Not constrained / fully constrained

[Anonymous]

You can see right down corner of the widow is saying sketch is fully constrained but green line shows sketch is not constrained.

How to solve the problem?

[mdavis22569]

I wouldn't have done it this way ... and would prefer to start it over.. Drawing the bottom of it first and offsetting inwards and closing the sketch.

but I'm explaining if from what you have shown

I deleted it because it wasn't parallel to the other line 

 by .27 degrees

I would have done this differently ... and would have used an offset for the .1 ...and extended the lines 

there are different ways to get to the end result though. I'm sure other will be posting them

[mwighton]

it is not fully constrained...

[Anonymous]

I wouldn't have done it this way ... and would prefer to start it over.. Drawing the bottom of it first and offsetting inwards and closing the sketch.

but I'm explaining if from what you have shown

I deleted it because it wasn't parallel to the other line 

 by .27 degrees

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What is the reason for giving contradictory signals?

[mdavis22569]

What I'm saying is ..I wouldn't have done it that way.

if it was me, I would have drawn the bottom and offset it from the bottom inwards .100.

But I'll show you the problem with what you have shown so far:

The line isn't right, you're on an angle of .27 degrees. So I've redrawn the line...

Is this clearer?

[Curtis_Waguespack · Accepted solution]

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@Anonymous wrote:

...How to solve the problem? 

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Hi fiatnm,

You could simplify this sketch as shown in this video.

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

[mdavis22569]

^^^^^^^^^^^^^^^^^^^^^^ @Curtis_Waguespack

what he did ... different ...and with an offset.

Nice video.

Curtis (I need to ask you an Ilogic question offline if that's possible)

Mike 

[Anonymous]

Excellent video. Thank you very much for your explanation.

[Curtis_Waguespack]

but it wouldn't go through?

[jjstr8]

How is this marked as solved?  It looks like the question is why does a sketch element show up as green when the status bar says the sketch is fully constrained.  I'm running into a similar issue.  When I add a dimension to go from "1 dimension needed" to "Fully constrained", everything in sketch turns green.  When I delete the dimension, everything that's still fully constrained turns black again.

[Curtis_Waguespack]

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@jjstr8 wrote:

How is this marked as solved?  It looks like the question is why does a sketch element show up as green when the status bar says the sketch is fully constrained.  I'm running into a similar issue.  When I add a dimension to go from "1 dimension needed" to "Fully constrained", everything in sketch turns green.  When I delete the dimension, everything that's still fully constrained turns black again.

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Hi jjstr8,

Most likely you have redundant sketch entities, or reduntatn sketch constraints, in any case your sketch is likely more complicated that necessary. Since this post is specific to a particular file, and it is marked solved (most likely by the original poster), you'd be best off to start a new post, and attach your file, mention the Inventor version, other details, etc.

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

[Anonymous]

Watch post 6 video. Instead of deleting lines, split it and change it into construction line this way fully constraint sketches will remain intact and this is an escaping way without falling into trap. Construction lines will not be realized as lines by Inventor therefore it will not affect Extrusion, Sweep and Loft functions.

You can apply this method to other sketches as well it is an excellent method.

[jjstr8]

Curtis,

I guess my comment was really directed to the original poster.  I thought that the original poster was questioning the discrepancy between the color of a sketch element and the status bar stating that it was fully constrained.  In my case, I don't have any redundant sketch elements, just bizarre behavior on Inventor's part.  I just don't see how fully constrained elements can become under-constrained for no apparent reason.  One thing I'm noticing now is, when things turn green, if I try to drag an element the sketch pops back to black.

Thanks,

Jeremy

[Curtis_Waguespack]

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@jjstr8 wrote:

... In my case, I don't have any redundant sketch elements, just bizarre behavior on Inventor's part. 

Thanks,

Jeremy

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Hi jjstr8,

You've got something in there causing the issue, I can feel it.  

Often it's a left over (redundant) sketch point that is left behind from deleting some other geometry.

If you use the Show All Degrees of Freedom tool  it might or might not show you where it is, it's something to try.

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2015...

I don't like to fight sketches, so I employ this type of approach. It'll save you a lot of time trying to figure out these perceived bizarre behaviors:

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

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

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

[Anonymous]

It looks like the question is why does a sketch element show up as green when the status bar says the sketch is fully constrained.
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Reason for this contradiction is as far as I know is software is not 100% perfect.

[Curtis_Waguespack]

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@jjstr8 wrote:

  I just don't see how fully constrained elements can become under-constrained for no apparent reason. 

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Hi jjstr8,

In looking at fiatnm's file again, I'm not seeing the explanation jump out at me,  I am curious if we can get the behavior explained. Maybe @johnsonshiue can have a look at this file Yoke.ipt ‏214 KB        

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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Curtis_Waguespack wrote: 

In looking at fiatnm's file again, I'm not seeing the explanation jump out at me,  m

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Redundant dimension - video to follow.

For the record - I did not view Curtis's video until after I had made this video.

Note how we both handled Sketch Polygon.

Because I teach beginners - I often see them get into unusual situations.  Deleting parts of Sketch Polygons is something that lends to unexpected sketch behavior.

Turn on your sound.

[Curtis_Waguespack]

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@Anonymous wrote:

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Curtis_Waguespack wrote: 

In looking at fiatnm's file again, I'm not seeing the explanation jump out at me,  m

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Redundant dimension - video to follow.

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Hi JDMather,

I was seeing the 1.75 dim as redundant , and one of the pattern/polygon (?) constraints as redundant. Deleting either of those (or the 0.583 dim) allows us to fix this sketch, but I guess I still don't see explanation concerning the behavior of why Inventor thinks it's fully constrainted. 

In any case, along the lines of what you mentioned, learning how to avoid this kind of thing with simple sketches, has always seemed more valuable than how to fix it!

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

[johnsonshiue]

Hi! Actually, the color coding is right but the status bar "Fully constrained" is wrong. There is indeed one DOF left. One of the end points on the green line can move horizontally. This looks like a corrupted constraint system to me. I don't have better explanation. It is possible there were leftover constraints or dimensions in the database causing the confusion. Do we know how to reproduce this condition from scratch? Many thanks!