Find leak in sketch geometry

[Helmi74]

Hi,

i did a relatively simple sketch geometry with some parametric values. I've been quite careful, used constraints as much as possible but still end up having a geometry which somehow isn't closed in the eyes of fusion. It doesn't show my geometry as closed and i can't do push pull and other things you would expect.

After inspecting visually i can't find anything problematic. What would be the right steps to follow to get rid of this problem?

Unfortunately i can't publish this document at the moment.

Thanks for helping

[TOwens777]

I'm having the exact same problem.  Happens frequently.  No rhyme or reason why... Very frustrating.

[HughesTooling]

What I've done when this happens is draw circles around corners or draw lines across sections of the profile. 

Mark.

[gwcude]

Have you tried "Compute All" under the "MODIFY" menu to see if there is a problem with dependencies? 

[Anonymous]

Unfortunately in Fusion it's really hard to interrogate a sketch for full definition. 😞 My only suggestion is to try to break every sketch you make manually by dragging stuff around before you move on.

[Helmi74]

thanks for your help guys.

Of course i also know the hacks around that but i thought there must be an official solution to that problem. Well, let's wait - probably someone from the team will step in later and present a good solution.

P.S. I don't get any email when someone replies to my forum topics even though i've checked "Email me when someone replies" below. I've already checked my Spam folder. Any known issues here?

[promm]

Frank,

In situations like this inspecting the sketch is the best way for me to understand what is happening and advise a solution.  One place to start is by deleting lines, arcs... one by one and redrawing them in order to understand which piece of the geometry is causing the issue.  Another option is to delete the constraints and then drag the geometry until you find the area that is not closed.  I am willing to do this for you if you can share the model with me directly by exporting a .f3d and emailing it to me at mike.prom@autodesk.com

I would also like to let you know that we are working on ways to make it easier for users to inspect their geometry.  In the blog post below we talk about the new sketch enhancements that will be in the June 20th update.  One of those enhancements allows users to enable a preview that colors sketch geometry based on constraints.  We also are developing a way to show when the ends of geometry are constrained or not.

http://forums.autodesk.com/t5/design-differently/june-product-update-preview/ba-p/5674451

Cheers,

Mike Prom

[HughesTooling]

Here are some pictures to show how I find gaps in profiles. You can find the gap quite quickly by drawing a few lines.

Open profile.

 

Horizontal line shows gap is in top half.

Vertical line shows gap is in left corner of profile.

Circle around corner with gap. Now you know where the gap is delete the circle and try extend on the arc and line.

A quicker way to fine the opening with a zip zag line. 

Mark.

[jeff_strater]

that's a great technique, @HughesTooling!  Very clever.

I agree, though, that Fusion needs some better debugging tools for sketches.  As @promm says, we are working on that....

Jeff Strater (Fusion development)

[macmanpb]

There is a plugin for Fusion to detect gaps:

https://apps.exchange.autodesk.com/FUSION/en/Detail/Index?id=appstore.exchange.autodesk.com%3asketch...

Hope that helps... 🙂

[LMD001]

Hello  macmanpb,

Installed this app and, for me, this works very well, it really helps in quickly finding gaps in sketches.

Thanks for the link. 

Best regards,

Ludo

[TOwens777]

I installed this plug-in and it identified several points that were "open."  However trying to close those points or replacing the lines or splines does nothting. 

One thing I notice...  When I attemp insert a line to close a sketch, one end of certain lines will show a green box around it to show it as a connecting point

whlie the other end of the line does not. Also, the points on the lines that do not generate a green box are not selectable. Any ideas?

[TOwens777]

I went back and used the plug-in along with the dividing lines method and was able to isolate my open segments.  They were invisible to the eye even with hightest magnification.

But I was able to fix them.  Thanks for the tips!

[arnaud.schaer]

Hi people,

I'm getting this behaviour too, very often now. And as you can see in the picture, there CAN'T be a hole in the sketch : I have a spline, an offset of it, and 2 big lines crossing it ... and yet fusion can't find the closed section.

NO, this is not a 3D sketch.

This is a real bug !

[HughesTooling]

@arnaud.schaer  Can you share the design as an f3d? 

Thanks Mark

PS Please don't attach pictures. There's an option Photos on the editor toolbar to embed them, please use this option.

[arnaud.schaer]

Hi, sorry, could'nt insert the picture in my post. For some reason (maybe the ctrl+v from windows capture tool), I did insert it with apropriate  post tool, but it did not get it to the final post.

Anyways.

I've found the issue in my case : the "show profile" checkbox went unchecked (but I did not uncheck it, I don't know how it went like that, maybe when sometime fusion disappears behind all open windows), that why I was not seeing closed profiles in sketches AND in 3D view (so it prevented me from extruding)

it's a conter intuitive that a checkbox in a sketch  disturbs anything beyond the sketch edition I think.

[laughingcreek]

---

@arnaud.schaer wrote:

...it's a conter intuitive that a checkbox in a sketch  disturbs anything beyond the sketch edition I think.

---

what do you propose would be a more intuitive approach to toggling the visibility of sketch profiles?

[arnaud.schaer]

I'm really a beginner in F360. But options that show on the panel when you open a sketch should be "per sketch". Global options should IMHO stay in the global preferences toolbox, until an override is allowed / useful "per sketch" (for example 3D sketch ; btw I find it odd that clicking on it in a sketch does nothing, you have to leave and reenter the sketch)

I don't see the benefit of this particular option "hide profiles" (need a pointer for a use case of it).

just my point of view as a F360 newbie (more or less)

[laughingcreek]

"hide profiles" in the sketch panel isn't a global setting, it's per sketch.  closed profiles are an important tool in solid modeling.  but when you have more than 1 sketch involved it can be helpful to have some sketches not highlight their profiles when mousing over.

[j9lemmon]

I'm having the same "leaky Sketch" issue. I tried Sketch Checker - thanks @macmanpb  - but I can't tell that it is showing me where the leak is. It says "Sketch must me active" which I took to mean do Edit Sketch.

I've attached the an F3d file with the Sketch. I drew a line across the Sketch as suggested, so I know the the area where the leak is, but cannot find it. Have tried re-creating the lines and adding constraints with no luck. 

Thanks for any advice.