difficulties with circular pattern of an opSphere

björn_britz

I have difficulties doing a circular pattern of operations, especially with the opSphere operation.

Don't know what's wrong and Onshape says regeneration complete. Any suggestions?

document link:

https://cad.onshape.com/documents/8e26d19f48d94a039d8e8399/w/d0ca70e6dd864413dcb64308/e/b830d5993f0ebf5a2041c6e8

Thanks!

Jake_Rosenfeld

@"björn_britz"

A couple issues here.  It is useful for debugging FeatureScript to use the 'monitor' functionality in the FS console.  Open the console by pressing the '{✓}' at the top of the screen, and then press the "monitor" button next to the part studio you want to monitor.

By doing this I first found that there was an issue with your sketch plane definition:


I think this ends up being o.k. on the backend, but you should really be defining those as:

plane(vector(0 * inch, 0 * inch, definition.Width / 4), vector(0, 0, 1));

Otherwise the x and y values of the vector are unitless and the z value has a distance unit, which is not optimal for the system.

The main problem here is the problem with the axis of the circular pattern:


It would be nice if the system could accept definition.axis as a `Line`, but unfortunately (because `circularPattern` is a feature, and `definition.axis` actually represents a selection box in circular pattern's feature dialog) you must pass a Query in for that parameter.

The easiest way to get around this would be to do something like:

opFitSpline(context, id + "axis", { "points" : [origin, origin + (vector(0, 0, 1) * inch)] });
const axis = qCreatedBy(id + "axis", EntityType.EDGE);

And then use that `axis` as `definition.axis`.

Hopefully this makes sense.  Let me know if you have additional questions.

Jake_Rosenfeld

@björn_britz

I took a look at your document, and it looks like you're trying to do these boolean operations on `opExtrude`?  `opExtrude` does not have a boolean option. The `extrude` function (and therefore the extrude feature of the part studio) has those boolean options by way of first calling `opExtrude` to make the necessary extrusions, and then `opBoolean` to to boolean everything together.  You could switch to using `extrude` if you want, but my suggestion would just be to collect all the bodies you want to joint together and call `opBoolean` on them.

Take note that if the bearings and the retaining ring only touch at one point, the boolean will fail because of that singularity (this would be a non-manifold body, which we do not support).  You may have to overbuild the spheres if this is the case.

MBartlett21

Try looking up the documentation of getRemainderPatternTransform https://cad.onshape.com/FsDoc/library.html#getRemainderPatternTransform-Context-map

Jake_Rosenfeld

@"björn_britz"

A couple issues here.  It is useful for debugging FeatureScript to use the 'monitor' functionality in the FS console.  Open the console by pressing the '{✓}' at the top of the screen, and then press the "monitor" button next to the part studio you want to monitor.

By doing this I first found that there was an issue with your sketch plane definition:


I think this ends up being o.k. on the backend, but you should really be defining those as:

plane(vector(0 * inch, 0 * inch, definition.Width / 4), vector(0, 0, 1));

Otherwise the x and y values of the vector are unitless and the z value has a distance unit, which is not optimal for the system.

The main problem here is the problem with the axis of the circular pattern:


It would be nice if the system could accept definition.axis as a `Line`, but unfortunately (because `circularPattern` is a feature, and `definition.axis` actually represents a selection box in circular pattern's feature dialog) you must pass a Query in for that parameter.

The easiest way to get around this would be to do something like:

opFitSpline(context, id + "axis", { "points" : [origin, origin + (vector(0, 0, 1) * inch)] });
const axis = qCreatedBy(id + "axis", EntityType.EDGE);

And then use that `axis` as `definition.axis`.

Hopefully this makes sense.  Let me know if you have additional questions.

björn_britz

@Jake_Rosenfeld

Thank you! it works just fine now.

But I also had to set the parameter "equalSpace" : true for the pattern.

Jake_Rosenfeld

@"björn_britz"

Oops! sorry about that!  Yes, 4 instances at 360 degrees with equal spacing ON is the same as 4 instances at 90 degrees with equal spacing OFF (if that makes sense).  Basically equal spacing chooses whether the instances are all spaced between 0 and `angle` (ON) or each spaced at `angle` further than the last (OFF).

björn_britz

@Jake_Rosenfeld

Now I'm trying to merge parts 1,2,3 and 4. I tried with "defaultScope": false and "booleanScope": Query but I couldn't manage to make it work. Any suggestions?

Jake_Rosenfeld

@björn_britz

I took a look at your document, and it looks like you're trying to do these boolean operations on `opExtrude`?  `opExtrude` does not have a boolean option. The `extrude` function (and therefore the extrude feature of the part studio) has those boolean options by way of first calling `opExtrude` to make the necessary extrusions, and then `opBoolean` to to boolean everything together.  You could switch to using `extrude` if you want, but my suggestion would just be to collect all the bodies you want to joint together and call `opBoolean` on them.

Take note that if the bearings and the retaining ring only touch at one point, the boolean will fail because of that singularity (this would be a non-manifold body, which we do not support).  You may have to overbuild the spheres if this is the case.

björn_britz

@Jake_Rosenfeld

oh right, my bad.

It works now!

Jake_Rosenfeld

Great to hear!