When I think about Bottom-Up Design, I picture myself pedaling my heart out mountain biking up a steep hillside. While to some, that may be the best part of the ride, I much prefer cruising DOWN the mountain instead. By that, I mean Top-Down Design.
What is Top-Down AKA In-Context Design?
Think about building a model whose shape and dimensions are driven by other components. The responsibility of matching the parts is on you, the designer. It entails opening individual windows, and having to make design changes in not one but two or more locations every trip around the design spiral to ensure a proper fit/alignment. A lot of extra time is being lost during this back and forth, and let’s face it, we just don’t have the time to waste.
This is where I introduce “Top-Down” or “In-Context” Design. Using this design method, parts can be designed from within the assembly itself to drive shapes, sizes and locations. No more opening new windows to model those easy brackets, plates, housings, etc. You can build them all right within the assembly, in the correct locations (because you never lose sight of the parent model).
On top of already being pretty awesome, a little bonus you also get when using Top-Down Design is the flexibility and stress free experience you get when/if design changes occur, whether it be from a customer, or something you just want to change, now your entire assembly, with all of the parts you designed within that assembly, will know how to update themselves based on the way you created them!
That is a HUGE timesaver considering all of the rework and attention that is no longer needed. And that is the point in which I was completely and utterly SOLD on this design method.
The Process
Here we have a basic circular enclosure that requires a top cover.
To add the top cover we first have to insert a New Part;
To do this, I selected ‘New Part’ from the Insert Components drop down menu on the command manager. You will then have to pick where you would like to build that part. The first option is to select an existing face or plane. This will align the front plane of the new part to your selection, creating a reference and automatically start a sketch. The second option is to select a blank region in the graphics area. This will align the origin of the new part to the assembly and will allow you to insert the new part with no references.
You can then reference the geometry of other components as needed.
Idea: Create base to show first method and lid to show second method.
I selected the top face of the cylinder because that is where the cover will be attached. I did a Convert Entities on both the outer and inner circles to match the size and width. I then extruded in (2) directions, up 10mm and down into the cylinder another 10mm.
If you are finished with the part for now, you can enter back into Assembly Mode by selecting the exit component icon in the right hand corner, or by re-selecting ‘Edit-Component’ from the Command Manager.
I placed the cylinder in a transparent mode so you can see what the newly added part looks like.
Circled in red you can see symbol designations that are not normally there. You may see up to (4) different variations of those designations;
In-Context – All references are working and all are up to date, the part can find the assembly and any other parts in the appropriate locations.
Out of Context – The assembly or part cannot be found where it was expected to be. Something may have been renamed or moved. You can edit the references and change them to files that can be found.
Locked Reference – This means the reference is currently locked, no updates will come through.
Broken Reference – A reference part or file is broken and cannot be retrieved.
You can easily see any reference and what it is related to by right-clicking on a file that shows one of the -> symbols and choose ‘List External References’. A dialogue box will open and show you the assembly name and location that holds the reference.
Now, when I selected the top face of the cylinder to be the insertion point of my new part, a mate was automatically created. This is called a ‘InPlace’ Mate and this mate will prevent any movement of the newly created part making it essentially fixed to the other part by the insertion point I selected.
If you are designing a part that you would like to move freely or be its own entity, the best option at this point would be to save your assembly, and then right-click and Delete that mate. You will get a warning explaining the following;
Click ‘Yes’ and delete the mate, you can now assign the appropriate mates that will allow any type of movement that is required. You can re-add any references you would like.
Note: This is also where you can see that if this part was inserted selecting a blank region in the graphics area, we would not have a mate to delete.
Lastly, you can save any component/part to its own external file by right-clicking the component and selecting Save Part (In External File). Alternatively, when you go to save your Assembly, you will be prompted to save the part either inside the Assembly, or to an External File.
Start saving valuable time, and take the ride from the Top-Down.