What Do These Mean; Why So Many Loop Errors? (Alibre Atom)

[Nigel Graham 2Participant @nigelgraham2]

Two oddities:

When opening this growing (with many growing pains) assmebly, firstly a small window appears with a list of files comp[lete with their directory paths. Accept it, then this opens:

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It does not seem to affect anything, so is it referring to earlier files or editions of them I have replaced but Alibre is still trying to find them? I have made a lot of changes to the assembly not only for design purposes but to simplify some sub-assemblies to single parts easier to control.

 

Then, this peculiarly tilted plane started to appear. The plane was intended and it is in the correct position and orientation, by why tipped over? It does not seem to matter. It was originally for placing a bearing as a bolted-on part, but I subsequently simplifed the Parts to a more diagrammatic base-plate with three integral, solid journals as one Part. This was because I kept having parts wandering about despite supposedly constrained. I just make the tilted plane invisible, but could such antics create real problems?

 

The loop errors are in creating polygonal features (usually rectangular). It seems every time I try to move to creating an extrusion the starting shape is full of unexpected “open loop”, “intersection” or “degenerate” faults. This seems to happen with library rectangles as well as figures built from lines.

Though the fault-finding tool shows the locations the faults are usually invisible; and then the only cure is much experimental trimming and redrawing. Sometimes I need extend the lines past their junction to temporary external ones, them trim them back; but that risks overlain line fragments. If you draw a line from one black node dot to another, shouldn’t they snap together? (I don’t know if Alibre uses the term “snap”, but it should give the same result.)

I even found rectangles quietly re-sizing themselves until I loked everything in sight.

I noticed in that video cited in another thread a while back, all the outlines are neatly defined and located, showing as all black lines. I don’t see that effect very often..

[JasonBModerator @jasonb]

First one is probable files that have been deleted but are still listed down the left side, renamed or copied but not using “save as”

The plane will only be tilted if you inadvertantly picked geometry that was at an angle when you created it. Right click the plane towards the top of teh left hand list and you can edit it.

It won’t snap if you have turned snap off or set it at a very short distance. I have no roblem. Orange-Red to Black are all related to how constrained a sketch is. the more you tie it down by giving lines a length or radius or set their position the closer you will be to a completely black sketch though I often work with quite a bit of a sketch still red.

[David JuppParticipant @davidjupp51506]

Nigel,

As Jason said – if you get a list of files/paths when you try to open an assembly or a drawing – this is an indication of missing files.  There will be some files in the list which have a red spot next to them.  You should select one of these, then use the ‘replace’ button at the bottom of the dialogue to re-link the file (assuming you have it somewhere).  Repeat until all missing items have been re-linked.

This happens if you have moved or deleted files that the assembly requires.

As for ‘open loop’ errors – after using the analyse tool, click on one of the problems in the list – it should now be highlighted on screen with small red squares.  Depending on the nature of the open loop, there might be a ‘Heal’ option available to automatically fix it.

I’m sure we’ve covered ‘snaps’ before – you can enable a grid and snaps in sketch mode (if you really want to), perhaps more usefully there is ‘snapping threshold’ setting which controls how close you have to get the cursor to an existing item for the new figure to ‘snap’ to it.  The allowed setting varies from 0 thru 5mm.  At zero, it is almost impossible to snap to existing figures, at 5mm it may be difficult to select the correct item to snap too in congested sketch.  The ideal figure for you will depend upon display settings and what you are modelling.  My system is set to 3mm.

The setting can be found in System Options -> Parts/Assemblies -> Sketching :  Snapping  (it’s right at the bottom of the dialogue).  There is an equivalent setting in the Drawings-> Sketching area.

[Nigel Graham 2Participant @nigelgraham2]

Thankyou. The “Heal” function in Atom seems to work on only one type of error, ‘Open Loop’ I think. It does offer a tolerance band with an extremely fine diameter, but as it doesn’t always work for me there must be something else wrong at those points.

Fortunately the wonky plane had tilted on its own plane so it didn’t actually do any harm there, but I was worried about similar happening somewhere else and causing damage.

[David JuppParticipant @davidjupp51506]

The tolerance value for Heal can be increased – then it will sometimes become active and available.

Heal can only fix small gaps in a loop – it can’t fix a short isolated line, or a line that extends beyond the boundary of a shape outline, because it isn’t clear what to do – usually these need trimming or deleting.

As we keep saying – if you have something you don’t understand just send the file.

Overlaps are typically harder to deal with, and degenerate figures can be be a bit of a mystery.

