Had Another Go

[Nigel Graham 2Participant @nigelgraham2]

Jason –

I’d not intended including bolt-holes on the CAD model because the real chassis is already made and the CAD’s purpose here is to help me design the next stages.

If I can’t use the mirror tool to reflect the finished beam, then I take it the only possible use is in duplicating the initial sketch to produce the section profile.

….

Nick – 

Sorry, but you’ve lost me there.

My problem is not being unable to use the sweep tool within a specific project, but being unable to use it generally.

I tried to understand it but it confuses me completely. I could not see how you place the line the profile is supposed to follow, or locate and orientate the sweeping object so it will follow the line.

I managed, sort of, to create a few bits of round “rod” but without really knowing what I was doing. They paralled the guide-line but away at some random distance to one random side. Yet that was “just” a circle along straight lines and regular arcs. Or is this supposed to happen? Does it matter? I’d assumed the profile would run along the line.

The manual did not help me. It apparently says the profile should be on a different plane. Well, I can see it can’t lie on the same plane as the guide-line, but also it does not need start on the line.   Which means that in sketch mode you can see one but not the other, and in 3D they have no clear relationship to each other, but if they cross, overlap or one passes through the other it won’t work. Or so it seemed to say.

Then when I tried other shapes I hit the usual problem of things facing the wrong way.

This is all why I concluded the Sweep tool is an advanced method beyond me.

 

As for “Creating dimensioned, mirrored, swept profile, fully editable chassis rails would be a good 5 minute in-person exercise“……

Five 5 hours genuinely would be a realistic estimate for me, based on how long other models have taken.

Even if I was able to complete it, and that’s extremely unlikely, it would leave a long trail of errors like failed constraints, and high move-count numbers.

“in-person”? Umm, well, obviously. The PC won’t drive itself! 🙂

[David JuppParticipant @davidjupp51506]

Nigel,

I think you have misunderstood the manual.

In simplest terms, imagine a round bar with some bends in.  A section across the bar (a circle) is the profile sketch for the sweep that models the bar.

A line along the centre of the bar is the sweep path.

In many cases the profile sketch is on a plane that is perpendicular to the plane that the path sketch is on – though the actual rule is that they can’t lie on the same plane (if they did, the resulting sweep would have zero thickness, hence not a valid solid).

[Nick WheelerParticipant @nickwheeler]

The in person isn’t you, but a tutor/mentor/guide/whatever you want to call them. Everything you need to know to create a reliable swept profile can be explained, demonstrated and followed by you in five minutes. If I was that person, I’d use your chassis as the demonstration as you need it, have the details and understand the part.

To get predictable results try this:

open a new file however Atom requires.

 

ensure that the origin and 3 base planes are visible, even if you don’t normally work like this.

 

create a new sketch on the XY plane

 

starting at the origin, draw a 3 piece cranked line with each length 150mm long, and 45degrees at both angles. That’s the path for your rails, and represent the shape. Dimensions are random guesses. Constrain the parallel lines so they’re also parallel with the Y axis.

 

create another new sketch on the XZ plane

 

To make the demonstration simple, use the rectangle tool to draw a 100×50 rectangle with one of the corners fixed to the origin.

 

Close both sketches, but leave them visible.

 

start the sweep tool, which will ask for a path – which is the line in the first sketch, and a profile – which is the rectangle in the second.

 

Click OK.

 

That will sweep the profile along the path to give a cranked solid bar. If you want it to be hollow, edit the second sketch by offsetting the rectangle lines by 5mm. You could alter the dimensions to 150×75(doesn’t actually matter), change to profile to a seven pointed star or whatever else takes your fancy.

This would be a basic five minute demonstration from an in person tutor sitting with you. Once you can repeat this reliably including editing after the sweep, then more complex(don’t think of them as advanced!) methods like not attaching the profile to the path, or creating the profile plane directly from the path could be discussed.

 

I agree that manuals for computer programs are absolutely hopeless for learning how to use it. They’re full of unexplained jargon, atrocious English, and terrible explanations. They read like they were translated from Chinese by someone who doesn’t speak English or Chinese but has a dictionary for each.

