“Your Sketch Is Not Closed,” says Alibre Atom, “So tough!”HERE?ERE?

[Nigel Graham 2Participant @nigelgraham2]

Any sketch the slightest bit complicated, such as containing fillets, produces this over and over again:

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I go round and round trying to chase every point in it but the errors are so mathematically tiny they are invisible, and nothing I do roots them out. Sometimes it seems to move them, because one or two lines will change colour between red and orange for no obvious reason.

How can it expect me to put them right when it does not shown what is really wrong and where?

(Many of the other Alibre Atom error messages are even in computer jargon, not geometrical terms at all, so meaningless to anyone not a CAD programmer.)

When I managed, once, to move the sketch to the model page, the programme disabled the Extrude tool and plastered some totally incomprehensible message over it.

Why does it have to be so damnably frustrating?

[Clive FosterParticipant @clivefoster55965]

Does Alibre Atom not have a “snap to point / line” or equivalent command to ensure intersections actually intersect and closed figures are closed? I can’t imagine any effective CAD program not having such a function. I’d have thought it essential for 3D work. But I’m a 2D dinosaur so what do I know.

Pretty effective in my old copy of VectorWorks provided the snap distance is set to something reasonable in relation to the drawing scale. Set it too small and its a right pain to join or close figures. Sounds like you need to investigate how the Aibre equivalent works.

On the rare occasions when VectorWorks has a hissy fit about joins and intersections I resort to typing exact co-ordinates into the shape data to force the intersection. Which often involves some creative shape editing to define the intersection point followed by restoration to the full shape when intersection has occurred.

Clive

[DiogenesParticipant @diogenes]

Can you not highlight, and then zoom in, to resolve them?

[Paul LousickParticipant @paullousick59116]

As well as checking that the lines in the sketch are joined, also check for extra, unwanted lines that may have been drawn while moving the mouse while making the sketch.

I use Solidworks, not Alibre and this sometimes happens if I snap to the end of an existing line and inadvertently move the mouse before closing the sketch.

[Nigel Graham 2]

On 27 July 2025 at 21:09 Nigel Graham 2 Said:

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The mind boggles at the thought of ‘Degenerate Figures’

MichaelG.

[JasonBModerator @jasonb]

How are you adding the fillets?

If you are attempting to place a circle close to a line by eye you will get problems. If using the fillet tools that should remove the bits of line you don’t need and add the curve correctly joining each end.

You may get a problem if you try to put two 0.188″ fillets onto a 0.375″ part but otherwise it works. This is likely the degenerative end

Often better to add fillets as separate items once the basic shapes have been sketched and extrudes rather than withing the sketch.

The errors are not invisible, just verty small . I’ve told you before to click one error on the list and then Alibre will highlight it with a red square, zoom in if it is not obviuos or alibre does not offer to “heal” it.

Have snap set to 3mm or 1/8″.

If trimming a line or circle make sure you remove all of it, it may only trim until it meets another sketch line or ctr line but the click to highlight will show these

See my fillets at the end after the rim, hub and spokes were done.

[Nigel Graham 2]

On 27 July 2025 at 21:09 Nigel Graham 2 Said:

.. …Any sketch the slightest bit complicated, such as containing fillets, produces t.. …

 

 

 

Jason types much faster than me..

..the penny drops – fillets, how?

If you are drawing boxes / angles and then using intersecting arcs & circles, yes, you probably will see error messages;

use of constraints can help to remove ambiguities, er, example;

..on the left side is the intersection of a ‘trimmed box & circle’ fillet as drawn – you can see two node points which indicate that there is trouble ahead – we want these lines to meet at a single point (node), the presence of a second shows that there is some discontinuity – here causing an overlap..

If you apply a ‘Tangent’ constraint between the arc and straight segments, as I have done at the bottom, the programme can ‘see what you are asking it to do’ and will rationalise the construction, placing a single node at the intersection.. ..

As said, not sure I’d be adding them in the sketch..

[David JuppParticipant @davidjupp51506]

Nigel,

As I emphasised when we did a screen share session a long time ago – KEEP SKETCHES SIMPLE.

That will make such errors less likely, it also makes later editing of the sketch easier.

As mentioned by Jason – set the ‘Snapping Threshold’ to a sensible value (I also use 3mm, but the best value is a bit dependent on your monitor resolution).  The setting is in System Options -> Parts/Assemblies -> Snapping.  It’s right at the bottom of the window, you may have to scroll down.  Snapping threshold helps to make sure figure meet; if it is set to zero for example, you’ll find it very tricky to get figures to join.

Whilst your can include fillets in sketches – it usually makes things easier and faster if you don’t.  Instead add them as 3D features later in the modelling.

For overlaps in sketches – if not obvious by selecting the error from the list, try right click near the indicated location and choose ‘Advanced selector’ from the context menu.  This opens a small window which lists all sketch figures in the immediate vicinity of your cursor, you can select from the list.  If nothing else this will make it clearer if there are 2 or 3 overlapping lines.

 

Often one problem figure in the sketch will produce two or three warnings in that sketch analysis list – so don’t panic.  Fix what you can find, and try again.  If you get stuck, send the the file to Alibre support.

 

[JasonBModerator @jasonb]

Taking Diogenes sketch when you get the error message, click one of the items on the list and it will mark the errors in red as I said above, then zoom in with the mouse wheel and you can then see that the circle overlaps the straight line

[Nigel Graham 2Participant @nigelgraham2]

Clive:

Alibre Atom does not use obviously snaps by name. Normally it seems to use “constraints” as equivalents, such as tangents, line-meeting, trim, etc. What can sometimes happen when combining curves and straights among various construction “reference” lines, is leaving little “frayed ends” just past the tangent points, and those only show on enlarging the display. So I did test for those.

Some CAD systems, such as TurboCAD, let you inadvertently stack such prunings, making further operations impossible (it doesn’t know which fragment you mean!) but using “Select” reveals them for deletion. Alibre seems helpfully to prevent you creating such stacks in the first place, but its frayed ends can be hidden by lines and node-dots.

That a CAD programme is 2D or 3d does not matter: it still needs entities to meet exactly and they have the mechanisms to do so. Unfortunately “exactly” means to extremely fine mathematical limits, not mere visibility, though Alibre helps by marking meeting-points and vertices as “nodes” indicated by black dots, and constraints by little symbols next to them.

 

Diogenes:

No: the errors are far too fine for magnifying to reveal them; but I tried al those things you demonstrate. I was going round and round what I think was the fault area, trying all sorts of re-drawings and re-constraining and all it did was make new errors.

That error-message table tells you the error type but in “Atom” the “Analyse” tool seems inoperative, and “Heal” says it isn’t.

The two words in the capitals in the title should have been “HERE? WHERE?” because I could not see where it was wrong. Nor what was wrong.

 

(Incidentally I have used a deliberate, tiny misclosure of a polyline figure with thick lines to generate a 3D view of an open-topped, thin-walled box. A fully closed polyline, in 3D CAD, would create a solid block. That was in TurboCAD. It would probably need a different method in Alibre, which does not extrude misclosures. )

 

David:

I keep the sketches as simple as I can but still outline what I am trying to design. Whatever was going wrong, all the various lines were shown in red with two or three in orange around the faulty area.

I narrowed the search to possibly, either a fillet not meeting the straight sides, or two of those straight lines not meeting correctly, but all the appropriate node and tangency symbols were there.

Trying to correct the area just made the lines change colour, as if some were entities not really connected to their fellows.

I tried extending the lines to temporary ones beyond the figure, and trimming back to create the junction. That slowed the black dots but the figure was still not closed.  I tried re-setting the tangent constraints – Alibre said they are already there.

Enlarging the image did not reveal any “frayed” ends that needed trimming off.

I did not know Alibre Atom has snap settings – I’ll have a look next time. I’d assumed if the lines were constrained to each other the snap is an automatic part of the constraint.

