Can't extrude solid

[Anonymous]

I was working on a part and have done 6 extrusions already, but all of a sudden when i try and do a new extrusion (after i sketch a box) it will only do the hollowed out thing that turns yellow, it will not extrude to a solid piece nor will it give me the option to make it solid (option is greyed out and un-clickable). Anyone know what's going on?

[jason.stephens]

Sounds like your sketch is not a closed loop. Check all end points to make sure they are connected properly.

[mcgyvr]

did you turn off constraint persistance and inference by chance?

Does the extrude dialog red plus mark come up indicating an open profile.

Post the part if you can.

[Anonymous]

Hey thanks for the help, I sort of fixed it. I had a some deleted faces that i put back along with a trim, and i deleted another extrusion, and now it works for some reason.

[JDMather]

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@Anonymous wrote:

I had a some deleted faces....

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When you Delete Faces you change your model from a surface model to a solid model.

At the top of your browser you will have a Solids and/or a Surfaces folder - keep an eye on these.

I recommend you attach your file here for suggestions on alternative techniques to improve the model.

JD VT '93

[Anonymous]

I'm trying to bend in the wings at the top, more or less.

[JDMather]

 Your Sketch1 is not constrained making use of the symmetry of this part about the origin planes.

Sketch2 and 3 are not needed.
If you had used Midplane Extrude for Extrusion1 you would not need WorkPlane1 or 3.

Sketch 10 is not constrained (in fact most of your sketches are missing constraints/dimensions).

Move Face1 is not needed (use multi-thickness in Shell feature).

While I fix up your model you might go through these documents -

http://home.pct.edu/~jmather/AU2006/MA13-3%20Mathe r.pdf

http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mat her.pdf

http://home.pct.edu/~jmather/skillsusa%20universit y.pdf

[Anonymous]

Wow, thanks a lot, those PDFs are really helpful. I now realize how much inventor i forgot over the past few years. I really appreciate the help.

[JDMather]

I just realized you aren't using 2011, so you won't be able to open my solution.  Just post again when you try the Bend feature.

I think I would model "as bent" rather than using Bend Part tool.... but maybe I don't understand your design intent.

[Anonymous]

I made another simple model from scratch, everything is constrained and i drew it already bent. See if this one looks better.

[JDMather]

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@Anonymous wrote:

I made another simple model from scratch, ... 

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Use symmetry.  Nearly everything in nature exhibits symmetry.  Nearly everything humans design exhibits symmetry.  If the geometry has symmetry - use to your advantage.  I made some changes to the location and dimensioning of your Sketch1 (see attached).  Notice by using symmetry I needed fewer dimensions.  Notice alos that one dimension you did not have with your method of dimensioning appears dubious to me.  I would expect that the opening of this slot is far more important than the length of the angle wedge.  And I can tell you from experience that it would be far easier to hold to tolerance in manufacturing than dimensioning length of angled line.

[Anonymous]

Right, I understand. How do you use symmentry in inventor though? For example, when i start a sketch, how do i make an odd shaped part symmetrical about the origin? Do i just sketch half of it on one side? How would i get the origin in the middle of the sketch? I'm sorry for taking up so much of your time but you are very helpful. Let me know if those questions make sense.

[JDMather · Accepted solution]

Search this forum for a new add-in called Center Point Rectangle - it is really slick.

For this particular design the CPR add-in also has a side midpoint rectangle tool that I would have used to start your sketch.

The way I would do it without the CPR add-in is to sketch the rectangle in space and then add a midpoint constraint between the projected origin and the midpoint of the leftside vertical line.

You can use Mirror to mirror one side of a sketch to the other - but that can be flakey in Inventor so I avoid sketch mirror (and sketch pattern) whenever possible. (Inventor has a problem combining patterned coincident points.)  In the SkillsUSA paper I linked earlier I think I demonstrated how Mirror can also result in regions that can't be selected.

What I do is sketch the other side myself and then add Symmetry constraints (thus you will usually see a horizontal and/or vertical construction line of symmetry in my sketches.

All of this take experience modeling thousands of parts and examining why the parts made by other people fail (or at least aren't as robust as they could be).  Every 6 days, 6 months, or 6 years that you look back the previous 6 days, 6 months, or 6 years at the work you did at that stage you will shudder with realization how clueless you were just a week, month or year ago.  I still do when I open my stuff.  I kid you not.

[Anonymous]

Ah okay, i'll keep working with it, again thanks for all the help.

[Anonymous]

Hey Im having trouble extruding as well, keep getting the shell.  Can someone help me out?

[JDMather]

You are in the wrong forum.

The AutoCAD forums are over here http://forums.autodesk.com/t5/AutoCAD/ct-p/8

You do not have a closed polyline.
Either use PE Join before extrude or better yet, use PressPull instead of extrude.

PressPull does not require a closed polyline.

[Anonymous]

Hey thanks for the quick reply.  Now that I have that going, Im stuck again with the push-pull not allowing me to select an area I have outlined to subtract away.  Also, how do I mark your repsonse as "accept as solution"?  Im new to Autodesk...

[Anonymous]

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@Anonymous wrote:

Search this forum for a new add-in called Center Point Rectangle - it is really slick.

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JD, I just searched for this and what you say about it being slick is spot on 😉

BTW this addin is working for me in 2013 as well, so I'm doubly chuffed

Thanks JD!

[JDMather]

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@Anonymous wrote:

BTW this addin is working for me in 2013 as well, so I'm doubly chuffed

Thanks JD!

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Uhmm, wasn't centerpoint rectangle one of the What's New features added to 2013?

[Anonymous]

Yes it was JD, but the addin puts the commands into a panel which gives easier access to them.

You can place the standard commands into a custom panel but this way works better for me at least.

Also, I wasn't expecting this to work in 2013 at all, only 2012 ... lol