How to show one hidden edge of a buried part in an upper level assembly drawing?

[bnemec]

I resisted hijacking another thread and going off topic, but I'm going to reference much of it here as it's a problem we're facing and we haven't figured out how to deal with it yet. There are other SE users here too so maybe they will understand what we're trying to do and how it's done in SW.

From the "Exploded View Issues" thread: viewtopic.php?f=3&t=409

Hold on. Then how does one ever attach items that aren't visible on the outside of the assembly (without great effort)?

One option would be to find the part in the tree, right-click, and choose "Show hidden edges". Of course on complex Assemblies finding that in the tree may be a non-trivial exercise.

Not wanting to do that work around. We have a ten pounds of parts in a 1 pound box.

+1 on that. Most of the time we just need a few hidden lines from one part on a top level drawing. This was SO SIMPLE in Solid Edge. Nearly impossible in Solidworks, its really embarrassing for me because I was the guy that checked functionality in Solidworks before we purchased. It wasn't even on the list of things to check, how could this not be a simple function in any quality CAD system?

This is a pretty common task for us, we just need to see the silhouette edges of a buried part as hidden lines, for example.

[Tom G]

I have a layer named H. It is red, lightweight, with dashed linetype. Make a similar layer to suit your needs if you don't already have one.

Show hidden edges on that component.
Make your H layer active.
Manually select the edges which you want to show.
Convert Entities. This creates lines on those edges in the active layer.
Hide hidden edges on that component. (Or, alternatively as I use it, hide the whole component because I use it to profile and "ghost" an obstructing but unimportant object in the foreground.)
Reset your active layer as desired.

Although it is not present in 2018, I believe that there is a silhouette edges or profile sketch command available in later versions. That may also help your process as I understand it. That may be a sketch feature within the component, in which case just show (or convert entities upon) the profiled sketch in the drawing.

Edit: Because this sketch entity(ies) in the drawing is related, this action is stable through my revision process, for if the item has moved. If my item was reoriented, however, new profile would need selected and recreated. Otherwise, the lines do follow those selected edges if they relocate between revisions. Similarly, if the component is missing, then the drawing will generate relationship errors on those orphan lines.

[bnemec]

I have a layer named H. It is red, lightweight, with dashed linetype. Make a similar layer to suit your needs if you don't already have one.

Show hidden edges on that component.
Make your H layer active.
Manually select the edges which you want to show.
Convert Entities. This creates lines on those edges in the active layer.
Hide hidden edges on that component. (Or, alternatively as I use it, hide the whole component because I use it to profile and "ghost" an obstructing but unimportant object in the foreground.)
Reset your active layer as desired.

Although it is not present in 2018, I believe that there is a silhouette edges or profile sketch command available in later versions. That may also help your process as I understand it. That may be a sketch feature within the component, in which case just show (or convert entities upon) the profiled sketch in the drawing.

Edit: Because this sketch entity(ies) in the drawing is related, this action is stable through my revision process, for if the item has moved. If my item was reoriented, however, new profile would need selected and recreated. Otherwise, the lines do follow those selected edges if they relocate between revisions. Similarly, if the component is missing, then the drawing will generate relationship errors on those orphan lines.

Well, that sounds... ...complicated, but if it's the only option I suppose. Man, I don't want to be the guy that shows this at the next department meeting.
"Hey guys, we found the straight forward way to show a few hidden edges of a buried part in a top level drawing...
step one, add a layer that we didn't know we needed in templates,
step two make that layer active
step three find the buried part and make it visible
....
step eight restart solidworks...
step nine go to step one..."

Hopefully they don't have tomatoes.

Sorry if I sound ungrateful. I do appreciate the suggestions.

[Glenn Schroeder]

I resisted hijacking another thread and going off topic, but I'm going to reference much of it here as it's a problem we're facing and we haven't figured out how to deal with it yet. There are other SE users here too so maybe they will understand what we're trying to do and how it's done in SW.

From the "Exploded View Issues" thread: viewtopic.php?f=3&t=409







+1 on that. Most of the time we just need a few hidden lines from one part on a top level drawing. This was SO SIMPLE in Solid Edge. Nearly impossible in Solidworks, its really embarrassing for me because I was the guy that checked functionality in Solidworks before we purchased. It wasn't even on the list of things to check, how could this not be a simple function in any quality CAD system?

This is a pretty common task for us, we just need to see the silhouette edges of a buried part as hidden lines, for example.

