjupp51506]

Nigel,

To edit an existing sketch, locate it in the Design Explorer (left hand side of screen), right click on it and select 'Edit' from the options in the context menu.

You should then be able to modify the sketch figures or dimensions.

Using the 'Activate 2D Sketch' button will open a NEW sketch. You can have multiple different sketches on any plane or flat face.

[blowlampParticipant @blowlamp]

It's no good. I'm downloading Atom just to see how hard it is to get my head around.

Martin.

[Nigel Graham 2Participant @nigelgraham2]

Aha! Some of you have hit the rivet on the head, not just in the specific example but in general.

I was trying things that seemed simpler than the tutorials, but obviously had not realised Alibre's underlying operating rules or principles, let alone grasped them. Not just knowing what each tool is for.

Trying to learn CAD from step-by-step exercises is rote-learning. Many manage that, but I don't. I need to know and understand the principles – perhaps others can to do that automatically.

I thought I was making quite good progress with Alibre then it all fell apart because I had only been following a list of moves, and still made a mess of that. So when trying my own drawings even though simpler than the exercises, I had no idea what I am really supposed to do, and why I failed.

After the tutorial exercises you are left to your own devices, but the whole aim of learning to use CAD is to help you design your own devices. If you have only followed instructions for fairly simple assemblies, how can you progress even to equally basic items of your own? The rest of you obviously found that jump easy, but I don't.

Although Alibre is a lot easier than other, comparable makes of CAD, I do not expect ever being able to design a complete project with many tens of components with complicated shapes. I had hoped though, I might be able to use it to draw individual, simple components and small sub-assemblies of a few of them; but am now not all confident I can.

[Nigel Graham 2Participant @nigelgraham2]

David –

I've just looked for that fault-ridden file to send to you as you invited, but it's not there.

I'm afraid I closed it without saving it – too frustrated and upset to think it any use to anyone.

I remember most of the faults were "Intersections" , and apart from one "degenerate" figure I think the rest were described as "open loops" . The "degenerate" one could be "healed" if I remember correctly, so I chose that but whatever it meant I could not see any difference. Presumably it's a fault at mathematical level rather than something visible.

Sorry!

'

I'll try the drawing again but in a different way……

[lee websterParticipant @leewebster72680]

Hello Nigel,

I wonder if you are up for a bit of reverse engineering? How about if you describe to us, in the way of a tutorial, how you go about designing a part. Either pick a part that is something you want to create in real life, or re-create an existing part in a tutorial. Teach us the steps it takes to make this part. Maybe those familiar with Alibre will see where you are having trouble. Now, you could either just write this tutorial as a series of steps, or actually do each step as you write it, then if it go's wrong, we will know where, and maybe know how to get you back on the right path.

I refuse to believe that you are incapable of learning cad. Anyone who takes on the task of building a steam lorry should be able to do it. It just hasn't "clicked" yet.

If you are unsure about investing in Alibre, maybe seeing it as wasted money, why not try a free cad programme like DesignSpark Mechanical? It isn't as powerful as Alibre, but it has a simple design interface. Draw a sketch on a surface or plane, extrude, cut, revolve the sketch to create the feature, etc. If you then think 3D cad is for you, invest in Alibre. DS is not a replacement for Alibre, even a dedicated fan of DS like me will admit that, but it does take some of pressure off having a deadline creeping up on you.

[Nigel Graham 2Participant @nigelgraham2]

Thank you Lee.

At 70, "deadline" is rather appropriate given that I embarked on this project in about 1978, with a gigantic mistake in trying to build it half-scale, started again at a more sensible one-third scale in the late 1990s, and two house moves and spells of utter loss of motive since then, still have a huge amount of work to do on it!

It is not easy to design, CAD or not, and I cannot guarantee it will even work.

I have always been a slow learner, have never been able to learn anything to a very high level, and 3D CAD is no exception.

'

A log of how I produce a drawing, as you suggest, would be a very long list of stupid mistakes, trial and error, objects in the wrong places, multiple attempts and deletions, very many "Undo" and "Esc" presses. It could only be a document as I cannot make a video like Jason's.

.