[Michael Gilligan]

On Michael Gilligan Said:

I hesitate to throw-in yet more advice, Nigel … but I think I may have found a tutorial that would suit your mind-set.

Caveats:

1. I have only watched a few minutes so far
2. it includes advertising for ‘Brilliant’
3. I am unlikely to ever actually use Alibre Atom

With all of that said: I plan to watch it later today, just for the sake of background learning.

MichaelG.

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https://youtu.be/YyXBWuQy3ss?feature=shared

.

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Nigel

Please don’t worry about why I am posting at this ungodly time … that’s my problem not yours.

 

For the sake of my sanity though  … Could you please watch the ‘Chapter’ about Sweep.

I don’t use Alibre, and have only watched his tutorial out of general curiosity, but this Chapter  [in the space pf less than three minutes] seems to perfectly convey the basics of using that tool.

MichaelG.

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[JasonBModerator @jasonb]

As for what sketch goes where, Again I will suggest for you that looking at the cube in the corner should guide you.

You will see the Z shape of the chassis when you look at the top of it so use the plane that is orientated the same as the top of the cube ZX

You will see the C section of the chassis when you look at it from the front so use the plane that is orientated to the front of the cube XY to draw the chassis cross section.

Nick suggests other planes but for your level of learning I have suggested these as the parts will be the “right way up” when files are opened, when they are inserted into an assembly or when you start a 2D drawing which will make things easier for you. It also corresponds to the names on the navigation cube which seems the obvious way Alibre intended it to be.

[DiogenesParticipant @diogenes]

A basic strategy that works for me..

I open a sketch in ‘XY Plane’ and draw out the path, starting the line at some easily remembered distance from the origin (here I made it -10).

When satisfied with the Path detail and dimensions I deactivate the sketch. In my mind, this is the ‘Plan view’ of the path.

Without doing anything else, I then click on ‘ZX Plane’ and activate another sketch – now I am looking ‘End-on’ along the path – I can’t see it, but I know the start-point lies -10 from the origin.

I now construct the Profile Sketch so that my ‘Path start-point’ is either enclosed within, or touching/co-incident with, an edge of it.

The sketch can now be deactivated and the sweep modelled.

..I suspect that there are more advanced ways of doing it..

 

 

[Nigel Graham 2Participant @nigelgraham2]

Like the model below, Nick?

I created it as you described though didn’t follow the lengths too closely as I have Alibre set to open in inches. I also looked at what happens if you edit the initial profile: the swept shape follows suit. I also tried it from the start as you suggested, as a pipe.

Alibre’s own manual is nothing like as you describe. It is in English not Chinese / English, but most such manuals are brief, sometimes more reminders for experienced users than introductory aids.

“Chinglish” is worst for power-tools, household appliances and gadgets and the like, manufactured in China; not IT apart from “smart”-‘phones… they come with no instructions anyway. Most software publicly available, including Alibre, is made in America so the supporting literature is written in English (well, the American dialect of it!).

Thankyou!

 

Michael –

I did start watching that video, but not wanting to sit right through at once as I would not take much in. I stopped at a break the author puts in, where he invites the viewer to try using Alibre. I’ve not yet returned to it. I must admit I’d not noticed it has a contents page.

 

[JasonBModerator @jasonb]

Much the same as I described 2 weeks ago except it is stood on end.

Now to see if you can apply it to your chassis which will see if you have just followed instructions or taken it in and appreciated the reasons why it is done a certain way.

[Nigel Graham 2]

On Nigel Graham 2 Said:

Michael –

I did start watching that video, but not wanting to sit right through at once as I would not take much in. I stopped at a break the author puts in, where he invites the viewer to try using Alibre. I’ve not yet returned to it. I must admit I’d not noticed it has a contents page.

I realise that you didn’t feel inclined to watch the video end-to-end, Nigel

BUT please, please, please … just set aside three minutes to watch that chapter.

With the experience that you already have, it should be extremely easy viewing and [I can only hope] will bring enlightenment.

MichaelG.

 

MOD EDIT this will take you to where Sweep starts

[Nigel Graham 2Participant @nigelgraham2]

Got There!

