Cut Revolve failed due to geometric condition 1

[bbrock]

I've seen a bunch of questions regarding the "failed due to geometric condition" error and I've looked through a lot of the responses. They typically refer to geometries where bodies are supposed to be connected by what is really a line, such as a surface tangent to a cylinder or two squares touching at a corner. None of these are the case here, as far as I can tell.

I've made a cap screw which is configurable using the design table. It's worked for a dozen threads and lengths, but for some reason one feature doesn't want to work with a #6 thread. You should be able to create any new thread/length using the first 3 columns of the design table, and the other dimensions should update accordingly.

Cut-revolve1 gives an error when I attempt to cut a full 360 degrees with a #6 thread. However it will work for any other cut 1-359 degrees, or even for 360 on other threads. I can't figure out why.

Using SolidWorks2011 Education Edition. Any help is appreciated.



PS: I know using the Toolbox would be a lot simpler than any of this, but it doesn't work on the network I'm on. It's been this way for months and the IT department doesn't seem to want to change that any time soon, so in the mean time I have to work with this.

 

[CorBlimeyLimey]

When I try to open the DT I receive the following message;

The design table file is corrupt. Delete the existing design
table and create a new one.

Are you really intending to use full helical threads on every fastener?

 

[kellnerp]

Please post files everyone can open.

Geometric condition errors typically have to do with inadvertently creating zero thickness geometry.

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[bbrock]

I appreciate the help CorBlimeyLimey. Not sure why it's telling you the design table is corrupt. I went and re-downloaded the file myself using the link and didn't have any trouble. One way or another, here's another without a design table.

And yes, full threads. The main deliverable here is an accurate computer animation/motion study, which will include a close-up of some bolts going in as the device is "assembled." No need for further simulation/testing so I can afford schematic threads. As far as the project goes, I could just delete the feature and be no worse off. At this point an answer is mostly for my own sanity.

Thanks again.

 

[CorBlimeyLimey]

Looks like kellnerp was spot on. Sketch6 in Cut-Revolve1 is creating an unsupported geometric condition. If the diameters in that sketch are changed to say .09 and .2, the feature works.

 

[bbrock]

In sketch 6 (the parent of the problem fature) the distances to the near point and far edge of the triangle are set exactly equal to the root diameter and major diameter. Given that I was going to be making a couple configurations, it was just easiest to define the distances this way when using the spreadsheet. I found that by adjusting the distance between the triangle's near vertex and the axis, I no longer get the error.

But still, I'm curious... There's no zero-dimension geometry that I can see, and even then why didn't SolidWorks generate the same error when the feature only went, say, 359 degrees around?

 

[CorBlimeyLimey]

Leaving the diameters but changing the angle (30 or 45 is more realistic) also allows the feature to work. So it looks like a zero thickness or unacceptable knife edge is being created on the "second" thread.

 

[bbrock]

mmm. thanks very much for the help.