I've looked at Jason's video just above and tried again more or less as he does it; as a completely new Part.

It took ages to make the hole circle because I could not see how to place the first circle where it should be. It kept sticking to the origin and I don't know why, nor how to stop that happening.

Eventually, with help from the Alibre Manual, I learnt how to use the Points and Move tool just enough to put a copy in the right place. Then I needed work out what the repeat tool means by "Centre", and how to select it.

So I could now make the basic shape: a full disc with a circle of holes. (Plus the register on the inside face and recess on the outside – those were easy).

.

Next to cut the segment from the side……

Jason shows doing it by developing a rectangle with its long edge the right distance from the centre and extruding that through. So that's what I tried….

Somehow though, I cannot make the Line and Rectangle tools work. They want to start from the origin and I can't understand why. Eventually I had a rectangle with one corner on the origin, but I can't quite recall how. I don't think it was simply clicking in two places. I tried various possible ways to move it to where it should be, but they all failed so the wrong methods – but I've no idea what.

'

Worryingly, for much of the time in Sketch Mode the outlines of the figure were red or orange (hard to tell which) suggesting "Undefined". How? I set their diameters when drawing them, set the thickness for the extrusions, and either automatically or by my setting, they are concentric to the origin.

So I obviously have something fundamentally wrong somewhere, perhaps in some generic setting right from the start; but what exactly?

It was all working when I tried the set exercises, and I didn't think I've done anything different, except change the dimensions to inches as it is for a real object.

.

The number of bolt holes in it is still undetermined. I may have to make a completely new cylinder block, replacing the one I made some twenty years ago. It is bored, has the ports and passages, but I've built in a lot of serious problems. From a drawing point of view it does not matter because either 5 or 6 studs, one still shares a central stud between the cylinders.

[JasonBModerator @jasonb]

Your 27 open loops sounds like you have just been dragging lines and circles about until they "look right" but infact they don't actually meet or the cross and you have odd ends sticking out so you don't have a true outline to extrude. Another reason can be leaving a bit behind when you trim an item that can happen if it intersects more than one other or an axis. When the Analyse window comes up you can click any one of the items in the list and it will highlight it in red on the 2D sketch so you can see where the problem is. Often you may need to zoom right in to spot things like a line and circle that you thought were tangental and are not.

You say you have given the circles a diameter, that is only their "magnitude" to fully define them you also need to set their position say in the case of the stud hole by how far it is from the ctr of the cylinder cover

If your circles are all from the origin or an axis you may have the snap set too high. If in doubt draw the item a reasonable distance from where you want it and then use dimensions and/or constraints to bring it to where you want it which will also help define it more fully

 

I would suggest you go back to the first part of the scibing block exercise and try that again, until you have grasped the basics of drawing lines, circles, etc where you want them you will find it hard to progress to even the most basic real parts.

As for the actual design aspect, CAD is just another tool, it won't design it for you but can be used as an aid. Take your stud positions, I see it is a compound so the bores and therefore covers will be different diameters so there are two options for placing that shared stud, one is simply in the middle of the metal between the two holes. the other is offset towards the smaller cylinder which gives a much better looking shape to the covers. Alibre can be used to derive the positions in either case but get the basics sorted first.

 

Edited By JasonB on 09/05/2023 07:29:53

[David JuppParticipant @davidjupp51506]

One thing which I've seen some people struggle with; when sketching a circle, rectangle, line in Atom3D you click AND RELEASE to place the first point (centre of circle, corner of rectangle, end of line), then move cursor to second point then click again to complete the figure.

Some people are so used to holding mouse button pressed whilst dragging that they forget to let go – the sketch tools in Alibre won't work if that happens.

Open vs closed sketches is covered in the Help manual

I know Nigel doesn't like videos, but this one covers common sketch problems and how to diagnose/fix them.

[David George 1Participant @davidgeorge1]

Hi David when drawing a thread for spiral extrusion  I often find it difficult to draw the thread shape so that there is no overlap and when putting on the radius on the root and crest of the form is there an easy way of doing that without getting a closed loop fault as well.

