Layout Based Assembly Design

Do you evaluate your mechanism assemblies before investing 3D modelling time?

Having participated in several design projects requiring the development of a mechanism, I’m sure I’m not alone in investing a fair amount of time in a mechanism assembly which, according to my trusty pen and notepad will function beautifully, to find that the reality is that its fundamentally flawed.  So, how can SolidWorks help in this stage between notebook scribbles and a fully solid model?

Layout Based Assembly Design allows us to create & evaluate our mechanism assemblies as 2D sketches.  The car jack seen below for example has been created as a typical SolidWorks assembly, with several individual parts mated together to provide mechanism movement.

When fully retracting the jack, a fairly obvious design flaw with the top link becomes evident, meaning the jack doesn’t retract low enough. 

Of course, we could make some changes in this assembly to overcome this flaw, however given that I’ve already spent time creating the assembly and now, I’m  looking to spend more making changes, it may have been more efficient to conceptualise my mechanism as a Layout Based Assembly Design, then create the 3D geometry.

 

We begin our Layout Based Assembly Design using the ‘create layout’ button, once we’ve done so, we’re ready to sketch in our first component.

 

When using Layout Based Assembly Design, sketch blocks represent individual parts so we’ll turn our sketch entities into a single block using the ‘Make Block’ button.

To represent the rest of our components, we could either create them or if we already have them (as I do here) we can use the ‘Insert Block’ button.

 

Once we’ve inserted our subsequent blocks, sketch relations can be used to associate the blocks together.  In this case, I’ll be using a concentric sketch relation

 

Now with all my sketch blocks in place and sketch relations added, I can move the mechanism and begin to evaluate it.  The issue we identified from the original assembly now becomes evident.  The difference here is, as I’ve not had to create 3D geometry or even mate the components together I’ve identified this issue in a matter of minutes.

 

Rectifying the flaw is as easy as deleting the offending block and replacing it with a new one. Evaluation tools such as measure are supported in a Layout Based Assembly Design, so we can be sure we’ve improved the design.

 

 

Once satisfied with our mechanism assembly we can convert the blocks to 3D geometry easily by right clicking on the block in the feature manager tree and selecting ‘Make Part from Block’

Notice at this stage the block is converted to a part file, which when right clicked has the option to either ‘open part’ or ‘edit in context’ from the toolbar at the top.

 

 

The end result of converting my sketch blocks to 3D geometry can be seen below.

 

 

Could Top Down Assembly Modelling save you time?

Having recently joined the SolidWorks technical team at TMS CADCentre a lot of my time has been dedicated to expanding my SolidWorks knowledge by participating in SolidWorks training courses.  Although I had used SolidWorks extensively in my own design work and considered myself as somewhat of a seasoned user I was amazed at some of the functionality covered in the training courses that I simply was not aware of.

Top down modelling from Assembly Modelling is a prime example of this and will be the focus of this article.  By ‘Top Down’ we refer to creating parts in the context of the assembly as we go, opposed to the more commonly used ‘bottom up’ method wherein all the parts are created separately.

The intention with the crank shaft model seen below is to add a pulley.  The pulley and associated parts could be created separately and added (bottom up technique) but as I need to reference other parts in the assembly it makes sense to use the Top Down in context technique.

Before beginning you can set any subsequent parts created in the assembly to save as external part files under system options/assemblies.  If you do so, you will be prompted to define a save location upon new part creation.

To start adding your new part go to insert components and when prompted select a reference planer face.

The assembly is now ready for the creation of a new part.  As the geometry I require to create the pulley already exists I don’t need to bother re-creating it and can instead just do a simple convert entities command and a basic extrude.  The outer diameter is taken from the pulley at the opposite side of the crankshaft and the inner diameter defined by the pulley end shaft.

The new part appears in block colour for clarity until clicking the confirmation icon in the top right corner.  Note how the new part is now inserted into the tree and appears in the defined save location if you chose to ‘Save new components to external files’.

And that’s it! I’ve quickly and easily added a new part to my assembly without even having to create a sketch by using in context top down modelling.  Using the same quick process I’ll also add another pulley to simulate how this crankshaft could connect to the camshaft.

Notice I’m not constrained to referencing a face when creating my new part – I can use a plane, which is what I’ll do here.  The camshaft pulley is created using some simple geometry and a boss extrude.  Mating this pulley in place is not essential as it’s likely I would go on to construct the camshaft which the pulley would be fixed to.

Lastly, to complete my in context modelled pulleys I’ll use a belt to link them using the Belt/Chain tool.  Notice how the belt/chain tool inserts only a representative sketch line.

A top tip with the belt tool is to select ‘Create belt part’ under properties.  This creates the belt as a separate part, meaning it can then be opened and edited.  This is useful here as it means we can extrude it and have a better representation of a belt than a sketch line.

I hope you find this functionality as useful as I do when it comes to simplifying and quickening the process of adding parts to an assembly.  Now go try adding some in-context parts to that old assembly you have!