 

Jason:

That error highlighting was just not happening, even if I enlarged the image!

I am not sure if I bothered to save the drawing. If I did I will try that.

 

 

 

[JasonBModerator @jasonb]

Trying to correct the area just made the lines change colour, as if some were entities not really connected to their fellows.

 

Well that could indicate that the are not correctly joined to other lines to complete the closed sketch

There are some that won’t show up no matter how far you zoom in. I see you had several overlaps in your list, you won’t see one line if it is sitting on another but may see the odd black dot where one starts and another ends.

Sketch below just looks like a rectangle but the system throws up errors.

Click th eopen loop and it change sthe colours of teh problem lines

Or click overlap and it changes the colour of the two lines that are one on top of the other, no amount of zooming will change what they look like

[David JuppParticipant @davidjupp51506]

Nigel,

Save design files that have problems – send them to Support.  You’ll either get help, or an issue in the software that needs to be addressed will be confirmed.

If you delete everything that doesn’t work – you are unlikely to learn from it.

The line colour in a sketch shows if the figure is fully defined / partly defined /undefined – ideally you should aim to have every figure in the sketch fully defined (that’s probably black or dark grey, depending upon the selected colour scheme) – but realistically that won’t always be achieved.

If a line changed colour during you edits, you probably fixed at least one issue.

 

As for outlines – you don’t have to include all the detail in one sketch.  First sketch might be simplified outline (to be sawn out), another sketch might add a cut for an opening or a notch in the outline.  Holes to be drilled added as another stage, and rounding of corners added as one or more 3D fillet operations.

[SillyOldDufferModerator @sillyoldduffer]

Nigel has smacked into a common 3D-CAD learner problem.  I recall a series on CAD in Model Engineer where the author mentioned the same difficulty without twigging what he was doing wrong.  And I struggled with it at first too.

The 2D sketches used by 3D-CAD have to be geometrically correct and there are a number of ways of messing them up:

• Appropriate snaps not selected.
• Finger trouble causing lines to over or undershoot so they don’t connect properly or create miniscule new sketches. That a sketch looks OK isn’t ‘good enough’, because the errors are often too small for the human eye. Therefore the operator has to pay attention to whatever clues are provided by the software.  Unfortunately, the clues have to be decoded by the operator, for example, when the problem was caused by a missing constraint or by snapping to the wrong feature.
• Working manually rather than using the tools provided.  In general, better to use the software tools because they don’t make human mistakes, but it does require the operator to learn how to drive them.
• Bad practice.   David Jupp mentions not filleting in the 2D-sketch.  You can, but it locks the fillet into the model and is a tad error prone.  Better to apply fillets to the 3D object later, where they can be removed or edited as needed.

This example of a bad sketch is apparently a simple triangle, but it has three faults that prevent it being extruded into a 3D-object! Looks OK but isn’t.

First, zooming into the top corner shows the lines don’t meet.    This is an ‘open loop’ that can’t be extruded.  The gap is only a few micrometres.

Bottom left has two mistakes, also tiny.  The two lines overshoot rather than join at the end, which is a “self-intersection” that can’t be extruded.  Also, a tiny square overlaps the line, creating an illegal combination, two objects in the same space.  A shaky operator with a cheap mouse can inadvertently add tiny lines and loops to the sketch.  He can’t see them, but the software insists on a tidy up.

Lastly, a degenerate triangle.  A triangle consists of 3 connected lines with a space between.  The triangle is degenerate when the space is too small, in this example the vertical is 30um with an 80mm long baseline.  Although FreeCAD can extrude this, at some point reducing the vertical height towards zero will cause it to gag.  A triangle with zero height is degenerate, same issue applies to all polygons – a loops defined by coordinates that cannot be extruded, because there is no space inside the object.

