Disable weird / annoying selections of hidden parts / faces

RyanAvery

I right click a face (to serve as a plane) and click new sketch. I draw a rectangle using no lines or features from that face. 

Then I draw another rectangle inside that rectangle. Now there are two areas that I can select. 

When I click in the outer rectangle to select it, instead of selecting it, it selects the boolean intersection of my sketch with some other hidden lines that I did not "Use" in this sketch. 

All these weird / random / useless areas are selectable even though I didnt click the line and hit "Use" and even though the part that they come from isn't even visible. This seems like a pretty big bug, and I'm not sure how to disable it. Is there any way to disable this or get around it? Or some sort of FS to disable it? 

RyanAvery

In the last picture, I "roll to" right after sketch 14. 
Then I hide all parts and sketches. 
Then I make sketch 14 visible. 
Then I use extrude tool and hover a portion of sketch 14. 
Instead of highlighting that portion of sketch 14, it highlights that portion of sketch 14 intersection booleaned with some other shape that is not visible and not even included in the sketch. 
This "auto intersection boolean your selection with invisible shapes" is what I would like to disable. 

MBartlett21

@RyanAvery
It selects regions if you sketch on a face rather than a plane
Select the sketch in the feature tree to select the sketch region you're wanting

RyanAvery

Is there a way to right click a face and do "new sketch from plane on this face" ? 

MBartlett21

No

MBartlett21

@RyanAvery

If you edit a sketch you can click the Extrude feature in the toolbar. This might make it a bit easier 

RyanAvery

I'm not sure what you mean. I use shift+e to extrude once I select areas...

MBartlett21

@RyanAvery
Don't select areas before you extrude from inside the sketch.

RyanAvery

So extrude first, then select the areas? That makes a difference? 

MBartlett21

When you are editing the sketch, use Extrude then. Don't select any areas before you Extrude. It should automatically select the area 

RyanAvery

mbartlett21 said:

When you are editing the sketch, use Extrude then. Don't select any areas before you Extrude. It should automatically select the area 

this makes no difference, i'm not sure what your on about.

owen_sparks

You can either close the sketch and then select extrude, or select extrude whilst you still have the sketch open.

In a similar way you can select sketch regions to extrude by clicking on the model viewing area of the screen, or select the whole sketch by clicking it in the feature tree.  Personally I'm not keen on selecting the whole sketch as it's more prone to introducing errors if you add to the sketch later, but that's just personal preference.

Owen S.

3dcad

I'm on same boat with @owen_sparks I rarely select whole sketch to extrude since one sketch can serve many extrudes and keep editing easier and feature list shorter.

@RyanAvery
Everything you create into single part studio should be somehow related to each other, so it's likely that you really wan't to be able to use existing geometry to create new. If you have stuff that are not related, then create another ps and put them there. This way you get the best performance and assembly is the place where parts become a product.
I thought of this because I don't recognize the problem you described.

owen_sparks

I'm beginning to change my tune on this issue.

I noticed @lana using this property as intended in one of her help posts.

Consider this example.



The workflow:-
Sketch rectangle on plane
Extrude rectangle to make blue part
New sketch on face of extrude
Extrude 2 to make grey part.

Note there is only a single line on sketch 2.  The sketch region is being inferred automatically and is actually pretty clever.  I'm pretty sure I've wasted loads of time projecting the perimeters of geometry onto sketches when OS would have happily worked it out for itself. 

What is annoying is these inferences being made to parts/sketches that are hidden.  It'd be great to be able to filter those out when they're not helpful.

"LEVERAGE the POWER of Inferred Sketch Regions, anywhere, and on any device.
[OS_InfomercialMode/Off] 

Cheers,

Owen S.

3dcad

So it should be some sort of hotkey, when pressed ignore hidden geometry on selection - or vice versa. That would be familiar from other cad(ish) software..

konstantin_shiriazdanov

3dcad said:

So it should be some sort of hotkey, when pressed ignore hidden geometry on selection - or vice versa. That would be familiar from other cad(ish) software..

I remember at least one thread about this silent face projection into the sketch, and I still think checkbox in sketch dialog to project face contour requared.

3dcad

+1 for checkbox instead of hotkey, but so that it can be freely toggled on/off without breaking any constraints.

owen_sparks

The Onshape folks are going to be shouting at their monitors in the morning.  There are only three of us online talking about this and already we have three different ways we'd like to implement it 

RyanAvery

3dcad said:

I'm on same boat with @owen_sparks I rarely select whole sketch to extrude since one sketch can serve many extrudes and keep editing easier and feature list shorter.

