Inventor 2011 IGES Thread Export Problem

[vkmaynard]

When exporting to an IGES format the threads are missing.

 

Why?

 

Thanks,

 

Victor

[JD Mather]

Cosmetic threads or modeled threads?

 

My guess is cosmetic (picture texture that sort of looks like threads). Zoom in and see if you have real threads (v-notch geometry).

[vkmaynard]

The threads were made by drilling a hole in a solid and specifying the thread type.

 

Victor

[Bishop]

Those threads are just an image map that Inventor applies to give the appearance of threads. They're not really there - it's just a smooth face of the appropriate diameter, as far as exporting goes. If you take a look in the Autodesk exchange, though, you can download an app - made by Autodesk - that will convert your threaded hole features into actual modeled threads. You can export those as actual geometry.

[vkmaynard]

What is Autodesk Exchange?

[Bishop]

This should have all the info you'll need.

[vkmaynard]

Thanks. Found it, installed it, does not show on the ribbon.

[Bishop]

Part modeling environment, tools tab, right side.

 

[vkmaynard]

Not there

 

[vkmaynard]

Problem solved thanks to PhilippeLeefsma Senior Developer Consultant.

He sent a link to the correct version for 2011.

Note: This tool converts a Thread Festure not a Hole Feature using a thread.

Thanks Philippe!!

[vkmaynard]

One last problem. I cannot use this on o.125" plate with any thread size. I get an error message

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Modelization Error

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Failed to create CoilFeature... Try with a bigger Pitch Offset value

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OK Cancel

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[Bishop]

Attach your part here, we'll have a look at it.

[vkmaynard]

Done. I was able to use the tool on a part with only 0.100" thickness.

 

Thanks,

 

Victor

Emergency Release Link 1.ipt

[Bishop]

Huh. That's ... interesting.

 

I think it's got something to do with the sketch that's getting used as a template for the coil feature, but I'm not positive.

[vkmaynard]

I was just told that the plugin does not work with sheet metal parts. Does not make sense.

[Bishop]

Looks to be the case.

 

As soon as I turned it back into a standard part, Thread Modeler worked out just fine.

 

That part though, it doesn't really need to use any of Inventor's sheet metal tools, so there's no need to make it as a sheet metal part.

[vkmaynard]

Agree on that part. I do have a sheet metal part that requires bening that has holes. Does not make sense.

[JD Mather]

You can always convert a standard part to sheet metal (or the other way around).

[Bishop]

Once you've used Thread Modeler you can't convert back to sheet metal, JD. Features are incompatible, unfortunately. Although ... this brings up another point: when you convert to .IGS, you're going to be losing all the tooling stuff that Inventor builds into the sheet metal parts. Your flat pattern, bend angles, etc., aren't going to come through. You'll just get a model, so you're really not giving away anything to just make the sheet metal part, then convert to a standard part and do the threads afterwards.

[vkmaynard]

Thanks. I made a backup then converted and threaded. 5 years later ready to send the design for production pricing.