[Nigel Graham 2Participant @nigelgraham2]

‘Heal’ – that’s the one! Yes, I have used it successfully a few times.

One place I see open ends develop is on tangential junctions between a straight line and an arc that started as a circle. These fragments can be so small that they are lost within the displayed thickness, but I discovered if you enlarge the image sufficiently they will start to show. I think they sometimes create curious node-pairs.

Over-lain lines, one lying right on top of another, won’t. I’m not sure if that’s what they mean by “Overlap”. It’s these that seem to respond to testing the line by “Trim”. The overlay will vanish without any obvious sign of change, so I Trim again until the line disappears completely then Undo it by one step.

The “degenerate” error seems to disappear if other errors are corrected, so I have just paused to see if the Help document will explain it. It doesn’t!

It tells us how to use the analyser but not really what the different faults mean. “Open Loop” is fairly intuitive, “Intersection” a bit ambiguous, and “Degenerate”…. I can’t think what that is at all.

[JasonBModerator @jasonb]

With your circles meeting lines are you using the “tangent” constraint when sketching or are you just visually placing the lines and circles? You should constrain the two and then there should only be one node where they make contact not two or a complete miss.

[David JuppParticipant @davidjupp51506]

Degenerate figures included things like a triangle with all three corners along a line – that would also give rise to overlaps, and maybe intersection errors.  So, YES, the alert for degenerate figures will often vanish as you fix other problems.

[SillyOldDufferModerator @sillyoldduffer]

My sympathies to Nigel – Learning new Solid Edge features is currently causing me gyp, including crashing the software!

My first reaction to missing files, tilted plane, and loop errors was these are all characteristic learner driver problems.  Fits my hypothesis that Nigel is trying to run before he can walk, attempting to assemble parts that are broken because the underlying sketches are wonky.   Lines not meeting might be caused by a trainee thinking visually close is good enough, not understanding snaps, not applying constraints etc.  (See Jason’s comment about tangents.)  If so, the cure is to spend a day doing nothing but practising sketches, getting them to go ‘black’, i.e fully constrained.   Tip: though not essential, fully constraining a sketch reduces the risk of “not visible to the eye” mistakes and prevents the object changing shape later by accident.

My second thought is that Nigel has ‘got it’ and is being sabotaged by his hardware.

• Chief suspect, the MOUSE!  CAD requires accurate positioning.  Cheap mice cause lots of trouble because they don’t read position accurately and their click switches are erratic.  Mid-range mice are more reliable, but need a good mouse mat to perform adequately; they can still cause ‘finger trouble’.  I recently invested in a £90 gaming mouse (Logitech MX Master 3S) and it is much better for CAD.  If the mouse is cheap and basic, upgrade it!   Especially if the operator is arthritic or trembly.
• Any personal computer less than, say, 10 years old should have the poke necessary to run CAD.  Older kit can be sluggish though causing problems due to the user clicking repeatedly because the first click seems not to have worked. Result is the CAD tool gets a succession of queued click commands, and who knows what they will do!   If serious about CAD, especially large models, it pays to own a fast computer with plenty of memory, not a machine bought yonks ago for light duties.
• A big screen helps!  My 15″ laptop noticeably cramps CAD and I make more select mistakes on it:  a 27″ inch screen opens up the workspace.
• Even better, two big screens!   Not essential, but a second screen allows CAD windows to be moved out of the way, and web instructions to be displayed alongside.

Keep at it Nigel, lots of impressive progress recently.

Dave

[SillyOldDuffer]

On SillyOldDuffer Said:

• Even better, two big screens!   Not essential, but a second screen allows CAD windows to be moved out of the way, and web instructions to be displayed alongside.

Though note that if the graphics adapter is marginal, or if it shares system RAM, a second monitor can be something of a burden.   Particularly noticeable with hi-res monitors.

There may be settings in CAD relating to rendering quality and certain fancy but unnecessary display options, that can help a marginal system to get by.

[NealebParticipant @nealeb]

To underline what both Jason and Dave have said – you cannot always rely on the CAD software realising what you are asking. I’m actually a Fusion 360/Solid Edge user and one thing I realised quite early on with both is that if, for example, you try to draw a line between two points in a sketch, the software will often “know” that the ends of the line are actually coincident with the two points and will automatically insert a constraint that binds them together. But not always, even if a quick glance suggests they are coincident. And if there is no constraint in place, all sorts of unexpected things might happen later. These days, I draw a line near to but not quite at the place required. I can then explicitly add “coincident point” constraints that force the end of the line to the correct place. Similarly, a line that is tangent to a circle or arc that also finishes at the point of contact might need both a tangent and a coincident constraint even if the software adds one, both, or neither if you just draw the line to seem to touch the curve. Draw the line to finish near the required point, add constraints to suit, and you know what’s going on. Similarly, I would never try to draw a line to an exact length – draw it near enough and then modify the dimension to get it exact.