@RyanAvery
Everything you create into single part studio should be somehow related to each other, so it's likely that you really wan't to be able to use existing geometry to create new. If you have stuff that are not related, then create another ps and put them there. This way you get the best performance and assembly is the place where parts become a product.
I thought of this because I don't recognize the problem you described.

I put everything in one part studio. 
I start buy putting ~20 variables at the top, then I make the entire design (last one was 300 parts) in the same studio. 
Then I change the variables to get things looking the way I want. 
This is because I don't know, for instance, when I start designing a cabinet how much I want the upper lip to hang over the cabinet. 
So I design the entire thing with variables that I can change so that when I'm done I can just tweak the variables and have the entire thing regenerate. 

owen_sparks

@RyanAvery, that sounds good.  Do you like cold weather?  If so  @3dcad, are you in need of another designer?

3dcad

  

3dcad

@RyanAvery
Have you already put your vote on global parameters?

RyanAvery

No but I don't think I would use that anyway. I never really make separate parts. 

3dcad

@RyanAvery
I'm in furniture design also and I used to make single solids (ie. not create separate parts) with Solid Edge and Alibre, since it was too slow to first create separate parts and then add one by one to create assembly using three mates for each part  
 
With Onshape, I strongly suggest learning to use full potential of parts, assemblies, BOM (cut list), render etc.. It will serve you in many ways, you can do collision detection if you create hinges, slides etc. with real limits. Of course it's also nice to see a photo of new product before ordering any material  

And when you have modeled each part separate (they can still be in same part studio), you have real manufacturing data and it is possible to add part numbers and other data properly - this is needed when expanding same parts to other collections and aiming for productive manufacturing.

lana

@owen_sparks
Thank you for paying attention . Making noise about inconveniences of this functionality is a good thing - we'll have to improve its usability.

RyanAvery

owen_sparks said:

I'm beginning to change my tune on this issue.

I noticed @lana using this property as intended in one of her help posts.

Consider this example.



The workflow:-
Sketch rectangle on plane
Extrude rectangle to make blue part
New sketch on face of extrude
Extrude 2 to make grey part.

Note there is only a single line on sketch 2.  The sketch region is being inferred automatically and is actually pretty clever.  I'm pretty sure I've wasted loads of time projecting the perimeters of geometry onto sketches when OS would have happily worked it out for itself. 

What is annoying is these inferences being made to parts/sketches that are hidden.  It'd be great to be able to filter those out when they're not helpful.

"LEVERAGE the POWER of Inferred Sketch Regions, anywhere, and on any device.
[OS_InfomercialMode/Off] 

Cheers,

Owen S.

When you change the distance of the vertical line from the edge of extrude one via a variable and the project regenerates, how will the project pick the correct region to extrude for extrude 2 if you are, at the time of regeneration, showing all parts vs hiding all parts? Or would the info about what was / was not shown at the time that the extrude was made be used in the regeneration? 

Jake_Rosenfeld

@RyanAvery

Part regeneration is independent of part visibility status.  When you make a dimension between that vertical line and some other piece of geometry, the dimension will reference the selected geometry whether it is visible or not.  In the same way, sketch inferencing has nothing to do with the visibility of the part you are sketching on.  If you click a planar part face to sketch on, its geometry will be inference into the sketch no matter whether that part is visible or not.

As a workaround for your initial trouble, to sketch on a face's plane without pulling in the face as an inference, you can first create an offset plane off the face (with 0 offset), then sketch on the plane rather than the face.
https://cad.onshape.com/help/Content/cplane.htm

RyanAvery

Yes but the visibility is what he was talking about 

Jake_Rosenfeld

Sorry, I misread your answer and didn't realize you were commenting on his suggestion.

Thanks for clarifying!

viktor_solenoid

I would LOVE to have an option for turning this "feature" off. An offset plane won't work in the most situations. I just opened a ticket thinking it's a bug and they've showed me a workaround for my particular case, but I had this issue so many times that I really want to see it fixed.

Jake_Rosenfeld

@viktor_solenoid

A 0-distance offset plane as the selection for the sketch plane should always disable sketch inferencing (as a workaround for now).  What situations are you imagining where it wouldn't work?