Autodesk Inventor

[#1]

I have a problem that has come up a few times before in my work.  We design long overland conveyors that can be kilometers long.  In two separate instances, I have extruded a profile along a path that is a few hundred meters long with no problem.  However, when the path gets to around 700 meters, the extrusion that worked fine at 600 meters simply falls apart.  Any idea what is going on?  Does Inventor seriously have a limitation to length of an extrusion?

[#2]

I am personally not aware of a length limit but what does "fall apart" mean?

[#3]

Hi DosSantosIntl,

See the reply from Johnson Shiue at this link:

http://forums.autodesk.com/t5/Autodesk-Inventor/Limits-of-an-Inventor-part-or-assembly/m-p/2642607#M...

I'm not aware of a solution, but it might help you find a workaround such as making your long parts in sections.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[#4]

Interesting - learned something new.  Glad I don't design anything that long.  Any reason it can't be broken up into multiple subs as Curtis suggested?

[#5]

Sorry, should have been a bit more specific.  By "falls apart", I mean that an attempt at the extrusion results in an error and the extrusion does not complete.  I can post the exact error message when I pull the model back up at the office tomorrow.

Based on the other posts though, it looks like Inventor just has a very small (for my industry) limit to part sizes.  I broke up the length on a previous part that was just for a proposal, but considering this is a continuous belt, it sure seems to me that it should be a single continuous part in my modeling software.  I'd really rather not fudge my way through this project as it is paid work.  I suppose I'll have to revert back to AutoCAD if there are no better solutions, but it's sad to know that the software limits modeling capabilities in such an arbitrary way.

If anyone has any other solutions, please let me know.

[#6]

Not sure if it would make any difference but try changing the part (belt) Units/>Length to metres. I just modelled a simple extrusion 700 metres long without troubles. Worth a try? Best of luck.

[#7]

Hi

I did the same, no issues. (The display gets a bit jumpy)

My part is 7KM long and shown below is a 50mm dia hole at the 7km mark.

[#8]

Nope, that didn't do it (changing units to meters)

It's somewhere between 671 meters and 672 meters that the extrusion fails.  Complete text of the error message is:

Slope Conveyor Belt.ipt:Errors occurred during update

     BeltLine: Could not build this Extrusion

          The specified inputs did not create sweep geometry (faces and/or edges). Try by changing path geometry and/or creating the profile on a sketch plane that is perpendicular to the path and contains one of the path vertices.

     LOBDischXition: Could not build this Loft

As annoyed as I am by the fact that Inventor is incapable of creating this extrusion, it seems like they could at least offer an error message that actually explains the problem.  Something along the lines of "This extrusion is too long.  Inventor cannot create a part this big" would work.

One thing that I think may make the difference (and what allowed the other posters to create a 7km extrusion) is that my profile does not coincide with the extrusion path.  I may try to change that to make this work, but doing so changes the intent of my design, and I really grudge modifying my design to accommodate the software.

I appreciate the suggestions offered so far!  If anyone else has any ideas, please keep them coming!

[#9 · Accepted solution]

In Inventor 2012 and earlier versions, the extrusion length is limited to 1 km (= 1000000 mm) for one direction and 2 km for both directions.  Good news is that this limitation no longer exists in Inventor 2013.

Four examples are attached here.

• extrude_1km_inv2012.ipt:  Extrusion in one direction.  Changing the extrusion length to 1000001 mm in Inventor 2012 will cause the extrusion to fail.
• extrude_2km_inv2012.ipt:  Extrusion in both directions.  Changing the extrusion length to 2000001 mm in Inventor 2012 will cause the extrusion to fail.
• extrude_7km_inv2012_wkaround.ipt:  Using Rectangular Pattern, the desired distance can be achieved. "len" is the parameter for the extrusion length.
• extrude_7km_inv2013.ipt:  Extruding 7 km in one direction.  In Inventor 2013, the 1 km limitation no longer exists.

Note:  If you open extrude_1km_inv2012.ipt in Inventor 2013 and change the extrusion length to 1000001 mm, the extrusion will still fail because the existing feature uses the old compute method.  To use the new compute method, you need to recreate the extrusion feature (i.e., Delete the existing feature, leaving the base sketch intact, and then create a new extrusion).

I looked at DosSantosIntl's model.  After I recreated the extrusion in Inventor 2013, I could extrude the profile by 1000000 meters, well above 671 meters.

Glenn

ASM Development

[#10]

This workaround will do it.  Incidentally, I found that in order to make the return belt work (separate feature that is also about 2km long), I only had to break up the lines that composed the path into 500m increments.  The sweep then generated as a single 2km feature.

Thanks for your help everyone.  This is the first time I've posted here to ask for help, and I'm very pleased at everyone's helpful responses.