I’ve done a few “intro to 3D cad” sessions for fellow club members and these tips sit alongside little mantras like “never use a dimension if you can use a constraint”. Things that are quite foreign to traditional draughting techniques but useful pointers in the CAD world.

[Nigel Graham 2Participant @nigelgraham2]

Dave –

I do use the Constraints!

I learnt a long time ago that CAD is Ever So Punctilious about making things meet but you need give it the right conditions for it to work.

Alibre puts big black dots everywhere that I took to be snap nodes, so if I track a line from node to node it will connect to the existing lines. Only, they don’t, not every time anyway – but does it also want a constraint applying?.

I think the tangent problem is where the tangency is very slightly beyond a reference centre-line. So when trimming the initial circle for a rounded end on a tapered object, it leaves a tiny fragment hiding in the displayed lines.

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Alibre Atom may be a bit of a tight fit but I did take some advice on selecting the computer, a factory-rebuilt DELL. David Jupp has given me some tips on making the software run more efficiently on it.

It has a reasonably large screen at 21″. Though if I need enlarge the image I can’t also move the picture while one or another tool is open, if the area concerned is over the border.

The mouse is of reasonable quality, probably not “Hi-Fi” but since I use it with a rather wobbly hand directly on a rather wobbly MDF keyboard shelf I think we can acquit it! (My GP says I’ve an “essential tremor”…. It’s not “essential” to me: it’s free to any takers!)

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David –

I read your PM notes and link, and have bookmarked that page.

I don’t think it is possible to add a second monitor to this PC.

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Nealeb –

I think you can use only one constraint per connection, in Alibre Atom. If you try to apply more it says “constraint already exists” or “over-constrained”. It should need only one, of course, but I might sometimes be using the wrong type.

So for that tangent to a circle, sketching the line by eye slightly beyond the circle then picking only the Tangent Constraint and both figures will connect them; even with a slight external or chordal gap but obviously within fine limits. If you trace the line closely enough it can snap them together automatically and display a little constraint symbol there to confirm it.

 

Atom asks you to enter a dimension unless the entity is from one node to another, when it can work it out for itself. E.g. a rectangle has two boxes in which to edit the tracked length and breadth; a straight line asks for its length and angle to the axis. (There are vertical and horizontal constraints, too, for lines at 0º and 90º to the axis).

I’m not sure it always does link two nodes though – the lines look as if there but the fairly coarse line display might hide tiny mis-closures preventing extruding the sketch.

[David JuppParticipant @davidjupp51506]

Tangent sketch constraint makes to line tangent to circle or arc, it does not fix the line end.  That would require either an additional coincident constraint or for the user to trim the ‘spare bit’ of the line.

It is possible to fix end of line to circle/arc first, then add tangent constraint, easier if the initial connection point is obviously some way from where tangency occurs.

[Nigel Graham 2]

On Nigel Graham 2 Said:

Dave –

I do use the Constraints!

Yes, but do you ensure sketches are fully constrained, signalled by the outline turning black?   Locking stuff down early can prevent trouble later, especially during the learning phase.

…It has a reasonably large screen at 21″.

My second screen is 21″ and it’s noticeably inferior to my main 27″ screen.  I occasionally use Solid Edge on a 15″ laptop and the small screen increases my error rate.   I’ve also connected to SE remotely with a 13″ laptop and that’s very difficult to use.   For CAD big is beautiful, if you can afford it.  21″ isn’t awful, just be aware that smaller screens tend to multiply ‘finger trouble’.

The mouse is of reasonable quality, probably not “Hi-Fi” but since I use it with a rather wobbly hand directly on a rather wobbly MDF keyboard shelf I think we can acquit it! (My GP says I’ve an “essential tremor”…. It’s not “essential” to me: it’s free to any takers!)

That combination may explain why you’re having such a hard time!  Though snaps and constraints help enormously, a tremor coupled with a ‘reasonable quality’ mouse on a wobbly shelf really is asking for trouble!   It’s the CAD equivalent of a lathe with worn bearings, loose gibs, and slipping belt on a bendy bench.