By ‘eck what a struggle.

Thankyou all very much.

Jason – I copied your annotated View Cube to a desktop picture for ready reference.

 

I do wonder if a lot of the antics I was having with planes is that I am too used to thinking of (X, Y) being flat on the floor (or milling-machine table, where I prefer to use the names rather than algebra for the travels) and (*, Z) as the walls. It seems Alibre defaults to the screen being the “floor”.

Also with this tool there are times when you can see only one sketch at a time as its mate disappears into its plane viewed edge-on, and that’s a bit disconcerting.

.

I made one then tried to use the Mirror tool to create the second (as a separate Part file). I knew if I reflected just the sweep line the profile would face the wrong way, but confused myself and ended up losing the profile on the second model, so having to re-draw it, facing the right way. At least that showed the swept figure will follow changes to the original sketches, provided of course the editing does not ask for something not possible.

 

[Nigel Graham 2]

On Nigel Graham 2 Said:

Like the model below, Nick?

 

I created it as you described though didn’t follow the lengths too closely as I have Alibre set to open in inches. I also looked at what happens if you edit the initial profile: the swept shape follows suit. I also tried it from the start as you suggested, as a pipe.

 

Yes, just like that.

Cool.

 

That leads onto a similar exercise for Mirror:

Start the Mirror operation

 

It will ask what you want to mirror and the plane to mirror it across.

 

What is the rail you just created, so select that in the appropriate box

 

The Plane is the one parallel to the sides of the rail, which is YZ in your fancy model. Select it from the browser list so you don’t accidentally pick something else and get a weird, hard to diagnose result.

 

Click OK, and you have a pair of handed rails. But they will be touching, which isn’t quite what’s wanted.

If you’re happy with modifying the Path sketch so the line is offset by half the chassis width from the axis it’s currently constrained to, do that. If not, start a new part and draw it like that.

 

Follow the same Sweep process, then the above Mirror. That will place the two rails so they look like the start of a chassis.

 

Follow on steps:

Banish the words Basic, Advanced, Difficult and Impossible from your vocabulary.

As Jason said, this demonstration annoyingly creates the rails vertically in the model. That’s because I picked universally named planes to make it work. Redo the exercise so the Path Sketch is on the plane that better represents Top and Bottom of the model, and the Profile Sketch on the one for the Front. Once my first part is under way, I turn off the visibility of all the planes because I find that thinking of Front, Top, Side, Centre, etc of the part saves a lot of grief.

change the  selected Mirror Plane to see how it affects the new part. One of them will create a single rail that is a copy end to end.

You don’t have to use a Plane for the Mirror; any flat surface in the model will work, which includes surfaces of the actual part you’re trying to Mirror. Mind bending, but extremely handy when modelling a symmetrical object, as you only need to model half of it. If it’s symmetrical through more centre lines you only need a quarter. Some thought(and probably experimentation) will make the above single rail the other way around….

If you’re not comfortable modifying sketches to delete or modify constraints, dimensions or positions that’s probably the most important thing to work on. Changing stuff as you work is one of the main reasons for using CAD.

Try different ways of creating custom planes to help model new parts. There are several different methods besides the basic obvious ‘offset from an existing one’. Make sure you immediately give them relevant names; ‘Front Axle Plane’ is far more informative than ‘Plane 23’ that the program gives it. That advice applies to any operation you do, part/sketch/object/axis you create.

 

Banish the words Basic, Advanced, Difficult and Impossible from your vocabulary.

That last point is so important I though it worth mentioning twice.

 

[David JuppParticipant @davidjupp51506]

Nigel,

If you want the opposite handed part in a separate file from the original, the simplest option is;-

After saving the original part, Save As using a distinctive name.

Use the Scale/Mirror Part command to mirror the entire part (you have to select mirror plane from the choices provided).

 

[David JuppParticipant @davidjupp51506]

You can rotate the workspace slightly when in sketch mode, to allow you to see the sketch on the perpendicular plane.  As long as Toggle Sketches is enabled.

[Nick WheelerParticipant @nickwheeler]

We posted simultaneously, and it turns out you’re already well down the road I suggested.