I won’t confuse by showing what FreeCAD does to help.  Though similar to Alibre, it’s different!  But FreeCAD, F360 and SolidEdge all support a similar process.  Faced with a sketch that won’t extrude:

• the error message may help.  Don’t blow a fuse if it’s “jargon”, look it up on the web and ask here.  Don’t expect too much, error messages often come from deep inside, and only reveal “SOMETHING IS WRONG”.
• The error message may be supported by a geometry checker – Jason describes Alibre’s.  The operator has to know the tool exists and how to drive it.
• Open the sketch editor and:
  • Check the sketch’s constraint markers.  Are those present correct?  Are any missing?
  • Zoom in on the joins looking for gaps, overlaps, and unwanted extra lines.  Correct them.

Best to avoid problems:

• Understand and apply snaps and constraints appropriately.  They are important.
• Do not over-constrain because locking down can block legitimate later changes.
• Under-constraining can be problematic.  Ideally a sketch should have zero degrees of freedom, meaning that all dimensions and coordinates are specified, and none of them are inferred.  In practice, none of the CAD packages I’ve used in recent years have been fussy about having degrees of freedom, but floating can cause trouble.
• Snapping to the grid causes problems because sketch lines have to connect to each other, not to a grid in hyper-space!  Grid snapping should be used sparingly in 3D-modelling, and some recommend not using it at all.
• Keep sketches simple.   Most of the model should be developed in 3D, not in the 2D sketch.
• Develop sketches step by step rather than testing a monster at the end.  And if a monster emerges, it’s probably unnecessary: consider ways of simplifying it.
• Learn what the markers on a sketch mean, and watch out for and tackle anomalies as you go.

Interesting in that bad sketches causes much grief at first and suddenly disappear once the operator has ‘got it’.  As always, it’s ‘easy when you know how’.  Some lucky folk pick stuff up naturally whilst others have to swot.

I have high hopes of AI.   The CAD tools I use all try to keep going in hope I will bring it together in the end.  Errors are thrown when the software can’t go any further with my instructions, at which point it it fails without considering the history, leaving me to look for clues and work the problem manually.   AI supported CAD might be able to backtrack and suggest where I went wrong.  Unfortunately, for the time being, we have what we have, and have to learn it.

Dave

 

 

 

[Nigel Graham 2Participant @nigelgraham2]

Thankyou.

I found the problem eventually, and it was one I had not expected at all in Alibre Atom (though I was familiar with it in TurboCAD, whose ‘Select’ tool will indicate it).

Not lines missing or overshooting each other, missing constraints or anything like that, but what I call “stacking” in the absence of any proper name for it.

By that I mean that although the entities are all on one Layer, there are complete entities or fragments of them lying on or under the visible lines as if on a parallel sub-layer.

Alibre’s “Select” tool does not reveal them, but carefully deleting each element one at a time did.

If the line vanished completely I knew that was fine and I’d restore it by “Undo”. If it showed another line or a fragment under it, I’d delete that in turn to see if it was hiding a third one. Eventually I’d be left with a gap to be refilled, with luck by “Undo”.

I did not know this would happen but experimented more from desperation than any analysis.

 

It comes from needing two or more attempts to edit something, either to correct a mistake or to improve the design. I thought Alibre simply works on one layer so over-writes anything already there, provided the entities match. If they don’t of course, the wrong bits would be visible.

 

I thought Alibre Atom guards against over-constraining?  It stops and says the sketch is over-constrained until I delete the constraints highlighted in red in Design Explorer.

 

Shouldn’t need “AI” to say where the errors are: just better error-traps that show what is wrong and where, even if they do not put it right. After all, MS ‘Excel’ does that if you miscount all those parentheses in a formula, using pretty colours to help you.

 

 

(Better error-traps…. available from all better mouse-trap stockists.)

 

 

[JasonBModerator @jasonb]

Nigel, see my post earlier about lines sitting ontop of each other and how Alibe DOES identify them. No need for AI just read what people are telling you.

[Nigel Graham 2Participant @nigelgraham2]

I see what you mean but I didn’t seem to be getting those error markers. When the table says things like the “Heal” option is not available I tend to take its word for it and read the whole tool as simply telling me the drawing’s wrong.

