View Full Version : A different workflow

07-06-2011, 08:57 PM
I've been using Inventor so far. It has a lot of nice features, but I've really gotten tired of the workflow, and I'd like to try a CAD program that uses a workflow I like. However, I don't know what CAD program uses this, and I'd like your suggestions.

Currently, in drawing a mechanism, I have to start by making the parts, and then assembling them into the mechanism. This is great if I know what parts I'm using, and just need to figure out what I can make with them. But this usually isn't the situation I'm in.

Usually I know what I want to make, but need to figure out what the parts will be. I want to start by drawing the size constraints, and making an approximation of what it will end up like. Then I want to take that and break it up into the different parts, so that this initial solid becomes an assembly. Thus each part is already assembled into the final product, and I simply have to add detail to each part (and possibly break them up further into more parts).

This workflow may seem strange to you. I've never actually seen anyone CAD like this. I like this workflow because it is how I develop software. It allows me to make big changes in the early stages of the design without worrying about the minutia, and my low-detail placeholders BECOME the final parts.

So, what CAD software can I use to work like this?

07-06-2011, 09:11 PM
That makes a lot of sense actually. I'm not really aware of anything that does quite what you describe. CAD modeling is usually a bottom-up approach rather than a top-down approach. I suppose you could roughly draw up parts, and go back and refine them after you get your assembly together, but that's just asking for trouble.

The mainstream CAD programs are

Creo Elements (ProE)

I have no experience with CATIA or Unigraphics, but I doubt they are what you are looking for. Solidworks, Creo, and Alibre are more or less similar to Inventor. Sketchup is designed for quick concept modeling. I was not at all impressed with it though.

07-07-2011, 12:19 AM
Wow, this couldn't be more perfect.
This summer I am interning at Autodesk and have been working with a group that is hoping to improve assembly generation. I was tasked with reproducing a model using three different methods of assembly creation, so I should be able to help you out. In some preliminary research, they have found that many of their users aren't aware of the different workflows available in Inventor. You mentioned that you don't like the bottom-up workflow that most people, including myself, use.
However, Inventor also has at least two different top-down workflows: sketch blocks and skeletal modeling.
Sketch blocks involves creating a layout of blocks, which come to represent parts in the final model. You then add sketch relations between the various blocks to create the geometry you want.
Skeletal modeling involves creating a "skeleton" of the assembly from one or several sketches, which are used to derive parts. The derived parts are then placed in an assembly and mated to the same origin (there's a special button to do this), making them all line up.
In both cases, you start out with sketches in a part file, but those sketches are ultimately used to determine location and association of parts in the end assembly.
Besides utilizing the top-down workflow that you like, these two methods of assembly construction are very powerful in that they allow you to use a single file to control dimensions and relations. It allows for very rapid iterative design.
Sorry if my explanations are a little confusing, but as I said, I'm used to the bottom-up approach and have only been learning top-down recently. Here's (http://www.youtube.com/watch?v=KsZA79Oaazc) where I began to learn skeletal modeling, and Autodesk's website has some okay tutorials.

07-07-2011, 08:09 AM
In previous years, when I quickly prototyped our robots for spacial constraints, I usually started with large 'blocks' that represent the drive train, mechanisms, etc. Then I extruded out holes from the blocks in order to represent the Aluminum Bar. Then I added holes where necessary. I could get a good concept of everything in about an hour and a half. Then I'd start a new assembly using a bottom-up approach. This is how we did our '08 bot. The frame was one of the more successful and robust frames we've done (2nd to our '11 bot). The methodology was useful for answering questions to our "can we do X" questions with regards to spacial constraints.

An example of this for our 2010 bot is here (http://www.chiefdelphi.com/media/photos/34576). The blue volume was eventually cut into for frame rails and other constraint testing, then I made new parts for the lower frame and attached them to the purple frame in that photo.

Another edit -- I'll also point out that I made that blue volume into a shell, which I then put around the [semi] detailed CAD as we went along through the design. That allowed me to verify that our kicker (for example) would also clear during a bump traversal.

07-09-2011, 10:31 AM
I looked at some videos for skeletal modeling and sketch blocks. I learned how to link parameters between parts, but that's not really what I was asking.
Is there a way to take a single part and slice it into several parts?
In LabVIEW I can select a piece of code, go to "Edit > Create SubVI", and that piece of code is moved to its own file, but stays in place and connected to everything around it. Why can't I do that here?

Jesse, are you saying you make rough prototypes to work out the geometry, and then constrain your actual parts to those prototypes?

