Part features supressed/unsupressed linked to configurations/representations

[0x3FA5]

Hi,

Assume there is a simple part with hole in it, and I would like to represent 2 different views on the drawing, one with suppressed hole, the other showing the hole.

Going further, I would like to be able to select a representation/configuration and previously selected features would be suppressed/unsuppressed.

This is very helpful in manipulation of the different stages of the design of a complicated part, especially since Inventor does not support folders in part environment.

Thank you for your replies!

[mcgyvr]

Are you asking for a solution/suggested workflow to achieve this currently or is this post intended to be an idea to improve the software in the future?

You can easily accomplish what you want right now by creating an ipart.. One member would have the hole present.. The other would suppress it.. You can then show either member in whatever drawing view you wanted and can toggle between the 2 in an assembly using the "change component" functionality or creating an iassembly there..

If this is an idea for future improvement then I suggest you sign up for beta to see what they "may" be doing in regards to configurations presently and I'm quite positive there is already a posted idea on the ideastation to implement "browser folders" and similar part level configurations..

[0x3FA5]

I am asking for a solution/suggested workflow to achieve this,

Thank you!

[Jose_Merino]

In your browser in View, make a new view, in that new view you can turn off  the visibility of your holes, if you make double click in master your will see your piece withe the holes, now when you transfer this to a

drawing you can choose which view you want to use.

 

[0x3FA5]

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@Jose_Merino wrote:

In your browser in View, make a new view, in that new view you can turn off  the visibility of your holes, if you make double click in master your will see your piece withe the holes, now when you transfer this to a

drawing you can choose which view you want to use.

 

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Not sure I understand..

In your browser in View - you mean in part or drawing? Did you mean just hiding the lines in the drawing?

[mcgyvr · Accepted solution]

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@0x3FA5 wrote:

I am asking for a solution/suggested workflow to achieve this,

Thank you!

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Ok.. So try making an ipart like I suggested above.. 3 or 4 different members each suppressing what you don't want in each.. Should be easy.. 

[Jose_Merino]

In your part screen. you can make a new view or views to have 3 different configurations, after in your drawing you can chose which configuration you want to use for work with.

[0x3FA5]

Please attach a detailed flow, since from what I see, the views are not related to features suppression.

[Jose_Merino]

If you want to suppress the other configuration then you can make a Level of Details. or make an ipart like our college mcgyvr, suggest.

[0x3FA5]

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@Jose_Merino wrote:

If you want to suppress the other configuration then you can make a Level of Details. or make an ipart like our college mcgyvr, suggest.

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Really guys, am I not getting something??

Aren't Level of Details for assemblies only??

Do I have some different Inventor from yours?

[JDMather]

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@0x3FA5 wrote:

Really guys, am I not getting something??

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I don't think these other responders understand your issue, so here we go again...

I don't own a rar extractor - I use only Windows to zip/extract files on my clean Inventor machine.

Can you use Windows to zip rather than rar?

[mcgyvr]

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@0x3FA5 wrote:

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@Jose_Merino wrote:

If you want to suppress the other configuration then you can make a Level of Details. or make an ipart like our college mcgyvr, suggest.

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Really guys, am I not getting something??

Aren't Level of Details for assemblies only??

Do I have some different Inventor from yours?

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I think Jose is confused..

Their suggestions don't make sense..

Try the ipart workflow..

[0x3FA5]

I apologize, for some reason it automatically creates rar.

[mcgyvr]

example ipart table.. I have a newer version than you so I can't edit/post the files.. 

[Jose_Merino]

Sorry, my mistake Level of Details is only for assembly, Sorry again.

ipart is the option.

[mcgyvr]

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@mcgyvr wrote:

example ipart table.. I have a newer version than you so I can't edit/post the files.. 

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and easily swapping between the 2 members..

[0x3FA5]

Thanks,

iPart seems to be the solution.

(It is actually a stripped version of SW design tables, lol).

The only thing I found strange, and I think it's some kind of a bug:

In my actual part, some of the features have sketched based on currently suppressed features, and even though the parent feature suppressed - the derived sketch is not!

I browsed through the iPart table interface and couldn't find how to suppress sketch based on "configuration", please point me in the right direction.

Thank you!

[SBix26]

I added this to the previous topic before I realized that you had started a new thread–

One possibility:

1. Model the part without the hole
2. Rectangular pattern the whole solid a convenient distance away, choosing New Solid option
3. Add hole feature to the new solid body
4. Create two View Representations, one with only Body 1 visible, the other with only Body 2 visible
5. Use these view reps to create your drawing views

The view rep can also be used in assemblies to show only the finished part.  If mass properties are important, then the finished solid could be derived into a separate part for that purpose.  This technique can be expanded to as many stages of manufacturing as you need, hypothetically.

This is definitely a workaround, but it works for most purposes, I think.  I'm hopeful that Autodesk can come up with a good competitive answer to SWx configurations.

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[0x3FA5]

Thank you for your detailed reply!

I mentioned holes only as an example of the feature I would like to suppress.. The actual part has some extrusions and radii, since it is a cast part that is going to be machined further.

[0x3FA5]

Nice workaround though, I will probably use it somewhere else!