David

Edited By David George 1 on 09/05/2023 07:54:51

[JasonBModerator @jasonb]

Here are two options for those cover studs, Alibre won't tell you which one looks better but it makes the job of deciding which easier.

Stud placed mid way between the two cylinder bores and flats on covers "cut" through that stud ctr. Leaves an nasty looking step where the two different dia covers meet

 

Stud position derived from where the tow outer diameters of the covers meet

Done buy using a couple of guide circles and a few known dimensions of the cylinder. There is a third option which is to place the stud hole central and then derive the cover diameters from that but not got time now to do it.

What was used above is really just basic schoolboy geometry except instead of using compass, set square, rule, etc CAD provides those tools. So if you had problems with maths which includes geometry lessons then you are going to have problems with CAD too.

Edited By JasonB on 09/05/2023 08:05:18

[David JuppParticipant @davidjupp51506]

Posted by David George 1 on 09/05/2023 07:53:14:

Hi David when drawing a thread for spiral extrusion I often find it difficult to draw the thread shape so that there is no overlap and when putting on the radius on the root and crest of the form is there an easy way of doing that without getting a closed loop fault as well.

David

Yes. Whichever of root/crest is in middle of profile shouldn't be a problem in the profile sketch – for the other rounding, don't try to put it in the sketch, instead apply a 3D fillet after the helical feature.

If still not clear – submit a support ticket to Alibre and include a part file that exhibits the problem. There is an issue this morning with the cloud service used to handle support tickets – I or a colleague will pick the ticket up when the service is fixed.

The MEW articles mentioned through this thread show one way to form the profile sketch to avoid overlapping.

[Nigel Graham 2Participant @nigelgraham2]

Jason –

Thankyou – I studied those two drawings carefully.

The photo is not very clear but does seem to show the original covers were two pieces. What is less clear is if we had both assumed the covers meet geometrically, or if in the "valley" between the two discs is partially filled by large fillets. They may even have been D-shaped!

It would be feasible to make a single-piece cover, finish-milling the arcs with a small cutter so the meeting-point is a tidy fillet. It would not need an inside register – in fact, neither do separate covers on the top, but the crank-end covers do need align accurately for the guide-bar mountings.

The block is made (though needs some drastic modifications or even replacing completely). So is the crankshaft. The wall between the cylinders is only 5/8" thick. The complete unit complete with the valve-chests forms a rectangular block, obvious in the photograph I have – it is very prominent as the engine stands upright between the seats of a vehicle supplied with at best, an optional traction-engine style canopy.

So these constrain the rest of the construction, including the central stud that has to be in mid-web.

Further constraints are where the other studs need be to allow space for the steam passages, and the cover flange widths to accommodate the nuts. You've shown only M5 studs but M6 / 0BA or 1/4" BSF would be more appropriate.

.

So the existing metalwork is driving the cover design, not the other way round. I had to work outwards from the cylinder bores and centres, and the central fastening. I had investigated turning the stud circles to straddle the web but the result looks and is horribly wrong.

The geometry is as you say, simple although it took me a while to spot it. I could have developed it manually but used TurboCAD for two reasons. I could copy the parts from an existing drawing, and geometrical construction is easy in TC's 2D mode. I don't know Alibre well enough for that.

Once I realised the radius of the second cover is from its centre to the first's intersection point on the centre-line, it was easy to make and print the reference drawing from which to model the covers in Alibre.

I did try the construction in Alibre, but could not see how, and became unsure if you can overlap figures in a Sketch.

.

Earlier on you said something about me apparently dragging objects about until they "look right". I can assure you I do not do that. I can't even make dragging work! I know CAD can only work if objects meet mathematically, and only the software can make that happen – but you do need know how to ask it.

Edited By Nigel Graham 2 on 09/05/2023 09:32:03

Edited By Nigel Graham 2 on 09/05/2023 09:33:27

[SillyOldDufferModerator @sillyoldduffer]

I hope Nigel persists because this is the first of several past attempts in which his understanding of what's going wrong matches my painful experience of learning CAD.

