Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.
First time visiting? Here are some places to start:- Looking for a certain topic? Check out the categories filter or use Search (upper right).
- Need support? Ask a question to our Community Support category.
- Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
- Be respectful, on topic and if you see a problem, Flag it.
If you would like to contact our Community Manager personally, feel free to send a private message or an email.
Selecting "something" behind a hidden object.
elio_boezio
Member Posts: 6 ✭
Hi, I'm new to Onshape and I'm still trying to forget how other CAD systems I've used behave. My present problem is in trying to select a point or line or whatever that happens to be "behind" another object (and that I can't reach by rotating the assembly. Hiding the intervening part doesn't seem to help: Onshape still knows it's in the way. In particular, I have this problem trying to work on a part "in Context", where reducing the visibility of the assembly to zero still doesn't allow me to access a feature on the part I'm trying to edit that is "embedded" in the assembly.
I have tried searching the Help facility and this forum, but my keywords are probably poorly chosen, as I haven't found anything. Any help will be very welcome!
Best Answers
-
joshtargo
Member Posts: 239 EDU
right click on the part that's in the way and select Hide Context Instance
0 -
joshtargo
Member Posts: 239 EDU
You don't have the option because a primary instance has not been set. For me, this is a confusing term, concept, and process, and I can't really say how it works, or how to fix it when it won't let you make one. But once it happens, the banner will be yellow and you will have that option.
1 -
joshtargo
Member Posts: 239 EDU
Onshape team, can you just remove the whole primary instance thing? No idea what it's for or why it's needed. Also, sometimes when editing on context, I never get the option to do anything that turns the banner yellow.
0 -
eric_pesty
Member Posts: 1,881 PRO
The primary instance is a different thing (it's what allows a context to be updated)…
The issue is that a context isn't actually "created" until you reference "something" from the context (that makes it turn yellow). That part is a bit odd but it does let you "back out" if you mistakenly end up in an "edit in context" situation (i.e. accidental double click on a part in an assembly instance tree).If you run into this you could for example create a sketch on a face of the context or create an "offset face" feature or whatever to get it to be yellow, you can delete it after.
0
Answers
Hiding the intervening part should definitely help. I often hide parts, sketches, and surfaces to be able to select the desired geometry. Another helpful tool: Select Other.
If you are in the sketch environment - right click close to where you expect to work and choose "select other". This gives a box with a list of various items to select from that are hidden behind objects , (just click the appropriate one). Matt's idea works great in the part studio.
in sketch you can hover and hit "~" to cycle through overlapping elements
Thanks for the reply, Matt. I must be doing something wrong because even if I reduce the visibility of intervening parts to "invisible", as I drag the mouse over the geometry I want to select, the outlines of intervening parts appear and I cannot select what I want. Select Other doesn't seem to help much either, as it brings up a list of similar (default!) names. But I shall persevere!
Thanks for the reply, Rick. I'm trying to edit a part in an Assembly, that I've opened in a Context. My part is visible, and the rest of the assembly is "dimmed". As long as none of the "dimmed" geometry intervenes, I can edit my part. Reducing the visibility of the assembly to "invisible" doesn't help as the "hidden" part outlines appear as I move the mouse over the part I want to edit. Using "Select Other" allows me to select specific bits of geometry, but I can't seem to select a point (for example, to create a 3-point plane). I've not had the problem in a Part Studio, maybe because I've always been able to manipulate the model to get the access I want: my problem seems specific to editing within a Context.
In the screenshot below, I'm trying to select the point indicated by the downward arrow, and the dimmed bit of curved geometry indicated by the rightward-pointing arrow is in the way, preventing me from doing so.
@josh_targo Thanks for reminding me about that one - learned that one a while ago, and then forgot about it. I've got a notebook where I write down those kind of things - I'll have to jot that one down. Thanks again.
While "in context", individual parts can be hidden to allow easy access or switch modes entirely for clarity. Another option is to set view to translucent making everything accessible then right click and select other if things are clustered.
right click on the part that's in the way and select Hide Context Instance
Hi Josh - thanks for responding. I don't get that menu option when I right-click on the intervening part, and I see the "banner" at the top of your screen is different to mine (see below). Can it be because an actual Context has not yet been created, as I got to this point by clicking on "Edit in Context" in the Assembly menu? When I select an actual (i.e. existing) Context to edit, it works for me as you've explained. I'm battling to get my head around this whole Context concept!
You don't have the option because a primary instance has not been set. For me, this is a confusing term, concept, and process, and I can't really say how it works, or how to fix it when it won't let you make one. But once it happens, the banner will be yellow and you will have that option.
Onshape team, can you just remove the whole primary instance thing? No idea what it's for or why it's needed. Also, sometimes when editing on context, I never get the option to do anything that turns the banner yellow.
The primary instance is a different thing (it's what allows a context to be updated)…
The issue is that a context isn't actually "created" until you reference "something" from the context (that makes it turn yellow). That part is a bit odd but it does let you "back out" if you mistakenly end up in an "edit in context" situation (i.e. accidental double click on a part in an assembly instance tree).
If you run into this you could for example create a sketch on a face of the context or create an "offset face" feature or whatever to get it to be yellow, you can delete it after.