You’ve probably got the ‘correct’ rails from an understandable process, and several odd looking combinations from experimenting.

 

If I was doing this demonstration in person, the next step would be how to split each rail into the three pieces that you would cut from real material. It’s easy to show, but time consuming to write.

 

That and the previous work would be a productive evening lesson.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou Nick, David –

I took Nick’s previous example – which I interpreted as the angled length of square pipe shown above – saved it as a separate file and used the Scale/Mirror tool to produce its reflection.

It puzzled me for a bit as the word “mirror” is not immediately obvious on the menu, but once I found it, here it is complete with the steps I used:

I have used the ordinary mirror tool and know that allows you to place the original and reflection symmetrically a set distance about a central plane.

[Nigel Graham 2Participant @nigelgraham2]

I’ve just the last, ooh, probably two hours building up the full chassis.

I found a use for that new-found “Scale/Mirror” tool: turning bits of channel the right way round. If they came floating gaily into the Assembly facing the wrong way I went back to their Part models and used that to flip them over. I don’t suppose that’s the tool’s “official” use – presumably you are expected to model everything pointing the right way in the first place.

I had to spend a lot of time trying to sort out the lengths. The built frame is an awkward beast to measure within 1/4″ with any accuracy, and I think I mis-measured some bits. Then of course in the Assembly model the two cross-members on that tapered section were the very devil to “fit”, with some revising of the Part drawings to try to make somewhere right. It is their distances from the front ends that count, though.

The curiously webbed appearance of the back end came from my thinking I’d placed the cross-member wrongly. It should go across the ends of the channels, where in fact I placed it first; but I could not put it right without risking ruining the whole thing. Luckily that error is unimportant. The only area of functional significance now is that wretched trapezoid so hard to measure and model accurately.  The rest is useful for Alibre practice and blood-pressure raising.

Somehow the Design index shows a lot of faulty constraints and although I can highlight them by pointing to their list entries it doesn’t really help me determine what was wrong, or what would go to pieces if I delete them.

 

 

[Nick WheelerParticipant @nickwheeler]

Instead of measuring the trapezoid, to tell the program how long to make the crossmember, use your increasing understanding of how CAD actually works by drawing the profile on your central plane and extrude to the inside edge of one rail. That’s probably in a menu attached to the distance box of the extrude command – Atom can’t be that different to Fusion. Using it saves the hassle already mentioned, and will form the end to the appropriate shape without any extra work from you. You don’t need to know the actual numbers until you’re about to cut real metal.

It also means that if you have to change the chassis width for any reason, the crossmembers will also adjust. This is another reason for developing CAD thinking, which is the opposite of the traditional drawing approach which says you should never measure off a drawing.

[Nigel Graham 2]

On Nigel Graham 2 Said:

 

The curiously webbed appearance of the back end came from my thinking I’d placed the cross-member wrongly. It should go across the ends of the channels, where in fact I placed it first; but I could not put it right without risking ruining the whole thing. Luckily that error is unimportant. The only area of functional significance now is that wretched trapezoid so hard to measure and model accurately.  The rest is useful for Alibre practice and blood-pressure raising.

 

Somehow the Design index shows a lot of faulty constraints and although I can highlight them by pointing to their list entries it doesn’t really help me determine what was wrong, or what would go to pieces if I delete them.

 

 

 

That’s 2 hours well spent, as you’re very close to a respectable model. But don’t spoil the progress by thinking its anything other than a learning exercise. If you don’t find the cause of the errors, or ‘risk ruining it’ now, you’ll never learn to avoid them in the future. And that will be utterly soul destroying when working on something that matters.

Don’t forget there’s an Undo command….

[JasonBModerator @jasonb]

The orientation of a part can all be done in the assembly, no need to alter it as an individual part. You can move it about with the mouse while holding shift to almost look right then constrain it as David has said several times in this thread. Or make the geometry visible and use that combined with flip to constrain the parts.

Somewhere in the thread I showed what Nick has just said about extruding to geometry so you don’t need to know the length or angle that the cross members meet the rails at.