The reason I want to convert a prototype part into several actual parts is that deleting a part and replacing it with another (and redoing all the constraints) is often messy and time-consuming.

07-10-2011, 04:50 AM
Inventor does have a Demote to subassembly operation to create a new subassembly from a collection of components, which seems kind of like LabVIEW's "Create subVI." The difference between this and what you ask is, of course, that this only works on the assembly level and not in parts. Would it work to combine this with in-assembly part creation (http://wikihelp.autodesk.com/Inventor/enu/2012/Help/0073-Autodesk73/0460-Assembli460/0461-Build_as461/0480-Componen480/0485-Create_p485)? You would have to create a new part whenever you wanted to add a feature to your "part" and your design would consist of a bunch of part files in the end that may or may not actually have meaning in your final design, but it seems like it would achieve what you're looking for.


07-10-2011, 11:48 AM
I suppose I could do it that way. It seems like I'd just be making it harder on myself, though - I wouldn't be sure what the actual parts were, and I'd be dealing with more constraints than ever.

Actually, I think the constrain tool is something Autodesk could really improve upon. I often have several parts that are connected in the same way. I'd need to think about this one more before making an actionable suggestion.

To clarify my metaphor, the VI is both a part and (when it contains subVIs) an assembly. The actual code are the features and solids.

But it sounds like there is no CAD software that is meant to work like this. That's unfortunate.

07-10-2011, 12:26 PM
This is actually very common, and SW/Catia have many features built in to facilitate this. I would assume Inventor has them as well.

Before any detailed component level design of a system, I ALWAYS make a sketch that fully shows the mechanism. If it's a gearbox, it shows all the gears, bolts, motors, etc... An Arm would show the whole system, and it's full range of motion. Sometimes I'll even draw multiple mechanisms on there equal, and not actually dimension the lengths, but dimension the desired end results. By geometry the lengths required for arm A and wrist B, etc. etc. will be solved automatically. This is GREAT for uneven 4 bars or pneumatic rotary mechanisms, but that's off topic.

You may find that after getting good at designing systems fully in 2d, you may not even want a reflexive option, as you know understand the system and it's associated sizes, parts and dimensions better. Pretty much, immediately going to drawing parts at the 3d component level is the WORST way to design in my opinion.

Well, once this sketch is created it can be linked a number of ways depending on whatever my preference was at the time. Austin Schuh got me into sketch blocks a while back, but I've been burned a few times by them breaking after large changes (he has as well), so I've shied away from them. Sketch blocks let you put that sketch into any number of parts and use it to pull dimensions/geometry off of. They're all linked to the original sketch as well. For simpler sketches they're fine, but 300+ features (like a whole robot), and they become a pain.

What I do now, which is far less clean than sketch blocks, but doesn't blow up as often, is to use assemblies to link parts. I'll create the same base sketch as before, and you'll still have to create the net shape of each part. After that, I'll create parts within the assembly that reference the other parts, or add equations to the original part, or just add features to existing parts that are concentric (or other relation) to their mating features on other parts.

Using this method, we currently have an elevator drawn up where we set the width of the outer section, the height of the outer section, and our bearing gap. It then makes all the appropriate changes to all parts.

02-12-2012, 03:12 PM
Sorry to bring back an old thread, but I just found something that seems to apply to this topic: Autodesk Inventor Multi Body Assembly Layout (http://www.youtube.com/watch?v=N5abPC8wAqw).

Not sure if this is the same as the sketch blocks that were referenced previously, but it allows you to make all the parts of your model within one Part file, then break them into individual parts within an assembly at some later time. Still not 100% because you have to split the features into new bodies when you create them, but it seems to be closer to the desired work flow.

02-14-2012, 03:22 PM
This is a great thread that highlights the need to improve our understanding of the design work flow. The good news is that many of you have responded correctly that using a 2D sketch to create your basic design, testing limits of motion, etc, is a good starting point.

In the excellent Built By Design videos, the FIRST team members highlight many of the issues brought up in this thread and provide solutions. Start by taking a look at this,


02-14-2012, 04:50 PM
Our team uses layout sketches and in-reference parts to plan out a lot of our layout in Solidworks. We add holes in assembly mode and then propagate them to the parts, which helps to ensure consistency between the pieces. I'd also recommend investigating some of the specialized tools CAD programs have for this. For example, we use weldments sketches and extrusions to lay out our chassis even though it's not welded, allowing us to do the whole thing in one part rather than seven, change dimensions much more easily, and automatically generate cut-lists.

JD Mather
02-24-2012, 05:43 PM
I recommend looking into multi-body solids techniques
and sketch blocks
and skeletal modeling