I have a method that might be easier than all the Layer, convert entities, method. Show the hidden edges, as I described earlier, then Ctrl+select the edges you don't want to show, right-click, and choose the "Hide/Show Edges" icon (or left-click on the view, choose the icon, then select the edges to hide). This method will also make it easier to make hidden edges visible if you want to later.

Does SolidEdge have an easier method? If yes, please explain. I'm curious.

[bnemec]

I have a method that might be easier than all the Layer, convert entities, method. Show the hidden edges, as I described earlier, then Ctrl+select the edges you don't want to show, right-click, and choose the "Hide/Show Edges" icon (or left-click on the view, choose the icon, then select the edges to hide). This method will also make it easier to make hidden edges visible if you want to later.

Does SolidEdge have an easier method? If yes, please explain. I'm curious.

What you describe is what they try to do now, except some times the hide/show Edges button doesn't hide the edge, but it does make it so I can not select that edge again. Just for fun I tried changing the color of a hidden line and it behaved the same; no change and now I cannot select it.
Also, the show hidden edges seems flaky on Imported bodies, it will show them for a moment then they're gone. Ctrl+B or Ctrl+Q do not make change.

Lastly when moving the mouse around is seems that ALL the edges, even those still hidden are selectable, so selecting the many many edges of the part is difficult.

The process to show the hidden edges of a part was similar, but in a properties dialog with it's own tree which was a bit less handy in some ways, but it always worked. Then there was a hide lines button for the view and the selection tool was the click drag window, right to left was all that were touched, left to right was all that were fully contained.

Maybe it's not that much harder here once we learn how, just a lot different.

[Jaylin Hochstetler]

Here's a video I recorded where I hide some edges on a part, show all the options of a drawing view, and show all the edges again in that drawing view.

Edit: Changed the attachment from a .7z to a .zip
Edit: Changed attachment to .wmv

[Glenn Schroeder]

Here's a video I recorded where I hide some edges on a part, show all the options of a drawing view, and show all the edges again in that drawing view.

Edit: Changed the attachment from a .7z to a .zip

1. Hiding and showing edges doesn't look much different from SW, except the command is on a toolbar instead of the right and/or left click menu.

2. I did find the view properties options interesting, though it went by too fast to see much of what they involve.

[zwei]

I am not sure is this a good idea....
But can a macro do this?

1. User select a drawing view and run the macro
2. Macro pop up a form, prompting user to enter part file name to have the hidden edge show
3. Macro search for the part in the drawing view and show the hidden edge

From my understanding, it seem to be doable...

[jcapriotti]

@bnemec

Not sure if there is exactly what you want. In the video I change the view to wireframe, open the view properties dialogue, select the component and apply. This prompts to set the view back to no hidden lines, you should see your selected component. Then show the Line Format toolbar and select the Hide/Show Edges command. Window the edges with left then right click when done.

Note: The Shift and Alt keys are a big help. ALT + select, unselects everything. SHIFT + select adds to the selectin set. No button just toggles the selection from hidden to shown.

[Merovingien]

if you want to show one specific edge of one part,
and if you are using correctly the "graphic filter" under SW (PRT-ASM-DRW)

you can open the PRT, create a sketch 2D or 3D, convert the edge.
exit the sketch, make it hide in the design-tree of the PRT.

return to the ASM, open the DRW, find the view on the left-panel,
expand it, expand ASM, expand the PRT, and simply :
right clic the sketch → show

and problem solved

[matt]

This would be a perfect place for the Invert Selection option, but it's not available when you select a single edge in a drawing.

Ah, hold it. If you use a Selection Filter and select an edge in a drawing view, Invert Selection does appear, but it just doesn't work. Whew, I thought that was a bug for a minute, but it's just something that doesn't work.

[mike miller]

This would be a perfect place for the Invert Selection option, but it's not available when you select a single edge in a drawing.

image.png

Ah, hold it. If you use a Selection Filter and select an edge in a drawing view, Invert Selection does appear, but it just doesn't work. Whew, I thought that was a bug for a minute, but it's just something that doesn't work.

image.png

Ahem.

It's actually....."unintended non-functionality".




I should work for Dassault.

[zwei]

Ahem.

It's actually....."unintended non-functionality".




I should work for Dassault.

This remind me of the verbiage that PTC often used in their support page which always make me mad
→ Not part of XXXXXXXXXX functionality
→ Work as product specification (even when it is some kind of weird workflow/bug)

[josh]

It's somewhat crappy, but you can insert an alternate position view, then hide everything in the alternate position view except the part you want to show.