Debugging featurescript failures and exceptions

stixpjr

I've using onshape for a while, designing various models for 3d printing, mostly to learn, for fun & curiosity. I've toyed with featurescript a little, but I'm finding some failures hard to debug. Currently, I have a "jigsaw" script which generates a cut-like childrens jigsaw (yes, this works remarkably well 3d printed). However, if I alter the size, gap, try "randomly" reversing the joiners, I get a variety of exceptions, the main two being:

@opExtrude: EXTRUDE_INVALID_ENTITIES

or:

throw THICKEN_FAILED

This obviously isn't really a purpose that onshape was designed to cope with, but it performs remarkably well, considering my creative abuse. Any suggestions to debug this further?

The shared example is:
https://cad.onshape.com/documents/38a2ab62dc640db1a306c3ab/w/282299abd1dcd0658656c041/e/51a3f73f17e2bc5043a4eafa

Jake_Rosenfeld

@stixpjr I would suspect that both of these issues arise from passing in bad input entities into opExtrude or opThicken.  Extrude requires faces or edges as input, and thicken takes faces or sheet bodies.  A good first step would be to add a:

debug(context, extrudeEntities); // extrudeEntities is the Query you intend to pass into extrude

before the extrude, and see what it highlighted/printed to the console.

If you do that for one of the failing cases, and it looks like you are trying to extrude the correct entity, please feel free to post here again, and we can look into it more closely.

stixpjr

Ok, that highlighted a bug (sketch edges overlapping, causing the failed extrude).
After fixing that, now I just get the "throw THICKEN_FAILED". Debug output is:
debug: Query resolves to 4 bodies (4 sheet)which looks sane?

Jake_Rosenfeld

@stixpjr

Couple things to try:

First I would try doing each body individually, to see if one specific body is the problem:

int i = -1;
for (var sheetBody in evaluateQuery(context, sheetBodies))
{
    i += 1;
    try
    {
        const thickenId = id + i + thicken;
        opThicken(context, thickenId, {
            ... thicken definition with `sheetBody` as the entity to thicken
        });
        debug(context, qCreatedBy(thickenId, EntityType.BODY)); // this will show all the successful thickens in red
        println("Thicken " ~ i ~ " was successful");
    }
    catch
    {
        debug(context, sheetBody); // this will show all the unsuccessful thicken inputs in red.
        println("Thicken " ~ i ~ "failed");
    }
}

You probably only want to have one of those debugs on at a time so you can piece out which thicken is failing.

Something else worth trying is:

const facesToThicken = qOwnedByBody(sheetBodies, EntityType.FACE);

and trying to thicken the faces rather than the bodies.  You can also run the faces through the same loop from above too see if there is one or a few specific problem faces.



If you can make a Version of your document where this failure is occurring, and then post the link to that Version, it would be easy to look into.
https://cad.onshape.com/help/Content/versionmanager.htm

stixpjr

Thanks for your suggestions - I've tried looping over the query entities, adding the exception handling, and trying to thicken just the faces, but I still get exceptions thrown, depending on the parameters chosen - "random joiner direction" seems to trigger most reliably. I also split the "thicken" into opThicken and opBoolean, for extra visibility.

Nothing strange in the debug output:

<div>debug: *** thicken failed, entity:
<span style="background-color: transparent; color: inherit; font-size: inherit; font-family: Flama, sans-serif;">debug: Query resolves to 1 face</span></div>

And the rendered face looks OK on screen.

The following is tied to a failing version:
https://cad.onshape.com/documents/38a2ab62dc640db1a306c3ab/v/b03bcf08a4a6ba3b56348d03/e/d884d38b90d792779b1742c1

Jake_Rosenfeld

@stixpjr

I wouldn't expect to be able to thicken a shape like this very much because it will quickly become self intersecting at the sharp corners:


I am brainstorming some solutions for how you may be able to achieve what you want, but the simplest solution would to just be to soften the turn where the bump meets the rest of the piece.  Are you working with a strict set of parameters, or could this shape be drawn a little differently?  To test out whether this is the case, I suspect that if you turn down the gap to be low enough (without changing the geometry), there is probably some threshold where the thicken will start to succeed.

stixpjr

Indeed, tweaking the shape to soften the curve a little makes it succeed. I'm a little surprised by the behaviour, however - it successfully thickened several other rotations of the same curve - 21 other instances, apparently. There shouldn't be any difference between those 3 and the others except rotation and translation (ok, mirroring, too).

