extrude/revole profile selection problem

[Anonymous]

I have problem with selecting profile for extrude or revolve operation. I have probably changed some setting by accident and I don't know how to get it the way it was before. When I choose EXTRUDE I can't select profile, instead I can select line then new profiles are created and I can select them (screenshot 3 & 4). Screenshot 2 shows how it was done before. Now I can't change selected profile in old files. Thanks in advance.

[mcgyvr]

Check your sketch constrain settings..

Did you possibly turn off Infer Constraints or Presist Constraints from the Interference tab of the Constrain settings dialog box?

Its also usually much more helpful to post actual Inventor files vs images.. 

[Cadmanto]

I agree.  Having the actual part file would be helpful.  When I look at images 3 and 4, it almost looks as though the profile sketch is not closed all the way around.  I see the projected geometry edges, but there needs to be a sketched closed profile to extrude.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[johnsonshiue]

Hi! Please attach the file here. And, read #6 post of the following thread.

https://forums.autodesk.com/t5/inventor-forum/having-a-problem-selecting-an-entire-loop-of-sketched-...

Many thanks!

[neljoshua]

@Anonymous,

Just a guess, but I have had issues with projected geometry not making closed sketches when combined with new sketch elements (even if the projected geometry was created based on a closed sketch). I suggest being careful about what you project. Sometimes I project things that do not really need to be projected.

An example of simplifying a projection is to project a line rather than a face or a point rather than a line. When projecting sketch geometry I have found that simpler is better.

[leowarren34]

Ensure all sketches are closed and constrained fully as I have misclicked previously leading to the extrude failing.

Also keep any sketches as simple as possible as that will also avoid mistakes, especially funky thinks like project have a tendancy not to fully link.

Any parts you can send would be appreciated.

[Anonymous]

@mcgyvr both Infer Constraints or Persist Constraints are turned on, sketch looks fine for me and I've always done sketches this way  but I've attached file so you can check it.

Cheers

[SBix26]

I am not able to fix your Sketch3 to enable choosing either of the profiles for a revolve cut.  Sketch Doctor found duplicate points and duplicate lines, but once I deleted the overlapping projected geometry and reconstrained everything, it still could not find the corner profiles.

However, deleting Sketch3 and recreating it allowed me to select the corner profiles... I have no idea what the problem is with your original sketch.

---

Sam B
Inventor Pro 2019.3 | Windows 7 SP1
LinkedIn

[pawel.gromanski]

@SBix26 deleting sketch and creating another one helps, but only sometimes. sometimes I am creating new sketch and have the same problem. I am creating sketches this way for last 2 years (6 months using Inventor 2019) and it have never happen before and now i had few other files with the same problem do it would be nice to find out why it is happening. 

Cheers 

Still @Anonymous logged on another account by accident

[WHolzwarth]

I don't know, why Sketchdoctor can't solve such a simple issue.

But I'd better use Project cut edges in this case. After that a successful revolved cut can be done

2019 IPT attached.

[johnsonshiue]

Hi! Many thanks for attaching the original file! Indeed, something is intriguing in the part file. Somehow of the end points of the lines do not carry coincident constraints. Although, the sketch is fully constrained, some constraints are missing for no apparent reason. This is a like a corruption. Do you know how to reproduce the behavior from scratch?

Thanks again!

[Anonymous]

I can recreate this behavior by creating for example ring, then I just project inner, outer and side surfaces. In created rectangle I  draw line from corner to the edge and I can not select profile in closed loop. Using Project Cut Edges instead of Project geometry solves problem.  

Cheers