Can't Select Geometry Located Below a Sketch Unless Sketch is Hidden

[Bug.Robotics]

Title says it all.  Screencast below.    I'm hoping I just have a setting configured incorrectly.  If not, what is the advantage of such a workflow? 

I've used Fusion since 2014 and these sort of weird things in the sketch environment drive me nuts and make it difficult to use for normal workflows where work must be done quickly.  I use SolidWorks daily so a bit unfair to compare the two but this along with a number of other issues with the sketch environment cripple the software IMO.

[Bug.Robotics]

So I found "Selection Priority" and changed that to "Select Edge Priority" and now I can select the edges of the body without the sketch hidden but now cannot select the sketch.  This is a strange workflow.  Can someone explain?

I could see it being done this way to avoid infringing upon some patent but if not and there is some other workflow that benefits from this sort of thing I would genuinely be interested in finding out.

[chrisplyler]

Fusion tries to select the thing nearest you under the cursor.

You can change the Selection Filters to only include the items you want to select. Kind of a pain to always change the list.

Or you can hover your cursor over the thing you want to select, HOLD DOWN your left mouse button for a second, and a pop-up list of stuff that is under your cursor will appear, allowing you to select the specific item you want.

[Bug.Robotics]

Thanks for the reply Chris.  Holding down the mouse button is a lot better than changing the selection filters. 

Any idea as to why the workflow was implemented like this?  Seems strange to block entire regions of model with the area inside a sketch and make the user use the long mouse press. 

[chrisplyler]

I dunno. I've never used any other similar software, so I don't know how it's usually handled. If there are multiple things under your cursor, the software has to make SOME kind of assumption about what you want to select, right?

[Bug.Robotics]

Thanks for the reply.  I agree that you should have the ability to select multiple items if they are under your cursor (pretty standard in all CAD packages). So in the example I posted where the sketched circle crosses any body entities, the user would have to select whether they wanted the sketch or the body line/point/face.

The thing I was seeking to understand is that the area bounded by the sketch (in the screencast I posted it was a circle) prevents the user from selecting the geometry underneath.  This doesn't make any sense in any workflow I have ever seen.  The area bounded by the sketch isn't important enough to cause extra mouse clicks.  Make sense? 

It would be cool to hear the reasons why from developers.  Hopefully I get to learn some new sketching workflow and I can stop loathing the sketch environment every time I use it.

[laughingcreek]

The "area bound by the sketch", AKA a profile, is actually a pretty important part of the work flow in fusion, since so many solid operations start with a profile selection.  The profile is an element just the same as the face of a body.

[Bug.Robotics]

Thanks for the reply laughingcreek.  Totally agree that the profile is vital when using the sketch as the foundation for another feature (cut/boss/revolve/etc).  This is similar to many CAD platforms. 

The issue that I'm referring to is that the sketch profile interferes with selection of entities underneath that profile at all times, regardless of whether that profile is used as a reference sketch or used as the base sketch for a feature.  This slows down the workflow, unless I'm missing something...and I indeed hope I'm missing something.

If this is ambiguous in any way let me know.

[laughingcreek]

if the sketch is visible, how would the software possible know you don't want to work on the profiles it contains?

You can turn off profile visibility from the sketch pallet, then they won't be select-able.  

[chrisplyler]

You can't "work" on a profile directly. It WOULD make sense to only have profiles selectable once a Create tool is activated.

[Bug.Robotics]

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if the sketch is visible, how would the software possible know you don't want to work on the profiles it contains?

I am referring to the area enclosed by the sketch.  There is no reason (that I know of) the dead space on the inside of a sketched profile, which contains no information other than a shaded region telling the user the sketch is closed, should interfere with the user's ability to select geometry.

Check out the screencast I posted.  The sketched circle limits my ability to select geometry like the vertices and inside edge.  The part of the body I am trying the select is in the middle of the circle.  I'm sure the developers could tell us quite quickly why this is the case.  

What is interesting is that you can select sketch geometry directly beneath another sketch without issue.  So the ability to do what I am asking is there just not applied to body geometry.

You can turn off profile visibility from the sketch pallet, then they won't be select-able.  

For sure.  The issue is I use sketches for layout/reference and may want the sketches visible so that I can reference them.

I use sketches for reference tools, layouts, toolpath containment/definition, as well as for base geometry used in features.  I always want to be able to reference sketches I create as well as determine whether those sketches are visible. What I don't want is the sketches I create to mask any other geometry I may want to select for reference during other operations.  Most of the time I am trying to select geometry for measurement.  In Fusion, the sketched profile masks the geometry beneath it and therefore causes the user to do a few more operations to get to the end result, like selecting a point or edge with a long click and then select from a list. 