[David JuppParticipant @davidjupp51506]

Nigel,

Heal can only apply to open loops, not any other issue.  Sometimes you can get it to become available by increasing the tolerance value.  It won’t always become available.

[JasonBModerator @jasonb]

As David says, Alibre will tell you something is wrong. Alibre will show what is wrong with the red markers. If it can Alibre will heal and issue. Otherwise it is down to you to correct your errors but at least you should know where to look as Alibre has located the position of the error for you.

 

Maybe this will complicate things but worth saying now. In some instances, you will want a sketch that is not closed and in that case you simply ignore the warning messages. Things like sketching the path for a sweep are a typical reason not to have a closed sketch.

Infact the same sort of sketch is one where you will want to use fillet at the sketch stage if say you want to “bend” a pipe or bar around a corner, if you don’t fillet the sketch Alibre will mitre the joint rather than bend the profile around the path of the sketch.

[Nigel Graham 2Participant @nigelgraham2]

I know a sketch has to be closed for it to be extruded; but so far at least I’ve not needed a sketch to be delberately open, so I am not sure how that might work.

Not in Alibre anyway. I could make it work in TurboCAD, to represent a sheet-metal box, because that lets you extrude a line using its “thickness” as the “width” of the entity. I think the same in Alibre would need the sketch to be a pair of closed, concentric outlines separated by the wall thickness.

I recall there is also a sweep function in Alibre to cover things like curved bars and tubes.

[JasonBModerator @jasonb]

I’m not sure if Atom has it but if there is an arrow below the extrude icon that will allow you to use “thin Extrude”

Image below was a simple U shape from 3 lines resulting in an open sketch. The thin extrude allows you to enter a thickness and whether that is to one side or the other of your lines.

Another opinion for a thin walled box would be Shell again if you have it. Sketch a rectangle, extrude it as a solid and then use shell to remove the inside leaving a thin “shell”

Some CAD including the top Alibre option also has a sheet metal option which will also fold out your box and allow you to produce a 2D drawing complete with bending allowances etc.

[David JuppParticipant @davidjupp51506]

There is no ‘Thin Extrude’ in Atom3D.

[Nigel Graham 2Participant @nigelgraham2]

This works:

Create the external outline.

Offset each side by 0.06″ remembering the two fillet radii differ by 0.06″.

Extrude.

If I want to add a floor, assemble to it an outline extruded to floor thickness as “height”, though I haven’t tried it.

[blowlampParticipant @blowlamp]

It would be easier to do as Jason suggested and extrude a solid from your external outline and then shell that to leave a uniform wall and floor thickness.

 

Martin.

[Nigel Graham 2Participant @nigelgraham2]

Json uses a higher-grade version of Alibre than Atom, which I have, so I am not sure if is by a different technique.

Atom would certainly let me generate the internal form and extrude-cut that to depth into a solid block; but would that be easier or more efficient than extruding two concentric polylines then adding the floor, as an Assembly with two Parts? I found the two seed polylines easy to form, involving the Offset and Trim tools, but there might be a more efficient method.

More so if needing internal features such as internal angles to hold the walls, or fittings as in a water-tank.

…

I based the box on a simplified form of my steam-wagon bunkers, whose walls are fitted to the floor by internal angles including the quadrant (physically, cut from a turned, flanged ring). Seven parts, ignoring the walls being of two pieces, and some small details. If I were to draw that fully in Alibre the easiest route would be assembling the angles to the floor, then the shell as above to that. As putting the real ones together. For practical purposes in furthering the project, since I have already made the bunkers, I would simplify their CAD model to the basic box.

[JasonBModerator @jasonb]

Looks like Atom has shell. Generally it is quicker and less error-prone to sketch the shape once as a single line, extrude and then shell rather than effectively drawing the shape twice to represent it’s thickness and adding a bottom. So shell is the faster and more accurate way.

Either way would really require the separate elements to be added, be that as “onepart” or as separate pieces of metal that can then be brought together and saved as an assembly. This would be the better option if you wanted to send out and have the parts laser cut or even to produce your own working 2D drawings to cut them from.

 

 

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