Top Down Design for Curvy Parts (Alibre Design Tips)1 Apr, 2008 By: Aaron Arnold
Save time when designing curvy parts by modeling the entire product first.
Let's say you're trying to make something ergonomic like a computer mouse. You know the overall shape you want to achieve, but it's composed of multiple parts that all have to fit together with perfect tangency on every edge. There's an easy way to accomplish this task and a hard, time-consuming, laborious way. Unfortunately most people intuitively use the second. If you're thinking to yourself, "this will require a lot of lofts and guide curves" or anything along those lines, then this tech tip is for you. Prepare to save a couple hours or days of work for these types of projects.
Let's use the example of an ergonomic computer mouse. As you can see from the image below, the model has several major components that combine to form one, smooth exterior surface. You can accomplish this design quickly, and you will not model each part separately. Once you've got this concept down, you can design things like this mouse in a matter of minutes.
The ergonomic mouse design used as an example.
Instead of modeling each part separately and from scratch, I will start with the completed model. Let me clarify: I am going to begin by modeling the entire mouse (except for the mouse wheel) as a single part. The idea is that I can whittle away at the whole design in such a way that doing a couple of Save As operations yields several parts that all come together in an assembly to form an exact copy of the original item, but incorporating multiple parts instead of a single part.
Step 1: Model the Entire Item
You can use any combination of tools to model the entire mouse as a single, solid part. I accomplished this step with one extrude boss, two extrude cuts, and some fillets.
Step 2: Start Whittling Away
Now that I have the outer surface of the mouse completed, I'll simply start cutting away to generate separate parts. First I'll create the bottom piece of the mouse. In essence, I want to remove everything that is not the piece I want. I'll do this by creating an extrude cut using the sketch profile below. The inside sketch defines the bottom piece and the outer rectangle ensures that everything between the two sketches will be cut, which leaves just the bottom. I will reuse this outer rectangle concept in every step, so keep it in mind.
The sketch profile used to create the bottom piece.
Click Save As and save it as BOTTOM. This is the orange piece in the assembly. Obviously this is not how the inside of the bottom piece would look in real life; it does however contain the exterior surface you're after, which is the whole point of this process. Later you would need to come back into each part and hollow it out and add any internal components or fastening mechanisms.
Step 3: Forming the Next Part
Now repeat the process. Your starting solid should represent everything except the parts you already cut out. In this case our starting solid is everything minus the bottom piece. To do this, edit the profile used earlier and delete the exterior rectangle. As you probably surmised by this point, this causes the bottom piece to be removed instead of singled out. So, edit that sketch, delete the exterior rectangle, and once the Extrude Cut feature is regenerated, you will see the image below.
The entire model minus the bottom piece.
Now you will repeat this process over and over until you have as many pieces as you want. Next form the blue piece in the assembly. The left side in the image below represents what you are starting with from the step above. The right side represents the end result.
Before and after an extrude cut.
To do this, sketch on the z-y plane so you're looking directly down on the mouse, and use a profile similar to the one below. I did a Sketch Mirror operation over the green reference line to halve my work. Once the sketch is complete, I'll use it for another Through All Extrude Cut command.
The sketch for using an Extrude Cut command.
Now, use Save As to save this piece as BUTTONHOLDER. Always remember to use the Save As tool when you have finished fleshing out a subcomponent because you want to be sure you don't overwrite a previous component.
Step 4: Onto the Buttons
Now, just as before, I'm going to design the other parts that haven't been fleshed out yet. This means I need everything inside the extrude cut I made earlier. I'm going to edit the sketch for the Extrude Cut I just made, but this time I'll put a big rectangle around everything. Now, everything between the two sketches will disappear and I'll be left with the blob of material that constitutes the buttons. Note that I modified the original sketch slightly on the left side to split the buttons.
The modified sketch for the Extrude Cut command.
To finish out the button section, I need to make an indention in the small piece that surrounds the mouse wheel. I'll use another Through All Extrude Sketch command to accomplish this, and then I'll Save As this part.
The sketch for the Extrude Cut command.
Now select Save As and name this part BUTTONS. As you may have guessed, the next step is to make the part that surrounds the mouse scroll wheel. As you may also have guessed, this lump of material is what was just removed with the last Extrude Cut operation. It's time for a big rectangle.
Step 5: Making the Mouse Wheel Support
Edit the sketch used by the previous Extrude Cut operation. Place a big rectangle around everything, and then exit Sketch Mode. All the material between the two sketches is removed, leaving only what you want.
Now, design a space for the mouse wheel to fit and add some fillets, etc. I did some basic modeling operations and achieved the part below.
Now, select Save As and name this part MIDDLEMOUSESUPPORT.
Now, select Save As and name this part MIDDLEMOUSESUPPORT.
Step 6: Putting It All Together
I'm going to skip the modeling of the mouse wheel -- it doesn't follow this process since it's not part of the curvy outer hull of the mouse. I've saved four parts now, and even though these parts all look drastically different, they share substantial portions of their feature histories with each other. In fact, as you've seen, these parts often differ only by a rectangle in a sketch.
It's time to insert these parts into an assembly. One great thing about this modeling method is that all these parts share the exact same local coordinate system, which means that constraining them becomes very simple, even though they are all very curvy.
Insert each part into the assembly, and make sure your cursor is hovering directly over the origin before you click to place the new part. This aligns the origin of the part you are inserting to the assembly origin (it visually lines it up, no constraints are placed). Since all the parts share the same origin, the whole assembly will line up because of the way you made these parts. The first image shows what each part looks like, and the second image shows what the assembly looks like if you've properly inserted the parts. (All your parts may be gray, just color them however you like.)
Each of the parts created.
All the pieces fit together perfectly if you insert them by clicking on the assembly origin.
If you wanted to constrain these parts together, right-click on each part in the Design Explorer, select Show Reference Geometry, and constrain those planes together.
Even though the assembly looks good, discerning readers know this is only the first step to the creation of this mouse. You've basically finished the outside look, but this model is still a solid hunk of plastic that doesn't have room for internal components. The next steps involve editing each of these pieces, removing internal material that is irrelevant to the exterior look, and inserting additional components and fasteners, etc. However, you have accomplished a task in a matter of minutes instead of an unbearable amount of time if you use a less-efficient method.