Why can it Boolean when other parts geometry is surpressed?

karl_mochel

When Connector Ring Ex is not suppressed it doesn't Boolean Connecotr2Rib and Slot so I end up with Part 3.


But when Connector Ring Ex is suppressed I get the desired result - Connector2Rib and Slot become one Part - Rib. 

tim_hess427

When you are creating your extrude features, there are options for "new", "add", "remove", and "intersect". Make sure you're using the correct one as appropriate. 

Then, if you're using "add" or "remove" - the feature will perform a Boolean union or subtract between the new body with any parts included in the "merge scope" box.

Its likely playing with those options your extrude features will solve the issue. 

karl_mochel

Initial Object - Connector2Rib is New


Slot - Add - correct Merge result is Rib


When Connector Ring Ex is Unsuppressed, the smaller part separates and becomes Part 3. When used as a Boolean the result is not the expected...Rib and Part 3 subtracted as a whole.

tim_hess427

What does your "Slot" feature look like when Connector Ring Ex in unsuppressed? 

Every time you make a change, onshape rebuilds every feature in the list below the change. So, when you unsuppress Connector Ring EX, onshape will rebuild everything that comes after it, including your Connector2Rib and Slot features. These features may be acting differently with that part unsuppressed. 

karl_mochel

Looks like this...

tim_hess427

Here's what I think is happening:

• With Connector Ring Ex suppressed, your Connector Top sketch has one closed region. 
• When you unsuppress Connector Ring Ex, the Connector Top sketch must be importing an edge from the Connector Ring Ex, creating two closed regions. But, when you extrude the Connector Top sketch, only one of those two regions is being extruded. Then, when you extrude the Slot, the two parts don't touch and don't merge. 

So - either fix Connector Top sketch so that it doesn't use an imported edge from Connector Ring Ex, or change your Connector2Rib feature to extrude both regions instead of one. 


As a side note: Why are you suppressing/unsuppressing Connector Ring Ex? If you are just trying to hide a part, you can hover over its name in the parts list and click the little "eye" icon. Then, you won't run into downstream issues like this. 

karl_mochel

Not sure what you mean by "importing an edge." However, I assume it means picking up an edge from another part so I tried rebuilding the sketches, making sure to create all new sketch geometry. I broke it into construction lines and edges to extrude. Was still broken so I tried changing the Sketch planes for Connector Top to Top Plane. When I did that the object extruded properly. As soon as I change the Sketch plane to Screw Connector Plate Ex (to use as the Baseline for the Connector2Rib and Slot extrudes) it is broken. I assumed that using a face as a Sketch plane doesn't affect the geometry being sketched unless geometry is snapped to it. So Sketch planes just provide 3D positioning, and do not infer anything else from the underlying geometry, correct?

- For my editor spaces, the eye icons are only available for Sketches, not 3D parts...  

Here is a link to the part if you want to play around with it.
https://cad.onshape.com/documents/2125aa07611f83e02e96aaf8/w/b311f32f43dfe8e7bbbb0493/e/a1ca32acd72561f15e7de695

tim_hess427

Yes - when you use the face of a part as a sketch plane, onshape automatically does some stuff with the geometry on the face. This can simplify some things, but if you're not aware of it, it can be really confusing. So, you can switch the sketch to a stand-alone plane, like you did. Or, you can edit your "extrude" feature and make sure you all of the regions you want to extrude are highlighted. If you just click on the sketch on the list, onshape starts making assumptions about what regions should be extruded from the sketch. You can actually click on individual sections of the sketch to select or de-select them. 

Another workaround for this is to use an implicit mate connector to define your sketch plane (click the little mate connector icon next to the plane selection box). This will allow you to reference the face of a part without onshape making assumptions about using edges on that face. 

To hide parts - make sure you're hovering over the part name in the parts list below the feature tree. A little "eye" icon should show up. If not, that's likely a bug. You can also right-click on parts and select "hide" from pop-up menu. 

karl_mochel

OK! - So both of your ideas of stand-alone sketch panes (In addition to Top, Left, Front) and mate connectors worked! Yea!

Originally I was selecting individual elements of the 3D objects to be the sketch plane. Now that looks problematic because I don't want any inferred assumptions, only explicit constraints. 

On the Hide comments. Somehow I do not get the same experience you do.

A sketch has the Eye icon...


3D shapes do not...


...and there is no Hide in the menu.

tim_hess427

In your screenshots you are hovering over the "extrude" features. Look further down where you see "Parts (2)". That is the parts list, and you'll see the "eye" icon for individual parts there. 

karl_mochel

Ah! Bach!

The prototype print...