Interestingly, when I try to etch a spiral in the top surface, 0.5mm of the 2mm thickness, again, a thicken operation fails. This is not featurescript, just regular onshape objects and operations:
https://cad.onshape.com/documents/38a2ab62dc640db1a306c3ab/v/2a21d21c586757f8ea1abbd2/e/d884d38b90d792779b1742c1

Jake_Rosenfeld

@stixpjr



It is the boolean postprocessing that is failing, not the thicken itself.  If you switch to NEW it should probably work.

As to why the boolean is failing, it looks like we are doing some highlighting to point out the problem area:


It might be that the cut creates some non-manifold geometry in there, or possibly just that there is a bug in our geometry kernel.  Is this etching intended as part of the final design, or just playing around to see when thicken fails or succeeds?

Jake_Rosenfeld

One thing I've noticed is that there are lots of these little slivers of geometry on the parts along the outer border:


These slivers may be causing some instability.

stixpjr

Yes, I'm just playing around

However, it seems useful to shake out the flaky behaviour - if I'm finding flakes, I'm sure more serious users may also be finding these.

Given the geometry here, I can't see how there's non-manifold geometry created - but floating point math is hard!

I previously noticed the slivers on the end of the thickened splines; given what the thicken op does, these make sense - I can also see why this might be causing some instability. Relatedly: I only just discovered sketch slots - these seem to be a useful way to avoid thicken entirely, and have sane behavior on the spline ends. However, I haven't found a FeatureScript API to this function?

Jake_Rosenfeld

There is no FeatureScript skSlot, correct.  But it would not be too hard to write one :

function skSlot(sketch is Sketch, id is string, pt1 is Vector, pt2 is Vector, diameter is ValueWithUnits)
precondition
{
    is2dPoint(pt1);
    is2dPoint(pt2);
    isLength(diameter);
}
{
    const pt1ToPt2 = normalize(pt2 - pt1);
    const push1 = vector(-pt1ToPt2[1], pt1ToPt2[0]);
    const push2 = vector(pt1ToPt2[1], -pt1ToPt2[0]);

    const radius = diameter / 2;

    const pt1Pushed = [
            pt1 + push1 * radius,
            pt1 + push2 * radius
        ];
    const pt2Pushed = [
            pt2 + push1 * radius,
            pt2 + push2 * radius
        ];

    // Semicircle around pt1
    skArc(sketch, id ~ ".pt1Arc", {
                "start" : pt1Pushed[0],
                "mid" : pt1 - pt1ToPt2 * radius,
                "end" : pt1Pushed[1]
            });
    // Semicircle around pt2
    skArc(sketch, id ~ ".pt2Arc", {
                "start" : pt2Pushed[0],
                "mid" : pt2 + pt1ToPt2 * radius,
                "end" : pt2Pushed[1]
            });
    // Lines connecting semicircles
    skLineSegment(sketch, id ~ ".line1", {
                "start" : pt1Pushed[0],
                "end" : pt2Pushed[0]
            });
    skLineSegment(sketch, id ~ ".line2", {
                "start" : pt1Pushed[1],
                "end" : pt2Pushed[1]
            });
}

https://cad.onshape.com/documents/99ba468fc24964026815d021/w/e019d82fdc06bc8f3de46f34/e/4c9e925ef8330ec2b9c4b335

stixpjr

Nice!

However, the built-in slot sketch tool also copes with splines as input - which require more than just a linear offset. I had originally thought that it would require offsetting each spline control point by the radius normal to the spline (at that point) - but that is too simplistic, and the transformation is deeper than that.

stixpjr

Ha, I think I've found what I need. Too late now to concentrate, but there's some nice FeatureScript code snippets under "Offset Curves, Using Onshape Constraints": https://www.onshape.com/cad-blog/everything-you-ever-wanted-to-know-about-onshape-splines-part-2-of-2

stixpjr

Ok, based on that doc and also looking at the generated code from a sketch slot based on a spline, I've tried adding various constraints to generate my own slot programmatically, but almost any combination just generates errors of the form:
Onshape encountered a problem with your last operation. If the problem persists, please contact support. Support code 93aa18d7efc1f4b37e50921f.I'm guessing the solver is unable to successfully solve based on the constraints. skConstraint is barely documented, given that it's mostly unnecessary, which makes it hard to debug. I also notice that the generated code includes a large blob of consts passed to skSetInitialGuess (undocumented) which likely helps the solver on its way.