Why can't this part extrude anymore?

[kperic777]

Hi,

I'm trying to modify the depth of extrusion feature "Extrusion1".

as you can see, it doesn't let me.  It only allows the extrusion setting "new solid".  Anybody know WHY? and HOW to correct this problem.  I've NEVER seen this in 6 years of inventor.

Please open attached file and take a look.

Kruno

[kperic777]

I'm attaching this screen shot of it, incase anyone is too lazy to open the attached .ipt.  As you can see, it only lets me make a "New Solid" when I try to edit the "Extrusion1" feature, and it doesn't work.

[SBix26]

I can't understand, either, why it won't allow editing of the feature-- the profile(s) are a selectable, but no preview is shown.

As for the New Sold, that's the only choice because there is no other solid to modify.  The first feature in a part is always a new solid.

Edit: I was able to get it "fixed" by opening Sketch2, deleting the 0 dimension and the two small construction lines that became unconstrained as a result, then editing the feature and re-selecting the piece of the profile that got lost.  Now it's editable as expected.  Not sure what was wrong with Sketch2, exactly, but it can be repaired.

[kperic777]

Did you try opening it and playing with it?  Come on YOU CAN DO IT 🙂

[cbenner · Accepted solution]

Sketch 2 contains an open loop.  Edit the sketch and in the middle of the two long horizontal lines, there is a short line segment on top of, or underneath.  Note on the the bottom it says (4) dimensions needed.  Erase these two short line segments from the sketch and the profile extrudes just fine.

See... I wasn't too lazy to help you out, despite my work load.

EDIT... btw, suggesting people might be too lazy to look may not be the best motivator when asking fellow CAD Monkeys for help.  Just sayin'....

[JDMather · Accepted solution]

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@kperic777 wrote:

 Anybody know WHY? and HOW to correct this problem.  I've NEVER seen this in 6 years of inventor.

Kruno

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I have never used a zero dimension in 10 years of using Inventor.
You have multiple zero dimensions to the same position.

The sketch could be created with far fewer dimensions.

I saw lines overtop of lines?

It is actually less work to use a more robust sketching technique and should elimate this problem.

[kperic777]

Yup,

When I had the sketch fully constrained, it allowed me to go back and edit it.  Sorry for the "lazy" comment.  I didn't intend for that to be taken as the true meaning of the word.  It simply wanted to get the information to you guys in the most convienient way, because I know everyone is very busy.

I greatly appreciate everyone's help, and I will now return the favor by browsing the forums to help other people.

the poor assumption I made was with the logic inventor uses in performing extrusions.  I thought it didn't care as long as it has a closed profile.  I will now always fully constrain sketches, and not use "lines ontop of lines", unless they are properly exected construction lines.

Kruno

[JDMather]

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@kperic777 wrote:

the poor assumption I made was with the logic inventor uses in performing extrusions.  I thought it didn't care as long as it has a closed profile.

Kruno

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It doesn't matter - except when it does.  Even when Inventor doesn't "care" I would worry about how the file migrates into the next few releases - is it suddenly going to fail 3 years down the road when Inventor "decides" that it does matter?

In any case, I think it is faster to Make it Right from the beginning as Mike Holmes would say.

Here is how I might dimension the first sketch.  Using symmetry, coincident and equal.

[kperic777]

OK,

the reason why I like to dimension the symmetry sometimes, is because what if you want to use this part later with an offset hole position instead of symetric.  I work in capital equipment, and we take parts all the time and copy them for something else.  What is the difference between referencing a dimension name (parameter) and deviding by 2, vs locking itin the midpoint of a line.

Kruno

[JDMather]

There are many ways that part could be dimensioned depending on design intent, inspection, manuf. process....

[Yijiang.Cai]

When I look into the history of the model you provided, this was created on R2009 and updated on R2011. So maybe you are not clear that a big functionality on R2010 is multi solid body, which allows that user can create multiple solids in one part document. For the behavior you saw, the "new" option is for multiple solid created. As Extrusion1 is the first feature in model history, it should be the first new solid. You could edit extrusion3 to see the other option like "join, cut, intersect". In this situation, it allows user to create a new solid or directly combine with existing solids using "join, cut, intersect".

Hope it helpful for you! 

[kperic777]

Thanks Yijiang

The problem was discovered earlier in the thread by two other users.  My sketch for "extrusion1" was not fully constrained, and I had lines on top of lines.  Once I eliminated those defects, the model functioned properly.