Why do some connected extrusions become separate parts?

kevin_white

I am using OnShape with my students for a new project. I tested out a way to design this with multiple parts, but I am not sure how or why my version separated all the extrusions into separate parts, all derived from one sketch, yet every time we try to do the exact same thing, they all combine into one part (which is what normally happens)?
I have 2 examples here, the first link is to a part where the extrusions all came out as their own parts, the second one, they all combine as Part 1? In many cases, I see this happen with certain student projects, where they end up with a lot of parts, we are a bit mystified. How why does OnShape decide to make some parts separate and combine others?

I ask, because I use OneRender a lot, and we benefit from having many parts, it gives us more options for the render selection points, textures and aesthetic.

From what I can see, these are both using the exact same method:
Version with Multiple Parts
https://cad.onshape.com/documents/7460dce49b2b71ed1800c182/w/9e2953471336d589b15ef6eb/e/8990d2a4958d3a5f0443ac2c

Version with Part 1 Only
https://cad.onshape.com/documents/7dbf0472258323fb7828b9b2/w/f8449d7f48e4bfacb00a5be2/e/ebde8bce62bbd0fa095ed262

terry_pipkin

Not sure but are all of the Extrudes set to Add or New in both models?

terry_pipkin

Not sure but are all of the Extrudes set to Add or New in both models?

mahir

Yep, what @terry_pipkin said. The first extrude will be New regardless. But if you want separate parts you'll have to edit each extrude and change it from Add to New. As implied by the names, New will generate new parts, while Add will add geometry to pre-existing parts with shared volume.

kevin_white

I appreciate the help gentlemen! I am not sure how or why the extrusions were making new parts, but this is a good know. Now I have a better understanding of how New and Add are different. I looked back in the sketch and extrusions to see what was different. It still seems like I had them all set to ADD in both versions, but in one version they came out as new parts. Does not really matter how it happened. I can use this knowledge of New and Add extrusions to make better designs in the future. Really appreciate the help!

michael3424

FWIW, I also recently had a problem with an "Add"-ed extrusion coming in as a new part.  It didn't really matter for my use so I just chalked it up to a glitch or error on my part.

https://cad.onshape.com/documents/5eaf454f32770df79e7238de/w/34bfa79b6e15332380e4dfb1/e/0ab707085466cbb806354bc1

The errant feature is Part 5, which I'd intended to be part of "RH Gear Chart".  Note that the last feature, a Boolean Union also fails to work but doesn't turn error out in red.

bruce_williams

@michael3424

Your Part 5 was created tangent to "RH Gear Chart" - so there is no intersection, only a single point touch.  An Add or Boolean Union results in two parts. (btw basically the same thing, Add is on creation, Boolean Union is after the fact).  You need to have at least faces touching to Add or Boolean Union.  As to not throwing an error on your Boolean, Onshape is somewhat unique in it allows Union to create multiple parts.

mahir

bruce_williams said:

@michael3424

You need to have at least faces touching to Add or Boolean Union.  As to not throwing an error on your Boolean, Onshape is somewhat unique in it allows Union to create multiple parts.

I was just about to say that. In OS for two volumes to be part of the same part, they must have a surface or volume in common. 

michael3424

bruce_williams said:

@michael3424

Your Part 5 was created tangent to "RH Gear Chart" - so there is no intersection, only a single point touch.  An Add or Boolean Union results in two parts. (btw basically the same thing, Add is on creation, Boolean Union is after the fact).  You need to have at least faces touching to Add or Boolean Union.  As to not throwing an error on your Boolean, Onshape is somewhat unique in it allows Union to create multiple parts.

I figured the tangency might be an issue, but shouldn't Extrude 15 throw an error (and turn red) in that case?

Also, what's the point of a Boolean Union of two parts returning the same two parts?  Shouldn't that also thrown an error and a red label on the Boolean feature?

It just seems weird to find these two issues in one simple project when OS is usually so solid and logical to use.

mahir

@michael3424,

OS methodology differs a little from other CAD. Case in point, if you delete a parent feature in OS, child features are not automatically deleted (like in SW). OS leaves them there for you to fix. I personally appreciate this a lot. For that same reason, a union that doesn't break when not actually joining any parts may seem silly, but it also allows flexibility when parts can move relative to each other or the number of parts is variable. For example, let's say I have a union of 10 parts that results in 2 parts. Now let's say that depending on the configuration, the number of parts can vary from 2 to 10. That boolean union can function as is without any modification regardless of whether there are 2, 5, or 10 parts. Granted, when there are only 2 parts it's a redundant feature, but it's nice not having to worry about suppressing that feature but only when there are less than 3 parts. I know the example is vague, but I hope it makes sense.

michael3424

@mahir - I'd agree that the results in your use case would be preferred.  I was just a little surprised at the results I got; a warning message would have been better but I suppose that there is a limit to how many messages a user would want to see.  Now that I think of it, the fact that the two parts were different colors *was* the warning in a way and it certainly caught my attention.  One just needs to understand what it is telling you and that wasn't at all obvious to me at the time.  The Extrude 15 not throwing an error still seems like a bug to me, though.  I've seen similar features throw errors in other situations, so at best it seems to be inconsistent behavior.  

Jake_Rosenfeld

Add-type operations that do not intersect with any previous geometry should have a pretty loud warning about what's going on:



Once you commit the feature, however, it quiets down and let's the operation succeeds:



This is for exactly the reason @mahir proposes.  The user may make some upstream change that makes these bodies touch, and then the boolean will succeed.  Then if the user moves the parts apart again, we don't want to fail the entire extrusion just because the boolean is no longer making any change.

Jake_Rosenfeld

Non-intersecting boolean union has a similar popup.

michael3424

@Jake_Rosenfeld - Thanks - I'd completely missed the Boolean warning message in both instances but see it now when revisiting the doc.  Tunnel vision, I guess.  In my case the warning shows up right at the top of the screen, just above the menu bar.  Does that location change with users screen size and resolution?

Jake_Rosenfeld

Hi @michael3424

Sorry for the confusion.  My screenshot was taken from our upcoming build, so that warning should be moving down to below the toolbar in our next release.  It's size will depend on browser zoom level, but it's location shouldn't.

michael3424

@Jake_Rosenfeld - no problem.  I really do like how responsive you guys are to even the smallest parts of the UI.

lesley_lemmens

Hello, I experience the opposite problem. Multiple features are 1 part, I need them to be separate parts. Split does not work.
https://cad.onshape.com/documents/f565cf5ca0d7a3cb8615a141/w/5d1b5bf3e6c730280de8dafb/e/1191e5996241d6079f022097
Part 1 contains multiple items.
Any suggestions?

lesley_lemmens

Sorry already founfd the solution. One part was still an add, somehow this connected 3 items together