Problem Extruding Profile or Constraining Sketch?

[JohnRpb]

All I'm trying to do is extrude a profile to create a part, but after creaing a sketch, Inventor will not recognize the profile loop when I try to use the extrude command.

I think my sketch is not properly constrained, like it's not connecting the ends of lines together and creating a closed loop, but I don't know how to get it to do that. It's always just done that automatically. I haven't changed any settings but all of a sudden I'm having this problem.

All help is appreciated, let me know if you need any more details.

[Curtis_Waguespack · Accepted solution]

Hi JohnRpb,

Most likely you're putting too much into your sketch, which is causing this issue. But sometimes (very seldom) the simple sketch approach is not the way to go, so you might need to use the Sketch Doctor to help find the issue. Another thing that might be the cause are the sketch Constraint Inference and Persistence settings.

About simple sketches:

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

About closed loops and Sketch Doctor:

http://forums.autodesk.com/t5/Autodesk-Inventor/close-loop-function/m-p/3673860#M452403

About Constraint Inference and Persistence:

http://forums.autodesk.com/t5/Autodesk-Inventor/Constraint-Inference-and-Persistence-not-working/td-...

There are also some suggestions here:

http://forums.autodesk.com/t5/Autodesk-Inventor/Ensuring-that-sketches-are-closed-loops/m-p/3799482#...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[JDMather]

And if you still have trouble - attach the ipt file here.

[brian.cranston]

What version of Inventor?  I'm on 2013 and I'm seeing some crazy sketcher anomalies like you mentioned. I have sketches that break after they are consumed in extrusions. I'm dealing with a lot of lost coincident endpoint constraints as well.  Review Curtis_Waguespack's suggestions and hopefully that helps.  I've had settings mysteriously change (most are my fault, somehow).  Otherwise, know you aren't alone.

-Brian

[JohnRpb]

Curtis - The sketch is very simple, I doubt complexity is the problem. But I'll look into those things you listed and let you know if anything works. Thanks.

Brian - I'm using 2013 as well. Sounds like the same problem - it all of a sudden stopped applying coincident endpoint constraints to my line segments. What settings ended up being the problem for you?

Is it a coincidence that I was playing around with Inventor Fusion before I encountered the problem? Could this have affected settings in Inventor or anything like that?

[JohnRpb]

So that was easy. Coincident Constraint Inference was turned off. All I had to do was check a box. I'm almost certain I didn't mess with those settings though...

Thanks for the help guys. I think that solves everything, I'll let you know if anything persists.

[Anonymous]

I am having the same problem.  I can extrude a circle or rectangle but I can not extrude a shape that has been drawn with the line command.    What did you have to turn on to make it work?   I am a teacher and all my other computers will extrude a shape made with lines.

[Curtis_Waguespack]

Hi 200d1,

Ensure that the options in this image are enabled, and then while in an active sketch right click in the graphics window with nothing selected and and choose Constraint Options and ensure that everything is selected.  Just post back if you still don't have any luck.

http://wikihelp.autodesk.com/Inventor/enu/2014/Help/1283-Inventor1283/1718-Parts1718/1923-Constrai19...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[JDMather]

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@Anonymous wrote:
.  I can extrude a circle or rectangle but I can not extrude a shape that has been drawn with the line command.    What did you have to turn on to make it work?  

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If you are using Inventor 2010 you have to be particularly careful with this as the students will mistakenly turn off Constraint Persistence because the icon looks very similar to Perpendicular Constraint.  In later releases they hid the icon in a drop-down so it is less of a problem.

[Anonymous]

Thanks a million. The extrude works great.

[igorthecat]

"Most likely you're putting too much into your sketch, which is causing this issue. But sometimes (very seldom) the simple sketch approach is not the way to go, so you might need to use the Sketch Doctor to help find the issue. Another thing that might be the cause are the sketch Constraint Inference and Persistence settings."

I've used Solidworks for over ten years, and have had little problem getting some pretty complex profiles to close.  Downloaded it four days ago and spent all of my time trying to extrude a single profile, and never got it to work.  This is the kind of profile Solidworks has very little trouble with.  I am considering returning this dog before my thirty days are up.This is what I had to do to get it to work. Ridiculous

[TheCADWhisperer]

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@igorthecat wrote:

 This is the kind of profile Solidworks has very little trouble with. 

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I use SolidWorks and Inventor every day.  (I’ve been a CSWP for over 15 years.)

First thing I notice from your image is that your sketches are not fully defined.  This would be poor practice in SolidWorks.

There is no difference in this respect, therefore I suspect you are doing something wrong. 
Attach your *.ipt and *.sldprt examples here for diagnosis.

[igorthecat]

Solidworks files are proprietary to the employer I retired from.  I do have a couple that I was developing in a coworking space.  Only having Inventor currently I am unsure of the complexity of the profile.  The Inventor file (1 so far) contains data I am hesitant to share at this time.  I have used Solidworks since 2010, and AutoCAD since v.10 in 1990.  I have been finding Inventor to be very cumbersome and very clunky by comparison to to Solidworks.  I work quickly, and time is money. In AutoCAD I was called a Mouse Puncher. It took me about ten hours to get as far as the attached image.  This is very quickly becoming unacceptable.

[TheCADWhisperer]

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@igorthecat wrote:

 I have used Solidworks since 2010, and AutoCAD since v.10 in 1990.  I have been finding Inventor to be very cumbersome and very clunky by comparison to to Solidworks.  I work quickly,...

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The SolidWorks file that you attached here has unconstrained sketches - this is considered >>poor practice<<.

We can remedy this technique as you learn Inventor.

I have been using AutoCAD since 1987 and SolidWorks and Inventor since 2002.  I have found Inventor and SolidWorks to be essentially identical. I work very quickly, and precisely.

I recommend that you start attaching *.ipt files here for help (make up dummy files that exhibit the same behavior as your proprietary data).  Within a few weeks you will be dissing SolidWorks.

[johnsonshiue]

Hi! Please feel free to share the Inventor file with me directly. I would like to understand the behavior better. On Inventor 2019 and earlier, the sketch profile is recognized based on sketch constraints. If there is no coincident constraint, the profile is not considered complete. It does have fair share of problems. On 2020 and later, it has been changed to geometry-based. The issue you are talking about should not exist.

I can sign NDA if need be. We do not share client data in public. You can also specify who can access the file and where the file is stored.

Many thanks!