Multi part holes

[zeville]

I have a 3 part assembly

Holes have to be made though the 3 parts

The holes can be made and snet/projected/though all/though distance  and this work fine

The holes are shown in each part and the participant command works fine

The holes are shown in a drawing file....all GOOD

BUT

The holes are NOT shown when each part is opened!

What am I missing?

[JDMather]

An assembly (*.iam) is worthless without parts (*.ipt) files.

You made the holes at the assembly level (called match machining in the real world).

I think there is a add-in at http://labs.autodesk.com to push the holes down to the part level.

A search here might turn up the exact link.

[SBix26 · Accepted solution]

You're missing a number of things:

1. Always post the version of Inventor that you are using in the first post

2. Opening an assembly file without its parts is like trying to drive a drawing of a car

3. Assembly holes are exactly that-- holes added after assembly.  This is how you deal with the need to first put parts together before trimming/drilling/tapping, etc.  There are a number of different techniques for getting holes in parts to line up with each other:

    a. Adaptive-- put holes in one part, then edit other parts from within the assembly and project those hole centers.

    b. Bolted Connection generator

    c. Multi-body solids/derived parts (my favorite)--  model all three parts in one part file as separate solids, then Make Components to create separate part files from the "layout" file.  All the cross-part relationships are done within one part file, making it much simpler to design.

Post the three parts for your assembly and tell us what version they are.  Someone here can show you one or more ways to accomplish this.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
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[IS200]

I convert the assembly to a weldment and place the hole feature under preparartions.

In the drawing environment I place a view of the assembly and, under the 'Model State' tab choose 'Preparation' and select the part I want to detail. This shows the part with any features added at the preparations level of the weldment.