Suppression of Solid Bodies in iPart

[justin.freriks]

I am wondering if there is a way to suppress entire bodies in a multiple solid body part, using iPart, without having to suppress each individual feature for it.  I am on Inventor 2013.

Any help is appreciated.

Justin

[johnsonshiue]

Hi! Yes and no. It depends on how you generate these solid bodies. Each body must be created by a feature. It cannot come from nowhere (or it would be a bug if you saw one). In order to suppress one solid body, you simply need to suppress the body-creating feature (BCF). You can find the BCF by doing the followings.

1) Go to Solid Bodies folder

2) Expand the body node.

3) Find the first feature under the body node.

One thing to note is that it really depends on how you establish the feature/body relationship. Let's say if each BCF is somewhat independent, suppressing the BCF will suppress the body. However, if somehow BCF2 (creates body2) depends on BCF1 (creates body1), then suppressing BCF1 will also suppress BCF2, leading to body1 and body2 both being suppressed.

Let me know if you have any question. Thanks!

[swhite]

As long as you created each body as a seperate body when extruding, yes. If however you used the default extrusion which simply adds them as additions to bodies, then no.

[Maarten65]

I disagree on the previous answers.

You cannot suppress a body. You can only suppress a feature which can result not creating a body. 

[johnsonshiue]

Hi Maarten,

Although I offered an explanation back in 2013, I think it is a needed feature. The user can hide a solid body (hard to control in iPart) or suppress the body generating feature. However, the implication is that some cross-body features may be suppressed as a result. Also, when feature/body dependency becomes intertwined, there isn't an efficient way to suppress the body-generating feature. Delete or suppress body command is needed.

There is a workaround I am not sure if you are aware. You can use Delete Face -> Lump selection to remove body geometry, not body definition. The command creates a Delete Face feature in the browser tree. It can be suppressed and unsuppressed on iPart table. However, the body definition remains there.

Many thanks!

[meGVGMF]

Hi @johnsonshiue 

If you're looking for a usecase (such as one may be)...

I'm modelling the volume of an assembly to be used externally to Inventor.

The assembly has two positions.

I have derived simplified/fused versions of each state into .ipt's, derived one of these again into another part where I've filled in the spaces. Finally, by deriving again into the same file, and then subtracting, the simplified version, I get the volume.

What I was hoping to do was make an iPart, so that I could swap out the final derivation+combine in members representing the two positions.

But without solid body suppression it seems like I'm stuck copying and pasting volume file and performing the substitution manually.

Thanks

[Anonymous]

Yeah sorry about that, I only noticed that part of your response after I posted, and already had my mind on other things.

You very probably right, although I've never actually heard of Lump Selection before.

I'll try to check it out tomorrow if I have a chance!

[johnsonshiue]

Hi! I could be wrong but I thought Delete Face -> Lump selection should work quite similar to "Delete Body" (not yet available). In an iPart, you can suppress the Delete Face feature. In one member, the body geometry is gone and in another member, the body stays. It should work.

Many thanks!

[Hunteil · Accepted solution]

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@johnsonshiue wrote:

Hi! I could be wrong but I thought Delete Face -> Lump selection should work quite similar to "Delete Body" (not yet available). In an iPart, you can suppress the Delete Face feature. In one member, the body geometry is gone and in another member, the body stays. It should work.

Many thanks!

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This works for me it seems. I had to hide a cable + multi-pin connector on my model.

[laurence.marshall]

This is a lot easier than the suggestions 

Within the iPart table, if you add in a new column with the name of Solid1 and the overall part number as "Potato" as below, it will allow you to Suppress or Compute that solid feature:

Solid1::Potato.ipt - Suppress / Compute

Works for me, as I have parts with 20+ Solids, allows me to turn them on or off as needed. Some might argue that drawing as an assembly would be better for this use case, but this works for the OP.

[johnsonshiue]

Hi Laurence,

I wish it was that simple. I am not aware of a syntax like "Soldi1::ipt." This seems very SWX-like. Please share a simple example that works the way you described. Where did you find this solution? ChatGPT?

Many thanks!