Editing in an assembly ...... pls help

[paulchapman71190]

Im working on a Steel, I need to make a hole for a bolt hole needs to disect to 'parts'. Normally when I edit parts in an assembly I just double click them, they become transparent and I can do all my edits. Since I need to make a hole that cuts into both parts, I just went to the 3D Model tab started a new sketch and extruded out the cut. However doing it this way does not reflect the changes when the parts are opened on their own. Is there a way to do this?

I have read a very similar post from a few years back, however, the solution was to re-draw the parts as surfaces which i certainly do not want to do.

i am using Inventor 2012

Thanks,

Paul

[JDMather]

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@paulchapman71190 wrote:

...

I have read a very similar post from a few years back, however, the solution was to re-draw the parts as surfaces ...

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I have never heard of a solution like that?  Can you attach the url?

The easiest way (if it will work in your case) is use the Bolted-Connection Design Accelerator in your release of Inventor.

If Bolted Connection is not appropriate for one reason or another - there are other ways.

[CCarreiras]

HI!

You can use the tool "Bolted Connection" to do this.

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[Curtis_Waguespack · Accepted solution]

Hi paulchapman71190,

There is a trick for doing this using the Bolted Connection tool.

You can use the Bolted Connection tool to place the holes without placing any hardware, and Inventor will "push" the holes from the assembly into both of the part files.

Create Bolted Connections

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-428F9F0B-9CB7-4734-ABBC-9CA9068214BD

About Bolted Connection Component Generator

http://help.autodesk.com/view/INVNTOR/2014/ENU/?guid=GUID-3A51B44B-7C58-44F2-A608-3932A9F787E7

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[paulchapman71190]

Yes, this problem had been flagged up previously, and as I have said, the solution was to redraw the parts as a surface (really!?). The problem was so greatly explained I copy and pasted a lot of the text and edited to suit.

Anyway, thanks a lot for the help this has answered my question!

Paul

[paulchapman71190]

Out of curiousity, what are the other ways if i am to encounter a problem with the bolted connection? 

[JDMather]

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@paulchapman71190 wrote:

Yes, this problem had been flagged up previously, and as I have said, the solution was to redraw the parts as a surface (really!?). .

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Can you provide the url for this reference?

[paulchapman71190]

http://forums.autodesk.com/t5/Inventor-General/Edit-multiple-parts-in-assembly-and-upating-parts/td-...

Unless I have got myself confused, the solution is to redraw the parts as surfaces?

Even if this solution is the right way to do it, i find it hard to follow, so any other solutions would be great.

Thanks

[JDMather]

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@paulchapman71190 wrote:

http://forums.autodesk.com/t5/Inventor-General/Edit-multiple-parts-in-assembly-and-upating-parts/td-...

Unless I have got myself confused, the solution is to redraw the parts as surfaces?.

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You mis-understood the instructions.

The OP has an existing part and is modeling around it.

Nothing is recreated.

Derived Components technique was used to place the existing part (as a surface body with no mass) into a new part file for modeling the box that goes around it.  This is an advanced technique that you will eventually get to, one way or another.

But again, nothing was "redrawn as surfaces".

[SBix26]

No, you're misunderstanding the other thread that you referenced.  Nothing in there about modeling parts as surfaces.  The surfaces referenced there were just the derived-in circuit board that the OP wanted to design around.

Assembly features in Inventor are just that: features created after assembly.  Bolted Connections is a special exception to that rule.  Multibody solids is a great way to design with inter-part features, but you have to start that way; it's difficult to convert to MBs late in the game.  

For your situation, if the Bolted Connection solution doesn't work, adaptivity is probably the best bet: in the assembly, edit one of your parts and create the hole you want, located where you want it.  Edit the other part and create the hole, but leave its location unconstrained.  Make the second part adaptive in the assembly, then constrain the two holes together-- this will make the "floating" hole line up with the fixed one.  You could also leave the hole size unspecified in the adaptive part and constrain the edges together, so both the location and size will adapt.

Hope that helps clarify things for you.

Sam B
Inventor 2012 Certified Professional

Inventor Professional 2015 Update 1
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

[CCarreiras]

Hi!

No Paul, Forget the surfaces...

In newer versions, there is a option to do that: "Send to Parts"

After this option in previous Inventor releases, i used to do that With a plugin Called Feature Migrator (I think this Pluggin is the parent of the feature  showed above).

Go to "Autodesk Exchange app" and try it.

https://apps.exchange.autodesk.com/INVNTOR/pt/Detail/Index?id=appstore.exchange.autodesk.com%3afeatu...

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