Inseparable Shrinkwrap

[FLETCHER.A]

Hi All, 

To protect IP I want to adjust a model to show only essential items before sending out of office. 

Logically I could just use shrink-wrap to combine everything as 1 solid then export this out. however if this file is then saved as a STEP file it will automatically revert to sperate parts allowing people to easily reverse engineer our product. to combat this I was exporting as a surface using simplified part, however this can also be easily reversed. 

I guess I really need a way to make something just 1 solid or surface with no possible way to reverse it.

Thanks 

Fletcher

Below you can see my short story of frustration

[James_Willo]

Try using one of these two options when shrinkwrapping. 

[FLETCHER.A]

Hi James, 

Thanks for the advice, I am already using merge without seams whilst inventor treats it at 1 solid when exported to STP it will split into individual solids again. The screens shots attached to the first post should show this.

Thanks,

Fletcher

[James_Willo]

I'm not seeing this issue, do you have 'make independent bodies on failed boolean' ticked?

Also, this will only work if the parts touch each other, if there are gaps they will appear as separate bodies:

[FLETCHER.A]

Hi James. 

I do not have "make independent bodies on failed boolean" ticked, should I?

I have attached 2 files, the ITP file is made from a part simplification and therefore appears in inventor as a single solid. if you open that file and save it you will get the attached STP. Reopening that STP in inventor will result in a separated model with 9 solids. This would allow someone to reverse engineer a design with ease. 

I therefore want this as a model which can not be easily separated as if I had modelled the whole part from just one solid originally. 

Thanks 

Fletcher

[johnsonshiue]

Hi! I see the behavior now. This is a very interesting issue. Inventor does create one solid body. However, this solid body contains 9 individual disjoint lumps. In Inventor, lumps are not bodies. You can have two separate extrusion apart from each other and they are still considered one body.

To prove my point, use Delete Face -> Lump selection -> pick a lump and delete -> repeat the process. You will see 9 disjoint lumps.

This concept is relatively unique in Inventor. Other CAD systems don't support disjoint lumps. There are advantages and disadvantages of having each. It is a separate discussion. Most of the neutral formats don't support disjoint lumps. As a result, disjoint lumps are mapped as bodies.

The problem here is these lumps are indeed separated in space. They are not merged regardless of options. If you want them to be merged, they need to intersect or fill with material. I suggest you use Shrinkwrap Simpify options to remove some details and see if it works better. Otherwise, you will need to use Envelope workflows to cover up geometry.

Many thanks!

[James_Willo]

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@FLETCHER.A wrote:

Hi James. 

I do not have "make independent bodies on failed boolean" ticked, should I?

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I asked because if it is not able to merge the part and you have this ticked, it would make separate bodies instead.

[FLETCHER.A]

Makes sense, I wasn't aware of lumps, but was confused as usually you can have 2 disconnected bodies that still acts as a single body. I will try envelope and see if that rectifies anything.

Thanks

Fletcher