At the beginning, it's important to master quite a few details before moving on. Most of them are simple enough in themselves, but they're not necessarily intuitive. Some lucky folk get going without much bother, others struggle. Previous experience can be deadly; many a professional 2d draughtsman failed to grasp 3D because tried and trusted methods no longer work. Similar pain ensues if the learner expects a 3D tool to work in a particular way, and it doesn't! For example, starting a new sketch on a face FreeCAD and Solid Edge take opposite approaches:

• FreeCAD requires the face to be selected, then the sketcher
• Solid Edge requires the sketcher to be started, then a drawing tool (line, circle, square etc), then the face is selected from the sketcher, and locked by pressing F3.

In addition to the tools, learners have to identify the 'rules', recognise when an earlier step needs fixing, and build a mental model of how 3D CAD works. At the beginning, this is horribly intimidating, but most CAD work is done with a few simple steps, notably sketching 2D perimeters and extruding them to make 3D solids, A common learner mistake is sketching a shape which looks OK on screen, but the lines don't make an unbroken circuit. An 'open loop' can't be extruded. The problem is easily avoided once snaps are understood – but this is more learning. I spent many hours learning to sketch correctly, which includes keeping them simple, after which progress became rapid. What previously felt bizarre, illogical and unnecessary suddenly made sense.

Learning 3D CAD isn't easy, and it can be very hard work, but once mastered the design benefits are enormous. CAD is less worth having if a workshop builds to other people's plans or majors in 'back of an envelope' work. At least half of what I make are simple objects dimensioned from a rough pencilled plan, with no need for 2D or 3D CAD. For the other half, CAD saves an enormous amount of time and material. Delivers a high-confidence before cutting metal that individual parts can be machined without special work-holding, and that complex assemblies will fit together.

I hope Nigel keeps going – I think he's much closer to mastering Alibre than he realises. Admittedly another bruising encounter with CAD but this time his understanding of what's tripping him up is much improved.

Best wishes

Dave

 

Edited By SillyOldDuffer on 09/05/2023 10:19:51

[Nick WheelerParticipant @nickwheeler]

Posted by Nigel Graham 2 on 09/05/2023 09:31:46:.

Earlier on you said something about me apparently dragging objects about until they "look right". I can assure you I do not do that. I can't even make dragging work! I know CAD can only work if objects meet mathematically, and only the software can make that happen – but you do need know how to ask it.

Do you have a grid displayed? If you do, you probably have grid snaps turned on as well. These are a really frustrating trap – turn them both off, and forget they are even possible. Then you can choose a sensible feature(corner, centre of a shaft or bore, etc) to fix to the origin and constrain/dimension from there.

One tip I found saved me a load of grief was to deliberately draw lines, boxes, etc so they obviously don't meet/align, and force them to do so with constraints before going any further.

[David JuppParticipant @davidjupp51506]

Nigel,

Send me a part file that you can't drag sketch figures in – I can soon check if this is because figures are fully defined, or if it might be to do with your installation, or your way of working.

[Nigel Graham 2Participant @nigelgraham2]

David –

I'm persisting because I want to be able to use it – and I've already spent so much time and money on CAD.

I learnt about Snaps right early on in TurboCAD, which has a menu of perhaps a dozen different types of snap and a ready All Snaps On/Off switch. I take it that Alibre uses them in a background way, within the Constraints system, but showing their presence by those little Node dots?

Most of my engineering is to rough sketches on paper, or other's drawings, but I want to be able to produce somewhere-decent drawings for the more serious stuff that might entail expensive materials. I realised some CAD's advantages from seeing the drawings at work, though I was not in the drawing-office or machine-shop. (They used SolidWorks.) While the MEW tutorial has a section that has you make a formal orthographic drawing with a little 3D image of the part in the corner, as Hemingway use for their kits.

Once I started on it I quickly realised further advantages such as object templates (lines, circles, polygons, etc.) readily edited to accurate dimensions. I like Alibre's active dimension method, and on Assembly its immediate ability to repeat Parts; for example. D.A.G. Brown's CAD primer, probably based on AutoCAD, illustrates using Groups for that, but Alibre neatly has its own way by one mouse-squeak each!

.

