Autodesk Inventor: Assembly techniques for Woodworkers

If you’ve had any training with Inventor at all, then you should be able to model a simple part, ready to be included into your Assembly. The trouble is, no one ever seems to point out to you that this is the easy bit!

Autodesk Inventor - Assembly required

Once you have picked up the bug for Inventor, I am sure that you will soon find that you will want to model Everything! and modelling Everything soon leads to massive assemblies with a huge number of cross part relationships that fall apart around your ears every time you try and change something.

But it doesn’t have to be this way! There are a number of different Assembly modelling techniques that you can use to help you build robust and easy to manage assemblies.

Each of these techniques is a description of a way of working with Inventor Assemblies – not a format that you must follow. As you become more experienced you will find that different Assemblies require different techniques, and that you may even combine different techniques within one model.

I have written a tutorial for each technique – based on items every Joiner, machinist, or woodworker will have made when they were starting out. Each PDF tutorial is complete with Inventor 2010 part and assembly files.


The Bottom Up Technique

Autodesk Inventor Bottom Up Modelling TechniqueThis is the traditional Inventor Assembly modelling technique that you will have learned in your basic training. The help documentation is written assuming that you will be using this technique.

The essence of the ‘Bottom Up’ Technique is that each part is created individually, and then all the parts are inserted into an Assembly and constrained to each other.

There is no link created between the parts, the parts fit together because you designed them to fit together. If you change one part, you’d better know which other parts will be affected by the change and make sure that they are updated accordingly!

This technique works well for small assemblies with only a few parts and, of course, if you want to show mechanical motion – you will have to use constraints. However, on large assemblies one change to a key part can lead to a ‘House of cards’ effect which can leave to you spending all afternoon straightening out a mess of cross part fits and constraints.

This technique can be used effectively on large assemblies which are built from many ‘Stock’ components that aren’t subject to change.

Click here to go to the tutorial page:
Modelling a Bench hook, using the ‘Bottom up’ technique.

The Top Down Technique

Autodesk Inventor Top Down Modelling TechniqueIn this technique you start with an Assembly file and build all your parts within the context of the Assembly.

This technique makes it easy to use Inventors ‘Adaptive’ sketches and features to link parts together in the Assembly. This creates an Assembly model that is controlled by a ‘Master’ part (or a series of Master parts). This is a great way of ensuring that parts that need to fit together always fit together, without any help required from you.

This technique is extremely intuitive and quick. On the downside you can still get yourself into a right pickle if you manage to build any self-referencing loops, so this technique is still only appropriate to small to mid size assemblies, where cross part relationships are readily apparent.

I would also like to point out that Adaptive parts are re-calculated every time you perform a local or global regeneration, so they place quite an overhead on your PC.

In the tutorial that demonstrates this technique I show how you can turn ‘Adaptivity’ on and off, to speed up Inventor’s performance.

Click here to go to the tutorial page:
Modelling a Shooting board , using the ‘Top down’ technique.

The Skeletal Modelling Technique

Autodesk Inventor Skeletal Modelling TechniqueYou won’t find a lot about this modelling technique in the help manuals!

Skeletal modelling uses Inventors ability to ‘Derive’ Parameters, Sketches, Blocks, Work features, Features, Surfaces and Bodies between parts.

Basically, you create all your Parameters and sketches in one part file and then Derive the required parameters and geometry into separate part files*. You then build your part features in each part file using this shared geometry.

The beauty of the technique is that when you come to place your parts into an assembly, no constraints are required! You can simply insert all you parts at their origins and ground them.

No constraints are required because all the parts are in the right place. Any changes to the underlying geometry in the ‘Skeleton Model’ part file will be propagated through all the parts that are based on the Skeletal model.

You can still ‘Un-ground’ a part and build in constraints if you need them. There is usually no call for Adaptivity, because the cross part relationships are handled outside of the Assembly model.

This technique would not necessarily be appropriate for Assemblies that use all ‘Stock’ parts. It is important to remember that the ‘Skeletal’ model file must be managed along with the rest of the files that make up the assembly. This technique is very useful when you are creating a model that uses a large number of Bespoke parts, that will not be useful in other assemblies.

*The ‘Master Part’ file which contains only parameters and geometry looks kind of ‘Skeletal’ – Hence the name ;-)

Click here to go to the tutorial page:
Modelling a Mitre block, using the ‘Skeletal Modelling’ technique.

The Multi-Body Master Part Technique

Autodesk Inventor Multi Body Master Part Modelling TechniqueO.K. This techniques doesn’t have such a catchy title. This technique is very similar to the ‘Skeletal’ modelling technique, but uses some new tools that were added to Inventor 2010.

Inventor 2010 allows us to create ‘Multi Body’ parts. Each body could be used to represent a separate part. This modelling technique is similar to ‘Skeletal’ modelling, except that we can ‘Derive’ a whole Body out into a part file to create a new part.

In this technique we can model an entire assembly in a part file, and use Inventor 2010’s ‘Make components’ tool to automatically create a derived assembly based on the Master part.

Similarly to ‘Skeletal’ modelling, no constraints are required – all the cross part relationships are managed via the ‘Master’ part file.

Once again, this technique is excellent for creating assemblies with a large number of Bespoke parts.

Click here to go to the tutorial page:
Modelling a Saw Horse, using the ‘Multi Body Master Part’ technique.

Combining Assembly Modelling Techniques

As I mentioned at the top of the article – these techniques are simply ways of describing how you might use inventor to create Assembly models. It is perfectly possible to combine different techniques within one model.

For example, ‘Library’ parts are probably best created as iParts and set up to be distributed via the server. You could even add them to the ‘Content center’ (The frame generator makes use of Skeletal modelling and the content center – but that’s next time ;D ).

It is possible to combine bespoke parts created by the ‘Multi body master part’ technique, within the same model as a frame generator sub assembly, Bolted connections and your own Library iParts.

Have fun with it, enjoy building your Assemblies and remember – don’t let yourself get into a Cul-de-sac, there is always another approach that could help you out!

Bonus – you can now watch these tutorials on Video as part of Autodesk University Virtual 2012 (may require a free login). Here’s the link: