topic Re: Shell Problem in Fusion Design, Validate & Document Forum

Shell Problem

Davidf01 — Thu, 16 Jul 2015 02:23:10 GMT

I have been trying to do a shell feature on part of this model but I keep getting an error that says it could heal the model or something to that effect. I have attached a picture with the red lines showing what I think the shell feature should do. I had it working but then I made a bunch of changes to the base sketch and now it wont work. I'm trying to get a .125" shell and made sure there was enough room for the shell to do that but it does not work. I'm not sure what is stopping it from working.

Any Ideas?

Here is a link to the shared file if that will help.

http://a360.co/1O7BW5v

Thanks

Dave

Re: Shell Problem

JamieGilchrist — Thu, 16 Jul 2015 16:43:41 GMT

I'm pulling your file down to take a look.

Re: Shell Problem

JamieGilchrist — Thu, 16 Jul 2015 18:56:33 GMT

Hi Dave,

what you are trying to do is not impossible, but considering the way you built your model using a sketch to define the shape including material thickness and revolving, your options for shelling essentially go away.

I'm also seeing areas where you're going to have injection molding problems due to inconsistent material thickness. This is a good introductory guide to designing plastic parts for injection molding

I was able to model a cutting tool to give you the results you want, but in my opinion this is a limiting method and a bit of a "hack". If you go and make changes to your design that occur early in your model, there is a high probability that the cutting tool will fail or give you grief when changes are made.

the cutting tool was made by offestting your top "swoopy" surface

building a sketch that offsets .125" to get the "shell" cut in the area you want

revolving this open sketch as patch surfaces

then a series of split bodies and merges to make a solid body as your cut tool.

see http://a360.co/1KaQx2f

I would aviod using this method, it's a good example of what not to do.

In my previous post the process of building whole solid bodies and letting the shell do your mateial thickness calculations gives you a lot more downstream flexibility for early design changes, such as profile shapes etc. as well as truly consistent wall thickness that will result in a better finished product.

One approach is do your sketch for the revolve (see below), but get rid of all the B-side or interior/material thickness attributes as well as the secondary corner rounds in your sketch then revolve, add secondary transitional details/rounds then shell. After that add your remaining B-side detail. see http://a360.co/1KaQ542. I stopped up to your sketch of the lid seal, as I'm not certain what you're trying to do there

if you compare the two modeling approaches linked here, Lid Sketch_jg_with Shell is a much cleaner model with fewer features and the design intent you want. This will help with file translation and sharing this data when you have to hand a file over to your tool maker to quote and do the production work on your mold.

hope this helps.

Re: Shell Problem

Davidf01 — Thu, 16 Jul 2015 21:09:49 GMT

gilchrj,

Thanks for the info about the shell command not working. I will figure out a different way to do it.

The injection mold issues have been taken care of with the original lid that is already being manufactured, There is a whole water cooling system in place

to handel the thicker areas. The model you see is not complete as I'm trying to convert the original lid into Fusion and make the adjustment of a

protruding sip hole compared to an inverted sip hole. The lid is very complex due to the collapseible travel mug it goes with. I have attached pictures

of the original lid so you can see the completed CAD file and not this half finished conversion.

Thanks for all your help

Dave