Sketch becomes invisible after edit

Hello everyone!

Recently switched to Inventor 2017 from Inventor 2013. Why sketch visibility is automativally turned off when I finish edit? Is there a setting to keep sketch visible? Must admit it is driving me mad.

By default the sketch visibility is off when a sketch is consumed by a feature. Is yours off when it is not part of a feature?

I think it is the part of a feature. Is it not possible to keep it on?

Off hand I don't know. I'll look into but I can't think of a reason to do that. Are you sure you want all used sketches visible? To reuse a sketch you need to right click on it and share it. Same as making it visible.

I am sure I want to have control over visibility of sketches, yes. I normally work in NX and use Inventor only sporadically. Guess I picked up some nasty habits from NX - like being able to control everything. I know about sharing sketches. It might be a usable workaround sharing it in order to make the always visible - I'll test that, thanks.

Well so when you make a sketch it is visible. That works right? When you use the sketch in a feature like Extrude it then goes invisible. I can't see any options to set it so that it is always visible. On the "VIEW" tab on the Ribbon Bar there is an "object visibility" but it has 2d/3d sketches visible by default. The sketch gets consumed when its used and is hidden. When you share it then it become visible, but its the same as just making it visible except you can actually use the shared sketch.

I dont know if your habits are bad or not, just different personally when a client sends me a file and it has the "all sketches hidden" option in something, but they are all visible when unchecked it drives me a little loopy. I like that Inventor and Solidworks hide the sketch after its used. I don't like that you have to share the sketch to reuse it. It always catches me off guard.

If i find something i will let you know but i dug through the settings and didn't see any mentions. There was something in the TSB section on Autodesk about Sketch visibility issues but that has nothing to do with what you are trying to do. It is possible to do it through rules and event triggers I am sure. ill have to play with it to see though.

This seemed to work. Go to the "Manage" tab and "Add Rule". In the rule copy the code below. Then from the "Manage" tab go to "Event Triggers". You can trigger model changes, parameters changes, saving etc to run that rule which should make all sketches visible. I tested it out and it works on my test file. I had a Sketch1 and Extrusion 1. I shared sketch1 and then hid it. I then added sketch2 and made an extrude 2. After OKing the Extrude Sketch 1 as well as Sketch 2 were visible. Its probably not the cleanest way but seemed to work.

Dim oDoc As PartDocument

oDoc=ThisDoc.Document

For Each oSketch In oDoc.ComponentDefinition.Sketches

oSketch.Visible = True

Next

iLogicVb.UpdateWhenDone = True

Thanks for suggestion! I'll try this.

You can right click on any consumed sketch in the browser and turn on Visibility.

Has always been this way - no change in behavior.

You can right click on any consumed sketch in the browser and turn on Visibility.

Has always been this way - no change in behavior.

 

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Yes but you can't reuse it without sharing. The Op wants all sketches to stay visible, even after being consumed. Do you know another way JD? You are a more experienced Inventor user than I am.

I don't know why anyone would want all (consumed) sketches to stay visible. That would drive me bananas.

Having said that, users familiar with SolidWorks will probably appreciate this setting in Inventor 2017

For several releases it has not been necessary to mark a sketch as Shared prior to reusing it for another feature.

Any visible sketch that has already been used for a feature is automatically Shared with any attempt to use for a new feature (except in one obscure location/feature which I fail to remember, and I think that was simply an oversight).

I said the same thing but it is an interesting question. My rule works but I didn't know if there was a setting I missed.

Also I have not had the same luck with sketches being automatically shared in 2017. I have had to share mine because they aren't valid selections for features otherwise. I'll try again to be sure but it was that way last week.

JD, I figured out what is happening when trying to share the sketch for another feature. It has to be Visible as you said. What i wrongly assumed is that when you select a sketch and it is visible(not right click > Visibility) that it would be usable. Essentially Visible and Share are the same thing. It becomes "shared" when its used. If you just click on a hidden sketch and its visible on the screen that is not allowed.

You can right click on any consumed sketch in the browser and turn on Visibility.

Has always been this way - no change in behavior.

Will it become always visible after that? Or become invisible after I finish editing it?

It will stay visible. Same thing my code was doing. The code shows the sketch. The other method you have to right click and show