Trouble creating flat pattern with assembly features

[darrynrow]

Hey Guys

Im having a problem with my assembly and creating a flat pattern from a sheet steel box created within the assembly.

I have done all my slots, holes and tabs within the assembly environment by projecting the geometry onto sketch planes and following through with cut out extrusions. The box's are to be laser cut and then cnc bent to form a chassis for a flat chain. How do I get my features to come out on the flat pattern and furthermore, save the flat pattern and its features as a laser friendly 2D sketch?

Regards

Darryn

[Rob67ert]

What is the problem you have?
The slots and holes you made are only in the assembly, not in the sheetmetal part.
Open the part and you will see.

I don't know if it is possible to get the slots and holes transferred to your sheetmetal part.

[darrynrow]

The problem is that when the sheet steel box is converted to a flat pattern, its leaving all the extrusions out. I do understand that it is still regarded as a seperate part by inventor, as it was creasted within an assembly.

If it is the case that these cut outs cannot be merged into the flat pattern, what would be the right way to go about sketching slots etc onto a folded part, because doing it on the folded model without any reference of where the slots and holes need to be would be extremely tricky and time consuming. 

[Rob67ert]

In the assembly, use edit part. If you now make a sketch, you can use "project geometry" But remember the parts will be "adaptive"

[IgorMir]

What you could do is to create an assembly of all the standard parts which are going to be fixed to the sheet metal frame. Then derive this assembly to a new part file. Save that part and derive it into a sheet metal part file. Now you have surfaces of the standard parts which you can use as references to build the sheet metal frame of yours.

Cheers,

Igor.

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@darrynrow wrote:

The problem is that when the sheet steel box is converted to a flat pattern, its leaving all the extrusions out. I do understand that it is still regarded as a seperate part by inventor, as it was creasted within an assembly.

If it is the case that these cut outs cannot be merged into the flat pattern, what would be the right way to go about sketching slots etc onto a folded part, because doing it on the folded model without any reference of where the slots and holes need to be would be extremely tricky and time consuming. 

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[SteveMDennis · Accepted solution]

@darrynrow

As the replies indicate by default assembly features are not ever pushed directly into the part, that's why they are defined in the assembly. Part files know nothing about assembly features.

There is a longstanding request to push assembly features into parts but that is not part of Inventor's functionality today.

If you used assembly features just to get projections from other parts in the assembly you can do this (as one reply states) by using cross part projections while editing the part in place in the assembly.  This seems like the fastest way to the goal line as far as I can see for the case you are describing.

[IgorMir]

And it is sure way to see the OP flooding this forum with questions why the assembly errors out all of the time!

Sorry Steven, just couldn't help it. 🙂

Cheers,

Igor.

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@SteveMDennis wrote:

@darrynrow

If you used assembly features just to get projections from other parts in the assembly you can do this (as one reply states) by using cross part projections while editing the part in place in the assembly.  This seems like the fastest way to the goal line as far as I can see for the case you are describing.

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[SteveMDennis]

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@IgorMir wrote:

And it is sure way to see the OP flooding this forum with questions why the assembly errors out all of the time!

Sorry Steven, just couldn't help it. 🙂

Cheers,

Igor.

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@IgorMir

While it is true the cross part projections can lead to very complex systems that will perhaps fail we have many customers using cross part loops to do many successful models that are fully updatable when the other parts change.

[mcgyvr]

@darrynrow

There is an app for that..

This will push assembly level features down to the part level..

This app bridges the open gap until Autodesk gets around to adding this functionality to the software.

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=4113747616755499758&appLang=en&os=Win32_64

In the future though you should learn to edit a part in the context of an assembly so that features can be created on the part and negate the need for the app.

This is done by ensuring that the file itself isn't open already then right clicking on the part and select "edit"..

You are at that point editing the part like you had the ipt file itself open.. But you can view/align/project,etc.. assembly level information for alignment,etc...