Which method is best, Top-Down or Bottom-Up

My company is converting/implementing SolidWorks and I wonder which
method is best, Top-Down or Bottom-Up. Understand the assemblies I
speak of have existed for many years. We re-configure them daily for
orders. They are built from many inventoried parts that contain
slight differences between them. Many parts are used in many
different assemblies. Any guidance would be greatly appreciated.

Gromit

 

If you're using models of existing parts, it would seem that bottom up
is the way to go.

 

The assumption here is that you don't have pre-existing SW parts, but
do have many parts in some other system. Not knowing specifics as to
what it is you are really talking about makes it a bit hard to
generalize, but generalize we will.

Do you have an existing PDM system? That might play into the answer.

How many parts in the typical assembly? High range and low range
please. Do the assemblies have many sub assemblies? Of the parts in an
assembly how many are those that contain slight differences?

There would be two approachs to implementing SW in the scenario you
have presented. Neither really has much to do with top down or bottom
up design.

1. For the parts with slight differences use Design Tables. This will
generate many configurations and this might impact performance and the
ability of your PDM to handle those parts. Ditto for assemblies, they
can also be made with design tables.

2. For the parts with slight differences use a database to create each
part from a generic part. This requires use of the API and is similar
to how the Toolbox works for fasteners. Each part will have one
configuration. Most PDM systems will be able to deal with the
subsequent parts.

and of course you could just model each part separately which is the
third and most basic method.

In general you use top down to control the geometry of parts related
by geometry through an assembly or inserted part. Since your parts are
already defined this would not be appropriate unless the pre-existing
parts in some way drive the sizing of parts in a top level assembly.
Then you would have to create a new configuration or a copy of the
assembly for each variation.

Using parts and assemblies that are configured assures that things
that are supposed to be common remain common. Using copies gives the
best performance and is easiest to manage files.

 

In addition to what other experienced users of SolidWorks in a company
environment have noted, I wonder whether you have considered hiring a
SolidWorks consultant to go over your specific company's needs so you
can get to bottom line "must avoid" and "must have" and then the grey
area decisions.

A number of people here on this board are consultants and their
websites list their type of work. Your VAR ought to know who is
available in your region.

These guys hired for 2 days might save you man months of wasted time
in the next year, and a large amount of frustration. Their fees may
be high, but they earn it by keeping you from avoiding the worst of
the known mistakes.

Bo

 

The quick way to know which route to go:

Is the part specific to that assembly?
That piece should be created top-down. Example: some edging

Is the part used in multiple assemblies?
Best to use bottom-up. Example: A screw

Even if it just has slight variations, it's best to use top-down
instead of configs. However, it is possible to tie those two together
and have a really fancy top-down assembly. How? Make an assembly that
is driven by a sketch, then tie the sketch to the top assembly. Sound
complicated a little I guess, but that will keep you from having to
make new drawings everytime and you can work configs into that
assembly.

 

Gromit,

I just worked a project that was entirely top down and will add a few
observations here on the subject that I haven't heard mentioned
before.

The model I built is for all practical purposes a simple open topped
box. The design intent is for the box's internal volume to meet
certain criteria. The criteria are contained in a spreadsheet from the
customer in the form of length, width and depth.

Step 1. Build a part with a design table driving this simple "box".
Cut and paste the customer's criteria into the design table
spreadsheet.

Step 2. Insert the "box" model into an assembly as an envelope.

Step 3. Model all the components off the envelope using in-context
references for all the features that might be driven by the "box"
geometry. This means the sides and bottom.

Step 4. Create a design table in the assembly and cut and paste the
customer's information into that table as well using the DT in the
assembly to drive which configuration of the "box" envelope part is
being used.

The assembly will now cause all the parts to change depending on which
configuration of the "box" envelope is being used. Note that the parts
in the assembly have only one configuration except for the envelope
part which has multiple configurations. This means that it would not
be possible to make a standalone drawing of the in-context parts
without also having the assembly also in the drawing to drive which
configuration is being used. For this project that is OK because the
customer only want's drawings of the entire assembly.

This excercise also demonstrates why having in-context features in
general can be very dangerous. When there is an in-context feature
driven by a configuration of another part through an assembly that
feature's dimensions will require the assembly to be open to update
and will not be controlled by anything in that part. The part with the
in-context reference will therefore have multiple configurations
without having them explicitly managed by the configuration manager in
that part. Instead they may be managed by configurations in either the
referenced part or the assembly. In fact the parts with in-context
references will only show one configuration and "Find External
References" will only show the currently referenced configuration for
that part.

TOP

 

Gromit,

As Top's example shows, there's no hard and fast rule that everything
must be one way or the other. Each situation has to be judged based
on the requirements of what is being created in SolidWorks. Also, Top-
Down is a tool for design of an assembly, but it can be dismantled
once the assembly is complete (e.g., remove all in-context
requirements after assembly desgin is complete). If you do have
common assemblies slighted edited to suit each customer, perhaps
consider an even more robust approach by controlling design with a
macro that gets minimal input from the user and automatically
generates the expected results. Just some ideas.

Matt
http://sw.fcsuper.com