"operation failed due to geometric condition"

[MesaTactical]

Now that I am using SolidWorks 2007, I see they have managed to come up with even more nebulous and mystifying error messages than ever before. This is certainly an accomplishment of sorts, as the software was already in my personal top five of most baffling error messages of all time.

So now I am trying to add a very simple extrusion to a body where two curved extrusions intersect. No big deal until the latest release, when attempting this invariably produces a build error with the helpful message, "Operation failed due to geometric condition." Oh dear, the geometric condition is not appropriate!

I have tried every combination of getting these features together in the same solid body, with no joy. Or rather, a little joy. I was able to design several clumsy workarounds which proved it's not a matter of a zero thickness error (one of the surfaces is tangent to another, but I get the problem even when I eliminate the tangent). But the workarounds result in a crappy part.

I doubt there are any workarounds I haven't tried, but is this "operation failed due to geometric condition" probably something that might have been fixed in recent bug fix releases? Anyone seen it before? Today is a first for me.

 

[ctopher]

Can you post a pic or file for us to look at?

Chris
SolidWorks/PDMWorks 08 1.1
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[CorBlimeyLimey]

I have seen this many times and agree that a more specific message would be very helpful.

Many times however, the reason is logical ... once the solution is found.

Can you post an image of what you were attempting when you received the error message? Maybe we can suggest an alternative solution.

 

[finisher]

I am dealing with the same frustrating, nebulous error message "Operation failed due to geometric condition." The failed op is a simple extruded cut starting from the interior of my body and trying to cut though four surface faces, two of which are mirrored lofts. Sorry, I can't post the file/image as the body profile is confidential.

Just wanted to add my input. I wish, like MesaTactical, SW could be more explicit in their error messages.


finisher SW2007 SP5

 

[TheTick]

No pic = no help. If you can, change the model to keep the error but disguise your secret. Your secrets are overrated, anyhow. No one really cares.

Most of these errors have solutions, but the cause is usually subtle. Sometimes it is a self-intersecting surface. Oftentimes it is a non-manifold body.

Types of geometry that generate non-manifold geometry errors:
[ul][li]Sheet metal corners that touch only on one edge o vertex[/li]
[li]tangent cylindrical surface[/li]
[li]helixes/springs where pitch = wire diameter[/li]
[li]tangency to surfaces that look like planes or cylinders but are no because they are B-surfaces resulting from lofts[/li][/ul]

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[EngJW]

I sometimes get this with 2006. It occurs when making a change to a part somewhere near the beginning, then as it rebuilds several errors show up. Usually there will be a visual error in one of the sketches, but after correcting it the message still occurs. All the lines are the right color, the sketch is fully defined, and running the error check for the feature turns up nothing. I have tried deleting and redrawing different lines without success, and finally have to delete the entire sketch and do it over.

 

[finisher]

OK, attached are four partial snap shots of the housing design, one of which is the cut extude sketch. The cut is currently successful to a depth of 8 mm. Again I'm trying to blast though all of the surfaces. If I go another .5 mm the cut fails.

finisher SW2007 SP5

 

[CorBlimeyLimey]

The link only downloads a single image.

 

[SBaugh]

Where the radius is at in the sketch could it be tangent with another arc? If so, that could be it. Maybe the lines are tangent with an arc... that would cause an issue. Thanks for posting the image, but its not real clear still to exactly what your doing or what the issue is. There could be anything behind that Surface.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[TheTick]

Use the sketch to make a surface that cuts all the way through and then examine carefully for zero-thicknesses and other suspect geometry.

 

[finisher]

I tried to post this yesterday but I see to no avail. Anyway thank you Tick and a star for you. The attached image is a section I made .5mm beyond the terminating (temporarily that is) face of the extrude cut. This is the point at which the cut failed. As you can see I discovered (only via this investigative skecth) two unintentional voids in my solid. The fact that the voids terminate/start at the surface of the solid is shame on me. The voids originate with a prior extrude boss operation. Now I have to figure out how to do that earlier boss in such a way as to avoid these voids.

finisher SW2007 SP5

 

[APPENG]

Just another thing to look for.. i get this a lot because I deal with really hairy geometry most of the time, and also imported data. when getting this message the first thing to do is to use the TOOLS/CHECK command and look for invalid faces.