If you are only doing this once in a while it's no problem but if you are working in the environment for hours on end each day then the extra time and clicks add up fast.   

The reason for bringing this up was two fold.  (A) I wanted to bring this up to see if this was a known issue (B) I'm genuinely curious about whether there are reasons behind this style of implementation.

[laughingcreek]

when you turn off profile visibility from the sketch tool pallet, only the profile is turned off (the yellow part). you can still see and select the sketch.

[Bug.Robotics]

Thank you!  So, I unchecked "Show Profile" and can select geometry underneath the sketch which is great for layout sketches, CAM stuff etc.  This will certainly help with my sanity.

You can't create geometry unless I turn the profile back on so this leads me to believe this "feature" was added to workaround some obstacle, legal or otherwise.  Or perhaps the developers just thought that allowing the user to prevent a sketch from being used in a feature would help keep the chaos down if you had many overlapping sketches and needed only one to be the feature. Hopefully a developer chimes in so we get to hear their thoughts.

Thanks to @chrisplyler and @laughingcreek for the responses.

[jeff_strater · Accepted solution]

Show Profile was added for two reasons:

1. To reduce visual clutter in the graphics area.  Some people don't want to see the profiles all the time.
2. To increase performance.  Sketch is faster when it does not have to calculate the profiles

As you note, you must turn profiles back on in order to consume them with a feature.

[Bug.Robotics]

Thanks for the reply @jeff_strater.  Great to hear the reasons why behind the feature.

What does the profile do for the user other than provide something to click on during feature creation?  If the profile was always off and then the sketch line could be selected for features couldn't the whole "Show Profile" feature and workflow be avoided thereby allowing geometry selection and feature creation while reducing the amount of work?

[chrisplyler]

I'm glad profiles are shown. It's just that they don't need to be selectable until you're creating a feature.

[Bug.Robotics]

I like that they show a closed sketch.  Is that why you like them? 

I agree that the profile doesn't do much until it comes time to use them in a feature.

[jeff_strater]

First:  Even if you think that the primary use of a profile is consumption by a feature, there is still the object-action workflow:  Select the profile, then invoke Extrude. 

Second: the profile can be used for more than just consumption in a feature:  You can use them for editing a sketch, creating an offset workplane, and other uses.

There are several methods to avoid the problems that you are experiencing, most of which are noted here:

• turn off the sketch visibility
• turn off profiles
• change the selection filter
• Select Other (hold left mouse button down for about a half second), and select what you want from the list

Hope this helps a bit

[laughingcreek]

I think you just have a different work flow.  For many, the general rule of thumb is to try to get from sketch to a 3d object as soon as possible.  With this work flow, you would have to be constantly be turning on profiles in order to use them.  They really are the primary basis for creating 3d objects, which is the primary focus of this particular software.

If you are strictly using them for reference, you might consider using construction lines, which won't produce profiles.

[Bug.Robotics]

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Thanks @jeff_strater for the reply.

First:  Even if you think that the primary use of a profile is consumption by a feature, there is still the object-action workflow:  Select the profile, then invoke Extrude.   I'm coming from SolidWorks where the sketch is selected to create a feature and it doesn't interfere with geometry selection below the sketch.   The sketch profile is fine in Fusion it's just that it interferes with geometry selection by default which seems odd.  Would it be possible to allow geometry selection underneath the sketch profile by default?  User controlled option?

Second: the profile can be used for more than just consumption in a feature:  You can use them for editing a sketch, creating an offset workplane, and other uses.  I can see some value in the editing realm- instead of double clicking the sketch icon in the history you could just double click the sketch profile and jump straight into edit mode.  I don't think I realize the value of the offset workplane because the sketch had to be placed onto a plane in the first place (looking for any guidance on the value). 

There are several methods to avoid the problems that you are experiencing, most of which are noted here:

• turn off the sketch visibility
• turn off profiles
• change the selection filter
• Select Other (hold left mouse button down for about a half second), and select what you want from the list

Thank you.  I'm aware of these workarounds (from previous posts).  They all involve extra steps which made me curious as to the why.  If the profile didn't interfere with geometry selection none of those workarounds would be necessary.

Not complaining just trying to understand from the developers perspective so I can better tailor my workflow and if there is room for adjustment  I'd like to ask for it via the IdeaStation because I haven't read a reason to block geometry selection with the sketch profile.

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