Extrude BoundingType Problems

S1mon

I'm working on an injection molded boss custom feature. I'm trying to get the bosses to extrude to the part with or without draft reliably. In doing so, I'm discovering weird things about UP_TO_NEXT or UP_TO_PART which are causing issues.

Here's a manual feature based version of this issue - if I use up to next or up to part, I get this weird face at the base of the boss where it's joining a complex wall. It doesn't matter if I add the draft in the feature or after, with this edge case, it always adds this surface where I don't want it. Is this a Parasolid bug?

If I use Through all, it does the right thing:

Obviously I don't want the extra bit on the outside of the part, and I can use delete face with heal to solve this, but I will need to be clever with queries to grab all the right faces, and then hope that heal doesn't do anything stupid.

I feel like I saw something similar in how some (all)? of the rib features are implemented. Is this a normal way to work? Is it more robust than up to next or up to part?

ry_gb

That's definitely behavior I would've never expected…

What happens when you try the Mounting Boss featurescript? Looking at the code, specifically at the extrudeBase function, they're just using Up to Body as the end condition.

S1mon

@ry_gb

Very interesting. On further experimentation in regular Onshape, New vs Add both with Up to part, gives different results (besides the obvious boolean). With New, and Up to part, draft is treated differently. It seems like the most robust sequence is to extrude with add, then add draft after. I would have thought that adding draft while extruding would be better for topology challenges. It seems like the mounting boss feature is doing exactly that - so I'm really baffled.

However when I try that in Onshape CAD with test cases where the undrafted cylinder doesn't overlap a tangent connected face, it does stuff like this (leaves a defect at the base of the boss on the left in this image):

Is there something I'm missing?

Here's the setup in @NeilCooke 's Mounting boss feature for the main boss (which behaves well):

var extrudeDefinition = {

    "entities" : qSketchRegion(id + ("sketch" ~ sketchId)),

    "endBound" : BoundingType.UP_TO_BODY,

    "endBoundEntityBody" : definition.booleanScope,

    "hasDraft" : definition.hasDraft,

    "draftAngle" : definition.draftAngle,

    "draftPullDirection" : false,

    "operationType" : NewBodyOperationType.ADD,

    "defaultScope" : false,

    "booleanScope" : definition.booleanScope

    };

robert_morris

I wrote the Mounting Boss featurescript that @ry_gb mentioned.

I believe I based it on a script that Neil wrote, but added some additional options so it would be more like the version in SolidWorks.

I wrote that quite a while ago, but I do remember having issues with the up-to-next end condition, which is why I used up-to-body in the script. That seemed to be a bit more reliable.

When adding a draft to parts, I have seen it either fail or do some weird things when the drafted surface crosses over onto a new face, like what you are showing. Have you tried extruding up to part as New, with a slight offset into the part, then adding the draft, before using a boolean to join them?

S1mon

@robert_morris
Sorry to misattribute that FS.

After I followed your code (or more accurately, after I told Codex to review your code and try doing it that way) I'm getting better results. The thing that really confuses me is it seems like the behavior of up_to_next when calling extrude.fs is very different in these edge cases than the user feature Extrude.