Redundant post

Nigel – I did some tests, the error message you report comes from the 3D feature that you tried to produce from a 2D sketch that has issues.  It is a generic message that can be caused by many different issues with the sketch.

You appear to have either turned off sketch analysis or are ignoring it.  Sketch analysis will give more specific information regarding what is wrong with the sketch.

If I had to guess, I’d suggest that the ends of the arc don’t quite meet the ends of the straight lines, or you may have used a rectangle in the sketch and failed to trim away the line segment that traverses the arc.

Using closed sketch profiles is critical to success in most 3D CAD systems.  If sketch figures cross, overlap, or leave gaps, there will be failures.

On 22 September 2025 at 09:24 Nigel Graham 2 Said:

 

I appreciate your offer of help but I need know how to create sketches that are not full of mysterious, invisible errors in the first place.

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But by sending the file to support they can likely see what the error wa sand then show you how to cure or avoid it in future

Maybe go back to the original Atom tutorials a sthey show how to make parts like the link which are basically a bar, with a hole and then the corners rounded off. They don’t show it being done with semicircles.

Most likely your rectangle was not tangent to the circle and that is why it would not trim properly, you would also have drawn one line over the top of another with your method but that should have been easily visible.

Gentlemen, your frustrations are really beginning to show, now!  I follow this continuing saga with a combined sense of frustration and metaphorical head banging against the wall. However, to be fair to Nigel, I have experienced mysterious sketch failures highlighted by the analyse tool which when the fault is clicked, displays no red highlights on the sketch.  I then have to painstakingly step back through the sketch to see where I went wrong, reinstating any deleted steps which turn out to be right utilising the “back” and “undo” arrow buttons on the ribbon.  It’s often a slow process with a large or complicated original sketch, but I always get there in the end.  I have to say that the majority of my errors seem to be overlaps, due possibly to my (over) use of the copy and paste facility.

John

Two rounded ends the bottom one done as you describe, the upper without extending the diametric line beyond the circle. Both “look” OK once the unwanted lines have been trimmed until you close the sketch then Analyse finds the faults all of which get highlighted as you click the error on the screen.

As the error is actually two lines ontop of each other but only 0.0005mm long you really need to zoom in a lot to see them. I’ve added a line 0.01mm ( 4/10ths of a thou) long so you can see how far I have zoomed in, that is 10,000 times magnified so without using the analyse to highlight the errors you have little chance of finding some errors

I should say that in the above example clicking “overlap” at the bottom of the list does not highlight it or change the colour of the line. But all the other errors are at one of the ends of the overlapping line so a good pointer as to where the error is.

And if proof were needed it now shows the overlap if I fully define the sketch.

David, as you still need to zoom in a lot to see just the colour change can I suggest overlaps are also highlighted in some way rather than just changing the colour, much like the other errors get highlighted.

Thank you, David (and Jason) for the explanations.  I assumed that it was me misunderstanding the analyse tool that was causing my problems.  I always go to the bottom of the error list first to sort the overlap errors.  This more often than not clears the fault, but not always.  Next time I get no highlights, I’ll send in a report, fully expecting it to be operator error.

John

David,

Very happy to take your advice. I will modify my approach accordingly.

John

Nigel. The way you have gone about it is very long winded for just a simple rounded end. As I said go back and look at the Atom excersizes.

Have a try of this. Move the divider bar up the tree on the left until it is above what you show so that your rod end goes back to having a square end.

Select “fillet” from the row of options along the top, enter a radius in this case 3/16  and then select the corners you want to round by clicking them, they will show as a blue line when the mouse in in the right place and a vellow fillit as you click. Click OK when you have them all selected.

Flat spot is either a slight difference in sizes or something not quite concentric, maybe the square end of the rod is 0.187 from ctr not 0.1875″ in cases like this entering a fraction can help so give the length as 3/16

Reading between the lines (pun intended!) and without being able to peer over Nigel’s shoulder, I can’t help thinking that one of the problems here is using 2D traditional draughting techniques, aimed at producing engineering drawings, to produce sketches (not drawings) as the first step in building 3D models. I have done a little bit of tutoring of 3D CAD to a number of my fellow ME society members, and a couple of my usual introductory remarks are to forget anything you know about traditional 2D draughting, and never use a dimension when you can use a constraint. As with all generalisations, there are exceptions to these “rules” but I find they help.

Looking at the various sketches that have been reproduced in this thread, I see no sign of using constraints but remarks like “I draw a line to cross existing lines and then trim back the excess.” Although I’m not an Alibre user I see from the help files online that there is a rich set of constraints available, so that can’t be the reason. My own approach to something like this, where I want to draw a line (or could be an arc or similar) that joins the end of a couple of lines is to draw the shape in roughly the right position, then apply constraints (typically coincident) to “drag” the new line into the right place, and fix its relationships with existing sketch elements. One problem (already noted by Nigel elsewhere, I think) is that if you try to draw the new line in the right position from the outset, it is quite possible that the software tries to be a little too clever and automatically adds the wrong constraint. Even worse, it thinks that you are trying to connect to a different point somewhere in the model and that can really put a spanner in the works.

In the current case, one approach might be to draw an arc “somewhere close” to where it is wanted, then make the ends of the arc coincident with the corresponding ends of the sides of the arm being drawn, and the centre of the arc coincident with the centre of the hole. No dimensioning needed. In addition, if you need to change the width of the arm, the arc will automatically modify itself to maintain those constraints. There are other ways to do the job, of course – there always seem to be several ways to achieve anything with 3D CAD! – but the principles remain.

I appreciate that many reading this thread will be way beyond “beginner” status but I shall be on the SMEE stand at the Midlands show next month specifically to demonstrate 3D CAD and maybe encourage a few model engineers to consider using it. By coincidence, my demonstration model looks very similar to Nigel’s arm with hole at the end and concentric semi-circular end! Be happy to discuss techniques with anyone passing.