A £10 mouse is adequate for ordinary purposes like web browsing where clicking nearby is good enough.  Their shortcomings show up as increased error rate when doing precision work though – games and CAD.  My experience is a £50 mouse reduces CAD problems considerably, and a £100 mouse is noticeably better again.   A ‘reasonable quality’ mouse will multiply tremor errors.  By the way, a professional CAD jockey might not consider a £100 mouse to be of ‘reasonable quality’!

An expensive mouse on a solid shelf won’t fix tremor, but better equipment might reduce the trouble tremor might be causing.  Learning CAD is difficult enough with a perfect computer/mouse/screen combo and trying to do it with a wobbly set-up might waste months of time.   CAD depends on mouse accuracy, and, if sketches are broken, parts and assemblies won’t behave.   Getting any weird inconsistent behaviors?  If mouse input is suspect the operator has to take extra care to make certain all is well before proceeding.  A good way of upsetting CAD software is to let errors persist until something breaks.   Though good quality control compensates for a poor mouse/wobbly operator, it’s cheaper to upgrade the mouse and that nasty MDF shelf!

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I don’t think it is possible to add a second monitor to this PC.

Almost certainly can, but not cheap!  Requires a graphics accelerator.   As a second screen is ‘nice to have’ rather than essential, I wouldn’t bother.   I only have a second screen because my games enthusiast nephew gave me a screen and accelerator.   Not good enough for him, he insists on three giant curved high resolution screens.  His rejects are fine for CAD though.

Dave

[JasonBModerator @jasonb]

I’d best get rid of my £12 mouse then and buy a mouse mat too😂 🐭

[David JuppParticipant @davidjupp51506]

Strangely I manage OK with an ‘amazon basics’ mouse – cost less than £5 when previous mouse failed (button switches were no longer reliable).  It is an optical mouse, used on a desk that has some pattern – no need to remove a ball to clean crud off the rollers.

For me, zooming in enough to see what’s going on, combined with having ‘snap threshold’ set to an appropriate value to make snapping to existing entities easy is key.

Personally I do not use ‘snap to grid’ at all – I find it hinders more than helps (but I know some people do like to use it).

[David JuppParticipant @davidjupp51506]

Nigel – some users who have hand motor issues of various types have reported that trackballs have advantages compared to mice for CAD – easier to be precise.  Could perhaps be something to take a look at.

[DiogenesParticipant @diogenes]

I seem to get much more reliable sketch results from joining a line to an ‘Arc’ rather than a ‘Circle’ – seems to result in less ‘miss-hits’.. (..?perhaps ‘cos there’s a node already at the end of an arc segment and the programme ‘sees’ it as a portion of a line rather than as a closed entity..?)..

To the point where I might use a Reference Circle to ‘layout’, but for the actual ‘sketch construction’, I use Arc..

Don’t have enough experience to know whether this is a real ‘thing’ or not..?

 

[JasonB]

On JasonB Said:

I’d best get rid of my £12 mouse then and buy a mouse mat too😂 🐭

On JasonB Said:

I’d best get rid of my £12 mouse then and buy a mouse mat too😂 🐭

Ah, but I’m trying to help Nigel, not a lucky chap who doesn’t have Essential Tremor. The exam question is ‘Why so many loop errors’, not ‘Is CAD possible with a cheap mouse’.

David Jupp’s suggestions are helpful: a tracker ball, and – of course – zooming in.  Anything that avoids selecting stuff by accident, missing the snap entirely, or activating a wrong constraint.

Solid Edge has a double edged facility.  When creating a part in place within an assembly, it highlights all the snap points available near the mouse pointer, and there are often many.   Excellent for sizing and positioning new parts based on existing parts, but causes baffling problems if the wrong one is accidentally snapped.   Was the main reason I had bother embossing the Enigma alphabet around a ring: the ring already had 27 cutouts in it and was being edited within an assembly.   If Alibre does similar, then Nigel might well be confused.  SE had me flapping until I realised what the issue was!

Dave

[NealebParticipant @nealeb]

I would agree that a trackball rather than mouse is useful for those whose hands are not quite steady for whatever reason. It can separate the “positioning” function from button-pushing when the act of pushing the button tends to move the mouse. Position the cursor and then press the button with no risk of the cursor moving.

David has confirmed that Alibre Atom does indeed allow multiple constraints between two given entities so that you can use a coincident and a tangent constraint for a line which is tangent to but terminates at a curve (circle or arc). He also mentions just trimming back the “excess” bit of the line as an alternative to using the coincident constraint.