Lee –

Turning off the grid snap seems counter-intuitive because it allows lines to lay at neat right-angles; but I see your point. I'll try that, and your positioning technique.

I know you can set the mutual angle as well as length of a line, and constrain them perpendicularly to each other.

The grid is displayed but sometimes as just a square with two orthographic centre-lines: does that depend if the scale is metric or inch?

[JasonBModerator @jasonb]

I don't use the grid but do allow the standard default snaps where say when your cursor gets near to an axis it will change slightly so you know it will snap. As an example watch the cover video again, about 12second is I select the circle too; and there is just a circle by my mouse, as I get close to where the two axis cross that circle changes to one with a "+" crosshair symbol to show it is going to snap to where the two axis cross. Suggest you run the video on slow speed or watch a couple of times.

The single square with cross lines is not the grid but the bounding box of the plane you are working on and the two other lanes/axis

0 & 90 deg or the common 30, 45, 120, 135 deg etc will come up as you get close which is another form of snapping but does not need the grid.

 

Edited By JasonB on 09/05/2023 13:20:35

[Nigel Graham 2Participant @nigelgraham2]

Hooray!

Thank you Lee.

I opened the drawing so far: the basic disc with 6 holes plus recess and register.*

Opened the initial Properties menus, found and switched off the grid and grid-snap.

Then cut the slice off as Jason had described: through-extruded rectangle of no special size but located by radial distance from the centre.

For good measure I lightly chamfered the edges (0.03" ), once I realised the interrupted edges needed special treatment.

*(In practice the latter is not necessary on the top end covers, but is on the crank-end. I'll also give the top covers a small screwed plug for injecting oil to protect the iron cylinder when out of use.)

[JasonBModerator @jasonb]

This shows what you are seeing when there is a Square and two lines, by simply rotating the view slightly you can see what those green lines actually represent. I then toggle the grid on and off a few times. Atom will have a slightly different tab to do that.

Edited By JasonB on 09/05/2023 13:31:30

[Steve Skelton 1Participant @steveskelton1]

Jason, how do you get the "sketch options" on the 2D Sketch Ribbon

Thanks

Steve

[David JuppParticipant @davidjupp51506]

Steve,

Jason is using Alibre Design Professional – Atom3D doesn't have the same options on the Sketch Ribbon – it is deliberately simplified.

[JasonBModerator @jasonb]

I'll have to leave that to David, as I said it is slightly different in Atom.

[David JuppParticipant @davidjupp51506]

Steve, if you are looking for Grid & Snaps settings they are accessed via 'System Options' – see image. Note that there is another set of Grid options for the 2D Drawing workspace sketching.

The Snap Threshold setting below the Grid Area is for inferential snapping to lines, nodes, axes etc. Have it too small and you have to be extremely precise to select anything, have it too large and it may end up offering items you'd rather not have. Best setting for you may depend somewhat on your screen size/DPI.

[Steve Skelton 1Participant @steveskelton1]

Thanks David/Jason. I tend not to use the grid options it was more the other tools in the sketch options I was more interested in and what they do.

[NealebParticipant @nealeb]

Some of the recent posts allude to a principle that I usually apply, but which is not just foreign but counter-intuitive to those brought with more traditional drawing-board-and pencil days.

Sketches are called sketches for several reasons, not least of which is that the lines and shapes you create in your sketch do not have to be the correct size or position initially. In fact, I will often draw, say, a circle roughly but not exactly the right size, and in roughly but not exactly the right place. This avoids being misled into thinking that it is aligned with a point when it is not quite there. I then add a dimension to get the circle to the correct size and use a constraint to lock the circle's centre to the point required. That way, I have forcibly defined everything I need and not relied on anything that looks about right but which cannot be trusted to be precise. This is also why I never use snap to grid or similar, or even bother unduly about making lines horizontal or vertical when I sketch them – there are constraints which will do this more accurately than I can draw! Note – I do not drag sketch objects into position. I use constraints to both move and fix reference points together.

I'm sure that someone must have mentioned this already, but it is a technique that is not obvious but becomes second nature after a while. While I do this in F360 and Solid Edge, I'm sure that an equivalent must exist in the Alibre suite.

[Author]

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