You will find that a lot of the times its something you did earlier and need to define better. I had this recently with a guy who was modifying an imported solid adding draft, and fillets, finally got the geometric condition error, and come to find out the imported solid had two bad faces that if he would have fixed those first the part would have not had any trouble

Regards,
Jon
jgbena@yahoo.com

 

[finisher]

Thanks APPENG for the tip on TOOLS/CHECK. Sure enough it indicates one solid face fault (no surface faults). I had never used this utility B4. It doesn't seem to show you the offending face however. Am I missing something? I also discovered using TOOLS/CHECK that the fault occurs very early in my construction. Attached is another image showing the point in the tree where the fault occurs. The left hand loft is mirrored and the mirroring induces the fault. The build is clean rolled back to the original, right hand loft. Does anyone have a tip to help me find my error?

finisher SW2007 SP5

 

[APPENG]

Its hard to tell from that picture really, but lets think about this a bit.. if there is no fault in the faces prior to the mirror, and bad faces after the mirror, then we need to look at how we are mirroring or how we are lofting. Something about the loft geometry is not happy when it is joined by its mirrored counterpart. so again we have only two choices.. redifine the loft so that it will work with its mirror twin, or redifine the mirror plane such that it works..

i might have a little time later, if you want to upload the part I will look at it for you..



Regards,
Jon
jgbena@yahoo.com

 

[finisher]

APPENG, thanks for the offer. Attached is the part file.


finisher SW2007 SP5

 

[APPENG]

finisher, sorry about the delay, i looked at the part, and basically it did that because when you mirror a "feature" you dont always get what you desire but more like what you ask for if you take my meaning.. mirroring a loft feature or other sketch based thing like that can sometimes lead to problems based on the reorientation of the sketch entities, guides, up to faces in extrudes and cuts, weird things. A safer way to do this is to mirror the body instead.

what i did was deleted your mirror, cut the model in with the right plane, then mirrored the whole body. the result was no more invalid face.

hope that helps here is the link to the part.

Regards,
Jon
jgbena@yahoo.com

 

[finisher]

Jon,

Thank you SO much for that super tip. A star for you! As I'm not yet on SW2008 (and therefore couldn't look at your posted file) I succeeded in following your instructions with a perfect result.

finisher SW2007 SP5

 

[MesaTactical]

Sorry for disappearing like that after I started the thread. Last month was our busiest month ever, and in addition to designing the products, guess who also works in the warehouse doing assembly and shipping?

Anyway, here's an illustration of my problem:

I was able to get the problem extrusion to show up by unclicking the merge checkbox in the extrusion feature. So now it's a separate body (the gray lobe in the illustration).

Now I get the error if I try to merge this extrusion with the rest of the part as long as it extrudes past the surface that is highlighted (or rather darklighted darker green). I am extruding from the front plane which is at the center of the part, and as long as I keep the end surface below the indicated surface, there is no error. But as soon as it crosses that surface I get the error.

Among workarounds I have attempted, I have tried to start the extrusion from a plane parallel to the front plane and extruded in toward the center. Again, when I attempt to cross that surface, I get the error.

 

[MesaTactical]

Now this is getting bizarre.

Until now, this feature was made by extruding from the front plane using the midplane method and going out 1.5 inches (.75 each way). This part is completely symmetrical over the front plane. So I experimented this morning on the left side of the part, using the extrude to vertex and blind methods to extrude the feature. Everything worked, so I just extruded .5" in one direction and then prepared to work on the right side.

Mirroring the feature over the front plane generated the error.

So did simply making a new feature, identical to the first, that extruded .5" to the right.

This is crazy, the part is completely symmetrical!

 

[TheTick]

How is the symmetry in the part achieved? Is the entire part mirrored? Or is it just symmetrical construction? If it is not mirrored, equal fillets on opposite sides might not be resolving with the same result.