That brings me to another discussion point – why do people bother to trim back unwanted lines and bits of line in a sketch? This smacks to me of drawing-board thinking where the finished drawing needs to look clean and tidy. However, I regard the “sketch” as used in 3D CAD as the equivalent of construction lines in 2D draughting – a means to an end and not an end in itself. Once you have extruded the sketch elements (correctly constrained, of course!) then any odd bits of lines are of no relevance. In fact, my own experience is that deleting these apparently excess bits of lines can sometimes create its own problems. Typically, this can be where the “excess” line being deleted has been used as part of adding a dimension on the sketch. I have also had this happen when trimming a circle back to an arc. OK, maybe when you come to the extrusion you need to make sure that all the relevant sketch regions are included but that’s only a mouse click or two. Once the 3D body has been formed, who cares what odd bits of line were in the original sketch?

Am I being daft here in looking to make things easier for myself, being unnecessarily contentious, or does it make sense? Maybe I’m over-reacting to having to tell people that I have worked with to forget hard-won and essential techniques that apply to 2D draughting but have no place in 3D!

I should add that I am a F360/SE user but I would have thought this approach fairly generic.

[David JuppParticipant @davidjupp51506]

Nealeb,

Sketches have to be closed profiles if they are to be extruded or revolved in Atom3D – so ‘extra bits’ of line that stick out are not acceptable.  Doesn’t matter for reference lines.

The ‘regions included’ thing you mentioned is not part of how Alibre works – it demands closed profiles.

[JasonBModerator @jasonb]

In Alibre the lines are trimmed as you need a solid “shape” to extrude and can’t extrude a sketch with odd lines beyond the solid.

Trimming the excess is probably quicker than going round again to “darken” the lines as you would with pen/paper drawing

[Grindstone CowboyParticipant @grindstonecowboy]

Just a bit on trackballs, I have a Logi (formerly Logitech) Ergo M575, and find it generally very good. The one thing I would like to change if I could is the fact that it is ridiculously easy to accidentally right-click – just gently resting your second or third finger on the right button is enough to do it, a touch more resistance would improve things no end. Takes a bit of practice and concentration to avoid menus popping up now and then.

Rob

[Nealeb]

On Nealeb Said:

…That brings me to another discussion point – why do people bother to trim back unwanted lines and bits of line in a sketch? ….

I should add that I am a F360/SE user but I would have thought this approach fairly generic.

SE here too.  Although it’s not necessary to trim overshoots in SE I always do because it avoids creating snap points outside the wanted part of the sketch.  Sod’s Law says “if it can go wrong it will”,  and trimming and removing unnecessary lines avoids one cause of trouble.   They’re more likely to cause bovver in big models than little ones, so the horses for courses rule applies!

Dave

[Nigel Graham 2Participant @nigelgraham2]

The mouse I use is a DELL optical one – but it does not give me a model number or anything. I forget if it’s one I bought, for rather more than £10, or it was the one that came with the PC. I know the other one of the two was dreadful, with nasty cheapskate flexible keys making its action very uncertain. No good for CAD, and probably not very good for things like ‘Excel’.

I use it with my right hand and that is less tremulous than the left anyway, but am sometimes still fighting a earthquake between myself and the shelf; and the finer the point I am trying to unearth the worse it becomes.

The shelf wobbles probably because it’s screwed to a pair of runners designed for filing-cabinet drawers and electronics racks, and so are not precision machine slides (they don’t need be, for their real purposes). Nor even nicely-made wooden furniture drawer slides. The action is actually yawing rather than up-and-down.

I could try a track-ball but a better test first would be improving the furniture!

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[Though not using CAD, one of my former work colleagues has quite small hands, and found a mouse styled vaguely as a model VW Beetle – really intended for children – was better for him. At the same time I developed arm pains and the company gave me a “Penguin”-branded, semi-joystick pointer used with a much more natural grip. ]

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I discovered the problems with line off-cuts long ago in TurboCAD, and Alibre Atom is the same in that respect. Neither can extrude an outline with burrs or over-lays – the latter hidden by being precisely on the intended line.  Atom indicates only the faulty nodes, and I’ve often been driven up the wall by going round the fault-tracing circle umpteen times to clear one sketch, sometimes without finding what was really wrong.

I had not known other CAD makes are more forgiving and will ignore or remove the burrs. It does seem good practice to remove them all anyway, even though the sketch is not the finished image.

Reference lines seem rather good at hiding things, too, and sometimes I’ve had to delete those and dimensions to try to see just where the fault lies.

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