So I've attempted to shell this part, on the back side of it, and it seems to create shell pockets everywhere in the model, where the space allows it. Pretty annoying when I just want to shell one surface/area, on the part.. lol
I've attached two photos to describe the issue - One showing the settings as I create the shell feature itself, and the other showing the after results.
Also, I've attached the part file for any troubleshooting/advise, that you guys can manage to help me out with!
Thanks so much ya'll.
Solved! Go to Solution.
I recommend that you start over - shell is usually done early in the process.
Many of your sketches are not constrained and have duplicated dimensions.
At beginner level you should probably not be using Delete Face command.
You might start here http://home.pct.edu/~jmather/skillsusa%20universit
Have you installed SP1.1?
Thanks for your prompt response JD, as I was hoping you'd come across this and offer some help.
I do not believe I have SP1.1 - I have Build: 138, Release: 2013 RTM of Inventor Pro 2013
What kind of difference would SP1.1 yield, in this particular situation?
The duplicate dimensions were from me going through and showing a colleague some things in Inventor (he's new to CAD stuff, and will just be helping out our department with detailing 2D drawings), so I didn't bother to go back and delete some of them in my sketches.
Regarding your comment that I should start over, I've attached a model of the part in the stage previous to my shelling and deleted faces used. Can you please help me get a better understanding of how to achieve the desired look, that was in my original model/part?
Thanks so much Mr. JD.
I would not even begin to try to work with something like this without starting over from scratch.
First thing I would do - create a dimensioned 2D drawing.
Referring to the drawing and your model I would start from scratch recreating the geometry in a more efficient and robust manner.
I try to avoid work - my motto is - get lazy.
Again, like I said, the dimensions were added, as I was going over things with a fellow colleague of mine. They aren't permanent, so I've deleted the ones that aren't necessary, and re-constrained the 2D's.
Let me rephrase my last question.... lol, what feature(s) can I use to create the end-result that I'm trying to produce on the back face of this frame, since the shell feature is a no-go. Basically, I'm trying to create a lip around the back surface, of about .25 wide, and protruding .375" from the face of the part (as shown on my other models/pics, that I previously attached).
Thanks again for the help.
Again, like I said, the dimensions were added, as I ....
The way I model Inventor would never even allow me to add those dimensions.
If you could clean up the model (which is exactly what I would do) I might take a second look.
Others might be willing to jump in here without a cleaner model.
Many thanks for posting your modeling issue to the forum!
Firstly, I would agree with JD that following good modeling practice is the key to success when modeling complex parts. Ensuring the part is clean and well-defined upstream with prevent a lot of problems downstream that require awkward workarounds. Starting a part from scratch is not something to be afraid of – even experienced modelers will sometimes make many attempts at modeling a complex part before settling on the optimum workflow.
Regarding your Shell problem – Shell is a global modeling operation which is designed to hollow-out an entire body, so the behavior you are seeing as expected. If you want only part of your model to be shelled, it is usually best to order your workflow so that Shell is performed before features that you don’t want to be hollowed-out.
For your model, a workflow that might work for you is to make use of multiple solid bodies to achieve your ‘local shell’. Since shelling is performed on a body-by-body basis, if you separate the section of your model you wish to be shelled as a separate solid body, you can then shell this in isolation and reattach it to the rest of the model afterwards. In the attached IPT (based on your second attachment), I’ve added a Split feature to split the model into two solid bodies, using a Boundary Patch as the splitting tool (rather than a work plane, which would also affect the other side of the model ‘fork’), then performed the Shell, and then reattached the shelled portion using the Combine tool.
I’ve also added the remaining part features as per your original attachment. Note that I’ve made use of the Shell command’s ‘Unique face thickness’ option to adjust the thickness of the shell offset where necessary, removing the need for any downstream Thicken operations. Also note the positioning and ordering of the Fillet features – it’s generally best to add fillets as late as possible (Fillet1 and Fillet2 were added earlier in the workflow because they affect the Shell result).
I hope this is helpful, and let me know if you have further questions.