exhasut transition piece: mirror error message

[MPRC]

The attachment has one pipe drawn and it was mirrored.  When attempting to use the shell command, an error message pops up after clicking OK.  A shell thickness of 5/16" was used.    Let me know how to fix this. 

[trumpy81]

First off, you have a LOT of unconstrained geometry, starting from the first sketch. Go back and fix that aspect of the part first. Try to avoid sketch patterns also, instead, pattern the features. In Flange, remove the pattern, extrude the hole after constraining the geometry, and then pattern the hole.

Next, there is broken geometry in Revolution2 that also needs to be fixed.

I removed Revolution2 and with the EOP above the mirror, I was able to shell the part using .312 thickness. However, the shell would not mirror after moving the EOP back to the bottom. I was unable to select the shell as a feature to be mirrored.

I also tried to shell after the mirror, but I recieved errors and the shell failed.

I did not fix the unconstrained geometry though, that may or may not help.

EDIT: Another point, and I hope I'm not being critical here, but the mirrored geometry that meets at the YZ plane seems to be a little off, there should be a small flat area there, seperating the two halves. Other than that, you seem to be on the right track. Also, the central revolved feature, are those measurements correct? It just seems a little large to me that's all, judging from the picture.

[MPRC]

I followed your advice dealing with contrains and using the feature to pattern.  There is still an error message with shell and mirror.  I'm working on to see whether the mirror line or one of the features (i.e. nose piece) is not symmetric along the YZ plane.  In the meantime, can you look at the attachment?  I circled (polygoned) a shelled burrow that is not supposed to be there.  Does this help identify the problem with shell and mirror problem or add to it?  Thank you

[trumpy81]

I took a look at your part file but I could not figure out what the problem was. Whatever the problem it is certainly strange.

Anyhow, I remodelled the part using your dimensions and I found that the shell tool refused to work, so I had to do a loft cut in order to complete the voids.

Two things to note, my part is in metric, but all dimensions were entered in inches and I have not completed the bottom features. I figure that you should be apt enough to figure that out

Check it out and adjust the dimensions as necessary to more closely resemble the part. It's difficult to know exactly how to model it without having it in front of you and being able to take actual measurements, but I hope it's close enough to be of use to you.

Happy Inventing!

[JDMather]

Among other problems - you are trying to do your shell at the entirely wrong time in your feature history.

Forget the easy stuff until afte you have completed the difficult geometry.

What is the url to the original thread you started on this problem (and why didn't you continue that discussion)?

Never mind, I went and found it myself http://forums.autodesk.com/t5/Autodesk-Inventor/Exhaust-Transition-Piece/m-p/3482194

Keep in mind that that is a casting.  You might hold off some of (most? all?) of the machined features until the casting is modeled. 

[bobvdd]

I think you are running into two problems here:

- the shell of a complex loft might be of low quality and will give problems downstream in subsequent operations like mirror

- you might risk of creating non-manifold edges than cannot be filleted etc

See attached part. I decided to create two lofts and subtract the inner loft from the outside loft.

This in my opinion will produce a higher quality feature that survives the mirror.

Bob