As for the rear rail after saving you could come down the left column, right click the read rail and delete or if you want just suppress that part which then gives you the option to leave it. After that import a new rear rail and have another go.

A third alternative is to again find the rear rail in the left hand list and then click the > next to it which expands the list, click the > next to constraints and then you have a list of all the ones applied to the rear rail. Right clicking any of those will allow you to edit or delete a constraint without having to search through the long list further up.

Here I have expanded the list for an eccentric

 

[David JuppParticipant @davidjupp51506]

And As I’ve said repeatedly – sort out or delete failed constraints immediately they occur.  At that time you know what you did most recently that triggered the constraint error.  If you leave it, errors will only accumulate.

You’ll probably find that fixing/deleting the most recently added constraint will clear the errors on other constraints.

Your chassis is an obvious example of where it’s possible to get a cyclic series of constraint references which are all mutually dependent and hence can’t resolve.   That may not be the reason for the errors in your case, but I’ve seen it many times in the past.   My default example for this is a simple picture frame – in real life you glue & pin all four corners, but in CAD you only constrain 3 – mathematically constraining the fourth corner is unnecessary (the other joints and all members are infinitely stiff).

If you can’t sort out the assembly constraint errors – create a Package file from the assembly and send that to me – I’ll diagnose and advise what I find.

[David Jupp]

On David Jupp Said:

And As I’ve said repeatedly – sort out or delete failed constraints immediately they occur.  At that time you know what you did most recently that triggered the constraint error.  If you leave it, errors will only accumulate.

…

Absolutely!  And the advice about not letting errors accumulate applies to the production of parts too.

I think Nigel has a learning problem.   When something doesn’t work out he tends to jump to something else instead of sorting out the problem.   Unfortunately moving on with insufficient learning is liable to create models with multiple faults.  These accumulate to breaking point later.

Nigel’s approach is smart and determined but not focussed.   The result is slow progress in which previous partial learning is punished by baffling malfunctions two or three steps later.

Long since decided Nigel needs a mentor.   Someone looking over his shoulder to explain there and then when a false step is taken.  As is, we have multiple posts trying to explain issues that would be easily demonstrated and explained conversationally.

Nick advised Nigel to: Banish the words Basic, Advanced, Difficult and Impossible from your vocabulary.  That’s important.  Wonder if Nigel grasped why?   It’s not obvious.  Like understanding how 2D drawing experience can fog the way, concepts are best explained by a Q&A session.

Could Nigel be mentored with Zoom?   Needs an Alibre expert with a spare hour every day for ‘n’ weeks.   May not be practical.

🙁

Dave

 

 

[Nigel Graham 2Participant @nigelgraham2]

I don’t always see the faulty constraints immediately, by an error-message. Some seem to disguise themselves until further down the line I’m told the object is “over-constrained”, then the disguised ones in the list all blush bright red with embarrassment.

So select each to let it highlight the broken area in the model, but still don’t know what I had done wrong.

…

Jason –

Oh, I can wave the object about as much as I like with the Shift key and mouse but it moves wildly (I have wobbly hands, which doesn’t help!) and some still refuse to face the right way.

 

Nick –

[Undo] will only work up to a point, although Alibre gives it an unusual ability to step back many times, but it’s best to use it immediately. If the fault is something built in a long time back and not showing then, Undo might Undo a lot you don’t want Undone – and it’s still not necessarily obvious what you did wrong. Nor how to put it right.

The major dimensions of the frame are correct as far as I could determine but the real thing is very hard to measure accurately. The two awkward cross-members are the most difficult and it never occurred to me they could be generated in place. I think Alibre does allow extruding to another part, but I’ve not used that.

[David JuppParticipant @davidjupp51506]

Nigel,

If rotating using shift + drag is too wild, try the other component placement tools that we looked at during the screen share.

[David JuppParticipant @davidjupp51506]

Over constrained will turn all involved constraints red.  The one added last (at the bottom of the list) is likely to be the one that triggered the error. Try suppressing that to see if errors clear.

[Nigel Graham 2Participant @nigelgraham2]

Tried to correct that frame as shown above – I had to delete the misplaced part and replace it, but I think I damaged the rest of the thing in the process!

[Author]

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