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"The attempted operation did not produce a meaningful result."

53 REPLIES 53
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Message 1 of 54
str8zstar
13792 Views, 53 Replies

"The attempted operation did not produce a meaningful result."

Getting the dreaded "The attempted operation did not produce a meaningful result. Try with different inputs." error. At first it was just if I tried to extrude something (in a weldment currently but seems to do it across the board). It was also giving me the error when I tried to Place a Content Center file. It said it couldn't build the extrusion and gave me a red cross. I'm baffled by this error since it seemed to just start here and there, so I'd reboot IV and it would usually work for at least a while. Now, it's doing it for pretty much every operation I try (except constraints, it seems). Such a weird deal, I wonder if anyone has come across this before? I thought it was a Graphics Card issue from my experience in the past, but could it also be a software issue?

 

I'm running Inventor Pro 2013 on an HP xw8600 Workstation with Windows 7 SP1 64-bit. Intel Xeon 3GHZ CPU, 8 GB of RAM, NVIDIA Quadro FX 4600 Graphics Card with 768MB GDDR3 RAM.

 

Any suggestions?

 

I've attached the extruding & Content Center errors as well.

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53 REPLIES 53
Message 41 of 54

Finaly! We'll get our support guy on it as soon as possible.

Message 42 of 54
hjurriaan
in reply to: frank.gavilar

Still experiencing this error, does anyone know a solution to it? 

Message 43 of 54
JDMather
in reply to: hjurriaan


@hjurriaan wrote:

Still experiencing this error, does anyone know a solution to it? 


Yes.

Attach your file here.


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Message 44 of 54
hjurriaan
in reply to: JDMather

I'm trying to extrude a chamfer off domeWEST.ipt so it aligns with domeNORTH.ipt and it gives me the error.

 

FYI, both sketches inside are the part are imported from AutoCAD

Message 45 of 54
JDMather
in reply to: hjurriaan

@hjurriaan 

An assembly without parts (*.ipt files) is useless.


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Message 46 of 54
hjurriaan
in reply to: JDMather

My bad. the part domeWEST.ipt is placed on the eastern side orientationally. to avoid confusion. because I was messing around on the western side i mirrored them to see if it worked on the other side.

Message 47 of 54
JDMather
in reply to: hjurriaan

Three files are still missing???

Missing Files.PNG

 

Also, 99 out of 100 times, when someone posts an assembly level cut - they really really intended to cut the part at the part level within the context of the assembly. Their intention was not to cut the parts AFTER assembly (think real world operations).

 

And, the usual practice is to fully define all sketches.

This all looks like beginner issues not related to the original thread.

 

 


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Message 48 of 54
hjurriaan
in reply to: JDMather

The 3 missing files are unrelated to the issue, I left those out

.

 

When trying to do a cut extrude on domeWEST.ipt i get the "The attempted operation did not produce a meaningful result." error.

extrude.png

I'm trying to stay on topic. I am indeed a bit of a beginner, and there's a bunch of issues going on at the same time. sorry about that..

Message 49 of 54
JDMather
in reply to: hjurriaan


@hjurriaan wrote:

The 3 missing files are unrelated to the issue, I left those out


I need the 3 missing files.


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Message 50 of 54
hjurriaan
in reply to: JDMather

My apologies, I have little experience with exchanging files with other individuals

Message 51 of 54
JDMather
in reply to: hjurriaan

Open the file domeWEST.ipt

Notice that there is an unresolved issue with Sweep4 and Sketch4 (indicated by i in circle).

Edit the sketch.

Notice the pink (sick) point.

Notice that there are no arcs in the profile (the apparent arcs are actually short line segments).

Notice on the T shape that there are two lines where one line would suffice.

 

I would create this simple profile from scratch (and correctly) in Inventor rather than use the flawed imported geometry.

 

Note also that Sketch1 is not connected to Sketch4 and that Sketch1 could be created with an arc rather than a spline.

No Connection.PNG

 

Note that the curve in Sketch1 of domeNORTH.ipt was created with an arc rather than a spline, but if dimensioned - the radius of the arc does not make logical sense?

 

domeNORTH.PNG

 

Edit:  The Sketch1 in Plafound dome is even worse.  Hundreds (thousands) of straight lines rather than arcs.

I would use this only as reference in creating proper geometry from scratch.


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Message 52 of 54
JDMather
in reply to: hjurriaan

I should have made it clear - there is nothing wrong with using imported geometry - as long as it it good quality geometry from the source.  In this case it is poor geometry from the source.


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Message 53 of 54
johnsonshiue
in reply to: hjurriaan

Hi! I took a quick look at the files you attached. The sketches used to create the extrusion features contain too much unnecessary detail. A straight line is broken into tiny pieces. An arc is broken into short pieces. I guess you got the sketches from a mesh model right? I suggest you recreate the sketch using lines and arcs. Removing the tiny geometry.

Inventor is a precise modeler, geometry accurate up to 0.00001mm. Each piece of geometry represents a function, a measuring target. Any unnecessary detail should be removed, unless it represents design intent.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 54 of 54
hjurriaan
in reply to: johnsonshiue

Hi! The sketches are from provided mesh .dwg model. Imported from AutoCAD to Inventor, for the dome. For building the ceiling plan (Plafond) I used my own measurements mostly, but for outer edge geometry I've used lines that were in this mesh because with measuring we could never get this properly done with high precision. (using a laser range finder)

 

When CNC'ing the ceiling grid we didn't run into any trouble. To fit in our dome inside the grid I used the exact same lines so that they surfaces connect as good as possible. I wasn't expecting that these lines would run me in to so much trouble, if only I had known beforehand. (now I do 🙂 ) I discussed with a co-worker and will either use moulds to widen up the existing gap for the dome with proper arcs or simply make the dome smaller.

 

I have re-created the T-shape, the imported geometry turned out completely asymmetric with straight lines broken into segments. Completely unnecessary indeed.

Ty for looking into it, JDMather. 

 

Atleast I know now the cause of the error, and that I should work more on cleaning up my work/resolving my skethes. Thanks in advance!

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